Re: [kicad-users] Creating multiple circuit layouts w/Kicad
Use the append board function. Remember to move the current board away from the centre of the screen first or the two can get overlaid. Andy On Fri, 03 Sep 2010 22:43:18 - glen gad241...@yahoo.com wrote: Is it possible to pull in multiple circuits schematics in Kicad board layout? If I have a 6x4 board, I would like to etch multiple circuit layouts without wasting the whole board for for a 2x2 layout. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] own libedit symbol .lib library file
Yes you can place the lib anywhere you want. I keep mine in my home directory (linux version). This is the best option anyway, because there is always the danger of libs getting overwritten during a program upgrade. Just remember to include your libs into the project with the preferences library tool. If this gets tedious (you have to do this for each new project) you can modify the default kicad.pro project and add them to this, then they will be available to each new project automatically. Andy On Fri, 03 Sep 2010 12:55:02 - transistorman57508 transistortoas...@fastmail.fm wrote: Hello, I just started using kicad's LibEdit and am saving my new symbols to c:\Program Files\KiCAD\share\library\device.lib. Is it at all possible to create and use my own .lib file? Can I have it outside the c:\Program Files directory? For the footprints I would like to do something along the same lines too, would that be possible? Thanks, Frank Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] please review my first kicad project (and pcb design): an ADXL335 accelerometer breakout board..
One other thing I've just realised: The IC is a surface mount device Usually the module is designed for the tracks to be on the COMPONENT side of the PCB. If you intend to produce the PCB in the conventional way with the components on the top, and the tracks on the other side, then you may have a problem. Check the orientation of the IC very carefully, as you will need to fit it to the underside (copper) side of the PCB, and that will usually mean that you have to flip the module. Andy On Sat, 28 Aug 2010 01:10:59 +0200 Fabio Varesano fabio.vares...@gmail.com wrote: Hi Andy, thanks for having a look at this. Please read below.. On 08/27/2010 11:38 PM, Andy Eskelson wrote: Personally I don't like lots of filled zones unless that really are necessary, but that's a fairly minor point. Well, I read that this is good practice as this make less use of etchant during the etching process. Isn't that true? several other points: Do try to put your connection pins on the edge of the board. It makes wiring up much easier. You could also consider some form of connector. Yep, that's the best I've been able to come out with.. I do know that it will be painful to plug this. Do you have any suggestion for a 6 pin connector? Somehow I didn't find something suitable in the library. How are you going to mount the board? Some hardware mounting holes might be useful. Yep, good point. How do you draw mounting holes with kicad? The tracks to the pins look rather thin. Thin tracks tend to lift when soldering, also a small speck of dust on the film can cause a break in the track. Using a thicker track will help in both cases. You mean the tracks to the accelerometer IC? Well, they quite match the IC pins size. I don't think I could have made them bigger. Maybe you are suggesting making them thin below the IC and bigger on the rest of the board? On single sided boards, don't be afraid to use a few links it makes life MUCH easier. An Easy way to do this is to treat the board as double sided, and use the top tracks as wire links. Beef up the vias to a suitable size to take your wire links. Obviously you need to manually route this. I understand. So you are using wires as bridges to pass over one or more track, right? Interesting.. Thanks for your suggestions. Really helpful. You rock! FV Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] default libraries
Modify kicad.pro see my post to philip on the 26th aug Andy On Sat, 28 Aug 2010 19:36:49 - James jamesrsw...@gmail.com wrote: Can somebody tell me how to set what libraries are added by default to a new project? Maybe this is obvious but I haven't figured out how to do it. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] please review my first kicad project (and pcb design): an ADXL335 accelerometer breakout board..
Personally I don't like lots of filled zones unless that really are necessary, but that's a fairly minor point. several other points: Do try to put your connection pins on the edge of the board. It makes wiring up much easier. You could also consider some form of connector. How are you going to mount the board? Some hardware mounting holes might be useful. The tracks to the pins look rather thin. Thin tracks tend to lift when soldering, also a small speck of dust on the film can cause a break in the track. Using a thicker track will help in both cases. On single sided boards, don't be afraid to use a few links it makes life MUCH easier. An Easy way to do this is to treat the board as double sided, and use the top tracks as wire links. Beef up the vias to a suitable size to take your wire links. Obviously you need to manually route this. I'm not going to comment on the actual circuit as I've never used this device. Regards Andy On Fri, 27 Aug 2010 21:18:29 +0200 Fabio Varesano fabio.vares...@gmail.com wrote: Hi guys, I just finished working on my first pcb design and I did it with Kicad. I'm a computer science master student so I'm pretty confident with computers and I know my stuff in the software side of things .. but we don't have courses on pcb designs nor on electronics (a part from some phisics which covers circuits and electro-magnetism.. but nothing deep), so that's been quite a challenge to get were I'm right now. I'm working on my final thesis project and we are working with different kind of sensors (accelerometers, magnetometers, gyros and more) to develop nice kind of user-computer interactions such as body movement recognition, tangible in objects UIs, etc.. Until now we used pre-made boards (Arduino and some breakout boards) with some soldering or bread boarding.. but I'm now feeling quite limited by this so I'm trying to move on and pass to the next step: developing my own circuits boards that fit my needs. So here I am. To make things simple I started creating something similar to something I already know: Sparkfun ADXL335 breakout board (http://www.sparkfun.com/commerce/product_info.php?products_id=9269#) I used this accelerometer in the past so I know how this works also on the electrical side of things. So, I designed using Kicad the schematics, the pcb layout and sorted out the libraries of kicad.. So, I'd like you to have a look at my Kicad project and let me know what you think. As I said I'm a complete beginner so that's likely I missed lot of things there.. Please note that the pcb design is going to be create with home made etching on a single side. This is the accelerometer I used: http://www.sparkfun.com/datasheets/Components/SMD/adxl335.pdf The schematic I wanted to copy: http://www.sparkfun.com/datasheets/Sensors/ADXL335_v10.pdf Here you find the project files http://www.varesano.net/temp/adxl335_breakout_board.tar.gz Thanks for your time, Fabio Varesano Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] please review my first kicad project (and pcb design): an ADXL335 accelerometer breakout board..
Zone filling does help with the etchant usage, but I don't tend to go overboard with it. For example I would not have bothered to fill the small area to the bottom left and bottom right hand corner of the IC (breakout board-back.pdf Also that long tail extending down between the top right hand connection pin and the one below. It looks as if it should be going to an IC pin, but it's part of the zone fill. No reason to remove them, just my personal preference. You will find that there is a lot of than in PCB work... There are lots of 6 pin conectors. A simple 0.1 inch header can be used, SIL-6 is one, or Head_4x2 (8 pins) pin_aray_3x2 to name a few. There are dozens of connectors, some will not be in the libs, you might find them elsewhere, but a simple connector is good practice for drawing up your own module give it a try. If you have not already done so, print out the module documentation from CVpcb. (display footprints list documentation) 3rd icon from right in my version. It useful to have that by your side when choosing modules. You can also find that document in : /usr/local/kicad/doc/help/footprints_doc or under kicad in program files if using windows. With mounting holes, so people just use a big pad and set the drill size to what they want, while others draw it graphically. If you are going to have the board made by a production house then you need to define it as the correct size. For home production I just shove a normal pad down. The hole when etched makes a good drill centre. The tracks, yes you need them the correct size for the IC pin spacing, But you seem to have made that the thickest track you have used. When hand soldering, thin tracks lift very easily. Likewise, give yourself plenty of clearance to avoid solder bridges when building the units. You will not have any solder mask on the board, so the extra clearance makes it less likely for solder splashes to happen, and if they do they are easier to clear. e.g. The tracks from the other side of some of the connection pads look thinner than the tracks from the IC, that could be a product of the pdf...I will check... No the postscript looks much the same. For such a small board you have a lot of PCB area, so make use of it. The links, yes spot on, treat them as component side wiring. If you had any wire ended components in the design, they can also be used be used to bridge over tracks. Andy On Sat, 28 Aug 2010 01:10:59 +0200 Fabio Varesano fabio.vares...@gmail.com wrote: Hi Andy, thanks for having a look at this. Please read below.. On 08/27/2010 11:38 PM, Andy Eskelson wrote: Personally I don't like lots of filled zones unless that really are necessary, but that's a fairly minor point. Well, I read that this is good practice as this make less use of etchant during the etching process. Isn't that true? several other points: Do try to put your connection pins on the edge of the board. It makes wiring up much easier. You could also consider some form of connector. Yep, that's the best I've been able to come out with.. I do know that it will be painful to plug this. Do you have any suggestion for a 6 pin connector? Somehow I didn't find something suitable in the library. How are you going to mount the board? Some hardware mounting holes might be useful. Yep, good point. How do you draw mounting holes with kicad? The tracks to the pins look rather thin. Thin tracks tend to lift when soldering, also a small speck of dust on the film can cause a break in the track. Using a thicker track will help in both cases. You mean the tracks to the accelerometer IC? Well, they quite match the IC pins size. I don't think I could have made them bigger. Maybe you are suggesting making them thin below the IC and bigger on the rest of the board? On single sided boards, don't be afraid to use a few links it makes life MUCH easier. An Easy way to do this is to treat the board as double sided, and use the top tracks as wire links. Beef up the vias to a suitable size to take your wire links. Obviously you need to manually route this. I understand. So you are using wires as bridges to pass over one or more track, right? Interesting.. Thanks for your suggestions. Really helpful. You rock! FV Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Libraries paths - default libraries
No problem glad to help, but remember that if you ever upgrade kicad, that kicad.pro file will be replaced with a new one, so either remember to add your libs again, or keep a copy of kicad.pro somewhere safe. Andy On Thu, 26 Aug 2010 17:11:26 - philippederenne philippe.dere...@gmail.com wrote: Hi Andy, And thank you for giving a little bit of your time to me ;o) I'm working with version 2010, and kicad.pro is located in share/template. The trick your explained works perfectly ! I opened kicad.pro, then eeschema, there I've set the libraries and paths, and then I've the same thing done in pcbnew... works great ! Thank you ! Phil. --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: bear in mind that I am still using the 2009 version so file locations make have changed... under the kicad tree thee is a template directory, in there you will find kicad.pro Unfortunately in my sytsem I also have a kicad.pro in share/template this may be a left-over from a previous install. So I am not 100% sure which one you need to edit. Open up kicad.pro just as you would with any other project, then add whatever libs you need and resave as kicad.pro This should then become the default settings for any new project. The libs are cached (in the case of eeschema) into the project, and modules are included into the PCBnew file so that the project is independent of any external libs. This can be a bit of a life saver if you overwrite your libs/modules with an update, which is why you should maintain your own libs elsewhere :-) Remember that the kicad files are simple text files, so if you open up the .pro, .sch, .brd files you can see exactly what the settings are. Andy On Wed, 25 Aug 2010 20:48:52 - philippederenne philippe.dere...@... wrote: Hi, I've been using Eagle for years, but I think Kicad is a great product, so I'm trying to switch to it. However, I've got a question... In Kicad, the libraries and the paths to find those libraries seem to be linked individualy to each project. Is there a way to define default libraries and paths, to avoid redefining the same things over and over for each and every new project ? Thank you for your help ! Phil. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Libraries paths - default libraries
bear in mind that I am still using the 2009 version so file locations make have changed... under the kicad tree thee is a template directory, in there you will find kicad.pro Unfortunately in my sytsem I also have a kicad.pro in share/template this may be a left-over from a previous install. So I am not 100% sure which one you need to edit. Open up kicad.pro just as you would with any other project, then add whatever libs you need and resave as kicad.pro This should then become the default settings for any new project. The libs are cached (in the case of eeschema) into the project, and modules are included into the PCBnew file so that the project is independent of any external libs. This can be a bit of a life saver if you overwrite your libs/modules with an update, which is why you should maintain your own libs elsewhere :-) Remember that the kicad files are simple text files, so if you open up the .pro, .sch, .brd files you can see exactly what the settings are. Andy On Wed, 25 Aug 2010 20:48:52 - philippederenne philippe.dere...@gmail.com wrote: Hi, I've been using Eagle for years, but I think Kicad is a great product, so I'm trying to switch to it. However, I've got a question... In Kicad, the libraries and the paths to find those libraries seem to be linked individualy to each project. Is there a way to define default libraries and paths, to avoid redefining the same things over and over for each and every new project ? Thank you for your help ! Phil. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Installing Kicad from Source files
Depends on the distro. type su at a command prompt is the normal method of becoming root. If you are using that awful Ubuntu system of sudo then the easy way is to open a shell and enter sudu su once you do that the the shell will remain as root, but BE CAREFUL not to exit it by accident. With normal Linux compile operations, you only need the root access for the final make install stage. The normal sequence is ./configure make make install Note that not all software follows this sequence, (most do) so be sure to read the install instructions of whatever package you use. I've never needed to compile Kicad, the binaries have always worked for me. Andy On Mon, 23 Aug 2010 10:38:15 - Andrew andrwp...@yahoo.co.uk wrote: Well I discovered yesterday that I had a problem with my installation of Kicad from the sources. Because I don't know how to make myself the root, I had to use the sudo command to run the ' make install' option. After coming back to Kicad yesterday, I found that the program would not run. No matter what I tried, so I decided to do total wipe of my system (I know its an overkill, but I got rid of Windows all together at the same time.) So now I need to know how to do it properly using the source codes available from svn and making myself root to perform the installation. Any ideas guy?? Andy --- In kicad-users@yahoogroups.com, Milan Horák konfere...@... wrote: Hallo, downloading binaries from http://kicad.1301.cz is not the option? Milan Dne 21.8.2010 17:14, Andrew napsal(a): Hi Bernd I've finally managed to do it. After reading various txt install and compile text files, I followed the guide i used upto the point where i got the error, then just used the cmake . cmd and then make and make install. I did the same for the Kicad-doc and Kicad-lib source files, and it all installed in the right place. What I like about the source files is the 3d packages. The resistors have all got there own values, with the appropriate colour bands on them. When I was using Kicad on windows, I was creating my own set of 3d modules, by adding bands to the resistor module, but it was very time consuming. Don't understand why these files are not included in the compiled packages that are available to download in the first place.. Thanks Andy Ps And your quite right. I am not an experienced developer. Wish I was though. I would love to be able to contribute to this wonderful program --- In kicad-users@yahoogroups.com, Bernd Wiebusbernd.wiebus@ wrote: Hello Andrew. So how do I install the latest stable version on Ubuntu 10.04 LTS using the source code??? A step by step guide would be very hellpfull Perhaps i would appreciate this for Debian Lenny (i think very similar but not equal) too. At moment, i run the version from 05-05-2010 for Ubuntu 8.10 at Debian Lenny. Or is it a little bit assumpting, to try building from the sources without being an experienced developer or system admin? With best regards: Bernd Wiebus alias dl1eic -- GMX DSL SOMMER-SPECIAL: Surf Phone Flat 16.000 für nur 19,99 ¿/mtl.!* http://portal.gmx.net/de/go/dsl Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Installing Kicad from Source files
I'm still using the 2009 final with SUSE 11.1 at the moment. (I use the centos versio on SUSE) I do have SUSE 11.3 installed but I have a annoying problem with my KVM which is preventing the system determining what monitor is connected, so I have not yet installed the latest Kicad on 11.3 as yet. I got the binaries from here: ftp://iut-tice.ujf-grenoble.fr/cao/ The 2010-05-05 final fore win, Ubuntu and Centos are all there. (The 2009 version is now in the old version folder.) The 3D issue is a bit odd, PCBnew should understand the Wings 3D files without any problem, however if you have tried to compile from source, it may be that something is missing. There is not much in the install text, apart from a link to the maiun wings 3d site, it may be worth having a look there. It would also be worth while disabling any graphics effects that may be switched on. sometimes they don't sit well with various apps, and can be the cause of quite a few problems. Things like 3D desktops, wobbly windows (yuk! that one makes me feel sick) and the other such things. (I did have a problem with Wings 3d on a windows box some years ago, which was related to wings choosing a video mode that was not supported by the monitor.) Andy On Mon, 23 Aug 2010 11:19:05 - Andrew andrwp...@yahoo.co.uk wrote: Thanks for the quick reply Andy. So which binaries do you use exactly??? I have tried using the Synaptic package manager, but the version it downloads is from 2009, and that version keeps crashing every time i select the 3D view. I am after the latest stable release Thanks Andy --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: Depends on the distro. type su at a command prompt is the normal method of becoming root. If you are using that awful Ubuntu system of sudo then the easy way is to open a shell and enter sudu su once you do that the the shell will remain as root, but BE CAREFUL not to exit it by accident. With normal Linux compile operations, you only need the root access for the final make install stage. The normal sequence is ./configure make make install Note that not all software follows this sequence, (most do) so be sure to read the install instructions of whatever package you use. I've never needed to compile Kicad, the binaries have always worked for me. Andy On Mon, 23 Aug 2010 10:38:15 - Andrew andrwp...@... wrote: Well I discovered yesterday that I had a problem with my installation of Kicad from the sources. Because I don't know how to make myself the root, I had to use the sudo command to run the ' make install' option. After coming back to Kicad yesterday, I found that the program would not run. No matter what I tried, so I decided to do total wipe of my system (I know its an overkill, but I got rid of Windows all together at the same time.) So now I need to know how to do it properly using the source codes available from svn and making myself root to perform the installation. Any ideas guy?? Andy --- In kicad-users@yahoogroups.com, Milan Horák konference@ wrote: Hallo, downloading binaries from http://kicad.1301.cz is not the option? Milan Dne 21.8.2010 17:14, Andrew napsal(a): Hi Bernd I've finally managed to do it. After reading various txt install and compile text files, I followed the guide i used upto the point where i got the error, then just used the cmake . cmd and then make and make install. I did the same for the Kicad-doc and Kicad-lib source files, and it all installed in the right place. What I like about the source files is the 3d packages. The resistors have all got there own values, with the appropriate colour bands on them. When I was using Kicad on windows, I was creating my own set of 3d modules, by adding bands to the resistor module, but it was very time consuming. Don't understand why these files are not included in the compiled packages that are available to download in the first place.. Thanks Andy Ps And your quite right. I am not an experienced developer. Wish I was though. I would love to be able to contribute to this wonderful program --- In kicad-users@yahoogroups.com, Bernd Wiebusbernd.wiebus@ wrote: Hello Andrew. So how do I install the latest stable version on Ubuntu 10.04 LTS using the source code??? A step by step guide would be very hellpfull Perhaps i would appreciate this for Debian Lenny (i think very similar but not equal) too. At moment, i run the version from 05-05-2010 for Ubuntu 8.10 at Debian Lenny. Or is it a little bit assumpting, to try building from the sources without
Re: [kicad-users] Pin types and power flags
Most people go through this process at first, but you seem to have got hold of the basics pretty quick. The purpose of power flags is to tell the ERC checking system that there is actually power being provided. Consider if your battery was a separate box and you connected it with flying leads to a connector. You would need to put a power flag on the ground and +volts pins to keep ERC happy. The gotcha that sometimes catches people out (but not you) is that a regulator is often defined with it's output pin as a power out, in that case you do not need a power flag on the regulator output. If you have invisible pins set to invisible, then yes again you are correct, these pins are automatically connected for you. This makes the cct MUCH neater when you have a lot of devices. With only one or two devices it does not make much difference. However if you make the invisible pins visible you then HAVE to connect them manually. With a uP such as the mega setting the pins to tri state is not really the correct way to go but it is a good starting point. Really you should set the pins to match whatever mode you are programming them to be. There is NOT a one size fits all setting for them. (I'll bet that a lot of users set the pins to passive and don't bother to change them for each design. That will work, but you can lose a lot of the ERC checking) With the HC595, I assume that you copied the same device twice. If so that should be OK. If this was an invisible pin then it should be automatically connected unless you changed the name for some reason. If you are manually connecting the power lines, then watch out for junctions. A junction is NOT automatically created when two lines join, you need to place a junction marker. With the reset pin issue, yes the warning is correct. You have to change the pin type to passive or similar I think setting it to type input will cure the problem as well, or another method is to pull up the pin via a resistor then the error will go away. Power in pins should only connect to power out pins directly according to the ERC rules. So when you try connecting a power out to something else then you get this error. It's down to the uP being rather more clever than the ERC system, so you have to make some allowances, you soon get used to it :-) Andy On Sun, 22 Aug 2010 14:26:27 -0400 Robert Bieber ro...@bieberphoto.com wrote: Sorry if these are horrifically stupid questions, I'm just getting started out trying to use Kicad. My first project is putting together a simple timer, and I'm running into a little trouble in EEschema dealing with pin types and the VCC/GND power ports. First I had to build a new part for the Atmega328p I'm using, since there wasn't one in the library. I set all the I/O pins to 3 state and the VCC/GND pins to power in, which as far as I'm aware is the right way to do it...I hope I'm correct there. Now in my schematic, I've got a battery connected to a power regulator with some filtering caps and such, and the ground of all that is connected to the GND power port and the 5v output connected to the VCC power port, and that seems to working correctly for the most part, as I've connected VCC and GND on the 328 to those ports and they're not complaining. There are still a couple of issues, though: - I have two 74HC595 shift registers in the schematic, the VCC and GND pins of which are invisible, but seem to be automatically connected to the appropriate power ports. However, one of them (but not the other) is giving me the warning Pin power_in not driven on its GND pin, even though I know that the GND port is properly connected to the power regulator, and all the other GND connections on the schematic work fine. What could be causing this? - When I connect the RESET pin on the 328 to VCC, it gives me the warning Pin 3state connected to pin power_in. The warning also appears on the VCC pin of one of the shift registers (the same one that gives the warning about the undriven GND pin). Is there anything in particular I need to do about this? I did connect a 3state pin to a power in pin, but why is that considered warning-worthy? Sorry if I'm missing something obvious, and if anyone has a better source of documentation than the FAQ on the Kicad site, feel free to direct me to it. -Robert Bieber Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Type Err(4) trace near pad issue in Kicad
Odd - not much I can add at this point. If you want, you can upload your files (best to put the sch, brd and netlist or as many of them as you have) to the files section and I'll have a look at it. (or email them to me directly) There maybe some other infringement of the rules going on that you have not spotted as yet. You CAN create PCB's manually. You have to turn off all the DRC rules. However you then miss out on the protection that DRC gives you. preferences general (middle of the window, DRC on/off tickbox) I'm still using the 2009 linux version of Kicad, so in the latest verson the menu locations may have changed. When you use DRC and then add a module, the system will complain, as DRC will not know anything about this component. Andy On Fri, 20 Aug 2010 22:34:07 - ma...@ymail.com mad...@free.fr wrote: Thank you for your answer. Maybe I'm thinking too simple, or Old school... Last time I successfully used a CAD was 15 years ago. Back then I could certainly make a PCB with Proteus lite without using ISIS (the schematic editor) nor making a netlist... According to the Kicad FAQ, I should be able to work this way... 5.1 How do I manually route a PCB? Manual routing is quite straight forward. You don't even need to have a schematic. I tried the thinnest trace possible, and even straight (with no angle at all) the error occurs! Axel --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: The problem is that you are thinking too simple... KIcad like most design software is designed to work via netlists and so on. As has been suggested you could simply turn off the design rules checking that will prevent errors and so on. By far the best method is to create a simple sch. in eeschema and then use that to generate the required netlist. It's well worth getting used to creating the circuit then the PCB and so on. The error is just giving you a warning that a track is too close to a pad. Tracks and pads have a clearance setting. The normal problkem is that you cut across the pad at an angle with a track, and you just clip the edge of the clearance limit. Centre on where the error is and zoom right in, and you will prob see the problem. Use a slightly thinner track, or re-route it to miss the clearance area. Like most packages Kicad takes a bit of getting used to, I used a lot worse! (and not just PCB packages) Andy On Fri, 20 Aug 2010 08:39:38 - ma...@... mad...@... wrote: Hello group! This is my first post, so I apologize but I'm afraid I need some help! I installed Kicad (2010-05-05 BZR 2356) on Ubuntu Lucid64. Fine. As far as drawing schematics, everything is ok. Now if I try to draw a PCB without schematic, without netlist, without autorouter... Just a simple one sided circuit board. I create a new project, open PCB new, place say a DIP-8_300 component, click on 'add traces and vias', start tracing... and get: Type Err(4) trace near pad What the hell am I doing wrong? I can draw a trace without problem as long as I don't get near to the component (which is not very useful!). It's not component related (same behavior with resistances, caps, and so on) Component and traces are both on the 'under' side. I tried different traces sizes, I searched in the manual, in the different tutos, in the web... Nada! I searched here but the search server is 'busy' please try again later! Plus I don't know what to enter in the search engine, 'manual routing' return results such as auto-routing in the kicad manual, and the likes! I'm quite convinced that this must be something really simple, but I can't find it! Thanks for your help Axel Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Type Err(4) trace near pad issue in Kicad
Yes, you are correct, DRC NEEDs other info in order to work. In regards to your old PCB requirement, many years ago when we had a similar situation in needing to recreate a PCB when the tape masters had been lost we would put the PCB on the copy camera and take a pic of it. If the board was rather dense, we would sometimes tweak the enlargement factor slightly to get the sizes 100% correct. Using the hi contrast films, we usually got an acceptable image for reproducing the PCB. A little lightbox work was sometimes needed but not often. You could prob. do just as well if not a better job with a good quality flatbed scanner. Andy On Sat, 21 Aug 2010 11:53:13 - ma...@ymail.com mad...@free.fr wrote: The error occurs only when I try to create a PCB without schematic nor netlist AND with the DRC active. I don't get any error when the DRC is OFF, or if I have a schematic and a proper netlist. So I guess my problem was that I expected PCBnew to work as a standalone app WITH DRC. Obviously it is not the case. Either I respect the workflow (schematicnetlistCVpcbPCBnew) which I understand and agree to when in 'designer' mode, either I have to sacrifice the DRC safety when I want to save some time and draw a PCB from scratch. Thanks to all for helping me clarifying that out! Axel --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: Odd - not much I can add at this point. If you want, you can upload your files (best to put the sch, brd and netlist or as many of them as you have) to the files section and I'll have a look at it. (or email them to me directly) There maybe some other infringement of the rules going on that you have not spotted as yet. You CAN create PCB's manually. You have to turn off all the DRC rules. However you then miss out on the protection that DRC gives you. preferences general (middle of the window, DRC on/off tickbox) I'm still using the 2009 linux version of Kicad, so in the latest verson the menu locations may have changed. When you use DRC and then add a module, the system will complain, as DRC will not know anything about this component. Andy On Fri, 20 Aug 2010 22:34:07 - ma...@... mad...@... wrote: Thank you for your answer. Maybe I'm thinking too simple, or Old school... Last time I successfully used a CAD was 15 years ago. Back then I could certainly make a PCB with Proteus lite without using ISIS (the schematic editor) nor making a netlist... According to the Kicad FAQ, I should be able to work this way... 5.1 How do I manually route a PCB? Manual routing is quite straight forward. You don't even need to have a schematic. I tried the thinnest trace possible, and even straight (with no angle at all) the error occurs! Axel --- In kicad-users@yahoogroups.com, Andy Eskelson andyyahoo@ wrote: The problem is that you are thinking too simple... KIcad like most design software is designed to work via netlists and so on. As has been suggested you could simply turn off the design rules checking that will prevent errors and so on. By far the best method is to create a simple sch. in eeschema and then use that to generate the required netlist. It's well worth getting used to creating the circuit then the PCB and so on. The error is just giving you a warning that a track is too close to a pad. Tracks and pads have a clearance setting. The normal problkem is that you cut across the pad at an angle with a track, and you just clip the edge of the clearance limit. Centre on where the error is and zoom right in, and you will prob see the problem. Use a slightly thinner track, or re-route it to miss the clearance area. Like most packages Kicad takes a bit of getting used to, I used a lot worse! (and not just PCB packages) Andy On Fri, 20 Aug 2010 08:39:38 - madax@ mad.ax@ wrote: Hello group! This is my first post, so I apologize but I'm afraid I need some help! I installed Kicad (2010-05-05 BZR 2356) on Ubuntu Lucid64. Fine. As far as drawing schematics, everything is ok. Now if I try to draw a PCB without schematic, without netlist, without autorouter... Just a simple one sided circuit board. I create a new project, open PCB new, place say a DIP-8_300 component, click on 'add traces and vias', start tracing... and get: Type Err(4) trace near pad What the hell am I doing wrong? I can draw a trace without problem as long as I don't get near to the component (which is not very useful!). It's not component related (same behavior with resistances, caps, and so on) Component and traces are both on the 'under' side. I tried different traces sizes, I searched
Re: [kicad-users] ERC Error in complex schematic - KiCAD Build 20100406 SVN-R2508
Where did you get the symbols from? Sometimes when importing from other sources things can go a bit haywire and duplicate pins can get created. Check the lib files very carefully, as it has been known for pins to get duplicated in the lib. (you will not see this in the graphical editor, as everything will be on top of each other, you need to look at the lib file itself) It's a text file, and with the number of errors that you are getting, if this is the problem it will be pretty obvious! Have a look at kipy, a set of python tools that can do some extra checking and it will pick up the duplicate pin entry issue it it exists. Andy http://code.google.com/p/pyeda/ On Tue, 17 Aug 2010 08:07:59 - greghicks70 greghick...@yahoo.com.au wrote: Hi I am working on a complex schematic where I use a bus between them. I have common schematics that I developed separately in a folder hierarchy then added them to a master diagram for a specific purpose. I am using 74HC595 Serial-Parallel latches and they interface via a pair of R8 packs for 17 of the wires and directly to 15 wires (display matrix), and I get this message on 172 occasions: ErrType(2): Pin not connected (and no connect symbol found on this pin) @ (4.4000 ,3.2500 ): Cmp D90, Pin 1 (passive) Unconnected ErrType(2): Pin not connected (and no connect symbol found on this pin) @ (5.1500 ,4.6500 ): Cmp AFF4, Pin 5 (input) Unconnected I am driving the LEDs or 7 seg displays from the latches and I am not sure if the problem is the interconnecton or something else. There are wires, labels etc all applied to the buses and individual wires, but there is still no luck resolving this issue. Can anyone help me with this? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: ERC Error in complex schematic - KiCAD Build 20100406 SVN-R2508
Your labels seem to be a bit odd. I don't normally use multiple sheets with connecting labels, so I might be way off base here... e.g. on the 7 segment devices you have S0,S1,S2, LED3...and so on, connected to an LED label You drivers have labels such as D0-D14 and S0-S16 so there seems to be a bit of a mismatch. Also the segment drive connection on the top sheet seems to be an INPUT to sheet Eng uP serial Signal, and that connects to another series of buses LED, Bar_Gr and so on which are also shown as INPUTS In contrast the Display select is shown as an OUTPUT connecting to an INPUT. I would have thought that an input should connect to an output and so on. again I dont use this form of connection myself so I could be wrong. On other BAR_Gr sheets, the symbol is different again. Cool Temp, Oil Press are different from the other BAR_Gr pages, likewise things like Tach0 have yet another type of connector symbol. This does not seem quite right to me. Andy On Tue, 17 Aug 2010 11:18:13 - greghicks70 greghick...@yahoo.com.au wrote: Hi Andy, Thanks for the advice. I am using the native symbols in the problem schematic. Perhaps if I post the pdf print up it will make more sense. Something else popped up since my post. Invisible pins (from the same Library Item) are also reporting the same error, but they change each re-run of the ERC rules check. Look in files for the copy. regards Greg --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: Where did you get the symbols from? Sometimes when importing from other sources things can go a bit haywire and duplicate pins can get created. Check the lib files very carefully, as it has been known for pins to get duplicated in the lib. (you will not see this in the graphical editor, as everything will be on top of each other, you need to look at the lib file itself) It's a text file, and with the number of errors that you are getting, if this is the problem it will be pretty obvious! Have a look at kipy, a set of python tools that can do some extra checking and it will pick up the duplicate pin entry issue it it exists. Andy http://code.google.com/p/pyeda/ On Tue, 17 Aug 2010 08:07:59 - greghicks70 greghick...@... wrote: Hi I am working on a complex schematic where I use a bus between them. I have common schematics that I developed separately in a folder hierarchy then added them to a master diagram for a specific purpose. I am using 74HC595 Serial-Parallel latches and they interface via a pair of R8 packs for 17 of the wires and directly to 15 wires (display matrix), and I get this message on 172 occasions: ErrType(2): Pin not connected (and no connect symbol found on this pin) @ (4.4000 ,3.2500 ): Cmp D90, Pin 1 (passive) Unconnected ErrType(2): Pin not connected (and no connect symbol found on this pin) @ (5.1500 ,4.6500 ): Cmp AFF4, Pin 5 (input) Unconnected I am driving the LEDs or 7 seg displays from the latches and I am not sure if the problem is the interconnecton or something else. There are wires, labels etc all applied to the buses and individual wires, but there is still no luck resolving this issue. Can anyone help me with this? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: 3 PCBs, 1 design
The hierarchical circuit system is there to help you split up a circuit into manageable sections. it is NOT a method to make separate PCBs as such. It is possible to make separate PCBs, but you will have to be careful regarding interconnections, and you would have to accept that. ALL the PCB's would be produced at once initially. You will also have to do some manual adjustments as well. If your design uses several PCBs DO NOT interconnect them on the circuit. Terminate the interconnection points as connectors or pins of whatever. This will keep each circuit module isolated. You can then continue with PCBnew in the normal way, When you place the components you will find that each circuit module will be isolated from the next. You can define several board outlines and place the components on them, (this can be tedious if the design uses many components) You may have to accept a few DRC type errors if the power arrangements get a bit messy. Once you have done with the layout you can then either plot all at once, or delete the unwanted layouts and just print the one that is left. Another option that I have seen suggested, is that you can open the sub sheet as a separate project and work on that, but that can cause it's own issues. (I've never tried this) A better method and the one that I prefer is to treat each PCB as it's own design, and then the problems generally go away. i.e. in a project I will have a PSU circuit, a processor circuit, a relay driver circuit and so on. Each with their own netlists, PCBnew files and so on. So the general rule is, if the final result is to be one PCB, then everything goes into one circuit, using sub sheets as required. If the end result is several different PCB's, then each PCB should have it's own circuit. (Which is what andrew suggests below) Power flags are not that hard once the penny drops. In the case of a design with an external power unit The circuit will only have a connector or a pin where the power will come into the circuit. It will NOT have any on board power. So in order for the ERC to work, you have to tell the system that a particular line is providing power. That is the function of a power flag. So if you have a design that needs 5V to power it, you would have a ground and 5V pin somewhere on it. Usually at this point on the circuit you would place a couple of power flags. One on the 5V pin and one on the ground pin. Then the ERC will be happy. (It seems a bit odd at first, but ground or 0V is treated as a POWER IN type pin) Of course there are gotchas that can trip you up. The ERC does it's checks by looking at the pin types on the various parts. For power it looks at pin types of POWER IN and POWER OUT. It's quite simple, in that every power IN must be connected to a POWER OUT somewhere. So on most devices say a 7400 chip, there will be a 0V and +5V on the part, and these will be defined as POWER IN types. You have to connect these to a POWER OUT source. A power flag is effectively creates a POWER OUT device. Some devices can have a pin defined as a POWER OUT. Typically this is on regulators such as a 78xx types, where the output pin is often defined as a POWER OUT type. In this case you don't need the power flag on that line, if you add one it will confuse things. Andy On Mon, 02 Aug 2010 08:06:40 - andrewdwork andrewdw...@yahoo.co.uk wrote: Hi Jim, I am struggling with hierarchical schematics too, but the idea is to make a single board from many sub-sheets, not seperate PCBs from each sub-sheet. Suppose you were building an audio amplifier. Maybe the circuit is complex and to make it more readable you would break it into sections such as PSU, pre-amp, power amp, protection circuit etc. The final result will still be one PCB. If, say, the the front panel was a seperate PCB, you would still have to do a seperate circuit. You could use hierarchical schematic for the overview of the unit, but not for the individual PCBs, as I understand it anyway. My problem is trying to resolve ERC errors with power flags / Global labels, but that's another story. --- In kicad-users@yahoogroups.com, jimofc300 j...@... wrote: Hi, Still new to KiCAD. I hope there's a simple solution to my rather simple problem, since it must be very common. I haven't been able to find one in the docs or by poking at KiCAD. Can someone help? I have a design that will have three PCBs within a lot of other hand wiring, such as switches, panel connectors, a power module, and so on. I've created a hierarchical schematic that leads to each eventual PCB as a separate schematic sheet. I want to convert each of these three schematics to PCBs, one-by-one. KiCAD, however, seems to think that I want a PCB of the entire mess, not just the single sheet schematic. It compains that component numbers haven't been assigned to the higher items in the hierarchy (they
Re: [kicad-users] Re: SINGLE COPPER SIDE IN NEW VERSION (2010-MAY)
Usually a zone with no net will still route on both sides, but it will attempt to create isolated tracks inside the zone. (I am still using the 2009 final version hence the ability to select only one layer) Andy On Tue, 20 Jul 2010 17:22:45 - dickelbeck d...@softplc.com wrote: --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: Set preferences general layers to 1 Autoroute will then do it's stuff, but there will normally be a few tracks that you have to do by hand. Andy Paulo, You are correct, the new PCBNEW has a minimum copper layer count of 2. Can you try this (I do not know if it will work): 1) Put a large copper zone on the side of the board that you do not want routed, filling the entire board on that side. Make this zone unconnected in PCBNEW, I believe this can be done when selecting the NET for the zone, (maybe netcode=0). If not, let me know. 2) Then route your board. It should be possible for the auto router to use only one side, the side without the no-connect zone. 3) Then simply throw away the gerber file(s) for that unused side. Feedback your results to the list please. Dick Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] SINGLE COPPER SIDE IN NEW VERSION (2010-MAY)
Set preferences general layers to 1 Autoroute will then do it's stuff, but there will normally be a few tracks that you have to do by hand. Andy On Mon, 19 Jul 2010 15:14:49 - Paulo cox_...@yahoo.com wrote: Hi everyone, I'm new around here.. I dont know if you answered it before, I try to search but I couldnt find any related, very sorry if double posted, really. Well, I've downloaded the last available version of KICAD from their website and, I'm not capable of autoroute in a only one side, its seems to be pre-configured with 2 layer of copper and I guess its cannot be modified. I've read a very good tutorial in the web and I could start a new project from zero knowledge at all of the program, I make the sch, then about 2 hours I have all components rady in the PCB with the vias, pads, etc BUT IT make me 2 layers, front I back, wich differs from various tutorials I found on the net.. Well, thank you for all of your time reading this, KICAD deserves my time too now and has won my entire attention, ITS A GREAT SOFTWARE!!! ;-) Kind Regards, Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] New component for schematic library
In library editor: Open the device you want to work on. Draw a selection box around the lines and other things you want to copy This will allow you to move the block. THEN RIGHT CLICK and from the context menu select copy block. That's it. I'm using the 2009 final on SUSE, I don't think that the newer version works differently Andy On Sat, 03 Jul 2010 12:32:23 - gerard f6...@wanadoo.fr wrote: I wish to create a new schematic component : DPDT. So I intend to start from a SPDT, duplicate it, rename the pins and save under the new name. Unfortunately I've been unable to copy twice the SPDT, I could only redraw completely the pins and all parts. If I select the SPDT as a bloc, there is a copy command with a right click, but nothing to paste the bloc somewhere else. Could someone help me? PS: I've used (very modestly) IRIS/ARES and Eagle, but KICAD is far less complicated to use, especially to create the components and to affect the modules to the components. Eagle has a huge library, but too big for ham use!! I prefer a small, and not so complete library, but easy to use!! Also I like the idea to create a schematic, and choose afterward which module to use. Thanks to the designer and to the user community. Best 73 from Gerard F6EEQ [=;]
Re: [kicad-users] Netlist Plugin and Hierarchical Nets
Kicad has a named net function and also global labels / hierarchical labels. Will these not do what you want? Andy On Fri, 02 Jul 2010 11:38:15 -0300 Matheus Degiovani math...@gigatron.com.br wrote: Hello, I'm using Kicad (eeschema) to draw schematics for the panel layout of an electrical installation I'm making (specifically, a CNC machine). I have two sheets: an overview sheet (showing the machine's motors, sensors, etc) and a hierarchical child sheet showing the layout for the electrical panel. I need a way to convert the net names into reference numbers, so that I can make all the physical wiring and label each wire with a number, for reference (so I know, for instance, that wire 1 is motor A+ phase, wire 2 is motor A- phase, etc). I figured I'd export the netlist from my project and write a netlist plugin that would process the names of the nets and write a corrosponding table with a wire number (I have to do this because the identifying net numbers are volatile and may change if I change the schematic - I would solve this by having an external database which never modifies the wire number, even if the net is removed from the schematic). However, even the net addresses' in the hierarchy and it's connections to components change when I reprocess the schematic. And this is done in an undeterministic way. An example (slashes denote the position in the hierarchy): I have the components /motorX and /panel/driverX. Both have pins named A+, A-, B+, B-. I have created the nets X A+, X A-, X B+, X B- and connected them to the motor and driver components (each at a separate hierarchical level, therefore they should actually be 8 different nets - /X A+ and /panel/X A+l, right?). However, when I generate the netlist, the temporary netlist file has a mix of the nets (some appear from the root sheet, some appear from the child sheet). I'm using hierarchical labels to pass the signals between the parent and child sheets. Bottom line: it seems that when exporting a netlist, eeschema treats all nets as global, so the first it finds with a name (like X A+) sets the address (of the net) to the correct value at the moment, but when processing hierarchical sheets that process breaks. I can provide the projects I'm working on and the custom libraries I built. Thanks. -- Matheus Degiovani Gigatron Software e Treinamentos Ltda. (18) 3649-4045 MSN: math...@gigatron.com.br -- Críticas ou Sugestões? Ligue para Ouvidoria Gigatron: (18) 3649-4048 Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] New to Kicad: trying to create schematic which includes TL084ACN Op Amp
There are a couple... The main help files are a good place to start, but be aware that the help files are separate for eeschema and pcbnew, eeschema will cover the creation of the schematic parts and pcbnew the creation of modules. There is also a tutorial, it is rather old and out of date, but it will give you the general idea. Work through the tutorial two or three times. It's not hard but like most programs it takes a little getting used to. When creating parts and modules, or modifying existing parts and modules remember to ensure that the pin numbers/names are the same. pin 1,2,3 on a transistor part, and e,b,c on a module is a fairly common error, and it means that the connections will not work. As you are new to this, do follow others advice regarding saving your parts and modules in your own library system. Module management suggestions are given in the pcbnew docs, chapter 11 in my version. It talks about creating a dummy board and using that to hold your modules. The actual mod files can then be created by using the archive footprint functions. It works quite well. The docs are in /usr/local/kicad/doc with directories for the help files and the tutorial. The only thing that you will run into, is that you have to add your libs to each new project in order for them to be found. If this gets to be a pain, you can modify the default template to include your libs, then they will be added to each new project. Andy On Mon, 28 Jun 2010 03:37:24 - Frank P qz9...@yahoo.com wrote: I'm new to Kicad and made an attempt to create a schematic which included a TL084ACN Op Amp. Unfortunately, the downloaded libraries did not include the op-amp and I had difficulties with adding/creating the component. Any advice would be appreciated. Are there any tutorials covering the creation of or modification of a component in the libraries? Thanks. Frank P. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] different footprint for the same component?
Pretty much the norm. You will find that so called standards vary a bit :-) As you use the system you will build up your own library of parts that you have tweaked to fit your requirements. You should save these into your own library so that it does not get overwritten due to upgrades. The help file in pcbnew details a way to document and organise your modules. Basically you create a dummy board and place your modules on it. You can then recreate the modules by using the export function. Andy On Wed, 23 Jun 2010 13:07:27 - yeshe66 yesh...@yahoo.se wrote: I used the standard symbol for a NPN transistor which i suppose fits the TO-92 footprint where pin1 = emitter, pin2 = base and pin3 = collector. Now, I have SOT-23-3 transistors, which always have pin1=base, pin2=emitter and pin3 = collector. I didn't notice, so the base and emitter pins was exchanged... I solved the problem temporarily by putting the transistor up-side-down om the board! Now, for the next layout , I've made a different footprint for SOT23-3 called SOT23EBC which have the pins numbers changed so it fits the NPN-symbol in EEschema. Is this the best solution to this kind of problem, or is there a better way? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] DIY Solder mask?
Mega also do a Photoimagable gree soldermask code 41-2004 There is a pdf document on how to use it about 2/3 down this page. http://www.megauk.com/screen_printing.php It may give you a few more ideas. Andy On Wed, 16 Jun 2010 10:01:36 +0300 Anders Gustafsson anders.gustafs...@pedago.fi wrote: Thanks, i have filed it away for reference. My initial posting might have been unclear though. I was talking about Solder Resist, the green stuff :) - Anders Gustafsson Engineer, CNE6, ASE Pedago, The Aaland Islands (N60 E20) www.pedago.fi phone +358 18 12060 mobile +358 40506 7099 fax +358 18 14060 Andy Eskelson andyya...@g0poy.co.uk 2010-06-16 00:00 It works very nicely as a stencil from the reports I've seen. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] DIY Solder mask?
Megauk sell photo resist coated brass sheet. http://www.megauk.com/brass_sheet.php This came about after a request from someone on another group I use asked them about it. It works very nicely as a stencil from the reports I've seen. Andy On Tue, 15 Jun 2010 13:34:25 -0600 Cat C catalin_c...@hotmail.com wrote: Yes, I was thinking stencil, sorry. To: kicad-users@yahoogroups.com From: anders.gustafs...@pedago.fi Date: Tue, 15 Jun 2010 21:18:26 +0300 Subject: Sv: RE: [kicad-users] DIY Solder mask? I think you are referring to masks for applying solder paste. I was thinking of the colour you use to stop solder from going where it should not. - Anders Gustafsson Engineer, CNE6, ASE Pedago, The Aaland Islands (N60 E20) www.pedago.fi phone +358 18 12060 mobile +358 40506 7099 fax +358 18 14060 Cat C catalin_c...@hotmail.com 2010-06-15 20:30 There's a guy in Montreal that can cut the soldermask for you out of mylar at a very reasonable cost. It will take me a while to find his details so I'll only do it if there's interest. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] graphics differences in multi-part components
On Tue, 15 Jun 2010 18:59:47 - It's a rather hidden function :-) When you draw the graphic line, if you right click on it and select properties there is a tick box - common to units Untick this and the graphic will appear only on the current part selected. Andy bbt5001 mo...@bluebelttech.com wrote: The library editor in eeschema permits the creation of multi-part devices. So, if I have quad pack of NAND gates I can draw one and have the graphic to be the same for all parts. But what if the parts are not identical? I know I can have unique text and pin numbers, but I can not figure out how to have the Part A graphics differ from the Part B graphics. Any line I modify on A is modified on B (and C) as well. The part I'm trying to create is the Avago HCNR200 optocoupler. This consists of one internal LED and two photo diodes (PD1 and PD2). I *could* create the eeschemea model as one library part with all the components in one box, but that forces my schematics to conform to the physical package constraints. The correct approach is to have these as 3 independent parts so that they can be placed in the schematic according to the functional flow. For example, I should be able to place PD2, the isolated photo diode, on the sheet for the isolation circuits, while LED and PD1 are on a different sheet. This could be extended to something like a relay: schematically, the coil should be separable from the contacts. Can this be done KiCad? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] PCBnew 3D viewer crashes
Has this ever worked? The 3D uses Wings3D, have you installed / checked that ? I have sometimes had a few problems with screen resolutions, not usually generating a crash, but sometimes the screen can blank and stay that way. Caused by the res settings in the driver having a mismatch between the actual screen res available. RivaTuner is a useful utility that allows you to edit the driver to only include what the screen can do or limit the choices. Andy On Sun, 13 Jun 2010 03:47:06 - lynchaj lync...@yahoo.com wrote: Hi! I am running WinXP with the latest KiCAD from windows binary at kicad.1301.cz. Everytime I try to get a 3D view of a PCB in PCBnew, the program crashes and get the Windows crash window. This is the error it is reporting: AppName: pcbnew.exeAppVer: 0.0.0.0 ModName: wxmsw28u_gcc_custom.dll ModVer: 2.8.10.0 Offset: 00043720 I have made sure the latest KiCAD and libraries are installed per the KiCAD.1301.cz site. Would anyone help me figure out what is wrong? I've searched on the problem but nothing so far. Thanks and have a nice day! Andrew Lynch Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] BOM - How can I set user's field IDs globally thus replacing Field 1, etc.
Kicad libs and mods are simple plain text files. So it's easy enough to write a perl, bash, awk, VB or whatever scripting system you prefer. And change any of the field parameters. (Please only work on a copy for safety) Andy On Fri, 28 May 2010 05:23:57 - Jeffrey jeffrey_fra...@yahoo.com wrote: Default user's fields are Field 1 Field 8. How can I specialize these globally as: Manufacturer Manufacturer P/N Distributor Distributor P/N Tolerance Rating DNP (do not populate) I can set each field individually when editing the part, but that is a very costly solution (time). Are there plug-ins that make BOM have more utility? --jlf Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Having trouble with component selection
The components are divided up into various libraries. Most of the common stuff is in devices When you get a few mins to spare, use the icon or menu item to place a component, then click on the by lib browser button in the requester. As it says, that will allow you to browse through the various libs and get an idea as to what is where. You soon get used to it, and once you do, you can simply select things from the lists. Andy On Thu, 27 May 2010 19:23:26 - jeff_seiffert jaseiff...@pdq.net wrote: Hi, I'm new to Kicad and I'm having problems finding components. I'm not sure what I'm doing wrong but I click on the sheet, the component selection shows, I type in bridge looking for a full-wave bridge rectifier. I get no results, I try full, wave, rectifier, nothing. I opened the Library Browser and find, under device, BRIDGE. What am I doing wrong? Thanks, Jeff Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Images/Logos in KiCad Schematic
Have a read of the help documentation for pcbnew, it recommends that module management be done with a dummy board file. If you have a hunt in the mods directories you will find these board files for the provided mods. Essentially you create an A4 size board, and place your modules on it. You can have one board per module lib, or whatever you want. To create the individual module files you use the archive footprints options, which can either recreate the entire lib, or update what is already there. I was not totally convinced that this would work, but after trying it, I found that it did in fact work very well. Andy On Mon, 24 May 2010 08:24:30 - mgebha mar...@jave.de wrote: Your software is very good. Thanks :) I tryied with a loto of logos and the result is very interesting. I think should be an instrument that kicad must to have inside IDE, do You agree? I think KiCad and its tools are a combination of small, loosely coupled tools (EESchema, CVpcb, PCBnew, GerbView, 3D Viewer, FreeROUTE). This concept seems to be quite powerful and allows independet development. So I rather think of extracting the module-conversion code from JavE and providing a stand alone application. Also what I have in mind is some kind of module manager: I want to be able to move modules from one file to another, refactor and rename them, etc. I cannot find these functions in KiCad itself, but it would help me a lot to be able to organize my libraries w/o working inside the .mod files with a text editor. -Markus Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: How to add a new sheet in PCBnew
The normal process is: When you draw the schematic in eeschema you test and annotate the circuit, and once all the corrections are done you save the netlist. You then run cvtpcb which allows you to assign modules to the various devices. When done you save the netlist again. In PCB new you create your board outline, and then open the netlist, this will dump all the modules on top of each other in one corner. (There are a few operations you can do that will spread out the modules allowing you to select them easier) It is possible to add modules directly to the PCB, just click on the add modules icon and select the one you want. If you do this, things like DRC will start to complain, as it will not have any netlist to test against, so you may have to switch off drc. Generally it's best to create a schematic for each project as it makes life a bit easier. Do read and work through the tutorial a few times, it is a bit out of date, so some things look a bit different but the process is still valid. Kicad is not hard to use, but like many large software products, it does need a bit of practice. You will also find extensive help documents for each kicad program, access these from the help menu, or if you prefer they are in the docs directory as simple pfd files. (as is the tutorial) Hope this helps. Andy On Wed, 19 May 2010 10:29:05 - vladimir_uryvaev vovan...@bk.ru wrote: --- In kicad-users@yahoogroups.com, quenelle120 quenelle...@... wrote: hello everybody, the question is in the title. i have a pcb card drawn but i want to had a module in new sheet. how can i do ? Just m#1072;#1082;#1077; new pcb file and import module netlist there. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Images and logo inside PCB
Have a look at TTConv in the group files. The one dated feb 8th looks to be the latest. One of it's functions is to import images, which may be what you want. If I remember correctly is intended to import things like logos rather than images as such. Andy On Wed, 19 May 2010 11:51:46 - ferraro.giuse...@ymail.com ferraro.giuse...@ingferraro.eu wrote: Hi, I'm trying to insert an image in PCB. How can I do? I'm using WINDOWS VERSION, last version. Bye G Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Module file documentation?
There are reference documents in: /usr/local/kicad/doc/help/file_formats Andy On Sat, 15 May 2010 18:40:31 - einazaki668 einazaki...@yahoo.com wrote: Hi, Is there a reference document for the .mod files anywhere? I'm thinking that, in some situations, it might be easier to create a footprint by directly editing the .mod file. Also, if there's a similar doc for the .lib file that might be nice too. Regards, eric Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Module Library madness
Module management is fairly easy, but it does not seem to be very well used. This is probably due to the way that the modules are installed, where everything is pretty much set up ready to go. If you have a hunt around in kicad/share/modules you will find some .brd files. these are the recommended method of managing / documenting modules. from the .brd files you can generate all the modules on them by using the archive footprints function. This method is documented in the help files of pcbnew. You can add modules to the .brd files then run the archive function to recreate the modules as needed. It is recommended that you create your ow .brd files for your own modules, as there is always the danger that modules can be overwritten during re-installs. I was not convinced at first by using .brd files for module management, but I've been convinced that it's quite a easy method. With the imperial / metric versions. the only thing I can think of is that it may be that because kicad (at least the 2009 versions) use imperial as it's base measurement system that someone created the imperial versions to avoid grid mismatches. Andy On Tue, 11 May 2010 21:25:03 -0500 Karl Schmidt k...@xtronics.com wrote: I'm not sure I understand why the library of modules is in the state it is? I would expect to see module files like SO.mod, DO.mod, DIP.mod, PLC.mod, discreet_SM.mod, etc. Am I missing something? Anyway, it appears that I should not trust what is in the library anyway. I got a copy of LP Calculator to work. should probably be three versions of the modules library for surface-mount work - General purpose - high reliability and very-high density. (There are settings to get these numbers out of LP-calculator). A = Most - reliable - but bigger B = Nominal - mid sized C = Least - very small For others that want to generate these pads - here are the clues From http://landpatterns.ipc.org/default.asp Download this link http://landpatterns.ipc.org/files/PCBM_LP_Calculator_V2009-0831.zip Get Winetricks from: http://winezeug.googlecode.com/svn/trunk/winetricks Save the script Then using a Terminal type in sh winetricks in script directory Select using the GUI dotnet20 and install There is one other detail that should get worked out - there are two ways that cap footprints are specified - and it generates confusion - metric and imperial - thus 0201 (02x01mils) = 0603 in metric (remind me to once again curse the creeps that stopped metrication back in the '60s). Complete list http://wiki.xtronics.com/index.php/Capacitor_Codes#Imperial_and_metric_case_size_codes There are two that overlap - there is are 0402 0603 in both imperial and metric. The library name ought to give a hint as to the units used.. The current lib lists these as SM0603 in imperial.. I'm thinking of creating a metric named lib with 0603M? Karl Schmidt EMail k...@xtronics.com Transtronics, Inc. WEB http://xtronics.com 3209 West 9th Street Ph (785) 841-3089 Lawrence, KS 66049 FAX (785) 841-0434 Let us live so that when we come to die even the undertaker will be sorry. -- Mark Twain Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] pin_array_25x2
There are dozens of different 50 way connectors. There are LOTs of connectors included in kicad, so Print out the footprint list document (do this from within CVpcp one of the icons on the top bar, or fiund it in the docs directory. page conn_HExx.brd looks promising. You can also: Check kicad lib . org http://www.kicadlib.org/ If nothing there, check out Pierre Launays' search engine, link at the bottom of the kicadlib.org page/ a better answer is to draw it up yourself, you will have to learn how to do this sometime, and a simple connector is a good starting point :-) Andy On Fri, 30 Apr 2010 12:40:11 + (GMT) Benidir Adel benidir.a...@yahoo.fr wrote: Hello, I want to create a pcb so, I didn't find on the netlist 50 pin IDC. Thanks.
Re: [kicad-users] PCBNEW
Likewise the tutorial document included with kicad describes the process, as does the PCBnew documents. Andy On Thu, 06 May 2010 10:50:00 +0300 Anders Gustafsson anders.gustafs...@pedago.fi wrote: Yes, there is. Use the module editor, see: http://wiki.xtronics.com/index.php/Kicad - Anders Gustafsson Engineer, CNE6, ASE Pedago, The Aaland Islands (N60 E20) www.pedago.fi phone +358 18 12060 mobile +358 40506 7099 fax +358 18 14060 Benidir Adel benidir.a...@yahoo.fr 2010-05-06 10:42 hello0, I want to create a new physical component to my circuit, I hope there is a solution with pcbnew. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Creating schematic componens
Bernd, you may have seen the pin definitions in the eeschma help document it's quite extensive. Most of them are fairly obvious, and you choose from them as needed. It is the pin assignments that DRC uses to The danger of using undefined and so on is that drc will then not work very well if at all. However for things like connectors, then passive is a reasonable choice. The ratsnest of the wires, that's another matter You can of course limit what you see with the show general and module ratsnest options, but the main problem is that Kicad will not know which pin the main board trace will connect to until you actually connect it. Hence ypou see the ratsnet. A small case of chicken and egg I'm afraid. As for the sheet name, well the docs do refer to this function, noted as not implemented, but the docs are for a rather older version, so it looks as if this idea has been thought of, but as far as I can see nothing has been done with it. Andy On Wed, 05 May 2010 10:07:20 +0200 Bernd Wiebus bernd.wie...@gmx.de wrote: Hello Andy. Don't specify the connector as signal and ground. In some cases that can cause a few problems. GND is considered a power line for example. Yes. Call it Side Contact or Frame or something. Give your schematic part pin numbers, just 2 of them. Use the same pin numbers for your footprint module. For the 4 ground connections, give that all the same number. Note that this is the method used in the 2009 version, things might have changed if you are using the later 2010 version of Kicad. (that did not work on my SUSE system, hence i still use 2009) So far i can see, this is the same in the Version from 06th. April 2010. I use it with Debian Lenny. But for me, the meanings of the Pin-proppertys are allways a little bit confusing. Different sorts of inputs and outputs and so on. I am only shure with not used :-) Once i read a good text about this, but i wasnt able to find it again. :-( The next point is: when i create a footprint with more than one pad belonging to the same potential, and i give them all the same number, they appear in the board with airwires for connecting between them. If i make copper connections between them at the footprints, then i will see this airwires in the board again, and they will only disappear, if i connect them again at the board. Is there a way to switch off this already connected airwires? This would cause a way to create Modules of a bunch of parts. So you could reuse them on different boards. Of Course, there would be a minor problem with the annotation. In a schematic, this works, when i use prefabrikated schematics as hierarschical sheets. Again, there it would be nice to give all devices at a hierachical sheet a certain prefix or suffix to the annotation number. No, i do NOT mean the reference. I mean something like :R12-VReg-IV which would mean Resistor number 12 at the hierarschical sheet VoltReg-IV. with best regards: Bernd wiebus alias dl1eic -- GRATIS für alle GMX-Mitglieder: Die maxdome Movie-FLAT! Jetzt freischalten unter http://portal.gmx.net/de/go/maxdome01 Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Creating schematic componens
DRC is not perfect, so you have to choose the most appropriate function to assign to a pin. With your 555, I would assign, pins 1 8 as power 7 open collector 3 outputs 2, 4, 5, 6 as inputs Of course you could use the 555 as a simple switcher and thus use it to provide some power, in such cases you either respecify the pin or you leave it as is and if needed add a power flag to the output connection to keep the rest of the circuit happy. You WILL get anomalies like this from time to time. Just wait until you use microprocessors where the pins can be inpiut output, bidir, timers or whatever o a programmable basis! You usually end up creating a specific part for a project. Diodes are usually defined as passive Likewise a battery is usually defined as a passive You might think that defining it as a power out is more logical, and you could do so. However you may be dealing with a rechargeable battery, so you would want to connect power INTO it for charging. If the Battery was defined as a power out then DRC would get upset again. What is causing some confusion is that you know what a device does, and are thinking of it in those terms. What you have to remember is that DRC is not very clever, (it does not need to be) all it needs is just enough to detect something silly, like you connecting two output pins together. or not connecting a power pin up. Something like a transistor would have the base as an input, but collector and emitter as passive simply because you can connect them up in various configurations and it's a bit pointless trying to define things any more than that. I understand what you are saying regarding the component numbering, but it looks as if that function is just not available, but it was thought about in the past. Most of the components you will use have already been defined, so if you are makig up your own libs and modules, you can always have a look at what similar parts have done. (That's what I usually do) It does get easier after you complete a few projects. Like most things there is a learning curve to work through, but I must admit that kicad was easier than some packages I've come across. It's also a lot more accessible, as all the files are simple text based, so it's possible to fix a lot of things externally when they don't quite meet your needs. You will see quite a few references to varioyus scripts that users have produced to cater for various requirements. Andy On Wed, 05 May 2010 23:51:16 +0200 Bernd Wiebus bernd.wie...@gmx.de wrote: Hello Andy. you may have seen the pin definitions in the eeschma help document it's quite extensive. Most of them are fairly obvious, and you choose from them as needed. Mmmmh. Think of a classical 555. You can enable it with setting Pin 4 high. Pin 4 is normally a signal input, but very very often it is tied to the power (personally, i prefere doing this with a 4k7 resistor).Pin 7, the output, is normaly a signal output. But it will turn to power, if you switch with this output the power of a small, but entirely complete circuit. What is an Accumulator? Is it output, input or is it passive like a capacitor? ;-) At the beginning, i used open collector even for single Transistors, because i did not notice, that this is only for the open collector switching stages of some ICs. I had to use the connections of a diode as passive, but for me, a diode is not necessarily a passive component. Perhaps it is only a mental problem for me, to make this decisions, but it is really a problem. It is the pin assignments that DRC uses to The danger of using undefined and so on is that drc will then not work very well if at all. However for things like connectors, then passive is a reasonable choice. Of course, with the drc i find all cases of pins not correctly attached to a wire. The ratsnest of the wires, that's another matter You can of course limit what you see with the show general and module ratsnest options, but the main problem is that Kicad will not know which pin the main board trace will connect to until you actually connect it. Hence ypou see the ratsnet. A small case of chicken and egg I'm afraid. I see. As for the sheet name, well the docs do refer to this function, noted as not implemented, but the docs are for a rather older version, so it looks as if this idea has been thought of, but as far as I can see nothing has been done with it. Oh. I do not mean, that the pre- or suffix must be only the sheet name. But it would be nice, if you could see by the component reference number, to which part of the board i will belong. As an example, using numbers 0-999 for the main schematic, numbers 1000-1999 for power supply, 2000-2999 for driver and power stages, 3000-3999 for safty circuit and so on. But i think, it could be easier use the reference number as a string, and add another string to it, than reserving hole number
Re: [kicad-users] Footprint for jumper?
Depends on what you mean by jumpers If you are referring to the small plug in links then no, such links are usually 0.1 inch spacing. For such links I normally use one of the header modules, SIL-2, 3, 6 or whatever suits the circuit. If you check GS2 with the module editor you will find that it's pad spacing is much smaller, and they are pads rather than thro-hole. You can check this with the module editor. If you have not already done so, print out the footprint document They are a very useful reference to have to hand when choosing which footprint to use. It's i the documents directory, or can be access from CVpcb one of the icons brings up the footprint doc. Andy On Tue, 4 May 2010 14:26:03 +0700 Nguyễn Hồng Quân ng.hong.q...@gmail.com wrote: Hello all, Please tell me which one is the footprint for jumpers in KiCAD lib? Is it GS2? *** * Nguyễn Hồng Quân* * Y!M: ng_hquan_vn* * Identi.ca: hongquan * *** Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Creating schematic componens
Don't specify the connector as signal and ground. In some cases that can cause a few problems. GND is considered a power line for example. Give your schematic part pin numbers, just 2 of them. Use the same pin numbers for your footprint module. For the 4 ground connections, give that all the same number. Note that this is the method used in the 2009 version, things might have changed if you are using the later 2010 version of Kicad. (that did not work on my SUSE system, hence i still use 2009) Andy On Tue, 4 May 2010 20:15:06 -0400 juliorz juli...@bellsouth.net wrote: I created a foot print for an SMA PCB mounted connector, but now I need to link it to a schematic symbol and specify electrical rules. I need to create a schematic symbol and link it to my foot print. I need to specify that the four outside pads are ground, and the inner pad is signal.
Re: [kicad-users] Merging outputs for double-sided boards
One method to use is to generate the required postscript files then import them into Inkscape, be careful not to resize them! Inkscape will allow you to move the images around however you ned them. Inkscape is available for Linux, Mac and windows. http://www.inkscape.org/download/?lang=en Andy On Sun, 02 May 2010 05:40:54 - susanmackay99 susanmac...@optusnet.com.au wrote: I have designed a double-sided board that I now want to print out on to the transfer material for use in the toner transfer PC creation method. (I've used this in the past for single sided boards OK). To make sure both sides of the board are aligned, I want to print then at the same time onto the transfer material with a bit of a space in between so I can fold the material over, line up the top and bottom holes and then slip the board in between before running it through the laminator. To do this, I need to transfer the top and bottom images onto the same document page and this is where I'm running into some problems. I have tried to create plot files using both the PostScript and PostScript A4 options but they both create full page sized surrounding boxes when I try to import them into Pages so I can combine them into a single print document. I've also tried using photoshop to trim the images down to the right size (the board is about 5cm x 5cm) which results in a much smaller image but the rasterizing File (sic) process seems to result in jagged edges to some of the lines. (The funny thing is that these lines tend to be the vertical and horizontal lines so I don't think this is an anti-aliasing effect). All of this is done at 1200 pixels/inch. I've tried saving as TIFF and BMP formatted files I'm looking for help from others who have managed to combine the images of both sides successfully as to how to achieve this. I am using the Kicad OSX V 2505 build(but I don't this this is question is version related). Thanks Susan Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] component with dissimilar parts?
Sorry, you did not mention pins so I assumed you had found that one... Top icon bar next to the part name there is a icon, edit pin per part or not. set this to enable you to add pins that are specific to individual parts of the device. Andy On Mon, 26 Apr 2010 19:54:23 -0700 David Gravereaux davyg...@pobox.com wrote: Andy Eskelson wrote: Yes easily. Select the part you want to edit. when you draw a circle. line or box, right click and select line/circle/rectangle options then untick the common to units box, whatever you drew will then only appear on that part and not the others. Andy I gave it a try, but I can't seem to find the 'happy place' yet. Pins are still in the same place for the ones I want different. Yes, the body can be different. The option doesn't seem to be applicable after the body parts are created. I may just edit the library in notepad! Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] component with dissimilar parts?
Yes easily. Select the part you want to edit. when you draw a circle. line or box, right click and select line/circle/rectangle options then untick the common to units box, whatever you drew will then only appear on that part and not the others. Andy On Mon, 26 Apr 2010 20:26:27 - David davyg...@pobox.com wrote: Is it possible to create, for example, a 12AX7A with three parts in it? Part A B are the triodes, but is it possible to have the third as the filament which isn't round but shaped different? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Wire connections will not connect to components
The alignment of the pin and the wire has to be exact. Sometimes a mismatch of metric and imperial grid sizes can cause this sort of thing. Try zooming in as far as you can and see if there is a grid mismatch. internally kicad works in imperial rather than metric. I have normally been able to fix such errors my placing a junction at the troublesome point, other people find that using imperial only helps. I have also found things like duplicate lines in the lib file, can cause confusion. As you connect to one entry and not the other. Patrick has written a python script that does a number of checks on the kicad created files, and it will pick up double entries, so it's worth running things through kipy when you hit problems. See: http://code.google.com/p/pyeda/ Andy On Mon, 19 Apr 2010 11:53:51 -0400 Paul Gress pgr...@optonline.net wrote: Hi all, I'm setting up a schematic prior to creating the pcb. The problem I'm getting is not all wire connections will attach to the schematic components. I don't understand why some will. Can anyone shed some light? Attached below is a small screnshot of what I'm talking about: screenshot As you can see, to the left side of R4 is not connected, but the right side is. Thanks for any help, Paul
Re: [kicad-users] Re: Feedback
You can do this to some extent with Kicad. Create a module, e.g. called Pad1 add one pad to it and set the shape to whatever you want. Click the copper and component tick boxes. Reduce the text labels to the minimium and set them to be invis. Don't add any outlines etc, remove the pad number entry. Save the module. You can now place that module on the board as per normal. The only gotcha is that to route the tracks to it easily, you need to turn DRC off. A slighty better method, but a bit more work is to use small vias and once the routing is done, place the pad modules over the vias, this way you can leave DRC on. Andy On Wed, 14 Apr 2010 02:06:02 - James jamesrsw...@gmail.com wrote: --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: I find that the problem with 0 ohm R and such like is that they are a fixed width, I also find it rather awkward to add them to a board, then to the sch and so on. I also prefer to have a sch. to work with. What I do for single sided boards is set the via size to the same as what I use for a normal through hole component Then I just route the board as normaly on the copper side, and where needed I switch to the component side and run tracks as if they were my jumper wires. The component side copper print becomes my jumper layout (if it ever gets that complex) For small home projects this works very nicely for me. Andy That's what I've been doing, and I've found it to be a usable workaround but it sure would be nice if there was a proper solution for this. Another program I tried at one point let me place standard pads anywhere, including the rectangular IC type pads that are nice if space is tight and then connect them with wires, it worked really well. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Problem with 78/79xx components being disconnected in PCB editor
The most common problem is that there is a mismatch between the pin names/numbers from the sch. to the module. This can happen if you use a different module for some reason, i.e. a different package. You can run into similar issues with transistors, ebc, 123 , bce and so on. Another thing to always do is to run a erc on the sch, just to pick up any non connections. Andy On Mon, 12 Apr 2010 14:39:57 + (GMT) Karl Ekdahl elektrodw...@yahoo.se wrote: Hi, i'm new to this group! I've been using KiCad for a while and i just experienced an error i've never seen before; while entering the PCB editor all pins to my 78/79xx voltage regulators are disconnected! AFAIK there doesn't seem to be any problem in the schematic (no errors except power-flag warnings i always get) and they WERE connected at one point. I've tried deleting the components and making new ones, assigning new packages but to no avail. Any clues? Thanks Karl __ Använder du Yahoo!? Är du trött på spam? Yahoo! E-post har det bästa spamskyddet som finns http://se.mail.yahoo.com Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Feedback
I find that the problem with 0 ohm R and such like is that they are a fixed width, I also find it rather awkward to add them to a board, then to the sch and so on. I also prefer to have a sch. to work with. What I do for single sided boards is set the via size to the same as what I use for a normal through hole component Then I just route the board as normaly on the copper side, and where needed I switch to the component side and run tracks as if they were my jumper wires. The component side copper print becomes my jumper layout (if it ever gets that complex) For small home projects this works very nicely for me. Andy On Sat, 10 Apr 2010 21:01:22 - Frank bennet...@digis.net wrote: --- In kicad-users@yahoogroups.com, Anders Gustafsson anders.gustafs...@... wrote: 1. Jumpers Agreed. I use oversized vias for that and although you can create a wire component, such component should be stretchable in increments of 2,54mm to be really useful How about a zero ohm resistor, either surface mount, thru-hole or 0.1x0.1xX headers? 2. Abitrary pads I just place the component 1PIN and make the size of the hole what I want. works great. To place connected stuff that is not in the schematic/netlist, you need to turn off DRC though. Every pin, even test points should be referenced in a netlist and/or a schematic to provide closure for a complete route. Hard to beat working with a schematic created netlist to drive a layout rat's nest...somebody has to veriry proper operation of the board and a schematic would greatly help that person. 3. Trace width Yes, a dropdown of common widths would help to get a more consistent board. What is standard? Seems to be more of a function of the tolerance to what PCB manufactures can handle. I think there is a global set track width and a set track width per net such as Power and ground. - Anders Gustafsson Engineer, CNE6, ASE Pedago, The Aaland Islands (N60 E20) www.pedago.fi phone +358 18 12060 mobile +358 40506 7099 fax +358 18 14060 James jamesrsw...@... 2010-04-09 23:39 No easy way to designate jumpers for single sided boards. I've been using enlarged vias but this is not ideal. It would be really great if I could just plunk down a couple of standard pads of the desired size/shape and designate them as connected. I've seen products that have a wire component that can be used to connect between points. Similarly, I can't just plunk down pads arbitrarily in the layout. I like to use pads to designate mounting screw holes and such, or for test points, flying leads, etc. It really ought to be possible to place pads without them being part of a package. Trace width selection is cumbersome, rather than a dropdown list of common widths with the option to enter an arbitrary list, it seems one has to create a list of trace sizes otherwise by default there is only one available, and there is a limit of 7(?) custom sizes. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Print several PCBs per page
Have you tried in pxbnew: fileappend board be a bit careful and note where the board is placed, use block move to get it out of the way when you append the next board. or you can end up with a mess. For multiple copies of the same board use the block copy command. Andy On Wed, 07 Apr 2010 10:27:54 +0100 Robert birmingham_spi...@gmx.net wrote: I've used the same technique as you for post-processing in Inkscape, but unlike the OP I wanted to produce gerbers (for production). I just wondered if you had solved that problem too. Regards, Robert. On 07/04/2010 10:06, Sergey A. Borshch wrote: On 07.04.2010 11:41, Robert wrote: If you do something like this, is there a way to generate gerbers from the Inkscape file? I don't know exactly. I use .pdf for home-made prototypes. My manufacturer use some CAM program for gerbers post-processing, but I don't know which one. I thought you was talking about prototyping as well. No virus found in this incoming message. Checked by AVG - www.avg.com Version: 9.0.800 / Virus Database: 271.1.1/2795 - Release Date: 04/06/10 19:32:00 Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Convert from Eagle to Kicad
Have you found this script: http://www.cadsoft.de/cgi-bin/download.pl?page=/home/cadsoft/html_public/download.htm.endir=eagle/userfiles/ulp eagle2kicad_sch.ulp ? I don't know if it's any good, I don't use eagle . Andy On Sat, 3 Apr 2010 14:27:01 +0200 (West-Europa (zomertijd)) Daniel Strang hi...@dds.nl wrote: To Whom It May Concern: I have been forced to switch from Eagle to Kicad because of the limited board space allowed. It is my greatest hope that it will not be necessary to redo all of my schematic files. However, I have tried exhaustively all the ULP files etc. which I could find on the Internet and nothings seems to work. This includes files which supposedly convert net files and schematic files. Can somebody please help me? Sincerely, Daniel Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] errors in eeschema
Hello Ale, The simple answer is that you MUST NOT trust lib and modules that you find on the net. Some are OK some have errors. You need to check and test each new part as you use them so that you can be sure that they meet your needs. You do not want to cancel the errors, they are there because there is something wrong. Fix the problem and they will go away. The unknown pin type is a fairly descriptive error, I would guess that one of the pins of whatever device you imported is not supported in kicad, (prob. a different name is used) you will have to find out what the pin is and then set it to the kicad equivalent. You do all this with the library editor. The draw command error is a bit more difficult, you will need to have a look in the lib file itself and see if there are problems. This sort of problem is normally due to import/export conversion issues. I would strongly suggest that you get rid on all the additional libs and mods, and only use the Kicad provided libs and mods at first, then add your own, one at a time as needed into your own lib directory. Take the time to read and work through the tutorial a few times (a bit old, but the methods are still valid) and also read the help files on each of the kicad software modules. Andy On Tue, 06 Apr 2010 14:17:52 - aleintrance aliensp...@libero.it wrote: hello all! I'm a new user of Kicad. I've designed a new scematich in EEschema, adding all the libraries I've found on the internet. I've deleted all the libraries that were not recognized by kicad (stuart.lib; m-pad-2.1.lib etc). Now when I open my schematich there are two warning messages, one in line 11 ( Unknown Pin Type [ ) and one in line 30 ( Error in X DRAW commando in line 30, aborted. ). Both error are invoked broesing the libraries. Is there a way to cancel those errors? Only to be sure my schematich is good and when I'll design the PCB all will be ok? Thank you in advance for support Ale Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Component management.
Component management is always a problem, and the question really is, is the parts in eeschema the right place to do this? There are probably as many answers to this as there are people who want to manage components:-) My two-pennyworth on the matter: eeschema is a generic schematic package, where the same symbol can be used to represent a wide range of devices. So if you want to include things like manaf and ordering info, then you will have to create an individual component for every different version of a device. Things get even more complex if you have multiple sources for a component. This always seems to be a clumsy method to me, especially if you are dealing with a lot of products. A more general method would be to use the component list output, and import that into a more conventional database. Then you will not be limited in data entry and other options. You may also find that things such as the component file generated by pcbnew will give you enough info as is, it lists the reference, value and module used. It needs a bit more processing for importing into a database, but it's fairly trivial. The main drawback with this method is that you have to maintain the database and ensure that any changes are applied correctly. However the ability to combine this with existing stock control systems and so on may outweigh this extra work. As for parts and footprints, talking to other designers who use all sorts of design tools, not just Kicad, the general opinion is that it takes very little time to draw up a device or footprint, and you only have to do this once. Doing this and creating your own libraries and modules, is the only way to be sure that you have the correct device/dimensions for your particular needs. (this is aside from 3D representations which is another matter). Maintaining your own libs and so on also safeguards yourself from things being overwritten during software upgrades. Andy On Mon, 05 Apr 2010 03:29:38 - Frank bennet...@digis.net wrote: Looking for parts - Checkout per your mosfet example: http://octopart.com/parts/search?q=2SK1058js=on This type of web site, I've been looking for for some time. These guys have also not said no to the possibility of someday including Kicad (and others) symbols and footprints for each part. -Frank --- In kicad-users@yahoogroups.com, marcmendezbermond marcmen...@... wrote: Hi all ! Progressing on my project, I have a question about component/library management. The Component list feature of eeschema is quite convenient but is there a way to accelerate data input ? I would like to use custom fields of components to store manufacturer, part number, ordering info and doing it a component at a time is quite annoying ... My idea would be to input this straight in my custom library, then using its symbols would replicate those info to my schematic. In the end, when I inserting a 2SK1058 mosfet that would result in a component with Manufacturer field set to Hitachi, Part No 2SK1058, Ordering No 1234567 in my favorite store, and so on ... Thanks in advance for pointing me out any method, M. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Coordinates in PCBnew
One is absolute the other is resettable. Pressing the space bar will zero one set, this is very useful for measuring distances and getting things like board edges to align. Andy On Mon, 05 Apr 2010 15:47:59 - Michael oniamien.angelf...@gmail.com wrote: I noticed that at the bottom of the screen there are two boxes which display coordinates, one with X Y coordinates, the other with x y coordinates. (Note the difference in capitalization, as that is what I am concerned with.) I understand how the coordinates displayed there correspond to position of my cursor on the diagram, but what I do not understand is why they are apparently the same. The lower case and uppercase coordinates always report the same thing, whether I am moving an object, selecting an area, or just placing the cursor on the screen, BOTH the lower and upper case coordinate boxes report the position of the cursor with identical numbers. I can't imagine they are actually supposed to report the same thing since that would be redundant, but the fact is they are always the same as far as I can tell. Am I missing something, like a situation where they DO display different coordinates, or are they really the same? Also, if there is any to customize what coordinate is displayed, for instance if I move an object, the X Y coordinates could be where the piece started, and the x y coordinates could be where cursor holding the object is currently positioned, please let me know because that would be endlessly more useful than two displays of identical information. Thanks for your help! Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Naming PWR and GND nets in eeschema?
Yes invisible pins are auto connected. The Power pin not driven catches most new users out. All that is happening is that DRC is checking that there is a source of power for a pin identified as power in. This can come in two ways, either a device that has a power out pin defined, such as a regulator, or in cases where there is no such device i.e. the power comes in from off-board, all you have to do is add a power flag symbol to the net. This tells DRC that you are providing power and that will sort things out. The only oddity is that GND is also considered a power in, so that needs to have a power flag on it somewhere as well. Have a read of the help document, there is a lot of useful tips in there. Andy On Sat, 27 Mar 2010 12:52:56 -0700 rocko sunblast...@gmail.com wrote: Huh? Not sure I understand your notes. The net is auto generated? Then why am I getting the ERC error on my VCC and GND symbols, Power pin is not driven in The invisible PWR pins on IC's are auto connected, really? if thats the case then that's pretty cool. On Sat, 2010-03-27 at 14:30 -0500, Karl Schmidt wrote: I made a few notes on this a while back - if any of this has changed please let me know. http://wiki.xtronics.com/index.php/Eeschema#Notes_2 I remember weirdness of how this works - -- Karl Schmidt EMail k...@xtronics.com Transtronics, Inc. WEB http://xtronics.com 3209 West 9th Street Ph (785) 841-3089 Lawrence, KS 66049 FAX (785) 841-0434 When angry count four; when very angry, swear. --Mark Twain -- Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Naming PWR and GND nets in eeschema?
GND symbol on the other, Kicad will auto assign to the GND net? Correct, same with VSS and so on. I often dot VSS power ports over the circuit for things like pull up resistors. More generally this will happen to ANY symbol that you use that is in the power port library, so there are VDD, VSS GND and so on. For auto connection, any pin on a device that has the same name as a power port pin will get connected to that particular net. Andy On Sat, 27 Mar 2010 13:39:07 -0700 rocko sunblast...@gmail.com wrote: AHA! Now I see, VCC and GND needs a Power Flag. That got rid of my DRC Errors. Just to be sure. So GND and PWR nets are auto generated? Say I have a battery symbol on one side of schematic and need to place a GND symbol on the other, Kicad will auto assign to the GND net? On Sat, 2010-03-27 at 20:23 +, Andy Eskelson wrote: Yes invisible pins are auto connected. The Power pin not driven catches most new users out. All that is happening is that DRC is checking that there is a source of power for a pin identified as power in. This can come in two ways, either a device that has a power out pin defined, such as a regulator, or in cases where there is no such device i.e. the power comes in from off-board, all you have to do is add a power flag symbol to the net. This tells DRC that you are providing power and that will sort things out. The only oddity is that GND is also considered a power in, so that needs to have a power flag on it somewhere as well. Have a read of the help document, there is a lot of useful tips in there. Andy On Sat, 27 Mar 2010 12:52:56 -0700 rocko sunblast...@gmail.com wrote: Huh? Not sure I understand your notes. The net is auto generated? Then why am I getting the ERC error on my VCC and GND symbols, Power pin is not driven in The invisible PWR pins on IC's are auto connected, really? if thats the case then that's pretty cool. On Sat, 2010-03-27 at 14:30 -0500, Karl Schmidt wrote: I made a few notes on this a while back - if any of this has changed please let me know. http://wiki.xtronics.com/index.php/Eeschema#Notes_2 I remember weirdness of how this works - -- Karl Schmidt EMail k...@xtronics.com Transtronics, Inc. WEB http://xtronics.com 3209 West 9th Street Ph (785) 841-3089 Lawrence, KS 66049 FAX (785) 841-0434 When angry count four; when very angry, swear. --Mark Twain -- Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Trying to add to library, Requesting help
welcom Lauri, When you say trying to add I am assuming that you mean a part in eeschema rather than a module in pcbnew. Are you drawing the part from scratch, or have you found a part from another source and you are trying to import it? Another common mistake is that when you place a unit of a multi-part package, you always get part A placed. To change to one of the other parts, right click on the part A, and select edit component part From there you can select whichever part you want. Andy On Thu, 25 Mar 2010 22:01:00 -0700 (PDT) Lauri Koponen lkop0...@yahoo.com wrote: Greetings, I am new to the group and just started using Kicad. I am trying to add a CD4041 to the library but the pin numbers remain the same on all parts A through D. Any assistance will be greatly appreciated. I am working on a solar tracker. The circuit is for a bidirectional DC motor controlled. I am hoping that I can generate a Grebber file so I can use my cnc mill to engrave the circuit and make my own pcb. Thanks again and best regards.
Re: [kicad-users] kicad kicad-2010-03-14-svn-R2456-final-UBUNTU_9.10.tgz
I reported this here a few days ago. I tried to install the Ubuntu version on SUSE, and I got the same error. The install.txt file mentions that you need libc.so6 as did the 2009 final. I have so.6 and 2009 worked fine. The install txt makes no mention of GLIBCXX_3.4.11 If you check /usr/lib/libstd* you will get something like this (ls -al) lrwxrwxrwx 1 root root 19 2009-06-24 17:34 libstdc++.so.6 - libstdc++.so.6.0.10 -rwxr-xr-x 1 root root 971048 2008-12-03 04:29 libstdc++.so.6.0.10 Where you can see that the link libstdc++ points to libstdc++.so.6.0.10 on my system. In the suse repository it looks like libstd++43 is the main file for so.6.0.10 There is a libstdc++44 available that contains so6.0.13 I have no idea if that is the required version. Judging from the various net postings, GLIBCXX_3.4.11 is causing all kinds of trouble. Probablly because it is not generally available and users don't know exactly what package they need. a bit of guidance as to what is needed would be welcome. Andy On Wed, 24 Mar 2010 01:40:03 +0100 Bernd Wiebus bernd.wie...@gmx.de wrote: Hello The previus version run in ubuntu 8.10, but this version give the follow error when I try to execute it: /usr/lib/libstdc++.so.6: version `GLIBCXX_3.4.11' not found (required by ./kicad) I had the same problem with debian lenny and the RC4 and RC5 versions. So i thought, it would be a debian only problem, but now i see, ubuntu gets the same problem. I asked about this problem here some weeks ago, and got the answer, i should try a backport from the debian testing squeeze version. I got also a suggestion about instaaling it from special backport repositorys. But there i did not find the expected material. Debian sqeeze uses only the 6.4.3 version of the *-dev package. So i got the suggestion, to build my own backports, but i am not so a skilled programmer. So i am using the 2009 Version of kiCAD. But this shows to me, that the Debian squeeze version will not solve the problem.have you tried the aktual ubuntu 9.10 already? With best regards: Bernd Wiebus alias dl1eic -- Sicherer, schneller und einfacher. Die aktuellen Internet-Browser - jetzt kostenlos herunterladen! http://portal.gmx.net/de/go/atbrowser Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] EESchema can't find libraries.
They live in usr/local/kicad/share/ Two sub directories off that, library and modules, for parts and pcb modules. The libs and mods used to be in the file list, but I cannot see them They ARE in the main download. The latest stable version is 2010-03-14 is on this site ftp://iut-tice.ujf-grenoble.fr/cao/ and has the libs in it, as does the previous version. The easiest method would be to grab this file and just do the install as per the install text, not forgetting the chmod (which is what I normally forget) Andy On Fri, 19 Mar 2010 23:36:20 - scottyaa2000 scottyafl...@sbcglobal.net wrote: Hi all, I've been a member for a few months, and reading the postings, but only now actually trying to use Kicad (I'm a student in my last term, and haven't had a need - or the time - before this). My issue may have been addressed before now, but I can't remember, and can't find any posts. I've built the latest stable version (20100314) from source (for Ubuntu 9.10 on AMD64 X2 machine), but when I open EESchema it can't find any of the libraries. I assume this is because they aren't included in the source archive, but I can't find a library archive file on any of the Kicad sites that I can download, and I'm not sure into which directory I should extract it (/usr/local/share/kicad/ ?). If someone could kindly point me to the Kicad library archive file (.tar.gz, .tgz, .zip, whatever), and give me a hint as to where I extract it, I will be forever grateful. BTW: I've been using Eagle for circuit board design, but only because when I was looking for a Linux ECAD application Kicad didn't show up in my searches (and Eagle was cheapest/best I could find). I can no longer afford to keep updating to the latest version, and prefer FOSS, so here I am. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
[kicad-users] Kicad 2010-03-14 error
I am just flagging this as a possible problem... Just as a test I tried the 2010-03-14-svn-R2456-final-UBUNTU_9.10.tgz I run SUSE, so I WAS expecting problems. Normally I load the CENTOS version without any problems which is not yet available as a binary install. On running it failed, and gave a short error message, it said it needed libc.so.6, in GLIBCXX 3. something I can't remember the exact version. The install.txt only mentions the requirement of libc.so.6, which is the same as for the 2009-02-16 version that I normally run without problems. This may be a UBUNTU specific issue, or maybe something else. if libc.so.6 is already available, then crashing out with a GLIB version issue does not seem correct. Of course it may be looking for something else as well. The install txt also mentions the chmod command, but on the kicad/linux directory, I think this should be the kicad/bin directory as per the previous version. Andy
Re: [kicad-users] Question and improvements
Welcome Carlos, You have come into the discussion a little late :-)) Undo in PCBnew has been one of the most requested enhancements, and the latest RC versions have this function, so you can either wait until the final release is ready, or have a play with the latest RC version, bearing in mind that there may still be bugs in it. Andy On Fri, 19 Mar 2010 02:54:25 - atarillusionmaker atarillusionma...@yahoo.com.br wrote: Hi! My name is Carlos Poloni and this is my first post. My first question is about command Undo (ctrl Z) in PCBNew program. I believe that an Undo command could help significantly during development. Could you tell me if there will be the implementation of the undo command in the future versions of Kicad PCBnew program? One suggestion: In the EESchema program, the implementation of rotate block command will be welcome. Thanks. Carlos André Poloni C.A.P. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] change net connection of invisible Pins
Vcc IS the power to the chip, U2A in this case. so why have you connected +5V to it as well? DRC is detecting that you have effectively shorted VCC to a different 5V supply as well, and is complaining about it. Power flags are defined as power out pins, and you only have one power out on a power net,m if you add a second power flag DRC will complain about that as well. I think you are assuming that you need to connect 5 volts to the chip, and so are adding the +5V port, which is another independent supply net. Hence the confusion. The system works as has been mentioned by the power port names. When a device has a power pin with a specific name, AND you set the pin to be invisible you DO NOT need to connect anything else to it. As soon as you put a power port with the same name onto the circuit diagram, that port is automatically connected to all device power pins with the same name. A power net needs to be energised or DRC will complain. That can be done in two ways. Either a device such as a regulator can have a power out pin, which will indicate that it is energised, OR you add a power flag, which simply says that the net is energised. You use power flags in situations where you are connecting an external power source to your circuit via a connector, flying leads and so on. The one oddity is that GND is considered a power out type net as well, so it also needs energising with a power flag. logic IC's have generally had their power pins identified by names rather than the voltage, so you have Vcc Vss Vdd and so on. When you run into such chips, the same will apply, power ports of the same name are already considered to be connected to the physical supply Andy On Mon, 15 Mar 2010 16:13:15 - mtheling p...@swapout.de wrote: Hi Robert, if I connect for example a net +5V to a component U2A which has an VCC input as invisible pin, I see that in PCBnew the pin is connected to the +5V net as soon as I set an Powerflag to +5V. But the ERC check in eeschema states this as error : ErrType(5): Conflict problem between pins. Severity: error @ (5,1000 ,6,7500 ): Cmp #FLG01, Pin 1 (power_out) connected to @ (4,4000 ,6,7500 ): Cmp #FLG06, Pin 1 (power_out) (net 3) If I don't connect a Powerflag to the +5V net, in PCBnew the Power Pin of U2A is still connect to the VCC net and not to +5V as set in the schematic. Please see schematic for example: http://www.swapout.de/example_schematic.pdf What I am doing wrong? Thank you, best Regards, Mark Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] change net connection of invisible Pins
You can manually connect the power if you enable show hidden pins in eeschema, but that means that you have to manually connect all the power pins up. What I don't know because I've never tried it, is if that over-rides the pin names for DRC. I would guess not. In practise the solution is very simple. Duplicate the library part and change the name of the power pins to something else. For example change Vcc to +5V, then you can use a +5V power port which will connect to just that chip. Obviously you save the part under a different name, then that part will connect to the new power net. You could also just identify the pins as power in, and not give them a special name untick the not drawn box, this would meant that you need to manually connect them. For small circuits this is not much of a problem, however it can get messy if you have a reasonable number of IC's to connect. Andy On Tue, 16 Mar 2010 14:07:21 + Robert birmingham_spi...@gmx.net wrote: Thanks for your replies Carl and Andy. Speaking for myself, I have designs that use two instances of the same micro, with each instance on a different supply rail. These micros all have a power pin named VCC and I have no problems with ERC, so Kicad isn't covertly connecting my VCC pins together. The OP (Mark) wants to have logic chips on two different supply rails, but it seems that Kicad joins up all the hidden pins marked Vcc, even if you connect the power pin to a different rail. Is the critical factor that the pins are hidden, is it that the name case sensitive, or is it a feature of multi-part components? It's not that the pin doesn't have a number, because the logic chip symbols have both name and number specified for the power pins (like the symbols I have created for myself). What is the critical thing that Mark has to change to allow him to connect two logic chips to two different supply rails. Regards, Robert. On 16/03/2010 11:14, Andy Eskelson wrote: Vcc IS the power to the chip, U2A in this case. so why have you connected +5V to it as well? DRC is detecting that you have effectively shorted VCC to a different 5V supply as well, and is complaining about it. Power flags are defined as power out pins, and you only have one power out on a power net,m if you add a second power flag DRC will complain about that as well. I think you are assuming that you need to connect 5 volts to the chip, and so are adding the +5V port, which is another independent supply net. Hence the confusion. The system works as has been mentioned by the power port names. When a device has a power pin with a specific name, AND you set the pin to be invisible you DO NOT need to connect anything else to it. As soon as you put a power port with the same name onto the circuit diagram, that port is automatically connected to all device power pins with the same name. A power net needs to be energised or DRC will complain. That can be done in two ways. Either a device such as a regulator can have a power out pin, which will indicate that it is energised, OR you add a power flag, which simply says that the net is energised. You use power flags in situations where you are connecting an external power source to your circuit via a connector, flying leads and so on. The one oddity is that GND is considered a power out type net as well, so it also needs energising with a power flag. logic IC's have generally had their power pins identified by names rather than the voltage, so you have Vcc Vss Vdd and so on. When you run into such chips, the same will apply, power ports of the same name are already considered to be connected to the physical supply Andy On Mon, 15 Mar 2010 16:13:15 - mthelingp...@swapout.de wrote: Hi Robert, if I connect for example a net +5V to a component U2A which has an VCC input as invisible pin, I see that in PCBnew the pin is connected to the +5V net as soon as I set an Powerflag to +5V. But the ERC check in eeschema states this as error : ErrType(5): Conflict problem between pins. Severity: error @ (5,1000 ,6,7500 ): Cmp #FLG01, Pin 1 (power_out) connected to @ (4,4000 ,6,7500 ): Cmp #FLG06, Pin 1 (power_out) (net 3) If I don't connect a Powerflag to the +5V net, in PCBnew the Power Pin of U2A is still connect to the VCC net and not to +5V as set in the schematic. Please see schematic for example: http://www.swapout.de/example_schematic.pdf What I am doing wrong? Thank you, best Regards, Mark Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad
Re: [kicad-users] Re: panelizing.
Not directly as in make 10 copies of this... However it does support append board (PCBnew file menu) You can use this to load another board into the current board. The only gotcha is to make sure that you move your current board away from the centre first, or the import can sometimes overlay the appended board over the top of the current which just makes a mess. Once loaded you can also use the copy block commands to create more copies as needed. Andy On Thu, 11 Mar 2010 00:30:21 - G.Dragon treg...@gmail.com wrote: does KiCAD support panelizing? --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: Sounds a reasonable workaround, just remember to leave enough room between boards for cutting. Andy On Wed, 10 Mar 2010 20:33:36 - G.Dragon treg...@... wrote: I am working on some PCBs that are pretty small (1.5x3 inches and 1.05x 5 inches) and am running into a cost issue. in small quantities, single PCBs like this are as expensive as larger PCBs. after talking with a rep from Advanced Circuits, he suggested that I panelize the boards to fit 7-10 or so of them on a board and then submit that, that way it would be far more cost effective. And since I'm not expecting to make a profit on these, and am only hoping to break even, that would be great. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] component and module linkage
Edit the footprint filter property then use automatic association when running cvtpcb. See section 12.5.4 of the eeschema documentation. Andy On Thu, 11 Mar 2010 06:41:55 - Panson suk...@yahoo.com wrote: It may be asked and answered somewhere before. Is it possible link a component and a module (footprint) in the library as that in Eagle. When we select a component in schematic capture, we select the footprint at the same time. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] panelizing.
Sounds a reasonable workaround, just remember to leave enough room between boards for cutting. Andy On Wed, 10 Mar 2010 20:33:36 - G.Dragon treg...@gmail.com wrote: I am working on some PCBs that are pretty small (1.5x3 inches and 1.05x 5 inches) and am running into a cost issue. in small quantities, single PCBs like this are as expensive as larger PCBs. after talking with a rep from Advanced Circuits, he suggested that I panelize the boards to fit 7-10 or so of them on a board and then submit that, that way it would be far more cost effective. And since I'm not expecting to make a profit on these, and am only hoping to break even, that would be great. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: Importing Footprint Module files - what file types are needed?
What you are saying is a little bit confusing, due I guess to however the part was created. Assuming that your module is called connect: Kicad uses the following files. connect.mod This is the actual module, open it with a text editor and you will see all the info, drawing commands and such like. This is the ONLY file that you actually need. connect.dcm This is a document file that describes the module. Not often seen in 3rd party modules, use it or not the choice is yours. It provides addition info only This could also be a blank file, again check with a text editor. connect.brd This is a standard PCB Board file. Again it's text based as are all kicad files, so you can check it out with a text editor. The point about providing board files is that you can use dummy boards to store and organise your modules, and from a board you can create or update the modules. (you use the archive commands on the file menu to do this) If you dig around in the standard kicad module directories you will find similar board files. These are what you print out as module documentation. Have a good read of the pcbnew documentation pcbnew help contents See section 11 generally, and 11.11 in particular. Assuming that the mod file is correct, all you need to do is copy it into one of your module directories, and make sure that your project can see it. Use preferences library to check and if necessary add. Watch out for silly things like duplicate names and so on. If the mod file is dud, load up the brd file into pcbnew, then open the module editor and get the module from the board. From there you can save it into a module directory or export it and so on. Remember that you need to make sure that your PROJECT can see the necessary locations for libs and mods, especially if you are placing them in your own directories (as you should be). Such additions are NOT carried over to new projects unless you replace the default template. So from here it looks like you have a couple of chances to get the module, either via the mod file directly, or from the board file. Whoever has created the mod seems to have done a reasonable job. Hope that clears things up a bit for you. If you get stuck, feel free to contact me off list, and I'll be happy to try importing your module into my system to see if it works. Andy On Wed, 24 Feb 2010 01:51:02 - john_henn...@bellsouth.net john_henn...@bellsouth.net wrote: The module was placed in a directory that Kicad knows about (one of the paths point to the directory where the file is). The file I downloaded was a *.mod file...it was the only file given for the part I downloaded. My question, again is: for a given part, how many different files are required to support the part? Three? The connect.mod file resides in the c:\program_files\kicad\share\modules directory. There are two files with the connect.* name - they are: connect.mdc and connect.brd. The error that I was getting specified the *.mdc file and that the program could not find it...I checked the library prefences in eeschema, cvpcb, and pcbnew...they are all set correctly. --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: The most common errors are that people have imported the modult into a directory that is not part of the libraries that a project knows about. Use preferences library to select which libs your project will search. The second is that when importing into an existing library the final save is not done. Andy On Fri, 19 Feb 2010 18:51:57 - john_henn...@... john_henn...@... wrote: I recently imported a downloaded connector module (con-headers-jp.mod) into the CvPCB footprint library. The footprints assigned without an error, but I get an error when I read the netlist into pcbnew. The error says that pcbnew cannot find the footprints for the connectors that I am using. When I re-run CvPCB, I get an error that the con-headers-jp.mdc cannot be found. When importing footprint files, what are all the required file types? Looking at the modules subdirectory, it contains *.brd, *.mdc, and *.mod files. Are all these necessary for a footpring library? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up
Re: [kicad-users] Re: pcbnew is amazing slow under windows 7
This may be a red herring, but there have been one or two suggestions that W7 is maxing out it's available memory more that anticipated. I saw this reported o one of the newswires in the last day or so. Andy On Fri, 19 Feb 2010 21:12:07 - o00batman00o o00batman...@yahoo.com wrote: I did not want to criticize kicad, I just wanted to know if other user experience the same issue as me. I'm really satisfied about kicad functions. For information, my configuration is the following: core2DUO P8700 2,54GHz with 4Gb of RAM. The graphic card ;) is a Intel GMA4500MHD. I dont think it's an hardware problem, it's just due to the bad openGL implementation since Windows Vista. Kicad is running very well on my desktop PC using XP with a lighter hardware configuration. --- In kicad-users@yahoogroups.com, Greg Dyess gregory.dy...@... wrote: OK, I think your rant against Windows is just a little over the top and adds nothing constructive to the conversation. Some people don't have the choice to run whatever they want and that must be recognized. KiCAD supports Windows and if there is a major performance issue, it should be looked into since the level of graphics processing is pretty minimal for KiCAD compared to real-time games, etc. Having said that, I run KiCad on a machine (quad core, 2.4 GHz, 2 GB RAM) that dual-boots Windows XP Pro and Ubuntu 9.10. I see no discernable difference in performance between the two, so it's highly unlikely that Windows vs Ubuntu can account for the performance issues the user is reporting. I also run KiCad on a 3-year old laptop (dual-core, 32 bit @ 1.7 GHz with 2.5 GB RAM) and have performance complaints there either. You didn't mention what hardware you are running this on, so it's hard to tell whether you are just simply underpowered for Windows 7. Does your system run other applications well? Have you checked the Task Manager and/or Performance Monitor to try to determine what resource is causing the bottleneck (CPU, Memory, Disk, Interrupts, etc)? I would suggest you check the following: 1. Check to make sure all of the third-party libraries are up to date and are compiled with the optimizing/release settings. 2. Make sure you have plenty of RAM (at LEAST 2 GB or more). 3. Make sure you have the latest optimized drivers for your video card. 4. If you have BOINC running, make sure none of your projects are using the CUDA to push processing onto your graphics card. If you do have this, make sure at lease you have it set to only use the GCU whenever it is not busy or your graphics willl be horribly slow on everything. Check to see if you have any viruses or anything else running in the background soaking up CPU/GPU cycles. Greg From: DanielW dan...@... To: kicad-users@yahoogroups.com Sent: Mon, February 15, 2010 1:53:09 PM Subject: [kicad-users] Re: pcbnew is amazing slow under windows 7 There's another solution you're missing: use a CAD package that's designed to work well under Windows, unlike KiCad. Someone who's willing to shell out hard-earned cash for Windows 7 should be happy to also buy a nice commercial CAD package, such as Orcad. Trying to run Free software on Windows is just silly. If you're going to buy into the whole commercial software thing, then don't do it halfway. Use paid, commercial software for everything you do in Windows, as the whole environment is one where Microsoft and its ISV partners work together to bring you the software experience they think you should have, for a fee, and if you're bought Windows, then that proves that you also buy into Microsoft's vision. Microsoft's vision does NOT include any Free software; they've stated this publicly over and over. Personally, I'm perfectly happy with KiCad running on Kubuntu. Dan --- In kicad-users@yahoogroups.com, dickelbeck dick@ wrote: --- In kicad-users@yahoogroups.com, o00batman00o anthony.siegrist@ wrote: Hello Since I upgraded to windows 7, I can't use pcbnew beacause the screen refresh is amazing slow. I can see dot grid showing up from left to right. I notice the same behavior on all PC running Windows Vista or 7. My temporary solution is to run Kicad under Ubuntu via VirtualBox. By this way refreshing rate is in my opinion 10 times faster. Does someone noticed the same issue? No, but I don't use Windows. Is there a solution ? Use Ubuntu? How much pain do you need, before you switch? I hit my threshold 6 years ago. I assume you use Windows for a reason, is that reason so that you can call Microsoft and get help on issues like this? Please read the Kicad FAQ in the group files section before posting your
Re: [kicad-users] Importing Footprint Module files - what file types are needed?
The most common errors are that people have imported the modult into a directory that is not part of the libraries that a project knows about. Use preferences library to select which libs your project will search. The second is that when importing into an existing library the final save is not done. Andy On Fri, 19 Feb 2010 18:51:57 - john_henn...@bellsouth.net john_henn...@bellsouth.net wrote: I recently imported a downloaded connector module (con-headers-jp.mod) into the CvPCB footprint library. The footprints assigned without an error, but I get an error when I read the netlist into pcbnew. The error says that pcbnew cannot find the footprints for the connectors that I am using. When I re-run CvPCB, I get an error that the con-headers-jp.mdc cannot be found. When importing footprint files, what are all the required file types? Looking at the modules subdirectory, it contains *.brd, *.mdc, and *.mod files. Are all these necessary for a footpring library? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: copy component from schematic to library editor
Not that I know of. The .sch file does contain a list of what libs it knows about, and that is what will appear in the library list when you use the editor. However the parts are only simple text, and once they are in the .sch file there is not really any need to refer to the actual lib. Also there are SO many devices available, both native and converted that to try to state what lib was used would be very difficult, especially if moving things from machine to machine (hence why the cache is created) This sort of thing all boils down to project management, You as the designer need to create a system that you can work with and maintain. As I don;t make to many PCB's, just what I do for home projects, I have a library set up in my home directory (I use the linux version of Kicad) and I drop any odd parts and mods that I use or create which are not in the standard library into there, For other libs when they are for a whole series of parts, rather like the microchip lib in the standard lib, I do create that as a stand-alone lib, but I make sure that I know where it is, it all goes into my own lib directory. What I don't do is include an entire set of libs from something like the oshec,org as a hugen monolithic lump. That just makes things very hard to manage. Andy On Tue, 02 Feb 2010 10:40:38 - tom_iphi i...@arcor.de wrote: Hi Andy, Dan, thanks for the hints. I found the cash and retrieved my components form there. They might still have been sitting in some library, but I couldn't figure out in which one. An info function would be handy that tells you from which library a component or module comes. Does KiCAD contain something like this? Tom --- In kicad-users@yahoogroups.com, Dan Andersson d...@... wrote: On Monday 01 February 2010 18:39:56 tom_iphi wrote: Hi, can somebody give me a hint how to copy a component from the schematic to library editor? Somehow some of my components have disappeared from the library, but I can still see them in the schematic. Thanks! Nope, you're wrong Tom. If you can see them, they are there. If I install a new KiCad without the VNWA2 libs and modules correctly copied, I see it in the schema or pcb drawing. Catch me on skype for a cgat. /Dan Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: KiCAD Parts Repo [was: S-100 and ECB homebrew computer templates for KiCAD/FreeRouting.net]
This was discussed some time ago as I remember As a matter of interest, who run kicadlib.org s that would seem to be an obvious starting place. I don;t think an automated system will work 100% but it is the obvious route for most operations. You would probably end up with a two stage system. The normal system where things are uploaded by contrib. when can be anyone, then a second set which has been audited as ok and locked to prevent any changes to the list. (obviously what a user does after download is up to them) What you must not allow is parts to be uploaded under any name or description, that causes chaos, so whatever system you use must allocate the critical names and identifiers. I've seen the results of allowing people to do that, and it's not nice - people would fill in equipment records with things like Cisco Hub, cisco switch, cis. switch and so on. This made finding things very hard. That was soon changes to a drop down list so that everyone picked the same name for a particular equipment type. The hardest part is just defining the minimum requirements that you really need. A part is only one file, and a module is maybe two if you include a 3d file as well. Including an image of the part or mod might be something to think about but that's open to debate. You also need to define a set of criteria that defines when a part is deemed to be audited as OK. It will not be sufficient to say that x people have use it, and say OK, as an example from the group over the past few weeks, a member found a problem where the silk screen covered the pads. Not an obvious thing to think of, but important for pcb production house builds. What you really want to avoid is getting bogged down in details that make things overly complex. Andy On Tue, 02 Feb 2010 08:40:28 -0500 mike m...@pikeaero.com wrote: Anders, Yes, I think that would be possible, however, I think you would wind up with something like the yahoo file area where you just have everything sort of scattered about unless you have a human gatekeeper of some sort. So I guess that's the first requirement, should it be automated or include a human gatekeeper of some sort? Personally, I would prefer an automated or semi-automated type of web based solution. My vision of a KiCad Parts Repository: Uploading parts: I goto http://kicadparts.org or whatever and create an account. I upload some widgets. Before the widgets can be published, I need to classify them into some sort of category structure. I need to provide a jpeg image, and a brief description. Downloading Parts: I goto http://kicadparts.org or whatever and type into the search box PLCC and I get a list of all the part hits that are PLCC sockets of some sort. Maybe there's a refined search where I can narrow the search. The downloading parts should even be almost like a shopping cart experience... I'll have one of those, one of those, I wonder if they have something like this You should be able to select categories of parts and have them assembled into a lib before downloading. Or how about even you add parts to a basket just like a shopping cart, and then you have the option of assembling parts in your basket into a lib at checkout Feedback on parts: You need some method of QA on parts...I suppose in a community based structure the best QA is some sort of feedback mechanism where you can leave feedback on parts that others can see. I suppose the parts should be able to have some sort of revision history so that that consumers can see if issues have been addressed with a particular part, etc.. My point is that if people are going to consistently use the repository, it has to be user friendly, custom tailored to this specific application...I think. There are a few issues with what I have proposed like the handling of known defective parts and non-responsive part owners, and things like that, but those sort of things would probably just fall to whomever is the admin as sort of policy issues I think. I guess what I am proposing, is a custom, one-off web based application solution. I know, it's a lot of pain up front but I think it would really pay off in terms of boosting KiCAD to a new level. Comments? Mike Sharkey On February 2, 2010 02:19:51 am you wrote: I think it is an excellent idea. Why not use sourceforge? - Anders Gustafsson Engineer, CNE6, ASE Pedago, The Aaland Islands (N60 E20) www.pedago.fi phone +358 18 12060 mobile +358 40506 7099 fax +358 18 14060 mike m...@pikeaero.com 2010-02-01 22:37 I would not mind lending a hand to coordinate some sort of repository effort if we can agree on what a KiCAD parts repository might look like for starters. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They
Re: [kicad-users] Re: KiCAD Parts Repo [was: S-100 and ECB homebrew computer templates for KiCAD/FreeRouting.net]
I may have misunderstood the point :-) I was responding to the comment that mike made but Yahoos threading sometimes gets things muddled up. Have you found the recommended way to organise modules? Section 11.11 of the pcbnew manual. Basically you create a A4 board, and just populate it with your modules This provides you with something that you can print, and by using the archive footprint That;s a very easy way to manage things at the level you are talking about. If you hunt through the kicad file tree you will find the .brd files from which the standard libs are generated from. If you want to share such things, then the file store here is as good a place as any for the time being, there are already an assortment of libs there. The 3D is a nice to have, and to be fair it does have it's uses. Like yourself I've never tried creating a wings 3D component. I'm not sure that my limited artistic talent would be up to it. Square(ish) blocks all the same colour -maybe- but anything more complex than that, things go downhill fast :-) Andy On Tue, 02 Feb 2010 20:29:30 - lynchaj lync...@yahoo.com wrote: Hi! That sounds like a good idea but I am not a KiCAD developer or library maintainer. I'm not suggesting to build up a common parts library infrastructure although that would be very helpful if such a thing existed. www.kicadlib.org is helpful but what you are describing is much more involved. I suspect we've all probably reinvented the wheel along the way at least once or twice. Basically I'm just an enthusiastic amateur homebrew computer builder. My home brew computer information is free and might be useful to others with similar interests. I've made several custom parts for S-100 connectors, board outlines, templates, and a lot of tweaks to Z80, 6809, and related vintage/classic computers. However it is kind of a specialty niche and is clearly not going to appeal to the wider KiCAD audience. S-100 stuff isn't exactly common these days... I am fairly sure none of my stuff would stand up to any sort of audit without major corrections. It's just the starting point not a completed works. For example, I've never made a 3D model since I haven't seen a need for one. The S-100 bus connector footprint works just fine and I know what it is on the PCB enough for it to be useful. The same for Propeller DIP, SY6545, and other custom parts libraries. What I have would be a useful starting point for another interested hobbyist but not sufficient for inclusion in any sort of official KiCAD part distribution, IMO. I guess I had more of a template approach in mind. Start with a sample board, rip out the parts you don't want, put in the stuff you do want, make adjustments, make your own board, build, test, pass it along to the next person kind of a deal. I hope this clarifies my intent. If there are other home brew computer enthusiasts using KiCAD please let me know and I might be able to help out with a somewhat better starting point than completely from scratch. Thanks and have a nice day! Andrew Lynch --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: This was discussed some time ago as I remember As a matter of interest, who run kicadlib.org s that would seem to be an obvious starting place. I don;t think an automated system will work 100% but it is the obvious route for most operations. You would probably end up with a two stage system. The normal system where things are uploaded by contrib. when can be anyone, then a second set which has been audited as ok and locked to prevent any changes to the list. (obviously what a user does after download is up to them) What you must not allow is parts to be uploaded under any name or description, that causes chaos, so whatever system you use must allocate the critical names and identifiers. I've seen the results of allowing people to do that, and it's not nice - people would fill in equipment records with things like Cisco Hub, cisco switch, cis. switch and so on. This made finding things very hard. That was soon changes to a drop down list so that everyone picked the same name for a particular equipment type. The hardest part is just defining the minimum requirements that you really need. A part is only one file, and a module is maybe two if you include a 3d file as well. Including an image of the part or mod might be something to think about but that's open to debate. You also need to define a set of criteria that defines when a part is deemed to be audited as OK. It will not be sufficient to say that x people have use it, and say OK, as an example from the group over the past few weeks, a member found a problem where the silk screen covered the pads. Not an obvious thing to think of, but important for pcb production house builds. What you really want to avoid is getting
Re: [kicad-users] copy component from schematic to library editor
You have may have lost the path to wherever you stored the parts in the first place. Otherwise Kicad maintains a cache of the sch. parts in the project directory, (the cache file) Open the lib editor and select the cache as the working library (it's normally right at the bottom of the list) , and you should see your parts there. Copy them to another lib and keep then safe. Andy On Mon, 01 Feb 2010 15:39:56 - tom_iphi i...@arcor.de wrote: Hi, can somebody give me a hint how to copy a component from the schematic to library editor? Somehow some of my components have disappeared from the library, but I can still see them in the schematic. Thanks! Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Spreading out module
It's not obvious that one... You have to enable the auto move and place. pcbnew, top icon bar third icon from right (mode manual and auto) Click that on, then when you right click you will get the context menu you are looking for. Andy On Fri, 29 Jan 2010 20:27:48 - bill_s_hung bill_s_h...@yahoo.com wrote: First time user here. I am following the mini-tutorial on page 10 on this section of Spreading out module. I click on the mode module and then right click on an open area, but cannot find Glob move and Place - Move all Module option any where. What am I missing ? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] ARM CORTEX M3 library
Welcome.. There are a couple of sites that you should bookmark. http://www.kicadlib.org/ http://per.launay.free.fr/kicad/kicad_php/composant.php The first two above are good sites for libs and modules. The kicadlib site has most of the standard libs and several others. at the bottom of the page is a link to Pierre Launay site, which has a load more libs, including links to the oshec site that has 1000's of converted libs. Unfort. can't see the STM32 listed. http://kicad.sourceforge.net/wiki/index.php/Main_Page http://kicad.sourceforge.net/wiki/index.php/FAQ#How_do_I_import_libraries_from_other_PCB_programs.3F The next two pages are the main wiki site for kicad, and in that I found a reference to a script that will export the eagle libs into kicad format. The script is in the groups file folder sub directory ConvertedEagleFootprints There is also a big zip file of converted libs, but I have NOT checked this to see if it has the part you want. Andy On Thu, 28 Jan 2010 09:18:13 - didcadarm didie...@free.fr wrote: Hi, i am a new user in cad system and hope to do my first pcb ;-) I am looking for ARM CORTEX M3 library (STM32F103 LQFP64 NXP1768 LQFP100), or else how to convert the eagle library stm32.lbr for example? Thanks ! Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Re: ARM CORTEX M3 library
Look in kicad/docs the file formats are all documented. This is also where all the help documents are, and a rather old tutorial. Andy On Thu, 28 Jan 2010 16:19:19 - Ban didie...@free.fr wrote: Thank's a lot, I discover yesterday Kicad .. and today micropendous and so on .. :-) I test today stm32f103 72mhz 2wait state flash (from olimex), with FreeRtos (eclipse) also CooCox(very nice IDE!). I think to use the future nxp1768 120mhz 0 wait state flash (phy usb otg inside like stm32f107). I'll try also footprintbuilder but still search to run it under win xp;-) I load eagle and run script exp-kicad-lib.ulp on stm32.lbr, output file is stm32.mod. I need to learn kicad's files format! (mod,dcm, mdc) Didier --- In kicad-users@yahoogroups.com, josh_eeg josh...@... wrote: Good choice of chips I think. Did you look into micropendous? he has a kicad cortex m3 arm open source design... Also leaflabs has a eagle cad one. This would be the foot print builder that will save you some time... http://cyclerecorder.org/footprintbuilder/ I also like the kicad library generator to make the schematic symbol name the pins the same as they are numbered in the footprint for faster building... I hope this helps. --- In kicad-users@yahoogroups.com, didcadarm didierfr@ wrote: Hi, i am a new user in cad system and hope to do my first pcb ;-) I am looking for ARM CORTEX M3 library (STM32F103 LQFP64 NXP1768 LQFP100), or else how to convert the eagle library stm32.lbr for example? Thanks ! Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Problem description
Yes I mentioned the same thing a few messages up the thread. Either that or a system that allowed circuit blocks to be created. Currently I have a couple of small circuit blocks that I keep on a separate board layout, and when I want to use them I import that board into the board I am working on, and then block copy the part of the circuit I want. This works but can get a bit messy. Andy On Tue, 26 Jan 2010 12:14:00 +0100 Jean-Paul Gendner jean-paul.gend...@orange.fr wrote: “What would be easier would be the ability to draw custom pad shapes with multiple drill points. That way there would only be one pad number to worry about.” The dream for me is to have the possibility with the module editor to add tracks (as in the board editor) AND dummy pads. I mean pads which are treated as tracks not as “numbered” pads. Regards, Jean-Paul Jean-Paul Gendner 03.88.27.03.44 _ De : kicad-users@yahoogroups.com [mailto:kicad-us...@yahoogroups.com] De la part de Andy Eskelson Envoyé : lundi 25 janvier 2010 16:37 À : kicad-users@yahoogroups.com Objet : Re: [kicad-users] Problem description People working with components from the scrap are fairly used to mount the components they have, and not they want. :-) To hell what shape a Capacitor has. He has to match capacitance, voltage, ESR..so its nice to have layouts which would accept more than one shape of component. I agree, my junk box is the same as everyone elses :-) However Kicad was not designed as that sort of program. So we have to workaround things as best we can. There is a lot of development going on with Kicad, so lots of improvements are being worked on. The next beta release looks like it will be fairly soon, but if not you can play wit the nightly builds if you want to. As kicad develops I would expect that there will be some easier methods to add multiple pads developed. There was some discussion several months ago regarding some components that have more than one power pin, This was a solution to some noise issues I think by the component manaf. however two power pins caused quite a but of confusion. So at least that sort of problem has been flagged up. I don't know if there is any solution to this so far as I've not been taking the nightly builds. If anything has been done then that might help. Of course. This would eliminate some other similar Problems ocouring with components which have more than one pad per connection. Worst i actual have is a screw terminal with ten pads in two rows, all the same connection...:-) That should not be an issue really, give each terminal pad it's own number and also create a connector part with a matching number system, then connections you make on the circuit diagram will be reflected onto the module, including any multiple connections. I have some terminal blocks that already have one side parallel connected, with the other side for wires. i.e. it forms a bus-bar type connection. Each pad is numbered differently and on the circuit I just make sure I parallel connect all the pins, that keeps everything happy. An other point would be a TO-92 footprint wich allows stright and molded Types. I saw it so often, but seldom you get a layout program, which allows this.. That's more difficult - you can end up with clearance issues and it can make track routing a bit awkward. I tried that some time ago and in the end I decided it was easier to simply have two footprints. :-) I am thinking, more than one pad per connection would create an logical problem for DRC. Perhaps there would be a way to let the DRC recognizing a (well declarated) group of pads as one pad? What would be easier would be the ability to draw custom pad shapes with multiple drill points. That way there would only be one pad number to worry about. Andy
Re: [kicad-users] Library Component Not Updating in Eeschema
our project has prob. lost the path to the lib where you are saving the part. Eeschema maintains a local cache of lib parts in the project directory, (the .cache file) If it cannot find the part in the libs it uses whatever is in the cache. This is done to allow a project to be moved from one machine to another without the need to transfer the entire library as well. (In PCBnew the modules are saved into the board file anyway so a separate cache is not needed) Make sure that you have ADDed the library that contains your part to your project. You can also try editing your component again, and select the project cache as the working library then save into that as well. Andy On Mon, 25 Jan 2010 19:19:17 -0800 Peter Polidoro peterpolid...@gmail.com wrote: I'm running into a frustrating problem and I'm hoping someone has some sort of workaround. I created a new component in a new library and placed it into a schematic. I made some changes to the component, but I cannot get those changes to update in the schematic. I save the component both in the new library on disk and in the loaded library in memory, but neither updates the component on the schematic. I tried deleting the component and placing it again, but it still shows up as the old component. The library browser shows the updated component, but when I place it into the schematic, it shows up as the old component. Is there any way to force Eeschema to reload the components from the libraries like you can reload the modules in PCBNew? I've tried exporting the modified component and importing it into a library with a different name, no luck. Do I need to redraw the component from scratch and save it with a new name or is there some easy trick I'm missing? I just don't understand the persistence, where is that information being stored and why can't I update it? I'm using 20090216-final on linux. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Problem description
I have the schematic of the block on file as well, so everything is picked up. I do have to watch out for component numbers. Other times I've deleted the components on my circuit block and then positioned the components on the design board over them, as I said it's a bit messy, but it does save laying out the tracks again. You can put pads as close together as you want. It's up to you the deal with the clearance issues. Change them to suite your needs. Do note that if you send boards to a PCB house to be made for you, then they will have all sorts of limits regarding clearance that you will have to follow. Andy On Tue, 26 Jan 2010 15:09:59 +0100 Jean-Paul Gendner jean-paul.gend...@orange.fr wrote: Ok. I suppose that using small circuit blocks is fine to built boards without having an electrical schematic, because I do not see how you may use board blocks with a net list? I suppose to that this way do not allow pads to be very close together. Thank you, Jean-Paul Jean-Paul Gendner 03.88.27.03.44 _ De : kicad-users@yahoogroups.com [mailto:kicad-us...@yahoogroups.com] De la part de Andy Eskelson Envoyé : mardi 26 janvier 2010 14:41 À : kicad-users@yahoogroups.com Objet : Re: [kicad-users] Problem description Yes I mentioned the same thing a few messages up the thread. Either that or a system that allowed circuit blocks to be created. Currently I have a couple of small circuit blocks that I keep on a separate board layout, and when I want to use them I import that board into the board I am working on, and then block copy the part of the circuit I want. This works but can get a bit messy. Andy On Tue, 26 Jan 2010 12:14:00 +0100 Jean-Paul Gendner jean-paul.gendner@ mailto:jean-paul.gendner%40orange.fr orange.fr wrote: “What would be easier would be the ability to draw custom pad shapes with multiple drill points. That way there would only be one pad number to worry about.” The dream for me is to have the possibility with the module editor to add tracks (as in the board editor) AND dummy pads. I mean pads which are treated as tracks not as “numbered” pads. Regards, Jean-Paul Jean-Paul Gendner 03.88.27.03.44 _ De : kicad-users@ mailto:kicad-users%40yahoogroups.com yahoogroups.com [mailto:kicad-users@ mailto:kicad-users%40yahoogroups.com yahoogroups.com] De la part de Andy Eskelson Envoyé : lundi 25 janvier 2010 16:37 À : kicad-users@ mailto:kicad-users%40yahoogroups.com yahoogroups.com Objet : Re: [kicad-users] Problem description People working with components from the scrap are fairly used to mount the components they have, and not they want. :-) To hell what shape a Capacitor has. He has to match capacitance, voltage, ESR..so its nice to have layouts which would accept more than one shape of component. I agree, my junk box is the same as everyone elses :-) However Kicad was not designed as that sort of program. So we have to workaround things as best we can. There is a lot of development going on with Kicad, so lots of improvements are being worked on. The next beta release looks like it will be fairly soon, but if not you can play wit the nightly builds if you want to. As kicad develops I would expect that there will be some easier methods to add multiple pads developed. There was some discussion several months ago regarding some components that have more than one power pin, This was a solution to some noise issues I think by the component manaf. however two power pins caused quite a but of confusion. So at least that sort of problem has been flagged up. I don't know if there is any solution to this so far as I've not been taking the nightly builds. If anything has been done then that might help. Of course. This would eliminate some other similar Problems ocouring with components which have more than one pad per connection. Worst i actual have is a screw terminal with ten pads in two rows, all the same connection...:-) That should not be an issue really, give each terminal pad it's own number and also create a connector part with a matching number system, then connections you make on the circuit diagram will be reflected onto the module, including any multiple connections. I have some terminal blocks that already have one side parallel connected, with the other side for wires. i.e. it forms a bus-bar type connection. Each pad is numbered differently and on the circuit I just make sure I parallel connect all the pins, that keeps everything happy. An other point would be a TO-92 footprint wich allows stright and molded Types. I saw it so often, but seldom you get a layout program, which allows this.. That's more difficult - you can end up with clearance issues and it can make
Re: [kicad-users] Trimpots
They are for that type RV2 for the small circular type and RV2X4 for the more conventional flat type. Andy On Sun, 24 Jan 2010 05:26:30 -0800 (PST) Foobar Foobar foobar.foo...@yahoo.com wrote: I would have thought trimpots would be in the library as standard. When I say trimpot I mean the small type you adjust with a screwdriver where the legs of the component are in a triangular arrangement as opposed to the potentiometer (POT) where the three legs are in a line. --- On Fri, 1/22/10, Andy Eskelson andyya...@g0poy.co.uk wrote: From: Andy Eskelson andyya...@g0poy.co.uk Subject: Re: [kicad-users] Trimpots To: kicad-users@yahoogroups.com Date: Friday, January 22, 2010, 5:36 PM Most groups do not allow attachments to messages. Instead members are asked to use the files and photo areas. Andy On Fri, 22 Jan 2010 18:09:40 +0100 Jean-Paul Gendner jean-paul.gendner@ orange.fr wrote: Hi, There are many kind of trimpot. I have built one and would attach the files to a message, however this do not work. How may I send files to the group? Regards, Jean-Paul Jean-Paul Gendner 03.88.27.03. 44 _ De : kicad-users@ yahoogroups. com [mailto:kicad-users@ yahoogroups. com] De la part de foobar.foobar Envoyé : vendredi 22 janvier 2010 12:39 À : kicad-users@ yahoogroups. com Objet : [kicad-users] Trimpots This may seem like a really stupid question but I seriously cannot find any trimpots in the library. I can find POT in the device section but I can't find a trimpot... are they called something else in kicad?
Re: [kicad-users] Problem description
Check your mod files, if you have two lines the same this will confuse DRC, and I think by duplicating pads then is what you will create. While doing things the way you are is fairly convenient, it's not really the accepted way to do things. The module should be designed for a specific component size. One solution which is I admit, a bit of a bodge is to only use one pad, but change it's shape and extend it to cover the range you want. The disadvantage is that you will only have one drill point, rather than a whole series of them. The other way is to create a module with just a few pads, nothing else, no numbers or whatever. Then place that alongside the pads of whatever component you want the adapt. You will have to join the extra pads with a track and connect them to the existing single pad of the component, but at least DRC will be happy. Andy On Sun, 24 Jan 2010 18:08:39 +0100 Jean-Paul Gendner jean-paul.gend...@orange.fr wrote: Hi, To realize the module for some components, such as resistors or capacitors, I have the habit to put some pads for the same contact. So, at mounting time, I am able to choice between different component sizes. I also do that with Kicad, but found strange unconnected contact messages with the DRC control: two GND connections connected together by GND zones are signalled as not connected! Off courses, the different pads for a same contact have the same pin number and are connected together. I have added a PB1.brd file to demonstrate simply the problem. Any help will be welcome, Jean-Paul Jean-Paul Gendner 03.88.27.03.44
Re: [kicad-users] Problem description
The reason that components are one fixed size is because components are only one fixed size. If the component were a different size it is a different component. Which is a convoluted way of saying that most users are building circuits with a defined set of components, so the issue does not arise. What would be a nice feature would be to have the ability to create sub-circuits complete with tracks so that you could build up a library of common circuit elements and just place them like footprints. With the one pin idea, try creating a 1 pin with no numbers or names assigned to it, that should prevent drc flagging them up. Or just set down a large via instead. Andy On Sun, 24 Jan 2010 20:44:40 +0100 Jean-Paul Gendner jean-paul.gend...@orange.fr wrote: Many thanks Andy and Martin, Ok for your explanations Andy. However, I do not understand that with as sophisticated software (not only Kicad), only one specific component size is allowed, when it should be easy to foresee some. What a pity. I have tried many, many possibilities with Kicad, and also the one exposed by Martin. However, in my case, the connections with 1-pins (which may be done with DRC inactive) generate “track near pad” error messages! If that is not the case for you Martin, please give me an example. As in most of the case my solution works well (problems occurs only with GND zones), I think I will continue to deceive the DRC by doing not really needed connections for the specific cases the DRC “fails”. Perhaps the DRC check maybe changed to allow this few cases without problem for a “near” future upgrade? Thanks again, Jean-Paul Jean-Paul Gendner 03.88.27.03.44 _ De : kicad-users@yahoogroups.com [mailto:kicad-us...@yahoogroups.com] De la part de Andy Eskelson Envoyé : dimanche 24 janvier 2010 18:44 À : kicad-users@yahoogroups.com Objet : Re: [kicad-users] Problem description Check your mod files, if you have two lines the same this will confuse DRC, and I think by duplicating pads then is what you will create. While doing things the way you are is fairly convenient, it's not really the accepted way to do things. The module should be designed for a specific component size. One solution which is I admit, a bit of a bodge is to only use one pad, but change it's shape and extend it to cover the range you want. The disadvantage is that you will only have one drill point, rather than a whole series of them. The other way is to create a module with just a few pads, nothing else, no numbers or whatever. Then place that alongside the pads of whatever component you want the adapt. You will have to join the extra pads with a track and connect them to the existing single pad of the component, but at least DRC will be happy. Andy On Sun, 24 Jan 2010 18:08:39 +0100 Jean-Paul Gendner jean-paul.gendner@ mailto:jean-paul.gendner%40orange.fr orange.fr wrote: Hi, To realize the module for some components, such as resistors or capacitors, I have the habit to put some pads for the same contact. So, at mounting time, I am able to choice between different component sizes. I also do that with Kicad, but found strange unconnected contact messages with the DRC control: two GND connections connected together by GND zones are signalled as not connected! Off courses, the different pads for a same contact have the same pin number and are connected together. I have added a PB1.brd file to demonstrate simply the problem. Any help will be welcome, Jean-Paul Jean-Paul Gendner 03.88.27.03.44
Re: [kicad-users] Placing The Correct Via
It works OK here, BUT during track layout when you change layer or hit V for a via, the via is shown the same width as the track. When you end the track tool the vias then show the selected size. Andy On Sun, 24 Jan 2010 22:24:31 - giordano.george giordano.geo...@yahoo.com wrote: When I place a via, the dimensions of the via don't match the dimensions in the pull-down menu for tracks and vias. The via has a 20mil hole and a 30mil overall diameter. Originally, the via had a 30mil hole and 30mil diameter. I corrected this but every new via still has the old dimensions. This requires me to edit every via and tell the tool to use the alternate dimensions (which I've preset to the same as the new default dimensions. Does anyone know how to get the tool to place the correct via with the correct dimensions? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Footprint for a Relay ?
Many relays have a standard numbering system, especially if they are intended to be plugged into some form of holder. there are some variations, but generally they are two digit such as 11, 12, 13, 21, 22, 23 and so on, the coils are normally A1 and A2. I have also seen some bases with a letter and a number as well. The numbers refer to the poles and contacts, so 11 is pole 1 contact 1, 12 is pole 1 contact 2, 21 is pole 2 contact 1 and so on. I can't remember offhand which is the normally closed/open and common connections, I usually end up buzzing it out to be sure :-) Miniature PCB mount relays tend to be a little more variable. As for footprint, well you use the footprint that matches the relay... (I cannot see one in the standard lib) I drew up a simple footprint the last time I used a relay. I've used this SPST 12V 10A directly soldered into the PCB http://www.rapidonline.com/searchresults.aspx?style=0kw=60-4600 and the 60-4110 Double pole socket http://www.rapidonline.com/Electronic-Components/Relays-Solenoids/PCB-Relays/Miniature-relay-sockets/28667/kw/60-4110 I have simple footprints for both, if they are of any use you are welcome to a copy. Andy On Sat, 23 Jan 2010 01:09:33 -0800 (PST) yukku yukkoo yukku19752...@yahoo.com wrote: Hi, I am using the Relay RELAY_2RT from the EEschema device library. I have a couple of question about it - 1. Why does it not use contiguous pin numbers instead using pins 1,3,5 8,9 and 12,14,16 ? My guess is it uses a standard package with missing pins to get double spacing. Please confirm. 2. What foot print should I use for it in cvpcb ? Regards yukku
Re: [kicad-users] Active and Inactive space
If I understand correctly what you are asking for, it's already there. Just add a range of components that you are using once. If you wish you can place them outside the drawing outline. Then right click on a component, select copy and place the copy wherever you need it. I generally don't bother adding components outside the drawing, if I've already used one I just copy it from where I placed the previous component. Andy On Sat, 23 Jan 2010 09:29:21 - h_manbeing h_manbe...@yahoo.com wrote: Hi all, I wish someday the Kicad developpers will have the time to divide a sheet (as of eeschema for example) as two independent spaces: (1) The area inside the page limits, in which all components and connections are treated as usual so it can be called active or Real. (2) Outside the active space, in which all components and connections are just ignored as if they don't exist, so this area may be called inactive or Unreal. But these do exist while saving/loading the sheet (very important) The difficult job might be at the boundaries and when something may belong to the two areas. This can be solved, I guess, by assuming the criteria: For any ambiguity that a boundary crosses an element, the element is supposed to be inactive (Unreal) as if it doesn't exist as a whole. But I am afraid that the benefits for being able to work on the same screen having the above two spaces could be appreciated by those who are creating new designs only. Because this gives a great saving of time while studying alternatives during the design. It allows to use just the 'Move' function most of the time instead of erasing/adding everytime a change would be needed. May I add... that like, for example, the flags V and I are for 'Visible' and 'Invisible', another pair of flags as R and U for 'Real' and 'Unreal' may need to be added for each element to implement this feature. Hope I will live long enough to work on this magic sheet :) Kerim Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Footprint for a Relay ?
One trick I sometime use if I cannot find a datasheet, (rare as you can usually find one in the various suppliers catalogues.) is to use a piece of matrix board. Most leaded components are on a 0.1 inch grid (there are exceptions but there are not too many) You can then count the hole spacing. The footprint is just that, an outline of the component. The critical part is any pad or mounting hole requirements. Just treat the leads as normal component leads, but I would suggest that you make the pads fairly large as they need to support a much heavier component than something like an IC. Andy On Sat, 23 Jan 2010 05:07:25 -0800 (PST) yukku yukkoo yukku19752...@yahoo.com wrote: Hi, Thank you for the answer. That brings me to the question as to what to do if I do not have a data sheet for the part. Can I measure various lengths on the part and gaps between the pins and create my footprint ? What should be the minimum tolerance (in inches) to get a decent footprint ? Regards shyam From: Veronica Merryfield veronica.merryfi...@shaw.ca To: kicad-users@yahoogroups.com Sent: Sat, January 23, 2010 2:51:38 PM Subject: Re: [kicad-users] Footprint for a Relay ? It all depend what actual device the part was based on, but essentially it is as you say. Relay bases have a long history. Find the data sheet for the actual relay you are going to use and pick the footprint from that. My suspicion is that the device in the library is a DIL16 part so you would need a 16 pin DIL 0.3 footprint for the library device if you are using the same part that the library is created for. Datasheet time. On 2010-01-23, at 1:09 AM, yukku yukkoo wrote: Hi, I am using the Relay RELAY_2RT from the EEschema device library. I have a couple of question about it - 1. Why does it not use contiguous pin numbers instead using pins 1,3,5 8,9 and 12,14,16 ? My guess is it uses a standard package with missing pins to get double spacing. Please confirm. 2. What foot print should I use for it in cvpcb ? Regards yukku Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Footprint for a Relay ?
you have mail... andy On Sat, 23 Jan 2010 05:17:11 -0800 (PST) yukku yukkoo yukku19752...@yahoo.com wrote: Andy, Thank you. Please send me the schematic part as well as the foot prints. Regards yukku From: Andy Eskelson andyya...@g0poy.co.uk To: kicad-users@yahoogroups.com Sent: Sat, January 23, 2010 4:36:45 PM Subject: Re: [kicad-users] Footprint for a Relay ? Many relays have a standard numbering system, especially if they are intended to be plugged into some form of holder. there are some variations, but generally they are two digit such as 11, 12, 13, 21, 22, 23 and so on, the coils are normally A1 and A2. I have also seen some bases with a letter and a number as well. The numbers refer to the poles and contacts, so 11 is pole 1 contact 1, 12 is pole 1 contact 2, 21 is pole 2 contact 1 and so on. I can't remember offhand which is the normally closed/open and common connections, I usually end up buzzing it out to be sure :-) Miniature PCB mount relays tend to be a little more variable. As for footprint, well you use the footprint that matches the relay... (I cannot see one in the standard lib) I drew up a simple footprint the last time I used a relay. I've used this SPST 12V 10A directly soldered into the PCB http://www.rapidonl ine.com/searchre sults.aspx? style=0kw= 60-4600 and the 60-4110 Double pole socket http://www.rapidonline.com/Electronic-Components/Relays-Solenoids/PCB-Relays/Miniature-relay-sockets/28667/kw/60-4110 I have simple footprints for both, if they are of any use you are welcome to a copy. Andy On Sat, 23 Jan 2010 01:09:33 -0800 (PST) yukku yukkoo yukku19752000@ yahoo.com wrote: Hi, I am using the Relay RELAY_2RT from the EEschema device library. I have a couple of question about it - 1. Why does it not use contiguous pin numbers instead using pins 1,3,5 8,9 and 12,14,16 ? My guess is it uses a standard package with missing pins to get double spacing. Please confirm. 2. What foot print should I use for it in cvpcb ? Regards yukku
Re: [kicad-users] Re: Active and Inactive space
Ahh! a slightly different way of working I miss-understood what you were saying... You can move things about on and off the circuit area wherever you want, but that's all. While designing I don't use erc or bom, that all comes AFTER the design is done, when I delete all the leftover parts and check the connectivity. For odd bits of circuits I just keep them on separate sheets and cut and paste them between sheets as needed. i.e. I have a couple of standard 78xx type regulator circuits that I often use, so I drop them into the main design as needed. (I have a .sch page called circuit modules that I copy into each project for this purpose) Note that this is not a hierarchical sheet, just a standalone sheet. Andy On Sat, 23 Jan 2010 15:09:10 - h_manbeing h_manbe...@yahoo.com wrote: Thank you Andy for your reply. In my turn and if I understood well, your Kicad version of eeschema allows you to place components and perhaps uncomplete connections outside the main page without worrying about their wrong/missing annotation or the non connected pins... etc. Isn't what you mean? I run the last stable version of Kicad on Windows XP. Working on eeschema, whatever is found anywhere on the whole sheet, has the same importance as all other elements. So ERC check, netlist and BOM see the inside and the outside of the main page as one space in which everything should be done correctly in order to pass the check and generate good files. So to my knowledge, there is no area on the sheet that can be seen as equivalent to a trash can hence its contents are ignored by ERC and others. Kerim --- In kicad-users@yahoogroups.com, Andy Eskelson andyya...@... wrote: If I understand correctly what you are asking for, it's already there. Just add a range of components that you are using once. If you wish you can place them outside the drawing outline. Then right click on a component, select copy and place the copy wherever you need it. I generally don't bother adding components outside the drawing, if I've already used one I just copy it from where I placed the previous component. Andy On Sat, 23 Jan 2010 09:29:21 - h_manbeing h_manbe...@... wrote: Hi all, I wish someday the Kicad developpers will have the time to divide a sheet (as of eeschema for example) as two independent spaces: (1) The area inside the page limits, in which all components and connections are treated as usual so it can be called active or Real. (2) Outside the active space, in which all components and connections are just ignored as if they don't exist, so this area may be called inactive or Unreal. But these do exist while saving/loading the sheet (very important) The difficult job might be at the boundaries and when something may belong to the two areas. This can be solved, I guess, by assuming the criteria: For any ambiguity that a boundary crosses an element, the element is supposed to be inactive (Unreal) as if it doesn't exist as a whole. But I am afraid that the benefits for being able to work on the same screen having the above two spaces could be appreciated by those who are creating new designs only. Because this gives a great saving of time while studying alternatives during the design. It allows to use just the 'Move' function most of the time instead of erasing/adding everytime a change would be needed. May I add... that like, for example, the flags V and I are for 'Visible' and 'Invisible', another pair of flags as R and U for 'Real' and 'Unreal' may need to be added for each element to implement this feature. Hope I will live long enough to work on this magic sheet :) Kerim Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] How to make an isolated zone?
The latest stable version of Kicad is here: ftp://iut-tice.ujf-grenoble.fr/cao/ kicad-2009-02-16-final-UBUNTU_8.10.tgz You do not have to build it as it is a binary distribution, installation is simple process, read the install notes, and remember to check the permissions on the bin directory. There are nightly builds of the next release available if you want to look at them - (on a different site somewhere) From comments posted here a while ago the next version will be a beta release fairly soon. For the zones, when you select the zone icon then click on the board you should get a requester box that lists all the nets on your board. Rigth at the top of the list there is no net just select that and then create your zone. Andy On Fri, 22 Jan 2010 04:45:29 - do_you_trust_god do_you_trust_...@yahoo.com wrote: Help find a way to make zone which is not connected to any net. I found this discussion: http://www.mail-archive.com/kicad-users@yahoogroups.com/msg05485.html . Here say: Click on the zone tool A window pops up, select the net that you want the zone to attach to, or no net for isolated zones How to select no net when PCBNew automatically selects first net in list by default? I use PCBNew version 20080825c-final from Ubuntu's 9.04 reposistory. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Trimpots
If you mean modules rather than eeschema symbols then there are three in the standard Kicad mods. POT_CMS (a surface mount variant) and RV2 and RV2X4 which are the more standard type of trimmers. However if by trimpot you mean a multi turn type, then I've not see such a module, but as ther are a simple oblong with three pins, it's not exactly a hard mod to draw up. Do print out the footprint documentation, it's a pdf file in the docs folder, and it is also accessabol for CVpcb, third icon from right. display footprints list documentation It's a handy reference to have beside you when choosing the footprints. Andy On Fri, 22 Jan 2010 11:39:20 - foobar.foobar foobar.foo...@yahoo.com wrote: This may seem like a really stupid question but I seriously cannot find any trimpots in the library. I can find POT in the device section but I can't find a trimpot... are they called something else in kicad? Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Trimpots
Most groups do not allow attachments to messages. Instead members are asked to use the files and photo areas. Andy On Fri, 22 Jan 2010 18:09:40 +0100 Jean-Paul Gendner jean-paul.gend...@orange.fr wrote: Hi, There are many kind of trimpot. I have built one and would attach the files to a message, however this do not work. How may I send files to the group? Regards, Jean-Paul Jean-Paul Gendner 03.88.27.03.44 _ De : kicad-users@yahoogroups.com [mailto:kicad-us...@yahoogroups.com] De la part de foobar.foobar Envoyé : vendredi 22 janvier 2010 12:39 À : kicad-users@yahoogroups.com Objet : [kicad-users] Trimpots This may seem like a really stupid question but I seriously cannot find any trimpots in the library. I can find POT in the device section but I can't find a trimpot... are they called something else in kicad?
Re: [kicad-users] libs silkscreens unusable
Have you unticked the print pads on silkscreen option? ( plot menu lower left hand corner) Andy On Thu, 21 Jan 2010 11:03:07 +0100 Stephrac74 stephra...@wanadoo.fr wrote: Hi group, I’ve noticed that most of the library components have unusable silkscreens. Most of the time, the lib silkscreen shows the component itself with pads and so on instead of a simple square or so, and the silkscreen often covers the pads which is amazing ! This is not usable for PCB industrialization. I’ve decided to don’t use anymore the Kicad libs and to redesign all my needed components ! This is a major issue according to me and a major waste of time… I have no time anymore to change the software. Regarding the different limitations I’m facing for a professional use, I’m starting having regrets to have chosen Kicad … L This is a fantastic software, and free, but the 2% of missing details makes this software not usable for professional use according to me and requires a lot more time even for an amateur use than an other software. Hoping it will be improved, but last release is already 1 year ago and the wish list is so long that I have not added my comments. Best Stephane
Re: [kicad-users] libs silkscreens unusable
I understand, there is not really much that can be done about that apart from a reedit. The only thing I can suggest is to have a look at some other libs. If you have a look here: http://library.oshec.org/ There are 1000's of converted libs and mods, and looking at some of them the outlines do keep clear of the pads, (at least on the sides needed for solder on the dpacks I looked at as examples.) At the top of the page is a link to download the whole lot, about a 12Mb download. That might save you a bit of time. The above site is linked via http://www.kicadlib.org/ then via http://per.launay.free.fr/kicad/kicad_php/composant.php Both the kicadlib and Pierre Launay's sites are worth bookmarking Andy On Thu, 21 Jan 2010 14:18:25 +0100 Stephrac74 stephra...@wanadoo.fr wrote: Hi Andy, In fact this option only enables you to add or not the pads footprint on the silkscreen. The problem is different. The components silkscreens in libs are drawn on pads making soldering impossible. I do not see other option rather than making the modification on each concerned component. This is usually the problem when libs are made by contributors and not checked. The problem occurs for instance for Vishay electrolytic caps, SMD crystals, sot223, DPACK, etc… I’ve started 5 hours ago to modify all the components I’m using on this board and once modified, creating my own libs. In the same time I can arrange libs in a better way but the work is huge and I’ve not really the time to do that for that project… but no way… Stephane De : kicad-users@yahoogroups.com [mailto:kicad-us...@yahoogroups.com] De la part de Andy Eskelson Envoyé : jeudi 21 janvier 2010 12:30 À : kicad-users@yahoogroups.com Objet : Re: [kicad-users] libs silkscreens unusable Have you unticked the print pads on silkscreen option? ( plot menu lower left hand corner) Andy On Thu, 21 Jan 2010 11:03:07 +0100 Stephrac74 stephra...@wanadoo.fr mailto:stephrac74%40wanadoo.fr wrote: Hi group, I’ve noticed that most of the library components have unusable silkscreens. Most of the time, the lib silkscreen shows the component itself with pads and so on instead of a simple square or so, and the silkscreen often covers the pads which is amazing ! This is not usable for PCB industrialization. I’ve decided to don’t use anymore the Kicad libs and to redesign all my needed components ! This is a major issue according to me and a major waste of time… I have no time anymore to change the software. Regarding the different limitations I’m facing for a professional use, I’m starting having regrets to have chosen Kicad … L This is a fantastic software, and free, but the 2% of missing details makes this software not usable for professional use according to me and requires a lot more time even for an amateur use than an other software. Hoping it will be improved, but last release is already 1 year ago and the wish list is so long that I have not added my comments. Best Stephane --- Orange vous informe que cet e-mail a été contrôlé par l'anti-virus mail. Aucun virus connu à ce jour par nos services n'a été détecté.
Re: [kicad-users] Bill of Material : how to group all values in 1 line ?
You will find that the format you suggest will not import very easily into excel, it gets very messy. The problem is that you don't know how many of the components such as C1, C2 and so on there will be on any line. So the totals would not appear in the same col. (That might not matter to you) If you only want a total of each value such as 100nF 6 off then you can get that directly via excel from the standard lst file. Use excels pivot table function. First import the lst file into a worksheet, you should end up with two cols, ref and value Click on the first cell start the pivot table wizard, it should pick up the limits of the imported data click finish (let the wizard do the work) On the pivot table worksheet (will automatically pop up) drop ref into col fields drop val into row fields drop ref into data fields That will produce a grid with the totals at the end if you don't want to see the data and just get the totals drop rep into the page fields as well, and 6that will hide the data You can do quite a lot with the formatting and such like so it's worth having a play and working through the tutorials on pivot tables . There is of course a problem... You really need to include the footprint data as well, because the default output does not tell you what type of cap or resistor it is. You might have 47 ohm 1/8 watt Resistors, and a couple of 47 ohm 10 watt jobs in the project, likewise for caps, you may have 10V working, 50V and so on. For purchasing you need to know this. You may find that it's better to process the stuff file generated by Cvpcb to extract the additional data. You could also process the cmp file created by pcbnew. In either case it's prob a task better suited to access or a bit of programming than excel. Andy On Mon, 18 Jan 2010 08:53:12 +0100 Stephrac74 stephra...@wanadoo.fr wrote: Hi all, I’d like to generate the bill of material with the following format : ValueReferencesQuantity 100nF C1,C2,C8,C10 4 47Kohms R1, R2, R3 3 Instead of having 1 line per reference like : 100nF C1 100nF C2 100 nf C8 That would be easier to import the BOM and use it directly in excel for purchasing. Is there any way to do ? I don’t find the correct configuration Regards Stephane
Re: [kicad-users] Pcbnew : How to make components values invisible ?
Try: Preferences colours Untick Text Module Invisible and apply. Andy On Mon, 18 Jan 2010 14:23:28 +0100 Stephrac74 stephra...@wanadoo.fr wrote: Hi all How to make the value on the board invisible without making the modification on each component in lib ? I’d like to have only the reference and not the value… Thanks Stéphane
Re: [kicad-users] New to Kicad, questions about CVpcb, and completeness of default library
On Mon, 18 Jan 2010 15:54:43 - oniamien oniamien.angelf...@gmail.com wrote: Hi Welcome to Kicad. First do note that the tutorial is rather old, most of it still applies and you should go through it a few times just to get the hang of how to do things. You will find the tutorial in kicad/doc/tutorial/ Also, there are much more detailed help files included with the each kicad program, you can access these from the help menu or read them directly. They are all pdf files located in kicad/doc/... Do take the time to read the help files, there is a lot of useful info in them. It is down to you to check that the package and pins are correct. Most are. But as you get into various projects you will find the need to edit or create your own modules. The thing to remember is that the pin number on the component in eeschema will map to the same pin number on the module. However the pins can be in any physical location. I must admit that I've never come across the need to physically shift a pin number around, but I can think of a couple of packages I've used in the past where that might have been necessary. CVpcb does NOT know anything about different pin assignments, it's purely a program to allow you to assign modules to components, That's where YOU decide on what module to use. If you print out the footprint documentation you will find a set of drawings off all the included footprints. I think that is the file you are referring to. There is an icon to access this on the top toolbar on CVpcb, but like other documents, it is in the doc directory, again it's a pdf file. I have a printed copy beside me when selecting components, it's quite handy. For the components in the tutorial, they should be in the list...Ahh looks like a change in names happened sometime, try DIP-16_300 With the standard set, you will not find many filters. (The 7400 has a couple.) Components can come is all sorts of packages. The physical package will be defined somewhere on the datasheets, and there can be loads of them. It's down to the manaf. as to which ones they use. However they are fairly sensible most times...at least for the common components. Usually it's you as the circuit designer that determines which particular package to use. e.g. if you were making a very small device, using surface mount components, then you would choose the various SM packages, and not something like a dip 16 300 :-) So you would already know what packages to use. Andy Hi! I am new to Kicad and learning to use it for an independent study at college. I have been going through the Kicad mini tutorial on the wiki and I have looked at the FAQs, but I have been having some issues. 1. Considering that Kicad has you put down a diagram of the chip on the schematic first with out associating a chip package to it (i.e DIP or QFP) how do I know that when I set the association in CVpcb that the pins will be correct since pin numbers can change drastically between packages for the same component. The components you use in the schematics generally have the function of a pin and its number on them, but I don't see how CVpcb will know how to reassign them if you choose one package as opposed to another. In the tutorial it does say there is some file that can describe the associations, but it doesn't say what that file is. Any clarification on this subject would be appreciated. 2. I downloaded the version of Kicad that is supposed to have libraries, docs, etc., already loaded in it, but I seem to be missing some things from my installation. For example, in the mini tutorial you need a to use the 16dip300 footprint, but this is not in my list of footprints in CVPCB. Furthermore, it says that you can narrow down the available options by selecting filter footprints, but not one component I have looked at has had any filters on it. In other words, for every component I have tried from the preinstalled library, the filtered list is exactly as long as the unfiltered list. Was there a different package I was supposed to download? I downloaded KiCad-2009-02-16-final-WinXP_full_with_components_doc_autoinstall.zip from http://iut-tice.ujf-grenoble.fr/cao/ If this is not the version with complete files then please let me know, or if it should have worked I would appreciate any advice about what might have went wrong. 3. Also, on the subject of narrowing down footprints to use, I wanted to know how I would figure out what footprint a chip had if the library did not include a list of options, or if I wanted to make a new library myself. Some information is obvious, like if a chip has 16 pins and is a DIP than that is easy to figure out. But, using the example I asked about previously, how would I know to use the 16dipâ€_300â€_ footprint? It may be the case that that particular question is moot if that is the only kind of package (i.e. there is no “400â€_) but what I would like to
Re: [kicad-users] NPN footprint
Print out the component sheets from CVpcb 3rd icon from right on top icon bar (Display footprint list documentation) On the first sheet descrete1, there are a dozen options, and a similar number on the SMD sheet You use whichever package your device uses. Do be aware that there are variations withing the package styles e.g. in TO92 the outlines show the pads in a triangular format, however some devices are pinned in line. Of course the in line pins can fit the triangular pattern, but this may not suit your needs. In which case you would need to create a new outline. (easily done by copying and modifying the TO92 one. Andy On Sat, 16 Jan 2010 14:26:45 -0800 rocko sunblast...@gmail.com wrote: Whats a good footprint for a NPN transistor for PCBnew ? I looked thru the docs but couldn't really find one. I suppose I could use any 3 pad footprint, but I want to use a correct one Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] power pin not driven??
Power flags do not say that there is a specific type/value of power available, they just say that the net that they are connected to is connected to power of some sort. Andy On Sat, 16 Jan 2010 16:40:39 -0800 rocko sunblast...@gmail.com wrote: Ok, thanks On Sat, 2010-01-16 at 18:38 -0600, Patrick Maupin wrote: ground IS power. So just use the same power flag :-) On Sat, Jan 16, 2010 at 6:29 PM, rocko sunblast...@gmail.com wrote: [Attachment(s) from rocko included below] The erc test keeps saying the last resistor (R13), which goes to GND is Not driven in Is there a special GND flag like the Power Flag that i can use to get rid of this? Schematic attached as Post Script file. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] problem in eeschema
On Wed, 13 Jan 2010 20:42:09 -0800 That usually means one of two things. 1. The device is expecting something to be connected to that pin, and there is nothing there. i.e. it.s an I/O pin which you are not using. If that is the case put a no connection X on it. 2. You have a mismatch in grid sizes between your drawing and the part. In order for a connection to be made, the wires and the part pins MUST be on the same grid intersection. Sometimes, esp. if you create your own part and get the grid spacing wrong, the two will not align. (The standard kicad libs should be OK) The cure is to either change the part, or the grid. setting the grid to the smallest possible, then zooming in may show you the problem. Andy Geoffrey Reed treg...@gmail.com wrote: It is always the same error :( ErrType(2): Pin not connected (and no connect symbol found on this pin) @ (3.0500 ,4.2500 ): Cmp P1, Pin 28 (passive) Unconnected Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] problem in eeschema
The output from ERC will tell you what the error is and where. So that should give a few clues as to what is going on. I must admit that I don't like your comment that things change when you have not moved anything. The two main problems in eescgema is making sure that you have junctions at the connection points where needed, and that the power nets are correct, and have power flags if required. Andy On Wed, 13 Jan 2010 01:50:45 - G.Dragon treg...@gmail.com wrote: I have been having trouble in eeschema, even though i have connected all the pins on a connector, some of them fail ERC, and occasionally some that pass ERC fail ERC later, even though I have not moved anything. I am primarily working on a mac pro under mac OSX, but i am getting the same behavior under windows. Please read the Kicad FAQ in the group files section before posting your question. Please post your bug reports here. They will be picked up by the creator of Kicad. Please visit http://www.kicadlib.org for details of how to contribute your symbols/modules to the kicad library. For building Kicad from source and other development questions visit the kicad-devel group at http://groups.yahoo.com/group/kicad-develYahoo! Groups Links
Re: [kicad-users] Kicad and making home made PCBs
Select the small drill point option in the plot requester, and then plot as POSTSCRIPT. For some reason when using normal printing the drill size always seems to be the actual drill size rather than just a small point. Gerber files will have a filled in pad, as that is what is required by PCB houses. I then display and print the postscript files using the Evince utility (SUSE 11.1 Linux) Andy On Mon, 11 Jan 2010 20:03:23 -0800 (PST) yukku yukkoo yukku19752...@yahoo.com wrote: Hi, I am interested iu making home made PCBs and a web site mentions its a a nice feature to have a small hole in the middle of the the filled circle (at the end of a track) so a home made drill can be accurately used to drill a hole into the PCB right in the centre. I saw Kicad does not provide holes in the middle of the PCB at the component position. Can I force Kicad to do this using some option ? Yukku
Re: [kicad-users] Tool for library management
Have you found the pdf file of the standard module library, and seen the suggested method of maintaining your own libs by creating a dummy board layout (section 11.10 in the pcbnew help file) I find that works better than trying to browse through things on screen as it gives me a better idea as to sizes. andy On Tue, 12 Jan 2010 16:02:33 +0100 Stephrac74 stephra...@wanadoo.fr wrote: Hi there, Do you know a tool in order to manage the libs easily under Windows ? I’ve tested the Vermod, Mod2mod, Verlibr and Lib2lib which unfortunately are in Portugese or so and do not accept the converted libs. Until now in order to find a component or footprint, the only way I’ve founded is to add manually the libs and to browse thru the lib editor or add component tool…. That’s definitely not efficient ! Thanks Stephane
Re: [kicad-users] Tool for library management
Hi Stephane, That is sort of what the system does. Dump the modules onto a page, and get rid of the modules you don't want. (or move them to other pages) Then you can use: file archive footprints create footprint archive which will create a new footprint library for you, from the modules on the page. As time progresses you can add modules to the page when you need to, then regenerate the library again. This means that the page with the footprints on them becomes the main library source. I admit that is seems an odd method to use, but it is pretty easy, and you automatically get some documentation to print out if needed. Andy On Tue, 12 Jan 2010 22:55:57 +0100 Stephrac74 stephra...@wanadoo.fr wrote: Hi Andy, Yes I’ve seen this method but regarding the number of components in lib, I guess this method would not suit in my case… My aim is to pick up some components I’m usually using from other libs and copy into my own lib. Thus I would be able to organize my libs as I think they should be… I’m really surprised that there isn’t any tool which ease the lib management (display, copy, erase, …) That’s really a needed feature. Best Stephane De : kicad-users@yahoogroups.com [mailto:kicad-us...@yahoogroups.com] De la part de Andy Eskelson Envoyé : mardi 12 janvier 2010 22:49 À : kicad-users@yahoogroups.com Objet : Re: [kicad-users] Tool for library management Have you found the pdf file of the standard module library, and seen the suggested method of maintaining your own libs by creating a dummy board layout (section 11.10 in the pcbnew help file) I find that works better than trying to browse through things on screen as it gives me a better idea as to sizes. andy On Tue, 12 Jan 2010 16:02:33 +0100 Stephrac74 stephra...@wanadoo.fr mailto:stephrac74%40wanadoo.fr wrote: Hi there, Do you know a tool in order to manage the libs easily under Windows ? I’ve tested the Vermod, Mod2mod, Verlibr and Lib2lib which unfortunately are in Portugese or so and do not accept the converted libs. Until now in order to find a component or footprint, the only way I’ve founded is to add manually the libs and to browse thru the lib editor or add component tool…. That’s definitely not efficient ! Thanks Stephane --- Orange vous informe que cet e-mail a été contrôlé par l'anti-virus mail. Aucun virus connu à ce jour par nos services n'a été détecté.
