Re: [kicad-users] dismembering relays in eeschema
Hi, Let's say your ralay has 5 pins, and 1 and 2 are the coil. Make pins 1 and 2 to be part A. make pins 3,4,5 to be part B. When using, the component, you can place part A and part B wherever you need in your design: I have place part A in a sub-sheet and part B in a different sub-sheet. You only need to tell eeschema that both parts belong to the same component by given them the same number. regards, Pedro. Hello, In the schematic tool, is it possible to create a relay such that the coil and each of the contact sets is a separate object? For instance, I have a DPDT relay and I want to place one set of contacts in one place, the other set of contacts someplace else and the coil in yet another place. (This, of course, could be extended to any number of poles). I've fooled with eeschema's library tool a little bit and while I can make the contacts as distinct sub-parts I can't do the coil or vice-versa. And yes, I did uncheck the common parts box. Alternatively, is it possible to do something like this: create a contact part and a coil part (as distinct parts). Place the coil and however many contacts I need and somehow combine the coil and the contacts into one physical part? Any ideas? TIA, eric
[kicad-users] Re: PLEASE help....Anyone out there???
--- In kicad-users@yahoogroups.com, kajdas kaj...@... wrote: But you always need to have the vias/nodes connected with traces first. Not with the most recent release. If a net is first selected when laying out a zone then the fill will add connections (using thermals) to pads that are part of that net. The resulting connections will (mostly) pass DRC so they are truly seen as connected. Zone fill is not 100% perfect -- some pads that appear to be connected may still show on the DRC as unconnected (not sure why), and I've had some 1-pin mounting holes become overlaid with the zone -- but it's much smarter than it used to be. One footnote. If a pad needs very narrow traces, such as a connection to a fine-pitch QFP, one may still need to make a manual connection with an appropriate narrow track if the track width that the zone uses is so wide that it can't get to the pad.
[kicad-users] Re: PLEASE help....Anyone out there???
--- In kicad-users@yahoogroups.com, Greg Dyess gregory.dy...@... wrote: I will try autorouting and tell it the layer pair is my component layer and the VSS layer and do an autoroute. You are wasting your time with the autorouter. The term the autorouter, is ambiguous since Kicad can work either with its internal autorouter or with freerouting.net's autorouter. My statement assumes the former. I think the internal autorouter has fallen into largely disuse, and there is no way it will ever catch up with the power and capability of the freerouter found at freerouting.net. But a simple search of this list would have told you that. Use the search feature of this mailing list please. Use freerouter, and do not autoroute, but manual route with it: 1) Place your components while in pcbnew. 2) In pcbnew, put in the zone perimeters and make sure their netcodes are correct, i.e. that they are tied to the correct net. You do not have to fill yet. 3) Export to DSN, and load the *.DSN file into freerouter. Learn it, it may take you a day. Feel free to search this list about it, and get support from their forum. 4) Manually route your board in freerouter. This is the only way you will have net specific control over the width of traces. 5) In freerouter, save a session file, as *.ses. Back import the session file into PCBNEW. Repeat steps 2 through 5 until you are happy. 6) Export to DSN one last time. Load design into freerouter. 7) check clearance violations and fix them. The clearance tolerances that freerouter uses come from your *.brd file and are established in pcbnew under the Dimensions menu choice. 8) back import one last time into PCBNEW. 6) Fill or re-fill your zones in pcbnew. 7) Run DRC check in pcbnew. 8) Export to gerber. Always do the fill in pcbnew near the end. You can view the DSN file and understand the nets, and copper areas. It can be a way to trouble shoot the kicad *.brd file in essence, in a more human readable form, one that is well documented. HTH, Dick
Re: [kicad-users] Re: PLEASE help....Anyone out there???
Thanks for the advice. I've been trying both the built-in autorouer and the freerouter. Both seem to just ignore my zone for some reason, except with DIPs. The freerouter also has trouble paying attention to the actual edges of the PCB and has a distorted shape. It looks as though hand-routing is the suggested method here. That's just a lot of routes to do with a 100-pin processor, 4 ASICs at 44 pins, and a few other components at over 40 pins each. Oh well, it will save me from having to figure out how to fully specify all my keepouts, which the internal autorouter seems to not understand anyways. Thanks for everyone's help. Greg From: Dick H. d...@softplc.com To: kicad-users@yahoogroups.com Sent: Monday, June 15, 2009 9:25:28 AM Subject: [kicad-users] Re: PLEASE helpAnyone out there??? --- In kicad-users@yahoogroups.com, Greg Dyess gregory.dy...@... wrote: I will try autorouting and tell it the layer pair is my component layer and the VSS layer and do an autoroute. You are wasting your time with the autorouter. The term the autorouter, is ambiguous since Kicad can work either with its internal autorouter or with freerouting.net's autorouter. My statement assumes the former. I think the internal autorouter has fallen into largely disuse, and there is no way it will ever catch up with the power and capability of the freerouter found at freerouting.net. But a simple search of this list would have told you that. Use the search feature of this mailing list please. Use freerouter, and do not autoroute, but manual route with it: 1) Place your components while in pcbnew. 2) In pcbnew, put in the zone perimeters and make sure their netcodes are correct, i.e. that they are tied to the correct net. You do not have to fill yet. 3) Export to DSN, and load the *.DSN file into freerouter. Learn it, it may take you a day. Feel free to search this list about it, and get support from their forum. 4) Manually route your board in freerouter. This is the only way you will have net specific control over the width of traces. 5) In freerouter, save a session file, as *.ses. Back import the session file into PCBNEW. Repeat steps 2 through 5 until you are happy. 6) Export to DSN one last time. Load design into freerouter. 7) check clearance violations and fix them. The clearance tolerances that freerouter uses come from your *.brd file and are established in pcbnew under the Dimensions menu choice. 8) back import one last time into PCBNEW. 6) Fill or re-fill your zones in pcbnew. 7) Run DRC check in pcbnew. 8) Export to gerber. Always do the fill in pcbnew near the end. You can view the DSN file and understand the nets, and copper areas. It can be a way to trouble shoot the kicad *.brd file in essence, in a more human readable form, one that is well documented. HTH, 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] PLEASE help....Anyone out there???
Someone wrote today that the latest version works with zones but not perfectly. I thought I am using the latest version but I am still using traces before filling the zones, so I did not test that. As to your question, you getting the idea but you need the second half explained. Once you connect your pad to a via, then on your VSS plane you continue your track to any other track in the same VSS node or to the VSS via in you power supply. Just like you would on any other plane. You basically have to have tracks to every via in your VSS plane connected with tracks. Once you have everything connected, you fill the plane/zone and the tracks get overlaid by the zone and appear as one single plane. Martin On Mon, Jun 15, 2009 at 7:57 AM , Greg Dyess wrote: I will agree with your assessment that I probably don't understand the way zones work. I was thinking of a zone as one huge trace that could be tapped. This is how the DIPs appear to work. The PCBnew just connects them to the layer without anything else having to be done. If I understand what you are suggesting, to connect the VSS and VDD pads of my surface mount chips I must start a trace from the pad and then create a via to the layer where my VSS or VDD zone will eventually reside and then ??? OK, I am lost now. I will play around with what you suggest and see if it becomes clearer. Thanks again, Greg From: kajdas kaj...@cox.net To: kicad-users@yahoogroups.com Cc: Greg Dyess gregory.dy...@yahoo.com Sent: Sunday, June 14, 2009 11:02:38 PM Subject: Re: [kicad-users] PLEASE helpAnyone out there??? I think you do not understand how Kicad works with the zones. You cannot connect to the zones directly. First, you have to lay your traces, even for the internal layers, (VSS, VCC, GND, etc.), connect all your vias to the internal nodes and traces, and after you are done, you mark your zones and fill them. When you fill them, you specify which node they connect to and then Kicad fills the properly by adding spaces for the non-connected vias and adding connections to the connected ones. But you always need to have the vias/nodes connected with traces first. Martin Greg Dyess gregory.dy...@yahoo.com wrote: OK, I am confused a little.. I understand your point that the VSS layer is not in the routing pair and perhaps that is the real problem. It would be nice if the autorouter understood connecting to underlying zones. I will try autorouting and tell it the layer pair is my component layer and the VSS layer and do an autoroute. Then try the same with the component to VDD/VCC3/... layer.
[kicad-users] Re: dismembering relays in eeschema
Pedro (or anyone else), Here's what I did: In eeschema, start up the library editor and select New Component. Select the appropriate number of Parts per Component (three in this case because I was doing a DPDT relay). Draw part A (the coil). A rectangular box w/ two leads. The Common to Units box is unchecked for all objects. Draw part B (contact block). Now here, for some reason, the two leads from part A have migrated to part B. (Just the leads, not the rectangle, so I have two pins on an otherwise blank sheet.) If I try to clear these leads on part B they are also cleared on part A. When I put the three leads on part B they migrate to part A. (Note the Common to Units box is still unchecked.) Is this a bug or am I doing something wrong? Am I taking the wrong approach? BTW I'm using ver. 20090216-final on XP. Thanks, eric --- In kicad-users@yahoogroups.com, Pedro Martin pki...@... wrote: Hi, Let's say your ralay has 5 pins, and 1 and 2 are the coil. Make pins 1 and 2 to be part A. make pins 3,4,5 to be part B. When using, the component, you can place part A and part B wherever you need in your design: I have place part A in a sub-sheet and part B in a different sub-sheet. You only need to tell eeschema that both parts belong to the same component by given them the same number. regards, Pedro.
Re: [kicad-users] Re: dismembering relays in eeschema
Hi, I have found what you need. On the top bar, the last icon on the rigth, edit pins part per part, solves your problem. Pedro. Pedro (or anyone else), Here's what I did: In eeschema, start up the library editor and select New Component. Select the appropriate number of Parts per Component (three in this case because I was doing a DPDT relay). Draw part A (the coil). A rectangular box w/ two leads. The Common to Units box is unchecked for all objects. Draw part B (contact block). Now here, for some reason, the two leads from part A have migrated to part B. (Just the leads, not the rectangle, so I have two pins on an otherwise blank sheet.) If I try to clear these leads on part B they are also cleared on part A. When I put the three leads on part B they migrate to part A. (Note the Common to Units box is still unchecked.) Is this a bug or am I doing something wrong? Am I taking the wrong approach? BTW I'm using ver. 20090216-final on XP. Thanks, eric --- In kicad-users@yahoogroups.com, Pedro Martin pki...@... wrote: Hi, Let's say your ralay has 5 pins, and 1 and 2 are the coil. Make pins 1 and 2 to be part A. make pins 3,4,5 to be part B. When using, the component, you can place part A and part B wherever you need in your design: I have place part A in a sub-sheet and part B in a different sub-sheet. You only need to tell eeschema that both parts belong to the same component by given them the same number. regards, Pedro.
[kicad-users] Re: Autorouting outside the board
--- In kicad-users@yahoogroups.com, gregory.dyess gregory.dy...@... wrote: I have run across a strange problem. I am very much open to chair-keyboard interface being the problem. I have a board that has two adjacent edge connectors separated by about an inch. These two connectors are tied together in the schematic. I have run across a couple of problems: 1. When I run the autorouter, it routes the traces completely outside the edges of the board! I *THINK* I have the PCB edges set properly and it appears to be correct, but it still routes traces off the board. Any ideas why this could be happening?? 2. The module editor insists on creating the attachment point in the center of the connector instead of at one end. Is there a setting to indicate that the trace connection should be at the inboard end of the finger instead of the middle? Thanks, Greg This may not be a solution but a workaround for you. Have you tried to manually route the two connectors together and then autoroute the rest of your pcb board.
[kicad-users] Display PCB Board with real dimensions
Sorry if this has been asked before. Using Kicad Build: (20080825c-final) on Ubuntu 9.04 I'd like to print out single sided PCB's on a printer at the actual size. When displaying an image on screen or printing, the physical size of components do not match the real life sizes. From the pcb editor (PCB New) if I press (print screen) and capture the image of a copper track PCB, what zoom level will create an actual 1:1 image? Sorry if my questions not clear, thanks in advance.
RE: [kicad-users] Display PCB Board with real dimensions
I do not have a linux version in front of me but for Windows, you go to File/Print and select 'Accurate Scale 1' and which layer you want to print. You do not want to capture screen. Martin On Mon, Jun 15, 2009 at 10:23 AM , hal8000b wrote: Sorry if this has been asked before. Using Kicad Build: (20080825c-final) on Ubuntu 9.04 I'd like to print out single sided PCB's on a printer at the actual size. When displaying an image on screen or printing, the physical size of components do not match the real life sizes. From the pcb editor (PCB New) if I press (print screen) and capture the image of a copper track PCB, what zoom level will create an actual 1:1 image? Sorry if my questions not clear, thanks in advance.
Re: [kicad-users] Exclude edges in gerber file or not?
Once I made a board with the board layer on... there was a copper track surounding all the board, wich of course amounted to many shorts between nets :) Alain Mouette Andres Cimmarusti escreveu: Hi, I have my board ready to print it as a gerber file to send it to the manufacturer, but I don't know if I should have the option exclude edged pcb checked or not. I want the borders of my pcb to be connected to my grounding plane...so what should this option be? Also, should I include the edges layer in the layers to be printed as gerber files? it not done by default, but it worries me. 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: dismembering relays in eeschema
I had somethign very similar to that happen on an IC I created. What I finally had to do was to hand-edit the text file to remove the duplicated parts. After that, I could edit the part to complete the fine touches. On a side note, are these formats documented anywhere? I figured out enough to hand edit it to get the duplicated parts. Greg From: einazaki668 einazaki...@yahoo.com To: kicad-users@yahoogroups.com Sent: Monday, June 15, 2009 11:25:33 AM Subject: [kicad-users] Re: dismembering relays in eeschema Pedro (or anyone else), Here's what I did: In eeschema, start up the library editor and select New Component. Select the appropriate number of Parts per Component (three in this case because I was doing a DPDT relay). Draw part A (the coil). A rectangular box w/ two leads. The Common to Units box is unchecked for all objects. Draw part B (contact block). Now here, for some reason, the two leads from part A have migrated to part B. (Just the leads, not the rectangle, so I have two pins on an otherwise blank sheet.) If I try to clear these leads on part B they are also cleared on part A. When I put the three leads on part B they migrate to part A. (Note the Common to Units box is still unchecked.) Is this a bug or am I doing something wrong? Am I taking the wrong approach? BTW I'm using ver. 20090216-final on XP. Thanks, eric --- In kicad-users@yahoogroups.com, Pedro Martin pki...@... wrote: Hi, Let's say your ralay has 5 pins, and 1 and 2 are the coil. Make pins 1 and 2 to be part A. make pins 3,4,5 to be part B. When using, the component, you can place part A and part B wherever you need in your design: I have place part A in a sub-sheet and part B in a different sub-sheet. You only need to tell eeschema that both parts belong to the same component by given them the same number. regards, Pedro. 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] Re: dismembering relays in eeschema
Pedro, Indeed you have and indeed it does, thanks! Not that it would've changed the outcome, but when the Libedit window first opens it looks like its default size is such that the Edit pins... button is obscured. A minor bit of bitching: When placing a multi-part part, it seems that when in the library browser window you can choose any of the alternate parts (A, B, C, etc.) but the A part is always the one that gets placed and you then have to Right-Mouse-Edit Component- Unit to get to the actual part that you want. Seems unnecessarily convoluted seeing as you can choose a subpart in the browser. Unless I'm not doing it right. Anyway, thanks again Pedro. eric --- In kicad-users@yahoogroups.com, Pedro Martin pki...@... wrote: Hi, I have found what you need. On the top bar, the last icon on the rigth, edit pins part per part, solves your problem. Pedro.
[kicad-users] Re: dismembering relays in eeschema
Too late now, but I think, based on my experience with my relay thing, You should be able to do what you wanted entirely within Kicad although you may have to read the docs very very carefully. (Maybe not even then, but Kicad certainly does seem to have the capability). eric --- In kicad-users@yahoogroups.com, Greg Dyess gregory.dy...@... wrote: I had somethign very similar to that happen on an IC I created. What I finally had to do was to hand-edit the text file to remove the duplicated parts. After that, I could edit the part to complete the fine touches. On a side note, are these formats documented anywhere? I figured out enough to hand edit it to get the duplicated parts. Greg
