Re: [kicad-users] Module Library madness
metric (remind me to once again curse the creeps that stopped metrication back in the '60s). Can I join you? The current lib lists these as SM0603 in imperial.. I'm thinking of creating a metric named lib with 0603M? Curiously I was thinking about this the other day, and came to the conclusion the metric names should start with M (eg M0603), to echo bolt naming (M3, M3.5 etc). Regards, Robert. No virus found in this outgoing message. Checked by AVG - www.avg.com Version: 9.0.819 / Virus Database: 271.1.1/2867 - Release Date: 05/11/10 07:26:00
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
[kicad-users] Re: Module Library madness
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. That's not the reason, with its 1/10mil resolution pcbnew has no problem handling metric modules (well, maybe until you need chip bonding, at least :D) The metric/imperial usage with passives is mostly a cultural one in the industry and varies from country to country... For example, here in Italy when we talk about common capacitor/resistors we usually use the imperial units (0603 being the most common AMT). Tantalium are referred as metric (or with case letter coding) and for inductors... well, smaller one are imperial but bigger one are referred as metric... also electrolytic are referred using the panasonic case names and tank/choke inductors using the S/M/L/XL size from wurth! So, at the end, everyone make its own standard... The IPC standard naming is IMHO unwieldy, too complex to use in the usual cases! (and, anyway, remember that there are around a dozen or so of SOT-23 variants, too!)
[kicad-users] Re: 3 PCBs, 1 design
Is there any way to force KiCAD to make a PCB of a single schematic sheet, even when buried within a larger hierarchical design? I had a similar issue with a sandwitch-board (i.e. two pcb mounted with risers). The trick is to use a single pcb file with all your boards drawn into it and declare the joining points (connectors, risers, whatever) as modules (like the CONN_ parts). Of course you have to manage manually the pinouts of these connectors to make them match! It is actually easier to build them later since you only have to submit *one* gerber/PnP set instead of three! You could also ask the manufacturer about how he would like the board aligned to ease panelisation and where to put scoring/rat-bites indications (but, anyway, they will have no trouble separating three boards from the same gerber set).
[kicad-users] Re: Placing lines by coordinates
In pcbnew, you can edit a line segment (for example, part of the board outline) and type in or change the endpoints. Is there any way to do this in the module editor? That would make it easier to draw silkscreen outlines or keepout areas. Sorry, IIRC this isn't possible ATM. You should make a feature request for that.
[kicad-users] Re: Auto pin pitch
I'm editing a module and I want to change the space between each pin automatically. How is it done? There is no way to do that... Many people use scripts to generate automatically .emp files with the desired pitch and size, but manually you have to move them one at a time (a custom grid helps a lot)
[kicad-users] Re: Trouble when creating module library using auxiliary board approach
--- In kicad-users@yahoogroups.com, andy_7945 hvbry...@... wrote: This is all okay, as I can use a revised approach by creating the library first, then inserting each module into the auxiliary board one by one after the fact. But this is not how the documentation says to do it. This causes me to believe that I'm somehow missing some important detail of how to specify the module name when using the above described procedure (Load module from lib, edit the module, change its reference field, then Insert module into current board). If so, how can I specify a new name for the module? Sorry but IMHO that's a bug. There is an hidden *footprint name* which is set during the creation but isn't editable anywere (if it isn't I haven't found it). IIRC it's the 'Li' field in the library... The only solution I can think about is to hand editing the component/board file (a search replace with the old name does the trick)
[kicad-users] Re: Gerber files
I'm having trouble converting the gerber code ( copper and component layers ) where the gcam software just dies in the KiCad code. Similar sized card with Eagle goes ok but there is a difference with the gerber code from KiCad. I suppose you're doing milling isolation and not photo processing, then. I never had trouble with kicad gerbers, I'd think about a bug in gcam... If you can you could eventually submit a bug report for pcbnew with the failing gerber to let us look at it, to see if it's defective.
Re: [kicad-users] Re: Module Library madness
Lorenzo wrote: The IPC standard naming is IMHO unwieldy, too complex to use in the usual cases! (and, anyway, remember that there are around a dozen or so of SOT-23 variants, too!) You can tell IPC standards was written by engineers that haven't done real life design work -- some of the text sounds like it was written by lawyers yuck. Anyway - the problem is there really isn't one pad size for an 0805 that works - there are variants for density vs reliability trade offs and to really optimize the pad you need to consider the thickness of the part. (should the 0805 (2012 Metric) be called a 201250 Metric?) I found this: http://www.xs4all.nl/~ljh4timm/pcb-fpw/pcb-fpw.html It would be cool if someone tweaked pcb-fpw to to produce kicad footprint libraries.. 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 Gumption is 99% of success. kps
Re: [kicad-users] Re: Module Library madness
Lorenzo wrote: You can tell IPC standards was written by engineers that haven't done real life design work -- some of the text sounds like it was written by lawyers yuck. You actually have found the specs or have you paid for them? I'd love to see the rationale for some of their formulas (like SOIC pads that sometimes are round and sometimes are squareds) You can find the specs via google A key to seeing what they are up to is in the ipc software that I posted the link to yesterday.. Anyway - the problem is there really isn't one pad size for an 0805 that works - there are variants for density vs reliability trade offs and to really optimize the pad you need to consider the thickness of the part. (should the 0805 (2012 Metric) be called a 201250 Metric?) Not only that, there are other technological constraint. Like when you work on 70um copper or you do a board to be conformal-coated, the pads' shapes change a little... I found this: http://www.xs4all.nl/~ljh4timm/pcb-fpw/pcb-fpw.html It would be cool if someone tweaked pcb-fpw to to produce kicad footprint libraries.. I could give it a look. I've already done some library generation, kicad format is actually trivial... pcb-fpw is sort of an opensource version of http://landpatterns.ipc.org/files/PCBM_LP_Calculator_V2009-0831.zip All of it is for supporting IPC-7351. pcb-fpw was written to support the competing opensource 'pcb' package - might work to have a script to translate the modules? pcb-fpw is open source, so it would be possible to modify add it to the kicad suite .. seems to be written in java-bloat.. The separate names for a cap and resistor 0805 package is silly - I could see building a library with 080505 to specify the thickness for out of the ordinary parts. I could also see having three libraries - as the SNM7351B SNL7351B SMN7351B. (I found a thermistor that is thin and matches the thickness of the SM MOSFETS so it it touches the heatsink).. The M,N,and L are for most, Nominal and least -- describes most compromises folks would run into.. I'm also making my modules with different silk screen and a part outline on the drawing level. There are also custom case numbers that should probably be organized via part vendor. One thing to point out is these case sizes originate in metric - the imperial notation is approximate. 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
[kicad-users] Re: Module Library madness
pcb-fpw is open source, so it would be possible to modify add it to the kicad suite .. seems to be written in java-bloat.. No, it's buggy plain C with GTK :P It actually contains a lot of hardwired size, too:P The separate names for a cap and resistor 0805 package is silly Actually it isn't... a ceramic cap has round plating, a chip resistor is an attached foil... I presume the mechanical properties are different (indeed the pads are different, too) The M,N,and L are for most, Nominal and least -- describes most compromises folks would run into.. You forgot Proportional for THT, too... and the Nominal one is good for 90% of the production projects, IMHO... One thing to point out is these case sizes originate in metric - the imperial notation is approximate. *Most* case size originate in metric:D
R: [kicad-users] Re: Module Library madness
For Cases, pads, etc., you can also refere to: New Surface Mount Design and Land Pattern Standard The official text for device farms. ciao Carlo, I2GOQ --- Mer 12/5/10, Lorenzo lomar...@tin.it ha scritto: Da: Lorenzo lomar...@tin.it Oggetto: [kicad-users] Re: Module Library madness A: kicad-users@yahoogroups.com Data: Mercoledì 12 maggio 2010, 18:19 pcb-fpw is open source, so it would be possible to modify add it to the kicad suite .. seems to be written in java-bloat.. No, it's buggy plain C with GTK :P It actually contains a lot of hardwired size, too:P The separate names for a cap and resistor 0805 package is silly Actually it isn't... a ceramic cap has round plating, a chip resistor is an attached foil... I presume the mechanical properties are different (indeed the pads are different, too) The M,N,and L are for most, Nominal and least -- describes most compromises folks would run into.. You forgot Proportional for THT, too... and the Nominal one is good for 90% of the production projects, IMHO... One thing to point out is these case sizes originate in metric - the imperial notation is approximate. *Most* case size originate in metric:D
Re: [kicad-users] Re: Module Library madness
Lorenzo wrote: The separate names for a cap and resistor 0805 package is silly Actually it isn't... a ceramic cap has round plating, a chip resistor is an attached foil... I presume the mechanical properties are different (indeed the pads are different, too) ?? not the parts I looked at - they are different depending on thickness CAPC0603x33N and RESC0603x33N have the exact same land pattern.. 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 The government consists of a gang of men exactly like you and me. They have, taking one with another, no special talent for the business of government; they have only a talent for getting and holding office. Their principal device to that end is to search out groups who pant and pine for something they can't get and to promise to give it to them. Nine times out of ten that promise is worth nothing. The tenth time is made good by looting A to satisfy B. In other words, government is a broker in pillage, and every election is sort of an advance auction sale of stolen goods. -- H.L. Mencken
