Re: gEDA-user: import schematics with local footprints
Kai-Martin Knaak k...@lilalaser.de writes: Ethan Swint wrote: I've got the line (component-library-search /../../footprints) in my gafrc file. Does that set a priority? I just double checked. This setting does not seem to affect the choice of footprints in any way. Correct. The term components in the context of gafrc exclusively refers to symbols. (Why is the parameter not called symbol-search-path?) I don't know the reason, but let's make one up: because the entries in the file format are called component entries and begin with the letter C. It's not like it can be changed now anyway. For gsch2cb the path to the footprint lib is set by the parameter --elements-dir on the command line, or in a project file. (Why isn't it --footprint-dir?) Because the PCB file format calls them elements? Peter -- Peter Brett pe...@peter-b.co.uk Remote Sensing Research Group Surrey Space Centre pgpxpTFSnAQC5.pgp Description: PGP signature ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
For gsch2cb the path to the footprint lib is set by the parameter --elements-dir on the command line, or in a project file. (Why isn't it --footprint-dir?) Because the PCB file format calls them elements? PCB calls them footprints *before* they're put on the board, and elements *after*. --footprint-dir would be more appropriate. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
DJ Delorie wrote: If you're using File-Import, gnetlist is not looking at the libraries at all. Only PCB is, so you just need to teach PCB how to prefer your libraries over the system ones. My library string in preferences does not mention the default libs at all. It currently reads: ~/geda/footprints:./packages:. So how would I teach PCB to prefer them? Besides, my aim is not only prefer my libs, but use them exclusively. ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de Öffentlicher PGP-Schlüssel: http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
On 06/06/2011 08:25 PM, Kai-Martin Knaak wrote: DJ Delorie wrote: If you're using File-Import, gnetlist is not looking at the libraries at all. Only PCB is, so you just need to teach PCB how to prefer your libraries over the system ones. My library string in preferences does not mention the default libs at all. It currently reads: ~/geda/footprints:./packages:. So how would I teach PCB to prefer them? Besides, my aim is not only prefer my libs, but use them exclusively. ---)kaimartin(--- I've got the line (component-library-search /../../footprints) in my gafrc file. Does that set a priority? -Ethan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
On 06/07/2011 06:05 AM, Ethan Swint wrote: I've got the line (component-library-search /../../footprints) in my gafrc file. Does that set a priority? -Ethan Not sure of the concept of priority, but I think yes. pcb probably uses the first it finds and that line will be the first searched. The library specified with lib-newlib = x in ~/.pcb/settings will also be available footprints. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
I looked into the code; if you set the newlib library it should override the default one, not append to it. Check the following locations: ~/.pcb/settings (look for lib-newlib) ~/.pcb/preferences (library-newlib) If that doesn't help, add '#define DEBUG 1' to src/file.c and rebuild. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
I've got the line (component-library-search /../../footprints) in my gafrc file. Does that set a priority? Not for File-Import. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
Ethan Swint wrote: I've got the line (component-library-search /../../footprints) in my gafrc file. Does that set a priority? I just double checked. This setting does not seem to affect the choice of footprints in any way. The term components in the context of gafrc exclusively refers to symbols. (Why is the parameter not called symbol-search-path?) For gsch2cb the path to the footprint lib is set by the parameter --elements-dir on the command line, or in a project file. (Why isn't it --footprint-dir?) ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de Öffentlicher PGP-Schlüssel: http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
DJ Delorie wrote: I looked into the code; if you set the newlib library it should override the default one, not append to it. Check the following locations: ~/.pcb/settings (look for lib-newlib) ~/.pcb/preferences (library-newlib) kmk@kwak:~/.pcb$ grep newlib * preferences:library-newlib = ~/geda/footprints:./footprints:. If that doesn't help, It doesn't. In addition to my footprints I get the default libs in the chooser dialog. add '#define DEBUG 1' to src/file.c and rebuild. The recompiled binary reports the following lines on load: $ pcb-head driver-in_proto.pcb In ReadLibraryContents, about to execute command /usr/local/bin/../share/pcb/ListLibraryContents.sh '.:/usr/local/bin/../share/pcb' 'pcblib' In ParseLibraryTree, looking for newlib footprints inside top level directory /usr/local/share/pcb/newlib ... In ParseLibraryTree loop examining 2nd level direntry . ... In ParseLibraryTree loop examining 2nd level direntry .. ... In ParseLibraryTree loop examining 2nd level direntry 2_pin_thru-hole_packages ... In ParseLibraryTree loop examining 2nd level direntry analog-devices ... In ParseLibraryTree loop examining 2nd level direntry burr-brown ... In ParseLibraryTree loop examining 2nd level direntry connectors ... In ParseLibraryTree loop examining 2nd level direntry crystal ... In ParseLibraryTree loop examining 2nd level direntry electro-optics ... In ParseLibraryTree loop examining 2nd level direntry headers ... In ParseLibraryTree loop examining 2nd level direntry msp430 ... In ParseLibraryTree loop examining 2nd level direntry not_vetted_ingo ... In ParseLibraryTree loop examining 2nd level direntry sockets ... In ParseLibraryTree loop examining 2nd level direntry tests ... In ParseLibraryTree loop examining 2nd level direntry keystone ... In ParseLibraryTree, looking for newlib footprints inside top level directory /usr/local/share/pcb/pcblib-newlib ... In ParseLibraryTree loop examining 2nd level direntry . ... In ParseLibraryTree loop examining 2nd level direntry .. ... In ParseLibraryTree loop examining 2nd level direntry gtag ... In ParseLibraryTree loop examining 2nd level direntry minicircuits ... In ParseLibraryTree loop examining 2nd level direntry amphenol ... In ParseLibraryTree loop examining 2nd level direntry connector ... In ParseLibraryTree loop examining 2nd level direntry crystal ... In ParseLibraryTree loop examining 2nd level direntry generic ... In ParseLibraryTree loop examining 2nd level direntry johnstech ... In ParseLibraryTree loop examining 2nd level direntry optical ... In ParseLibraryTree loop examining 2nd level direntry pci ... In ParseLibraryTree loop examining 2nd level direntry amp ... In ParseLibraryTree loop examining 2nd level direntry bourns ... In ParseLibraryTree loop examining 2nd level direntry cts ... In ParseLibraryTree loop examining 2nd level direntry geda ... In ParseLibraryTree loop examining 2nd level direntry panasonic ... In ParseLibraryTree loop examining 2nd level direntry index.html ... In ParseLibraryTree loop examining 2nd level direntry broken.html ... In ParseLibraryTree loop examining 2nd level direntry optek ... In ParseLibraryTree loop examining 2nd level direntry nichicon ... In ParseLibraryTree loop examining 2nd level direntry candk ... In ParseLibraryTree, looking for newlib footprints inside top level directory /home/kmk/IQO/Projekte/Stromverteiler ... In ParseLibraryTree loop examining 2nd level direntry supply.sch ... In ParseLibraryTree loop examining 2nd level direntry science-monitor.sch ... In ParseLibraryTree loop examining 2nd level direntry timer_proto.net ... In ParseLibraryTree loop examining 2nd level direntry stromverteiler.cmd ... In ParseLibraryTree loop examining 2nd level direntry print ... In ParseLibraryTree loop examining 2nd level direntry szenarien_proto.cmd ... In ParseLibraryTree loop examining 2nd level direntry documentation ... In ParseLibraryTree loop examining 2nd level direntry timer_proto.g2p ... In ParseLibraryTree loop examining 2nd level direntry monitor-supply.sym ... In ParseLibraryTree loop examining 2nd level direntry stromverteiler.g2p ... In ParseLibraryTree loop examining 2nd level direntry D-NFET.sym ... In ParseLibraryTree loop examining 2nd level direntry stromverteiler.pcb ... In ParseLibraryTree loop examining 2nd level direntry driver-in_proto.pcb- ... In ParseLibraryTree loop examining 2nd level direntry science.sch ... In ParseLibraryTree loop examining 2nd level direntry science-monitor.sym ... In ParseLibraryTree loop examining 2nd level direntry timer.sym ... In ParseLibraryTree loop examining 2nd level direntry driver-in_proto.new.pcb ... In ParseLibraryTree loop examining 2nd level direntry szenarien_proto.net ... In ParseLibraryTree loop examining 2nd level direntry szenarien_proto.sch ... In ParseLibraryTree loop examining 2nd level direntry PCB.00011524.save ... In ParseLibraryTree loop
Re: gEDA-user: import schematics with local footprints
Try setting ~/.pcb/settings: lib-newlib = /envy/dj/geda/gedasymbols/www/user/dj_delorie/footprints:footprints ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
DJ Delorie wrote: Try setting ~/.pcb/settings: lib-newlib = /envy/dj/geda/gedasymbols/www/user/dj_delorie/footprints:footprints Does not help. Schematic import still prefers the default footprints. (If I move the default libs out of the way, I get footprints from my lib) ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de Öffentlicher PGP-Schlüssel: http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
DJ Delorie wrote: I think this is the m4 before newlib bug, so you need the magic ~/.pcb/settings incantation to disable the m4 library completely: lib-contents-command = /bin/true Thanks. For the archive: In addition to the lib contents-command I had to move the default libraries out of the way. mv /usr/local/share/pcblib-newlib /usr/local/share/pcblib-newlib_not mv /usr/local/share/newlib /usr/local/share/newlib_not I suggest to add an option to gnetlist that makes it ignore the default libraries. A better solution would be to have an exclusive search path with no hidden back-doors. Fall-back to some default introduces can be a source of errors that go unnoticed into production. ---)kaimartin(--- -- Kai-Martin Knaak tel: +49-511-762-2895 Universität Hannover, Inst. für Quantenoptik fax: +49-511-762-2211 Welfengarten 1, 30167 Hannover http://www.iqo.uni-hannover.de GPG key:http://pgp.mit.edu:11371/pks/lookup?search=Knaak+kmkop=get ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
If you're using File-Import, gnetlist is not looking at the libraries at all. Only PCB is, so you just need to teach PCB how to prefer your libraries over the system ones. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
No, you're doing it right. Run PCB and open the library window. Do you see your footprints there? Do the names in square brackets match the footprint attributes? Those are the key things to using the importer. The most likely newbie mistake is pointing your local libraries one level too far up/down... ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
On Fri, 2011-06-03 at 11:27 -0400, DJ Delorie wrote: No, you're doing it right. Run PCB and open the library window. Do you see your footprints there? Do the names in square brackets match the footprint attributes? Those are the key things to using the importer. I remember myself having to delete the pcb library to let my footprints be used instead of default library's equivalent (when there is a footprint with the same name as mine in the default library). Is this fixed ? The most likely newbie mistake is pointing your local libraries one level too far up/down... ___ geda-user mailing list [1]geda-user@moria.seul.org [2]http://www.seul.org/cgi-bin/mailman/listinfo/geda-user -- Felipe De la Puente Christen References 1. mailto:geda-user@moria.seul.org 2. http://www.seul.org/cgi-bin/mailman/listinfo/geda-user ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
DJ Delorie wrote: No, you're doing it right. Run PCB and open the library window. Do you see your footprints there? yes. Do the names in square brackets match the footprint attributes? What square bracket? Yes, I have the footprint attributes set correctly. The traditional gsch2pcb has no trouble locating the footprints. The import action works fine for components that have a unique name in my lib. But for generic footprint names like 0805 the import action chooses the version from the default lib. This is very certainly not what I want. If it were me, there should be no defaulting to the default lib at all. The most likely newbie mistake is pointing your local libraries one level too far up/down... Been there, done that -- about five years ago. ---)kaimartin(--- -- Kai-Martin Knaak Email: k...@familieknaak.de Öffentlicher PGP-Schlüssel: http://pool.sks-keyservers.net:11371/pks/lookup?search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: import schematics with local footprints
What square bracket? In the library window, at the end of each M4 footprint's description, is the string to use for footprint= in brackets, like [0603]. For file-based footprints, you of course use the file name. But for generic footprint names like 0805 the import action chooses the version from the default lib. I think this is the m4 before newlib bug, so you need the magic ~/.pcb/settings incantation to disable the m4 library completely: lib-contents-command = /bin/true ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
