Re: gEDA-user: Strange gsch2pcb error
On Thu, 2011-01-20 at 22:39 -0500, Ben Gamari wrote: On Fri, 21 Jan 2011 01:07:23 +, Peter Clifton pc...@cam.ac.uk wrote: Error sounded like it might be a classic: Don't put - in footprint names Ahhh. That would explain it. Those packages came from http://www.luciani.org/geda/pcb/pcb-footprint-list.html. Are none of these correctly named? John doesn't use the M4 library at all, so he sticks to his convention. It is really a bug that we don't handle this better. -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Friday 21 Jan 2011 15:16:45 Peter Clifton wrote: On Thu, 2011-01-20 at 22:39 -0500, Ben Gamari wrote: On Fri, 21 Jan 2011 01:07:23 +, Peter Clifton pc...@cam.ac.uk wrote: Error sounded like it might be a classic: Don't put - in footprint names Ahhh. That would explain it. Those packages came from http://www.luciani.org/geda/pcb/pcb-footprint-list.html. Are none of these correctly named? John doesn't use the M4 library at all, so he sticks to his convention. It is really a bug that we don't handle this better. Is Ben's problem a duplicate of this bug then? https://bugs.launchpad.net/geda/+bug/698806 Peter -- Peter Brett pe...@peter-b.co.uk Remote Sensing Research Group Surrey Space Centre ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
Peter Clifton wrote: It is really a bug that we don't handle this better. ack. It hurt me badly like five years ago and it was already a known issue back then. ---)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: Strange gsch2pcb error
On Thu, 20 Jan 2011 22:41:04 -0500, DJ Delorie d...@delorie.com wrote: Ahhh. That would explain it. Those packages came from http://www.luciani.org/geda/pcb/pcb-footprint-list.html. Are none of these correctly named? John's library doesn't use m4, so if you're using his library, you should disable m4. Then you don't have the problem. Thanks everyone! That fixed it. Cheers, - Ben ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Thursday 20 January 2011 23:59:24 Ben Gamari wrote: [1] gito...@goldnerlab.physics.umass.edu:beagle-daq What's the password, please? Thanks, Peter -- Peter Brett pe...@peter-b.co.uk Remote Sensing Research Group Surrey Space Centre signature.asc Description: This is a digitally signed message part. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Fri, 21 Jan 2011 00:08:03 +, Peter TB Brett pe...@peter-b.co.uk wrote: On Thursday 20 January 2011 23:59:24 Ben Gamari wrote: What's the password, please? Doh. Sorry about that, wrong URL. Please use, git://goldnerlab.physics.umass.edu/beagle-daq Thanks for the quick response! - Ben ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
Hi Ben, Works for me. See attached log. Peter -- Peter Brett pe...@peter-b.co.uk Remote Sensing Research Group Surrey Space Centre -*- mode: compilation; default-directory: /home/peter/Projects/geda/beagle-daq/ -*- Compilation started at Fri Jan 21 00:30:26 make pcb gsch2pcb -v project | tee pcb.log SCM_STRING_CHARS is deprecated. See the manual for alternatives. scm_must_malloc is deprecated. Use scm_gc_malloc and scm_gc_free instead. Returning non-0 from a smob free function is deprecated. Use scm_gc_free et al instead. (You just returned non-0 while freeing a object.) Loading schematic [/home/peter/Projects/geda/beagle-daq/beagle-daq.sch] SCM_STRING_CHARS is deprecated. See the manual for alternatives. scm_must_malloc is deprecated. Use scm_gc_malloc and scm_gc_free instead. Returning non-0 from a smob free function is deprecated. Use scm_gc_free et al instead. (You just returned non-0 while freeing a object.) Loading schematic [/home/peter/Projects/geda/beagle-daq/beagle-daq.sch] SCM_STRING_CHARS is deprecated. See the manual for alternatives. scm_must_malloc is deprecated. Use scm_gc_malloc and scm_gc_free instead. Returning non-0 from a smob free function is deprecated. Use scm_gc_free et al instead. (You just returned non-0 while freeing a object.) /usr/bin/m4: cannot open `/home/peter/opt/share/pcb/m4/common.m4': No such file or directory = gsch2pcb backend configuration: Variables which may be changed in gafrc: gsch2pcb:pcb-m4-command:/usr/bin/m4 gsch2pcb:pcb-m4-dir:/home/peter/opt/share/pcb/m4 gsch2pcb:pcb-m4-confdir:/home/peter/opt/etc/pcb gsch2pcb:pcb-m4-path: /home/peter/opt/share/pcb/m4 /home/peter/opt/etc/pcb $HOME/.pcb . gsch2pcb:m4-command-line: /usr/bin/m4 -d -I/home/peter/opt/share/pcb/m4 -I/home/peter/opt/etc/pcb -I$HOME/.pcb -I. /home/peter/opt/share/pcb/m4/common.m4 - beagle-daq.new.pcb --- Variables which may be changed in the project file: --- gsch2pcb:use-m4:yes = Using the m4 processor for pcb footprints Loading schematic [/home/peter/Projects/geda/beagle-daq/beagle-daq.sch] GPIO/U1: can't find PCB element for footprint SSOP24 (value=unknown) So device GPIO/U1 will not be in the layout. U5: can't find PCB element for footprint SSOP8 (value=unknown) So device U5 will not be in the layout. Reading project file: project schematics beagle-daq.sch output-name beagle-daq Processing PCBLIBPATH=/home/peter/opt/share/pcb/pcblib-newlib:/home/peter/opt/share/pcb/newlib Adding /home/peter/opt/share/pcb/newlib to the newlib search path Running command: gnetlist -g pcbpins -o beagle-daq.cmd beagle-daq.sch Running command: gnetlist -g PCB -o beagle-daq.net beagle-daq.sch Default m4-pcbdir: /home/peter/opt/share/pcb/pcb/m4 gnet-gsch2pcb-tmp.scm override file: (define m4-pcbdir /home/peter/opt/share/pcb/pcb/m4) (define gsch2pcb:use-m4 #t) Running command: gnetlist -g gsch2pcb -o beagle-daq.new.pcb -m gnet-gsch2pcb-tmp.scm beagle-daq.sch GPIO/U1: need new file element for footprint SSOP24 (value=unknown) psu/U1: need new file element for footprint SOT23-5 (value=unknown) Found: packages/m4/SOT23-5 psu/U1: added new file element for footprint SOT23-5 (value=unknown) U5: need new file element for footprint SSOP8 (value=unknown) U5: deleted element TSSOP-65P-640L1-8N (value=) U4: changed element TSSOP-65P-640L1-20N value: - unknown dac1/U1: changed element TSSOP-65P-640L1-16N value: - unknown U1: changed element TSSOP-65P-640L1-20N value: - unknown psu/U1: deleted element SOT23-95P-280L1-5N__LTC_S5_Package (value=) GPIO/U1: deleted element TSSOP-65P-640L1-24N (value=) U6: changed element TSSOP-65P-640L1-20N value: - unknown dac3/U1: changed element TSSOP-65P-640L1-16N value: - unknown U2: changed element TSSOP-65P-640L1-16N value: - unknown dac4/U1: changed element TSSOP-65P-640L1-16N value: - unknown dac2/U1: changed element TSSOP-65P-640L1-16N value: - unknown -- Done processing. Work performed: beagle-daq.pcb is backed up as beagle-daq.pcb.bak1. 3 elements deleted from beagle-daq.pcb. 1 file elements and 0 m4 elements added to beagle-daq.new.pcb. 8 elements had a value change in beagle-daq.pcb. 2 elements could not be found. So beagle-daq.new.pcb is incomplete. Next steps: 1. Run pcb on your file beagle-daq.pcb. 2. From within PCB, select File - Load layout data to paste buffer and select beagle-daq.new.pcb to load the new footprints into your existing layout. 3. From within PCB, select File - Load netlist file and select
Re: gEDA-user: Strange gsch2pcb error
On Friday 21 January 2011 00:32:29 Peter TB Brett wrote: Hi Ben, Works for me. See attached log. Now that I've installed PCB properly, I can reproduce the bug. It's *probably* a gEDA bug, so please file a bug report so that I remember to look at it after I've had some sleep. https://bugs.launchpad.net/geda/+filebug Peter -- Peter Brett pe...@peter-b.co.uk Remote Sensing Research Group Surrey Space Centre signature.asc Description: This is a digitally signed message part. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Fri, 21 Jan 2011 00:41:33 +, Peter TB Brett pe...@peter-b.co.uk wrote: Now that I've installed PCB properly, I can reproduce the bug. It's *probably* a gEDA bug, so please file a bug report so that I remember to look at it after I've had some sleep. Bug filed[1]. Thanks a ton! - Ben [1] https://bugs.launchpad.net/geda/+bug/705695 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Thu, 2011-01-20 at 19:22 -0500, Ben Gamari wrote: On Fri, 21 Jan 2011 00:08:03 +, Peter TB Brett pe...@peter-b.co.uk wrote: On Thursday 20 January 2011 23:59:24 Ben Gamari wrote: What's the password, please? Doh. Sorry about that, wrong URL. Please use, git://goldnerlab.physics.umass.edu/beagle-daq Don't forget to unmask the soldermask for your mounting holes vias. -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Thu, 2011-01-20 at 19:22 -0500, Ben Gamari wrote: On Fri, 21 Jan 2011 00:08:03 +, Peter TB Brett pe...@peter-b.co.uk wrote: On Thursday 20 January 2011 23:59:24 Ben Gamari wrote: What's the password, please? Doh. Sorry about that, wrong URL. Please use, git://goldnerlab.physics.umass.edu/beagle-daq Thanks for the quick response! Are there any symbols you're using as part of a local library not in that git repository? WARNING: Found a placeholder/missing component, are you missing a symbol file? [ad7606.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [at24c01.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [dac8568.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [lm78xx.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [lp2981.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [ref50xx.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [sn54ahc139.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [tca6416.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [tps7a4901.sym] WARNING: Found a placeholder/missing component, are you missing a symbol file? [txb0108.sym] -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Thu, 2011-01-20 at 19:22 -0500, Ben Gamari wrote: On Fri, 21 Jan 2011 00:08:03 +, Peter TB Brett pe...@peter-b.co.uk wrote: On Thursday 20 January 2011 23:59:24 Ben Gamari wrote: What's the password, please? Doh. Sorry about that, wrong URL. Please use, git://goldnerlab.physics.umass.edu/beagle-daq Error sounded like it might be a classic: Don't put - in footprint names grep footprint *.sch | grep - footprint=SOIC-127P-600L1-8N footprint=SOIC-127P-600L1-8N I found it in this dir: ./packages/m4/SOIC-127P-600L1-8N Why did you name that sub dir m4? You can get away with it (I think), if you don't use any (actual) M4 symbols, and you pass the --skip-m4 option to gnetlist, or put skip-m4 inside the project file. -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) Tel: +44 (0)1223 748328 - (Shared lab phone, ask for me) signature.asc Description: This is a digitally signed message part ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Fri, 21 Jan 2011 01:07:23 +, Peter Clifton pc...@cam.ac.uk wrote: Error sounded like it might be a classic: Don't put - in footprint names Ahhh. That would explain it. Those packages came from http://www.luciani.org/geda/pcb/pcb-footprint-list.html. Are none of these correctly named? grep footprint *.sch | grep - footprint=SOIC-127P-600L1-8N footprint=SOIC-127P-600L1-8N I found it in this dir: ./packages/m4/SOIC-127P-600L1-8N Why did you name that sub dir m4? Good question. This was done long ago. On this note, what is the recommended file naming convention for footprints? Do you use the .fp extension? You can get away with it (I think), if you don't use any (actual) M4 symbols, and you pass the --skip-m4 option to gnetlist, or put skip-m4 inside the project file. I'll just fix the directory name. Should I just move the contents of packages/m4 to packages/newlib (or perhaps just packages/)? Thanks! - Ben ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Fri, 21 Jan 2011 01:03:13 +, Peter Clifton pc...@cam.ac.uk wrote: Are there any symbols you're using as part of a local library not in that git repository? WARNING: Found a placeholder/missing component, are you missing a symbol file? [ad7606.sym] ... In case you didn't already figure this out, just run make. These are generated by the makefile with tragesym. - Ben ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
On Fri, 21 Jan 2011 00:59:16 +, Peter Clifton pc...@cam.ac.uk wrote: Don't forget to unmask the soldermask for your mounting holes vias. Good point. Thanks for the tip! - Ben ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Strange gsch2pcb error
Ahhh. That would explain it. Those packages came from http://www.luciani.org/geda/pcb/pcb-footprint-list.html. Are none of these correctly named? John's library doesn't use m4, so if you're using his library, you should disable m4. Then you don't have the problem. On this note, what is the recommended file naming convention for footprints? Do you use the .fp extension? Yes. File-based footprints should be named *.fp ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
