Re: gEDA-user: Strange gsch2pcb error
On Fri, 2011-01-21 at 15:22 +, Peter TB Brett wrote: > Is Ben's problem a duplicate of this bug then? > > https://bugs.launchpad.net/geda/+bug/698806 Yes, marked as such. That bug now has two duplicates ;) -- 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, 20 Jan 2011 22:41:04 -0500, DJ Delorie 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
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+kmk&op=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 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 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 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
On Thu, 2011-01-20 at 22:39 -0500, Ben Gamari wrote: > On Fri, 21 Jan 2011 01:07:23 +, Peter Clifton 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
> 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
Re: gEDA-user: Strange gsch2pcb error
On Fri, 21 Jan 2011 00:59:16 +, Peter Clifton 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
On Fri, 21 Jan 2011 01:03:13 +, Peter Clifton 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 01:07:23 +, Peter Clifton 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 Thu, 2011-01-20 at 19:22 -0500, Ben Gamari wrote: > On Fri, 21 Jan 2011 00:08:03 +, Peter TB Brett > 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 Thu, 2011-01-20 at 19:22 -0500, Ben Gamari wrote: > On Fri, 21 Jan 2011 00:08:03 +, Peter TB Brett > 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 > 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 Fri, 21 Jan 2011 00:41:33 +, Peter TB Brett 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 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 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
Hi Ben, Works for me. See attached log. Peter -- Peter Brett 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
Re: gEDA-user: Strange gsch2pcb error
On Fri, 21 Jan 2011 00:08:03 +, Peter TB Brett 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
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 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
gEDA-user: Strange gsch2pcb error
Hey all, I've been working on a data acquisition board using the geda toolchain exclusively and so far I have been quite pleased with the results. Unfortunately, a few days ago gsch2pcb inexplicably stopped working. In particular, it appears that m4 fails with the following, $ make pcb gsch2pcb -v project | tee pcb.log Loading schematic [/home/ben/lori/beagle-daq/beagle-daq.sch] Loading schematic [/home/ben/lori/beagle-daq/beagle-daq.sch] /usr/bin/m4:stdin:45: bad expression in eval: /2 If I kill the gsch2pcb process with Ctrl+\ I can see the command line arguments of the failing process, /usr/bin/m4 -d -I/usr/share/pcb/m4 -I/usr/etc/pcb -I$HOME/.pcb -I. /usr/share/pcb/m4/common.m4 - >> beagle-daq.new.pcb I have no idea what might have prompted this behavior and thankfully the design is pretty much finished, but I would like to know what might be wrong. I am using both gaf and pcb from git, although I have tested versions back to 1.6.2 with no change in behavior. The project is available through git at [1]. I am thoroughly perplexed and any help would be greatly appreciated. Thanks! Cheers, - Ben [1] gito...@goldnerlab.physics.umass.edu:beagle-daq ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
