Re: gEDA-user: More robust support of multi-part symbols.
John Griessen wrote: > Ben Jackson wrote: > I'd love to know how >> the big boys handle it. Obviously you can't draw wires in gschem and >> then swap pins in pcb and expect the wires to be asthetically re-drawn >> in gschem. So do you only do it with busrippers and netname attributes? >> > > Not having back annotation IS s 80's. Slots could disappear and I > wouldn't miss them. while I certainly can't claim extensive backannotation, we do have the ability to renumber reference designators in pcb where the numbering groups by physical location and then back annotate that change to the schematic. I think ultimately we'll end up needing a netlist (including attribute) comparison tool. The way pads does both forward and backward annotation is you generate a schematic and a layout netlist. Then you run a program on those two netlists and tell it which direction you want to go in. It will then produce an engineering change order (.eco) file that either the schematic or layout tool loads and makes the changes. When using gschem as the schematic frontend for pads, that flow pretty much works. gnetlist generates the schematic netlist, pads makes the layout netlist. Then the pads compare tool generates the .eco file which pads layout can deal with for forward annotation or gschem can deal with via the pads_backannotate utility. Some changes are applied automatically like refdes renumbering. Others are reported to you like "you must perform this schematic change". I started to pursue one of the open source netlist comapare utilities ages ago but never got really far. The other thing that would be useful I think is if libgeda had an external api for applying .eco changes instead of relying on a perl program that has its own .sch parser. .eco may not be the desired format and perhaps this is the right place to start work on the translator system that Al has proposed. Make gnetlist, pcb, and the (not yet cleaned up) netlist compare tool all read some well defined verilog based file. Really, I'm not sure we can get there without a general purpose netlist compare tool because our schematic tool and layout tool are sufficiently decoupled that we don't have any other way really of always enforcing a link. anyway, just a thought. -Dan p.s. netgen exists and it probably makes sense to contribute to it rather than reinventing that wheel. http://opencircuitdesign.com/netgen/ but good grief. spice format. ick. at a minimum someone should teach that tool to read verilog netlists since at least there is a standard there. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Patches: Submenus for electronics-menu
Hello there and PeterC, Fedora Electronic Lab includes too many EDA software and the actual electronics-menu drowns the user into confusion. I have created submenus on electronics-menu as you can see on this screenshot: http://chitlesh.fedorapeople.org/submenu/snapshot.png The idea is that the packager added the category "Electronics" to the desktop file and hence the electronics-menu automatically shift it to its appropriate submenu. Below are 2 patches and the additional sources, they have been tuned so that they are distribution independent. http://chitlesh.fedorapeople.org/submenu/electronics-menu-1.0-makefile.patch http://chitlesh.fedorapeople.org/submenu/electronics-menu-1.0-submenus.patch http://chitlesh.fedorapeople.org/submenu/electronics-menu-1.0-submenu.tar.bz2 I am currently pushing it to the fedora testing repositories. Tomorrow, you can yum update electronics-menu --enablerepo=updates-testing Else you can pull it from here http://koji.fedoraproject.org/koji/packageinfo?packageID=5787 Release: 1.0-4 Happy testing and I hope other distributions will adopt it as well. Kind regards, Chitlesh ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: More robust support of multi-part symbols.
On Thu, 09 Jul 2009 18:22:07 +0200, igor2 wrote: > This means the user can swap whatever he wants on the PCB > and his schematics becomea haystack with red lines, then he can go and > clean it up when he finished swapping pins on the PCB. Rats nests in the schematic! The topological auto router may be handy to resolve the mess ;-) ---<(kaimartin)>--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=get&search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: More robust support of multi-part symbols.
On Thu, 9 Jul 2009, Dave N6NZ wrote: >Ben Jackson wrote: >> On Wed, Jul 08, 2009 at 09:20:54PM -0700, Steve Meier wrote: >>> Let alone, how at the layout level we can do pin swapping and back >>> annotation. >> >> I've thought about working on that, because I've dealt with that problem >> in almost every project I've done with geda/pcb. I'd love to know how >> the big boys handle it. > >Often poorly. > >> Obviously you can't draw wires in gschem and >> then swap pins in pcb and expect the wires to be asthetically re-drawn >> in gschem. So do you only do it with busrippers and netname attributes? > >The first thing to realize is that for large projects, hand placed line >corners don't scale. The in-house CAD systems I've used on large >(30-300 engineer) projects had auto-routed drawings. In some ways, >auto-routing a drawing is more of a challenge than auto-routing a PCB, >since aesthetics matters as well as connectivity. An in no case were >the drawings "perfect" -- that is to say what a good draftsman would do. >But all the systems produced readable drawings, and nobody hand to spend >much time making them readable. gpsim (Free PIC microcontroller simulator) tries to do something similaron the breadboard feature. The breadboard looks like a schematics, you see there the PIC being simulated, and if you have external modules (LCD, rs232 terminal, LED, etc), you see them as well. The netlist is visualized by drawing black lines between the pins. The lines consist of horizontal and vertical segments and gpsim tries its best to add as many segments as required to avoid crossing components or other lines. Of course it works well only if you have 2..3 boxes and max 6-8 lines :) I agree that this may be a bit overkill. However, swapping pin numbers may work for the big box symbols. Maybe we could mark groups of pins in a symbol, let's say GPIO1, 8 pins is a group, if any two of these are swapped, just swap the pin number on the schematics. If you swap a GND with a GPIO1 pin, it won't work, because they are not in the same pin group. I think something similar may be applied on slots. Another option is defining net lines with different color in gschem. If two pins are swapped, gschem deletes the two net segments connceted to the pins and draws two new segments simply crossing eachothers with this different color. This means the user can swap whatever he wants on the PCB and his schematics becomea haystack with red lines, then he can go and clean it up when he finished swapping pins on the PCB. Regards, Tibor Palinkas ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: More robust support of multi-part symbols.
Ben Jackson wrote: I'd love to know how > the big boys handle it. Obviously you can't draw wires in gschem and > then swap pins in pcb and expect the wires to be asthetically re-drawn > in gschem. So do you only do it with busrippers and netname attributes? > Not having back annotation IS s 80's. Slots could disappear and I wouldn't miss them. I think the best of ECAD still handles back annotation as a to-do list of edits the schematic drawer does. Just that would be plenty valuable without any schematics-drawn-on-auto. Symbols drawn on auto -- now that would be handy for chip design and hierarchic pcb design. I think we are fairly close to auto-drawn-symbols. If we made a program to generate a symbol from the gnetlist-verilog netlist, the port lists could be put so inouts are at bottom ins at left and outs at right and also put out a shorthand symbol description file in djboxsym format, one could rework the symbol quickly. John -- Ecosensory Austin TX ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: More robust support of multi-part symbols.
Ben Jackson wrote: > On Wed, Jul 08, 2009 at 09:20:54PM -0700, Steve Meier wrote: >> Let alone, how at the layout level we can do pin swapping and back >> annotation. > > I've thought about working on that, because I've dealt with that problem > in almost every project I've done with geda/pcb. I'd love to know how > the big boys handle it. Often poorly. > Obviously you can't draw wires in gschem and > then swap pins in pcb and expect the wires to be asthetically re-drawn > in gschem. So do you only do it with busrippers and netname attributes? The first thing to realize is that for large projects, hand placed line corners don't scale. The in-house CAD systems I've used on large (30-300 engineer) projects had auto-routed drawings. In some ways, auto-routing a drawing is more of a challenge than auto-routing a PCB, since aesthetics matters as well as connectivity. An in no case were the drawings "perfect" -- that is to say what a good draftsman would do. But all the systems produced readable drawings, and nobody hand to spend much time making them readable. I agree that back-annotation is one of the top problems gEDA needs to address. It's one of the things gEDA needs to scale up to large projects. In general, gEDA does not scale up well. -dave ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: minipack issues
Duncan Drennan wrote: > Once the compilation is done, will the files run "as is" or do the > dll's have to be installed into specific windows directories? The dll's should remain beside the exe's in the "bin" directory. Currently, to run the resulting exe's, you have to set the following environment variables: set GEDADATA=[path_to_geda]\share\gEDA set GUILE_LOAD_PATH=[path_to_geda]\share\guile\1.8 Regards, Cesar ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: minipack issues
> In the command-line, please type: > > echo passive_ftp=on >> ~/.wgetrc > Thanks Cesar, I'll try that out. I just manually used wget and the passive ftp option to grab the sources. Busy compiling now (on cygwin) which seems to be taking quite long. Hopefully I'll actually get some functional .exe files out. Once the compilation is done, will the files run "as is" or do the dll's have to be installed into specific windows directories? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: minipack issues
Duncan Drennan wrote: >> It seems wget is failing to get the source for the JPEG library for some >> reason. > > After a bit of searching I found out that if I use the --passive-ftp > option with wget then the download succeeds. > > Is there a way via a config or recipe file to set flags for wget? > In the command-line, please type: echo passive_ftp=on >> ~/.wgetrc This will add the passive FTP option to the configuration file of Wget itself. If this doesn't work, please give me the output of: wget --version which wget Regards, Cesar ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: More robust support of multi-part symbols.
On Wed, 08 Jul 2009 12:18:12 +, Kai-Martin Knaak wrote: > 1) gnetlist should look for a footprint in every instance of a refdes I just struggled to locate the place where this could be changed. The function that does actually fetch the attributes seems to be char *o_attrib_search_object_attribs_by_name() But where does gnetlist loop through all symbols to collect attributes? s_traverse.c seems close, but I only recognize searches for pins and nets ---<(kaimartin)>--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=get&search=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
