Re: gEDA-user: Breadboard drawings with pcb?
On 5/26/09, Michael Sokolov msoko...@ivan.harhan.org wrote: Right now I just do vi OSDCU_??.usch, then check with uschem-print | lpr Hmm, I wonder if your lpr outputs onto reusable media. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Ineiev ine...@gmail.com wrote: Hmm, I wonder if your lpr outputs onto reusable media. No, it does not. I kill trees. I know, I am a bad boy. Setting up a system for viewing PostScript on an X11 display that's usable from my 4.3BSD-Quasijarus VAXen is on my *very* long list of things I'd like to get done some day if I have the time. MS ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Breadboard drawings with pcb? (first result)
Hello,
I have first results of my breadboard project (and some questions, too).
So, here's what I've done:
- to represent the holes and connections on the breadboard, I used
(locked) lines+arcs on the solder layer.
- I have written a small perl script (included below in this mail)
to create the pcb templates in various sizes. It takes the number
of rows/columns as command line parameters
- for my first test, I used the example from the gsch2pcb tutorial.
I have attached the resulting pcb (stripped from font symbols) at the
end of this post.
There is still room for improvement, though.
Problems when placing parts:
- The rats (BTW: where comes the name from?) immediately connect to
the arcs, since almost whole board is populated with arcs+lines. So
there's no visual hints how to move the parts in order to minimize
the rat-crossings.
- maybe there's an option for the rats to ignore the existing
copper?
- maybe the lines+arcs should go to the solder silk to avoid this
problem. But solder silk is shown only when the board is
reversed.
- Since ElementLines are in 50/100mil raster, they exactly overlap
and obfuscate the traces.
- this would easily be solved by special parts
- On a real breadboard, there's waaay more flexibility. For example,
resistors can easily be stretched/shrink-ed. Or R101 could easily
be placed quasi-parallel to R102.
- guess, there's no solution for that? At least, stretching/shrinking
would be highly desirable. Then R102 could be placed in parallel
to R101.
Problems with routing:
- To give the traces a look like real wires (as opposed to the perfect
traces), I tried to use arcs. But they seem to come out only in
rasters of 90 degree. I was not able to connect points that are not
on the diagonals or to connect to a line with 45 degrees. Although
the documentation says they can be rotated and shrink-ed, I could not
find out how.
Problems with printing:
- There seem to be no way to control the order of the layers. Sometimes
the routes are hidden by the grey solder layer.
-o- So here's the perl script --o--
#! /usr/bin/perl
use strict;
use warnings;
my ($rows, $cols) = (shift, shift);
$rows = 1 unless defined $rows;
$cols = 1 unless defined $cols;
my (@via, @solder, @component);
header;
for (my $c=0; $c($cols+1)*18; $c+=18) {
if ($c$cols*18) {
my %off=(A=5, B=6, C=7, D=8, E=9,
F=12, G=13, H=14, I=15, J=16);
foreach my $arr (0, $rows*6+3.4) {
foreach my $l (A..J) {
push @solder, text ($c+$off{$l}-0.12, $arr, $l);
}
}
}
push @solder, line ($c+1, 3, $c+1, $rows*6+1);
push @solder, line ($c+2, 3, $c+2, $rows*6+1);
push @solder, text ($c+0.9, 2, +);
push @solder, text ($c+1.9, 2, -);
push @solder, text ($c+0.9, $rows*6+1.5, +);
push @solder, text ($c+1.9, $rows*6+1.5, -);
for (my $r=0; $r$rows*6+3; $r++) {
unless (($r-3)%6) {
vbar (0, $c+1, $r);
vbar (0, $c+2, $r)
}
if ($c$cols*18) {
hbar (1, $c+5, $r+1);
hbar (1, $c+12, $r+1);
foreach my $x (4, 16.5) {
if ($r==1 || ($r0 $r%5==0)) {
push @solder, text ($c+$x, $r-0.3, $r);
}
}
}
}
}
footer;
sub domul { map { 1*$_} @_; }
sub text { sprintf ('Text[%d %d 0 100 %s lock]', domul(@_[0..1]), $_[2]) }
sub arc { sprintf 'Arc[%d %d 2000 2000 2000 2000 0 360 lock]', domul(@_); }
sub line { sprintf 'Line[%d %d %d %d 1000 2000 clearline,lock]', domul(@_); }
sub vbar { my ($hl, $x, $y) = @_; bar ($hl, $x, $y, $x, $y+4); }
sub hbar { my ($hl, $x, $y) = @_; bar ($hl, $x, $y, $x+4, $y); }
sub bar {
my ($haveline, $x1, $y1, $x2, $y2) = @_;
if ($haveline) {
push @solder, line ($x1, $y1, $x2, $y2);
}
for (my $x=0; $x=$x2-$x1; $x++) {
for (my $y=0; $y=$y2-$y1; $y++) {
push @solder, arc ($x1+$x, $y1+$y);
}
}
}
sub header {
my $x = $cols*18+3;
my $y = $rows*6+5;
print _EOF_;
FileVersion[20070407]
PCB[ $x $y]
Grid[1.00 0 0 1]
Cursor[0 0 0.00]
PolyArea[2.00]
Thermal[0.50]
DRC[1000 1000 1000 1000 1500 1000]
Flags(nameonpcb,uniquename,clearnew,snappin)
Groups(1,c:2,s:3:4:5:6:7:8)
Styles[Signal,1000,3600,2000,1000:Power,2500,6000,3500,1000:Fat,4000,6000,3500,1000:Skinny,600,2402,1181,600]
_EOF_
}
sub footer {
my $component = join (\n, , @component, );
my $solder= join (\n, , @solder, );
print join (\n, , @via, );
print _EOF_;
Layer(1 component) ( $component )
Layer(2 solder)( $solder )
Layer(3 GND) ( )
Layer(4 power) ( )
Layer(5 signal1) ( )
Layer(6
Re: gEDA-user: Breadboard drawings with pcb? (first result)
- The rats (BTW: where comes the name from?) http://www.delorie.com/pcb/docs/gs/gs.html#rat It's called a rat's nest because of its messy appearance when first created, ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Tue, 26 May 2009 21:15:22 +0200, Josef Wolf wrote: pcb -x ps --psfile board.ps board.pcb Ah, that's fine! Unfortunately, it's not mentioned in the documentation anywhere. I added a section on command line printing to the wiki: http://geda.seul.org/wiki/geda:pcb_tips#is_is_possible_to_produce_output_without_gui_intervention ---(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: Breadboard drawings with pcb?
On Tue, 26 May 2009 14:12:16 -0600, Miles Gazic wrote: I have this same problem, because I automate my build with makefiles, and I'd like to have a build machine (that doesn't run X) be able to build everything Ack. Scripting is a weak point of pcb and in particular gschem. IMHO an expert-friendly app should allow for non-interactive use. This would make the suite much more powerful. ---(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: Breadboard drawings with pcb?
On Wed, 27 May 2009, Kai-Martin Knaak wrote: On Tue, 26 May 2009 14:12:16 -0600, Miles Gazic wrote: I have this same problem, because I automate my build with makefiles, and I'd like to have a build machine (that doesn't run X) be able to build everything Ack. Scripting is a weak point of pcb and in particular gschem. IMHO an expert-friendly app should allow for non-interactive use. This would make the suite much more powerful. FYI, pcb-gpmi allows non-interactive use. You can create actions and call them from pcb command line directly. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 06:33:01PM -0400, DJ Delorie wrote: Vias connect the two sides, so you can test for connectivity. That's all I was thinking. If connectivity can be done another way, then you have other options. What about using lines+arcs on the solder layer to represent the wiring of the breadboard? Placing through-hole parts would then connect fine to the lines/arcs on the solder layer, IMHO. The (black) paths would then be routed on the component layer. That way no special footprints would be needed and even DRC might be possible. The only drawback I see with this approach is that paths along the breadboard paths would be doubled: one goes on solder, the other on component side. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Josef Wolf j...@raven.inka.de writes: I'd prefer something more scriptable, since I expect to have _lots_ of circuits. But at a first glance, it looks like the ps/eps outputs are easy to postprocess. Try gerbv, with a .gvp file as script. This allows to order and color the layers as you like, with transparency. Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 09:51:11PM -0300, John Coppens wrote: On Mon, 25 May 2009 22:58:26 +0200 Josef Wolf j...@raven.inka.de wrote: I'd prefer something more scriptable, since I expect to have _lots_ of circuits. But at a first glance, it looks like the ps/eps outputs are easy to postprocess. If you want publishing (printing) quality output, you'll have to pass through ps anyway. There are a lot of utilities on the 'net that let you combine ps outputs in many ways, using command line utilities. I am not going to publish it by some publishing company, I just want to include it into a latex file. But scriptability is a concern, though: is it possible to create the ps/eps from a script/Makefile without GUI intervention? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On 5/26/09, Josef Wolf j...@raven.inka.de wrote: But scriptability is a concern, though: is it possible to create the ps/eps from a script/Makefile without GUI intervention? (Do you mean you do it _with_ GUI?) pcb -x ps --psfile board.ps board.pcb PCB even does not requires X for this task. BTW I couldn't achieve this with gschem --- it doesn't work from text terminal for me. Regards, Ineiev ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Josef Wolf wrote: On Mon, May 25, 2009 at 06:33:01PM -0400, DJ Delorie wrote: Vias connect the two sides, so you can test for connectivity. That's all I was thinking. If connectivity can be done another way, then you have other options. What about using lines+arcs on the solder layer to represent the wiring of the breadboard? Placing through-hole parts would then connect fine to the lines/arcs on the solder layer, IMHO. [jg]Yes. The (black) paths would then be routed ([jg] by hand) on the component layer ([jg] in black). That way no special footprints would be needed and even DRC might be possible. [jg]Sure. The only drawback I see with this approach is that paths along the breadboard paths would be doubled: one goes on solder, the other on component side. [jg]That won't stop netlisting. The black paths on component side would be for emphasis. You won't be able to show a component grouped with a black trace stretching over vias (or pads on same layer) that represent plugboard holes. They will have to go off to the side to represent the 3D path through the air of a leaded component on a plugboard. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Ineiev wrote: On 5/26/09, Josef Wolf j...@raven.inka.de wrote: But scriptability is a concern, though: is it possible to create the ps/eps from a script/Makefile without GUI intervention? (Do you mean you do it _with_ GUI?) pcb -x ps --psfile board.ps board.pcb ... and then you might be able to use pstools to merge in a background image, rotate and crop, etc. Hmm... b.g. -- Bill Gatliff b...@billgatliff.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Josef Wolf wrote: On Mon, May 25, 2009 at 03:46:00PM -0300, John Coppens wrote: On Mon, 25 May 2009 19:55:23 +0200 Josef Wolf j...@raven.inka.de wrote: - How can I make the breadboard drawing appear light-grey in pcb's postscript output? A trick I've used is to export or print the board to postscript. Then you'll have many pages, one of them the vias alone, and on another the silkscreen. You can then combine both in GIMP and color the vias any color you like. I'd prefer something more scriptable, since I expect to have _lots_ of circuits. But at a first glance, it looks like the ps/eps outputs are easy to postprocess. I wonder if LaTex and pstricks would be useful here? b.g. -- Bill Gatliff b...@billgatliff.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Ineiev ine...@gmail.com wrote: BTW I couldn't achieve this with gschem --- it doesn't work from text terminal for me. That is exactly why the circuit which you'll be laying out has been done in uschem instead of gschem! MS ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On May 26, 2009, at 5:34 AM, Ineiev wrote: On 5/26/09, Josef Wolf j...@raven.inka.de wrote: But scriptability is a concern, though: is it possible to create the ps/eps from a script/Makefile without GUI intervention? (Do you mean you do it _with_ GUI?) pcb -x ps --psfile board.ps board.pcb PCB even does not requires X for this task. BTW I couldn't achieve this with gschem --- it doesn't work from text terminal for me. You can print using the print.scm from a text terminal or script as long as there's an X server for gschem to flash the page on. A minor annoyance, I think. Regards, Ineiev ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Michael Sokolov wrote: Ineiev ine...@gmail.com wrote: BTW I couldn't achieve this with gschem --- it doesn't work from text terminal for me. That is exactly why the circuit which you'll be laying out has been done in uschem instead of gschem! I keep seeing references to uEDA and uschem, but I can't find any mention of it on the gEDA page or with Google. What is it? Where is it? Chris -- Chris Smith cj...@zepler.net signature.asc Description: OpenPGP digital signature ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Chris Smith cj...@zepler.net wrote: I keep seeing references to uEDA and uschem, but I can't find any mention of it on the gEDA page or with Google. What is it? Where is it?= The following cvs checkout command: cvs -d :pserver:anon...@ifctfvax.harhan.org:/fs1/IFCTF-cvs co ueda ifctf-part-lib OSDCU will give you uEDA, my part library for it and a sample project done with it. The documentation under ueda/doc is still in the process of being written. MS ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
John Doty j...@noqsi.com wrote: You can print using the print.scm from a text terminal or script as long as there's an X server for gschem to flash the page on. A minor annoyance, I think. That minor annoyance was enough for me to write uschem (from scratch) to replace gschem. uschem currently has no GUI at all, in fact there is no program named uschem like gschem, there is only uschem-print which generates PostScript and uschem-netlist which generates a netlist, both traditional UNIX-style non-interactive programs intended to run from a Makefile. uschem itself is actually a language I have invented for schematics, not a program. What's currently missing is uschem-edit, a graphical editor for files in the uschem language. Right now I just do vi OSDCU_??.usch, then check with uschem-print | lpr, which I admit is rather poor when I need to edit the graphical aspect of my schematics. MS ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Hi Josef, On Tue, 2009-05-26 at 12:42 +0200, Josef Wolf wrote: On Mon, May 25, 2009 at 09:51:11PM -0300, John Coppens wrote: On Mon, 25 May 2009 22:58:26 +0200 Josef Wolf j...@raven.inka.de wrote: I'd prefer something more scriptable, since I expect to have _lots_ of circuits. But at a first glance, it looks like the ps/eps outputs are easy to postprocess. If you want publishing (printing) quality output, you'll have to pass through ps anyway. There are a lot of utilities on the 'net that let you combine ps outputs in many ways, using command line utilities. I am not going to publish it by some publishing company, I just want to include it into a latex file. But scriptability is a concern, though: is it possible to create the ps/eps from a script/Makefile without GUI intervention? Pondering on this for some time now (actually two years++) I stumbled upon this thread. Have a look at my Work In Progress at: http://www.xs4all.nl/~ljh4timm/downloads/WIP_bread_board_stuff/ I have the idea of coding/building some sort of plug-in around this pcb and footprints for doing the gschem -- breadboard stuff in a somewhat automated/scripted way (perhaps I call it gschem2bb, or just gBreadBoard ;-) So far I have not looked at one line of code in the Fritzing tarball due to the bread on the table-project that keeps me busy all day ;-) as the Fritzing idea looks promising and could be extended to gpl eda. Maybe this all happens during a private Summer of Code session whilst on holiday in Southern France in July (while sipping gallons of Free Wine, as in Freedom of Beer). Kind regards, Bert Timmerman. ___ geda-user mailing list geda-user@moria.seul.org 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: Breadboard drawings with pcb?
On Tue, May 26, 2009 at 03:34:43PM +0400, Ineiev wrote: On 5/26/09, Josef Wolf j...@raven.inka.de wrote: But scriptability is a concern, though: is it possible to create the ps/eps from a script/Makefile without GUI intervention? (Do you mean you do it _with_ GUI?) pcb -x ps --psfile board.ps board.pcb Ah, that's fine! Unfortunately, it's not mentioned in the documentation anywhere. Only pcb --help shows this usage. BTW: Where can I find a list of color names for the --layer-color-X options? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Tue, May 26, 2009 at 10:24:03AM -0500, Bill Gatliff wrote: Josef Wolf wrote: On Mon, May 25, 2009 at 03:46:00PM -0300, John Coppens wrote: On Mon, 25 May 2009 19:55:23 +0200 Josef Wolf j...@raven.inka.de wrote: - How can I make the breadboard drawing appear light-grey in pcb's postscript output? A trick I've used is to export or print the board to postscript. Then you'll have many pages, one of them the vias alone, and on another the silkscreen. You can then combine both in GIMP and color the vias any color you like. I'd prefer something more scriptable, since I expect to have _lots_ of circuits. But at a first glance, it looks like the ps/eps outputs are easy to postprocess. I wonder if LaTex and pstricks would be useful here? Yeah, that was my original plan: - draw schematics with gschem, export to eps - draw wiring with pcb, export to eps - write description in latex and include the drawings there ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
BTW: Where can I find a list of color names for the --layer-color-X options? They're #RRGGBB hex format. No names. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Josef Wolf wrote: I wonder if LaTex and pstricks would be useful here? Yeah, that was my original plan: - draw schematics with gschem, export to eps - draw wiring with pcb, export to eps - write description in latex and include the drawings there Well, I was thinking along the lines of something that would convert the gschem and pcb files themselves to pstricks, so that you could use all the tools of LaTeX to manage them as documents rather than as images. But after a little more Googling myself (I may need a similar solution soon), I think the following is a more concise answer. I've seen LaTeX scripts that could automate the construction of directed graphs. Seems like it would be straightforward (albeit perhaps nontrivial) to translate a gschem netlist into a graph specification--- and then you could let one of the aforementioned scripts do the actual wiring using colored arcs: http://graphviz.org/ http://dirkraffel.wordpress.com/2007/11/19/include-eps-files-in-latex/ It may turn out that if your circuits are simple enough, you could just specify them in the native language of the graphing program and then skip the gschem step as well. /me shrugs, and apologizes in advance for sending you off in a completely different direction :) b.g. -- Bill Gatliff b...@billgatliff.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
I have this same problem, because I automate my build with makefiles, and I'd like to have a build machine (that doesn't run X) be able to build everything (mostly software, but also PNGs and PDFs of my schematics, along with running DRC, making a netlist, etc.) I did a search for an alternate way around the problem, and found this: http://stackoverflow.com/questions/834723/a-dev-null-equivilent-for-display-when-the-display-is-just-noise I haven't tried it yet, but plan to soon. - Miles On Tue, May 26, 2009 at 9:35 AM, John Doty j...@noqsi.com wrote: On May 26, 2009, at 5:34 AM, Ineiev wrote: On 5/26/09, Josef Wolf j...@raven.inka.de wrote: But scriptability is a concern, though: is it possible to create the ps/eps from a script/Makefile without GUI intervention? (Do you mean you do it _with_ GUI?) pcb -x ps --psfile board.ps board.pcb PCB even does not requires X for this task. BTW I couldn't achieve this with gschem --- it doesn't work from text terminal for me. You can print using the print.scm from a text terminal or script as long as there's an X server for gschem to flash the page on. A minor annoyance, I think. Regards, Ineiev ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ j...@noqsi.com ___ geda-user mailing list geda-user@moria.seul.org 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: Breadboard drawings with pcb?
Bill Gatliff wrote: /me shrugs, and apologizes in advance for sending you off in a completely different direction :) Completing the sabotage: :) http://www.linuxdevcenter.com/pub/a/linux/2004/05/06/graphviz_dot.html b.g. -- Bill Gatliff b...@billgatliff.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Breadboard drawings with pcb?
Hello,
I am about to write an introduction into electronics for kids. This
introduction will also contain small circuits to experiment with. For
building the circuits, I'd use a breadboard like this one:
http://produkt.conrad.de/45973183/steckplatine-eic-108.htm
To draw the schematics, I'd use gschem (obviously). But I wonder how
to create the drawings for placing the components. I'd like to have
the holes and connections of the breadboard be drawn in light-grey. On
top of that, I'd draw the actual components and the paths of the current
in black.
I can think of two ways of doing this:
1. Create the breadboard drawing as a component on its own, so it would be
included into gschem. This method would probably clutter the schematic
with a useless component.
2. Add the breadboard as a drawing into pcb. I've done a little perl
script just to see how this could look like. I've attached the script
below.
Now here are my questions:
- How can I make the breadboard drawing appear light-grey in pcb's
postscript output?
- Is there a way to make pcb aware of the fact that the holes in the
breadboard are connected?
- Any other suggestions?
#! /usr/bin/perl
use strict;
use warnings;
my @texts;
my ($rows, $cols) = (shift, shift);
$rows = 2 unless defined $rows;
$cols = 1 unless defined $cols;
header;
sub text {
my ($x, $y, $text) = @_;
push (@texts, sprintf ('Text[%d %d 0 100 %s ]',
($x*1, $y*1, $text)));
}
for (my $c=0; $c($cols+1)*18; $c+=18) {
if ($c$cols*18) {
my %off=(A=5, B=6, C=7, D=8, E=9,
F=12, G=13, H=14, I=15, J=16);
foreach my $arr (0, $rows*6+3.4) {
foreach my $l (A..J) {
text ($c+$off{$l}-0.12, $arr, $l);
}
}
}
for (my $r=0; $r$rows*6+3; $r++) {
unless (($r-3)%6) {
vbar ($c+1, $r);
vbar ($c+2, $r)
}
if ($c$cols*18) {
hbar ($c+5, $r+1);
hbar ($c+12, $r+1);
foreach my $x (4, 16.5) {
if ($r==1 || $r%5==0) {
text ($c+$x, $r-0.3, $r);
}
}
}
}
}
footer;
sub vbar {
my ($x, $y, $o) = @_;
$x *= 1;
$y *= 1;
print _EOF_;
Element[ vLine5 vLINE5 $x $y 0 0 0 100 ]
(
Pin[0 0 6000 3000 6600 3800 1 1 ]
Pin[0 1 6000 3000 6600 3800 2 2 ]
Pin[0 2 6000 3000 6600 3800 3 3 ]
Pin[0 3 6000 3000 6600 3800 4 4 ]
Pin[0 4 6000 3000 6600 3800 5 5 ]
ElementLine [0 4 0 0 1000]
)
_EOF_
}
sub hbar {
my ($x, $y, $o) = @_;
$x *= 1;
$y *= 1;
print _EOF_;
Element[ hLine5 hLINE5 $x $y 0 0 0 100 ]
(
Pin[0 0 6000 3000 6600 3800 1 1 ]
Pin[1 0 6000 3000 6600 3800 2 2 ]
Pin[2 0 6000 3000 6600 3800 3 3 ]
Pin[3 0 6000 3000 6600 3800 4 4 ]
Pin[4 0 6000 3000 6600 3800 5 5 ]
ElementLine [0 0 4 0 1000]
)
_EOF_
}
sub header {
my $x = $cols*18+3;
my $y = $rows*6+5;
print _EOF_;
FileVersion[20070407]
PCB[ $x $y]
Grid[1.00 0 0 1]
Cursor[0 0 0.00]
PolyArea[2.00]
Thermal[0.50]
DRC[1000 1000 1000 1000 1500 1000]
Flags(nameonpcb,uniquename,clearnew,snappin)
Groups(1,c:2,s:3:4:5:6:7:8)
Styles[Signal,1000,3600,2000,1000:Power,2500,6000,3500,1000:Fat,4000,6000,3500,1000:Skinny,600,2402,1181,600]
_EOF_
}
sub footer {
my $texts = join (\n, , @texts, );
print _EOF_;
Layer(1 component) ( $texts )
Layer(2 solder)( )
Layer(3 GND) ( )
Layer(4 power) ( )
Layer(5 signal1) ( )
Layer(6 signal2) ( )
Layer(7 signal3) ( )
Layer(8 signal4) ( )
Layer(9 silk) ( )
Layer(10 silk) ( )
_EOF_
}
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Hmmm... perhaps you could make the breadboard with vias, lock them, connect them on the solder side, and change the via color to match the far side color? The breadboard wouldn't be an element itself, but a template .pcb file. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, 25 May 2009 19:55:23 +0200 Josef Wolf j...@raven.inka.de wrote: - How can I make the breadboard drawing appear light-grey in pcb's postscript output? A trick I've used is to export or print the board to postscript. Then you'll have many pages, one of them the vias alone, and on another the silkscreen. You can then combine both in GIMP and color the vias any color you like. Some of the silkscreen drawings of the standard components may have to be edited a little for 'aesthetic' purposes. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
For the PCB layout I would make a breadboard footprint (along the lines of the patterns of [1]http://tinyurl.com/5bxzgh ). (* jcl *) -- You can't create open hardware with closed EDA tools. [2]http://www.luciani.org References 1. http://tinyurl.com/5bxzgh 2. http://www.luciani.org/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 02:09:49PM -0400, DJ Delorie wrote: Hmmm... perhaps you could make the breadboard with vias, lock them, connect them on the solder side, and change the via color to match the far side color? Sounds good. There seem to be a couple of drawbacks, though: - The via/solder color from the preference menu is not stored in the .pcb file and is lost when the program is quit - The color setting seems to affect only the GUI. I would like to have the grey style in printouts (eps, included in latex, so it can be printed along with the description and the schematics, resulting in a small book) - The parts of the breadboard traces which are actually used by the circuit should be black instead of grey The breadboard wouldn't be an element itself, but a template .pcb file. How would I specify the template when creating the initial .pcb with gsch2pcb? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 03:46:00PM -0300, John Coppens wrote: On Mon, 25 May 2009 19:55:23 +0200 Josef Wolf j...@raven.inka.de wrote: - How can I make the breadboard drawing appear light-grey in pcb's postscript output? A trick I've used is to export or print the board to postscript. Then you'll have many pages, one of them the vias alone, and on another the silkscreen. You can then combine both in GIMP and color the vias any color you like. I'd prefer something more scriptable, since I expect to have _lots_ of circuits. But at a first glance, it looks like the ps/eps outputs are easy to postprocess. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Josef Wolf wrote: - The color setting seems to affect only the GUI. I would like to have the grey style in printouts (eps, included in latex, so it can be printed along with the description and the schematics, resulting in a small book) Maybe you could use the image in the background feature of pcb. If the grey image was located carefully to align with a grid you could then snap footprints corresponding to connected places onto the breadboard image. That would still leave all the interconnectivity of the breadboard undone though. to get a correct netlist, you would need to add that in a copper layer. - The parts of the breadboard traces which are actually used by the circuit should be black instead of grey some black and some grey is beyond pcb's abilities at the moment -- would be a u-code-it project, or would just be done manually. John Griessen -- Ecosensory Austin TX tinyOS devel on: ubuntu Linux; tinyOS v2.0.2; telosb ecosens1 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 02:52:31PM -0400, John Luciani wrote: For the PCB layout I would make a breadboard footprint (along the lines of the patterns of *http://tinyurl.com/5bxzgh *). Umm, thats not the type of breadboard I am talking about. See, this project is meant to be an introduction to electronics for total beginners. So it should be easy/fast to build and modify the circuits. So the breadboard I am talking about is the type where you push the pins of the components into little holes (organized as 100mil grid) to get them connected. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 5:05 PM, Josef Wolf [1...@raven.inka.de wrote: On Mon, May 25, 2009 at 02:52:31PM -0400, John Luciani wrote: For the PCB layout I would make a breadboard footprint (along the lines of the patterns of *[2]http://tinyurl.com/5bxzgh *). Umm, thats not the type of breadboard I am talking about. See, this project is meant to be an introduction to electronics for total beginners. So it should be easy/fast to build and modify the circuits. So the breadboard I am talking about is the type where you push the pins of the components into little holes (organized as 100mil grid) to get them connected. I realize you are doing a different type of breadboard but the **idea** can be modified to your type of breadboard by changing the arrangement of the pads. Pads having the same number are considered connected. Take a row of square pads (all the same pad number) and connect them with thin rectangular pads (all the same pad number) and you have a connected row. Draw a silkscreen rectangle around the row of pads and you have a picture similar to a bread board row. (* jcl *) You can't create open hardware with closed EDA tools. [3]http://www.luciani.org References 1. mailto:j...@raven.inka.de 2. http://tinyurl.com/5bxzgh 3. http://www.luciani.org/ ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
John Luciani wrote: I realize you are doing a different type of breadboard but the **idea** can be modified to your type of breadboard by changing the arrangement of the pads. Pads having the same number are considered connected. Take a row of square pads (all the same pad number) and connect them with thin rectangular pads (all the same pad number) and you have a connected row. Draw a silkscreen rectangle around the row of pads and you have a picture similar to a bread board row. (* jcl *) Hmmm Maybe one could get the desired some grey some black if used by the way he made footprints. Include some portion of the connectivity of the breadboard, and by putting down footprints, much of the connection to rails would just happen. 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: Breadboard drawings with pcb?
How would I specify the template when creating the initial .pcb with gsch2pcb? You don't. You copy the template to the .pcb, and only use gsch2pcb to *update* it. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
DJ Delorie wrote: How would I specify the template when creating the initial .pcb with gsch2pcb? You don't. You copy the template to the .pcb, and only use gsch2pcb to *update* it. So, if the template was a sea of vias, would footprints be without vias even though they represent legs of components? Their connection points could be pads and the connectivity would work and netlist well. One would just have to get over the way it seems like using through hole parts with surface mount footprints. John Griessen -- 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: Breadboard drawings with pcb?
You'd have to test pcb and see what it does if you overlay a pad on a via, or a pin on a via. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Josef Wolf wrote: Umm, thats not the type of breadboard I am talking about. See, this project is meant to be an introduction to electronics for total beginners. So it should be easy/fast to build and modify the circuits. I think, You want to create figures like this one: http://www.robotika.sk/misc/circuit1.png The picture is taken from the What's a microcontroller book, issued by the Parallax, Inc. and available here: http://www.parallax.com/Portals/0/Downloads/docs/books/edu/wamv2_2.pdf I am afraid, that this type of figures is far beyond the PCB capabilities. Richard Balogh ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 04:08:55PM -0500, John Griessen wrote: Josef Wolf wrote: - The color setting seems to affect only the GUI. I would like to have the grey style in printouts (eps, included in latex, so it can be printed along with the description and the schematics, resulting in a small book) Maybe you could use the image in the background feature of pcb. You mean the method described in http://www.delorie.com/pcb/bg-image.html? That was also my first attempt. But it seems to work only for the GUI, no image on printout. If the grey image was located carefully to align with a grid you could then snap footprints corresponding to connected places onto the breadboard image. That would still leave all the interconnectivity of the breadboard undone though. to get a correct netlist, you would need to add that in a copper layer. Maybe that's not as bad as it sounds. Guess, I'll have to route the traces manually anyway, since footprints on a breadboard are much more flexible than in usual designs. For example, a resistor can span anything from 100mil to 1000mil in any angle :-) - The parts of the breadboard traces which are actually used by the circuit should be black instead of grey some black and some grey is beyond pcb's abilities at the moment -- would be a u-code-it project, or would just be done manually. With the grey part being only a drawing, the routed traces on the component side would overlap the grey drawing and give exactly the desired effect (i think) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
DJ Delorie wrote: You'd have to test pcb and see what it does if you overlay a pad on a via, or a pin on a via. Oh, right. pcb footprints don't keep any traces, just pads, pins. (Yet.) JG ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 11:38:13PM +0200, Richard Balogh wrote: Josef Wolf wrote: Umm, thats not the type of breadboard I am talking about. See, this project is meant to be an introduction to electronics for total beginners. So it should be easy/fast to build and modify the circuits. I think, You want to create figures like this one: http://www.robotika.sk/misc/circuit1.png Yeah, kind of. Although they don't need to be so good-looking as this one. I am afraid, that this type of figures is far beyond the PCB capabilities. Hmm, I have the feeling that with the help of this list, I am already pretty close to the solution: - Use pads (instead of vias) on the solder side to represent the holes - connect them on the solder side with lines - lock pads+lines - fiddle eps output to change the color of the solder side - place parts as usual - use copper on component side for routing. The routes appear black in the printout Have I missed something? ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, May 25, 2009 at 05:57:52PM -0400, DJ Delorie wrote: You'd have to test pcb and see what it does if you overlay a pad on a via, or a pin on a via. So why not use pads instead of vias? Pads on solder side would represent the holes in the breadboard and special footprints with pads instead of pins for the components. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Vias connect the two sides, so you can test for connectivity. That's all I was thinking. If connectivity can be done another way, then you have other options. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
Josef Wolf wrote: Hmm, I have the feeling that with the help of this list, I am already pretty close to the solution: - Use pads (instead of vias) on the solder side to represent the holes - connect them on the solder side with lines - lock pads+lines - fiddle eps output to change the color of the solder side - place parts as usual - use copper on component side for routing. The routes appear black in the printout Have I missed something? It sounds like you will have a grey solder side layer, so the pads will only be on one side at all -- routes that the netlister and drc checks use need to be on the same side as the pads. So, if you do not use vias your black to grey change to .ps output can't be for the whole side, that would get the pads, (connected to the routing), and the routing. all would be grey. I think that is ready for some testing. One thing you could do with your template .pcb drawing is include some trace segments of the right lengths to align well as part of a copyable library of parts for students to use. That is, if they are going to be doing layout. So try what DJ mentioned. Test if connectivity is made by overlapping a footprint pad on a via without creating errors or not allowing it. If there is a trouble with that, each component will have to have some trace attached to each pad also and the trace makes the netlist connectivity as usual. vias connect to the other side and allow easy grey postprocessing of .ps other side output. John -- Ecosensory Austin TX tinyOS devel on: ubuntu Linux; tinyOS v2.0.2; telosb ecosens1 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Breadboard drawings with pcb?
On Mon, 25 May 2009 22:58:26 +0200 Josef Wolf j...@raven.inka.de wrote: I'd prefer something more scriptable, since I expect to have _lots_ of circuits. But at a first glance, it looks like the ps/eps outputs are easy to postprocess. If you want publishing (printing) quality output, you'll have to pass through ps anyway. There are a lot of utilities on the 'net that let you combine ps outputs in many ways, using command line utilities. John ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
