gEDA-user: let's play guess the netlist with gsch2pcb!
This caught me out today. Consider this circuit: http://vivara.net/images/gschem_example.png The symbols are from the standard library, specifically: /usr/local/share/gEDA/sym/analog/resistor-1.sym /usr/local/share/gEDA/sym/power/generic-power.sym Anyone want to guess what gsch2pcb will make of the netlist? Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Feb 17, 2010, at 12:35 PM, Mark Rages wrote: This caught me out today. Consider this circuit: http://vivara.net/images/gschem_example.png The symbols are from the standard library, specifically: /usr/local/share/gEDA/sym/analog/resistor-1.sym /usr/local/share/gEDA/sym/power/generic-power.sym Anyone want to guess what gsch2pcb will make of the netlist? With the trickery your implying. and without seeing the other attributes. im guessing V5 R1:1, R1:2 or something like that Steve ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Wed, Feb 17, 2010 at 2:49 PM, Steven Michalske smichal...@gmail.com wrote: On Feb 17, 2010, at 12:35 PM, Mark Rages wrote: This caught me out today. Consider this circuit: http://vivara.net/images/gschem_example.png The symbols are from the standard library, specifically: /usr/local/share/gEDA/sym/analog/resistor-1.sym /usr/local/share/gEDA/sym/power/generic-power.sym Anyone want to guess what gsch2pcb will make of the netlist? With the trickery your implying. and without seeing the other attributes. im guessing V5 R1:1, R1:2 or something like that You are close: it's a one-line answer. I just clicked on the visible net= attributes on the power symbols and edited them, then added the footprint= attribute to the resistor. I will attach the schematic to this message. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com untitled.sch Description: application/geda-schematic ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
here is what i got V3 R1-1 V5 R1-2 with gsch2pcb --version gsch2pcb 1.6 On Feb 17, 2010, at 12:56 PM, Mark Rages wrote: untitled.sch ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Wed, Feb 17, 2010 at 3:59 PM, Steven Michalske smichal...@gmail.com wrote: here is what i got V3 R1-1 V5 R1-2 with gsch2pcb --version gsch2pcb 1.6 OK, here is what I get: Vcc R1-1 R1-2 also with gsch2pcb --version gsch2pcb 1.6 I don't think there's anything too weird in my Ubuntu 9.04 system. I just created a new user and ran from that account, with the same result. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Thu, Feb 18, 2010 at 8:59 AM, Steven Michalske smichal...@gmail.com wrote: here is what i got V3 R1-1 V5 R1-2 with gsch2pcb --version gsch2pcb 1.6 Ditto. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Wednesday 17 February 2010 22:07:29 Mark Rages wrote: On Wed, Feb 17, 2010 at 3:59 PM, Steven Michalske smichal...@gmail.com wrote: here is what i got V3 R1-1 V5 R1-2 with gsch2pcb --version gsch2pcb 1.6 OK, here is what I get: Vcc R1-1 R1-2 also with gsch2pcb --version gsch2pcb 1.6 I don't think there's anything too weird in my Ubuntu 9.04 system. I just created a new user and ran from that account, with the same result. Please run gschlas -e filename.sch and post the result to the list. 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: let's play guess the netlist with gsch2pcb!
Please run gschlas -e filename.sch and post the result to the list.
Thanks,
cat untitled.sch~
v 20090328 2
C 4 4 0 0 0 title-B.sym
C 47800 46400 1 0 0 resistor-1.sym
{
T 48100 46800 5 10 0 0 0 0 1
device=RESISTOR
T 48000 46700 5 10 1 1 0 0 1
refdes=R1
T 47600 46200 5 10 1 0 0 0 1
footprint=0805
}
C 47300 46800 1 0 0 generic-power.sym
{
T 47500 47050 5 10 1 1 0 3 1
net=V3:1
}
C 48800 46800 1 0 0 generic-power.sym
{
T 49000 47050 5 10 1 1 0 3 1
net=V5:1
}
N 47500 46800 47500 46500 4
N 47500 46500 47800 46500 4
N 48700 46500 49000 46500 4
N 49000 46500 49000 46800 4
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Wed, Feb 17, 2010 at 4:16 PM, Peter TB Brett pe...@peter-b.co.uk wrote: On Wednesday 17 February 2010 22:07:29 Mark Rages wrote: On Wed, Feb 17, 2010 at 3:59 PM, Steven Michalske smichal...@gmail.com wrote: here is what i got V3 R1-1 V5 R1-2 with gsch2pcb --version gsch2pcb 1.6 OK, here is what I get: Vcc R1-1 R1-2 also with gsch2pcb --version gsch2pcb 1.6 I don't think there's anything too weird in my Ubuntu 9.04 system. I just created a new user and ran from that account, with the same result. Please run gschlas -e filename.sch and post the result to the list. Here it is. Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com untitled-e.sch Description: application/geda-schematic ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Wednesday 17 February 2010 22:19:43 Geoff Swan wrote: Please run gschlas -e filename.sch and post the result to the list. Thanks, cat untitled.sch~ [snip] Hi Geoff, You didn't actually post the embedded schematic. In any case, yours appears to be working correctly, so... :-) 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: let's play guess the netlist with gsch2pcb!
On Wednesday 17 February 2010 22:20:26 Mark Rages wrote: On Wed, Feb 17, 2010 at 4:16 PM, Peter TB Brett pe...@peter-b.co.uk wrote: On Wednesday 17 February 2010 22:07:29 Mark Rages wrote: I don't think there's anything too weird in my Ubuntu 9.04 system. I just created a new user and ran from that account, with the same result. Please run gschlas -e filename.sch and post the result to the list. Here it is. Hmm... looks like an attribute promotion problem -- note that the Vcc net= attributes are still present in the symbol, but should be overridden by the attributes in the schematic. Here's my netlist, using gnetlist -g geda: ## START header gEDA's netlist format Created specifically for testing of gnetlist END header START components R1 device=RESISTOR END components START renamed-nets END renamed-nets START nets V5 : R1 2 V3 : R1 1 END nets ## Please follow the following steps: (1) move or rename your personal gnetlistrc and gafrc files (in $HOME/.gEDA). (2) move your testcase to a directory without gnetlistrc or gafrc files. (3) run gnetlist -i -v filename.sch (please use the embedded one) (4) post the output. 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: let's play guess the netlist with gsch2pcb!
On Wed, Feb 17, 2010 at 4:35 PM, Peter TB Brett pe...@peter-b.co.uk wrote: On Wednesday 17 February 2010 22:20:26 Mark Rages wrote: On Wed, Feb 17, 2010 at 4:16 PM, Peter TB Brett pe...@peter-b.co.uk wrote: On Wednesday 17 February 2010 22:07:29 Mark Rages wrote: I don't think there's anything too weird in my Ubuntu 9.04 system. I just created a new user and ran from that account, with the same result. Please run gschlas -e filename.sch and post the result to the list. Here it is. Hmm... looks like an attribute promotion problem -- note that the Vcc net= attributes are still present in the symbol, but should be overridden by the attributes in the schematic. Here's my netlist, using gnetlist -g geda: ## START header gEDA's netlist format Created specifically for testing of gnetlist END header START components R1 device=RESISTOR END components START renamed-nets END renamed-nets START nets V5 : R1 2 V3 : R1 1 END nets ## Please follow the following steps: (1) move or rename your personal gnetlistrc and gafrc files (in $HOME/.gEDA). (2) move your testcase to a directory without gnetlistrc or gafrc files. (3) run gnetlist -i -v filename.sch (please use the embedded one) (4) post the output. OK, I created a new user with an empty home directory. t...@midwesttelecine:~$ gnetlist -i -v untitled.sch gEDA/gnetlist version 1.5.2.20090328 gEDA/gnetlist comes with ABSOLUTELY NO WARRANTY; see COPYING for more details. This is free software, and you are welcome to redistribute it under certain conditions; please see the COPYING file for more details. Loading schematic [/home/test/untitled.sch] -- Verbose mode legend n : Found net C : Found component (staring to traverse component) p : Found pin (starting to traverse pin / or examining pin) P : Found end pin connection (end of this net) R : Starting to rename a net v : Found source attribute, traversing down ^ : Finished underlying source, going back up u : Found a refdes which needs to be demangle U : Found a connected_to refdes which needs to be demangle -- - Starting internal netlist creation C CpnnnPpnnnP CpnnnP CpnnnP DONE - Staring post processing - Naming nets: pnpnpnpn DONE - Renaming nets: DONE - Resolving hierarchy: DONE DONE - Staring post processing - Naming nets of graphical objects: DONE Internal netlist representation: component R1 pin 1 (1) Vcc R1 1 [538] pin 2 (2) Vcc R1 2 [533] component SPECIAL pin 1 (1) Null net name R1 1 [538] component SPECIAL pin 1 (1) Null net name R1 2 [533] gnetlist -- Mark Rages, Engineer Midwest Telecine LLC markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Wednesday 17 February 2010 22:41:07 Mark Rages wrote: OK, I created a new user with an empty home directory. t...@midwesttelecine:~$ gnetlist -i -v untitled.sch gEDA/gnetlist version 1.5.2.20090328 I'm sorry Mark: I've compiled and installed 1.5.2, and I still can't reproduce this issue... ## C CpnnnPpnnnP CpnnnP CpnnnP DONE - Staring post processing - Naming nets: pnpnpnpn DONE - Renaming nets: DONE - Resolving hierarchy: DONE DONE - Staring post processing - Naming nets of graphical objects: DONE Internal netlist representation: component R1 pin 1 (1) V3 R1 1 [538] pin 2 (2) V5 R1 2 [533] component SPECIAL pin 1 (1) Null net name R1 1 [538] component SPECIAL pin 1 (1) Null net name R1 2 [533] ## Smarter minds than mine are needed here, I fear! 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: let's play guess the netlist with gsch2pcb!
On Wed, 2010-02-17 at 22:56 +, Peter TB Brett wrote:
On Wednesday 17 February 2010 22:41:07 Mark Rages wrote:
OK, I created a new user with an empty home directory.
t...@midwesttelecine:~$ gnetlist -i -v untitled.sch
gEDA/gnetlist version 1.5.2.20090328
I'm sorry Mark: I've compiled and installed 1.5.2, and I still can't
reproduce
this issue...
Are you 100% sure you are picking up the right libgeda / gnetlist?
which gnetlist
ldd `which gnetlist`
This strikes of a bug which was fixed long ago in the 1.5.x series.
commit e869033324d7595cc11d42007109a605823e1640
Author: Peter Clifton pc...@cam.ac.uk
Date: Mon Aug 17 12:01:24 2009 +0100
gnetlist: Fix problem with attached net attribute not being honored.
Bug tracked down and fix proposed by Robert Fitzsimons.
Seems to be an artifact introduced by the change to use the new
attrib API (b4996e267b5d9696f7e8122c40b31482ef852904).
Signed-off-by: Peter Clifton pc...@cam.ac.uk
Tested-by: Robert Fitzsimons robf...@273k.net
diff --git a/gnetlist/src/s_netattrib.c b/gnetlist/src/s_netattrib.c
index b813869..8c7d6c9 100644
--- a/gnetlist/src/s_netattrib.c
+++ b/gnetlist/src/s_netattrib.c
@@ -279,7 +279,7 @@ char *s_netattrib_net_search (OBJECT * o_current, char *want
start_of_pinlist = char_ptr + 1;
current_pin = strtok (start_of_pinlist, DELIMITERS);
-while (current_pin !return_value) {
+while (current_pin) {
if (strcmp (current_pin, wanted_pin) == 0) {
g_free (return_value);
return net_name;
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Feb 17, 2010, at 3:56 PM, Peter TB Brett wrote: I'm sorry Mark: I've compiled and installed 1.5.2, and I still can't reproduce Mark: post your gafrc. 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: let's play guess the netlist with gsch2pcb!
Ah! On Wed, Feb 17, 2010 at 5:05 PM, Peter Clifton [1]pc...@cam.ac.uk wrote: On Wed, 2010-02-17 at 22:56 +, Peter TB Brett wrote: On Wednesday 17 February 2010 22:41:07 Mark Rages wrote: OK, I created a new user with an empty home directory. t...@midwesttelecine:~$ gnetlist -i -v untitled.sch gEDA/gnetlist version 1.5.2.20090328 ... Date: Mon Aug 17 12:01:24 2009 +0100 ^^ Regards, Mark markra...@gmail -- Mark Rages, Engineer Midwest Telecine LLC [2]markra...@midwesttelecine.com References 1. mailto:pc...@cam.ac.uk 2. mailto:markra...@midwesttelecine.com ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: let's play guess the netlist with gsch2pcb!
On Wed, 2010-02-17 at 17:11 -0600, Mark Rages wrote: Ah! On Wed, Feb 17, 2010 at 5:05 PM, Peter Clifton [1]pc...@cam.ac.uk wrote: On Wed, 2010-02-17 at 22:56 +, Peter TB Brett wrote: On Wednesday 17 February 2010 22:41:07 Mark Rages wrote: OK, I created a new user with an empty home directory. t...@midwesttelecine:~$ gnetlist -i -v untitled.sch gEDA/gnetlist version 1.5.2.20090328 ... Date: Mon Aug 17 12:01:24 2009 +0100 ^^ DOH.. You confused me in your second post with this: gsch2pcb --version gsch2pcb 1.6 Apparently, the gsch2pcb versioning is separate to the rest of the suite! Upgrade to 1.6.1 and all will be shiny. Best wishes, Peter C. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
