Re: gEDA-user: Creating new symbols
Stefan Salewski wrote: Following the documentation we always have to do the translation to 0/0, when we save a symbol. Yes, the documentation is a bit too rigorous at this point. The only consequence of a symbol not translated to 0/0 is a potential inconvenience on placement. The symbol may be offset from the mouse cursor. ---)kaimartin(--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=getsearch=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Creating new symbols
Stefan Salewski wrote: And that is a real problem. gschem should really be able to to this automatically when saving symbols. IMHO, it should not. Every translation breaks instances of the symbol in existing schematics. A better solution would be the notion of an origin, similar to the diamond in pcb footprints. ---)kaimartin(--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=getsearch=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Creating new symbols
Den 2010-12-24 22:16:18 skrev Stephan Boettcher boettc...@physik.uni-kiel.de: Johnny Rosenberg gurus.knu...@gmail.com writes: At http://www.geda.seul.org/wiki/geda:gsch2pcb_tutorial the following is written: ”When all the edits are done, it's very important when editing symbols to do a Edit→Symbol Translate to zero before saving. Do that and then save the symbol with File→Save Page” My problem is that there is no ”Save Page” in the File menu. File-Save But first it is important to recognize that there is a difference between editing a symbol, and editing a schematic with a symbal instance and instance attributes. Until now we were talking about editing a symbol instance in a schematic. To make a new symbol version, you must open the symbol file itself. You can do that by selcting the symbol in a schematic and do Hierachy-Down Symbol (Shift-H s) You will discover, that the symbol still has no value attibute. You can add it in the symbol file. The value attribute must be promoted when the symbol is instantiated. There are (not so?) complex rules which attibutes get promoted, and which not. I think, a visible, unattached attribute, called _value_ will be promoted. N.B., this is a dark side of gschem in my oppinion. Which attibutes get promoted should be defined in the symbols, independently of visibility or any strange configuration settings. After adding the attibute, value=? with proper placement and alignment, you can do File-Save_As to save the new symbol in your own symbol collection. Edit-Symbol_Translate will probably not be required, if you just do a minor modification to an existing symbol. Then you go back to your schematic, Hierachy-Up (Shift-H u) and delete the old symbol instance, and replace it with an instance of your own. How to reload the available symbols from a running gschem? I don't know. Usually I restart gschem, to reread the available symbols. You'll first need to add the location of your own symbol collection to the search path in .gafrc or something. Thanks for the information, I'll try that later; hopefully it will work. By the way, when you say ”Shift-H”, you really mean Shift+h, or just H, right? Because H is already ”shifted”, and I guess you don't mean Shift+Shift+h (which is a possible key combination since there are two shift keys on at least my keyboard). Well, I guess I can test that myself, on the other hand… -- Kind regards Johnny Rosenberg ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Creating new symbols
On Sat, 2010-12-25 at 09:17 +0100, kai-martin knaak wrote: Stefan Salewski wrote: And that is a real problem. gschem should really be able to to this automatically when saving symbols. IMHO, it should not. Every translation breaks instances of the symbol in existing schematics. A better solution would be the notion of an origin, similar to the diamond in pcb footprints. ---)kaimartin(--- Hm... Following the documentation we always have to do the translation to 0/0, when we save a symbol. When we really have to do it always, it can and should be done automatically. Indeed, I can remember that I onece forgot that translation, got a broken symbol with pins not aligned to 100 multiples of grid and start symbol creation again from scratch, because I was not sure how to fix it after storing to disk. But I have never really investigated this step. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: Creating new symbols
At http://www.geda.seul.org/wiki/geda:gsch2pcb_tutorial the following is written: ”When all the edits are done, it's very important when editing symbols to do a Edit→Symbol Translate to zero before saving. Do that and then save the symbol with File→Save Page” My problem is that there is no ”Save Page” in the File menu. -- Kind regards Johnny Rosenberg ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Creating new symbols
Johnny Rosenberg gurus.knu...@gmail.com writes: At http://www.geda.seul.org/wiki/geda:gsch2pcb_tutorial the following is written: ”When all the edits are done, it's very important when editing symbols to do a Edit→Symbol Translate to zero before saving. Do that and then save the symbol with File→Save Page” My problem is that there is no ”Save Page” in the File menu. File-Save But first it is important to recognize that there is a difference between editing a symbol, and editing a schematic with a symbal instance and instance attributes. Until now we were talking about editing a symbol instance in a schematic. To make a new symbol version, you must open the symbol file itself. You can do that by selcting the symbol in a schematic and do Hierachy-Down Symbol (Shift-H s) You will discover, that the symbol still has no value attibute. You can add it in the symbol file. The value attribute must be promoted when the symbol is instantiated. There are (not so?) complex rules which attibutes get promoted, and which not. I think, a visible, unattached attribute, called _value_ will be promoted. N.B., this is a dark side of gschem in my oppinion. Which attibutes get promoted should be defined in the symbols, independently of visibility or any strange configuration settings. After adding the attibute, value=? with proper placement and alignment, you can do File-Save_As to save the new symbol in your own symbol collection. Edit-Symbol_Translate will probably not be required, if you just do a minor modification to an existing symbol. Then you go back to your schematic, Hierachy-Up (Shift-H u) and delete the old symbol instance, and replace it with an instance of your own. How to reload the available symbols from a running gschem? I don't know. Usually I restart gschem, to reread the available symbols. You'll first need to add the location of your own symbol collection to the search path in .gafrc or something. -- Stephan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Creating new symbols
On Fri, 2010-12-24 at 22:24 +0100, Stefan Salewski wrote: On Fri, 2010-12-24 at 22:16 +0100, Stephan Boettcher wrote: File-Save But first it is important Some of your fine explanations may be already at http://geda.seul.org/wiki/geda:gschem_symbol_creation More is here: http://geda.seul.org/wiki/geda:faq-gschem#gschem_symbols And how we can use our own libraries may be explained here: http://geda.seul.org/wiki/geda:faq-gschem#gschem_configuration_customization Really not too bad. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Creating new symbols
On Fri, 2010-12-24 at 20:34 +0100, Johnny Rosenberg wrote: At http://www.geda.seul.org/wiki/geda:gsch2pcb_tutorial the following is written: ”When all the edits are done, it's very important when editing symbols to do a Edit→Symbol Translate to zero before saving. And that is a real problem. gschem should really be able to to this automatically when saving symbols. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: creating new symbols
Hi,
I encountered a segfault trying to connect a net to my shiny little
newly created symbol (attached below). I created a few symbols,
only one of those is causing a segfault (gschem from ubuntu 10.10 repos).
I would be grateful for pointing out the error in creating this symbol
Michal Dwuznik
mic...@jabberwocky:~/pcb$ cat LM1108SF33-1.sym
v 20100214 2
B 200 300 1400 1000 3 0 0 0 -1 -1 0 -1 -1 -1 -1 -1
N 200 1100 0 1100 1
{
T 0 900 5 10 0 1 0 0 1
pinnumber=2
T 300 900 5 10 1 1 0 0 1
pinseq=2
T 300 1100 9 10 1 1 0 0 1
pinlabel=Vin
T 0 1200 5 8 0 1 0 0 1
pintype=in
}
N 1800 1100 1600 1100 1
{
T 1400 900 5 10 1 1 0 0 1
pinnumber=3
T 1900 900 5 10 0 1 0 0 1
pinseq=3
T 1100 1100 9 10 1 1 0 0 1
pinlabel=Vout
T 1700 1200 5 8 0 1 0 0 1
pintype=out
}
N 900 300 900 0 1
{
T 700 400 5 10 1 1 0 0 1
pinnumber=1
T 1000 100 5 10 0 1 0 0 1
pinseq=1
T 900 400 9 10 1 1 0 0 1
pinlabel=GND
T 600 200 5 8 0 1 0 0 1
pintype=pwr
}
T 200 1400 9 10 0 1 0 0 1
devicename=LM1108SF-3.3
T 200 1800 9 10 0 1 0 0 1
description=LM1108
T 200 1600 9 10 0 1 0 0 1
footprint=SOT23
T 200 0 8 10 1 1 0 0 1
refdes=U?
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: creating new symbols
Micha? Dwu?nik wrote:
mic...@jabberwocky:~/pcb$ cat LM1108SF33-1.sym
v 20100214 2
B 200 300 1400 1000 3 0 0 0 -1 -1 0 -1 -1 -1 -1 -1
N 200 1100 0 1100 1
This is a net, not a pin. Pin definition lines start with the letter P.
{
T 0 900 5 10 0 1 0 0 1
pinnumber=2
T 300 900 5 10 1 1 0 0 1
pinseq=2
T 300 1100 9 10 1 1 0 0 1
pinlabel=Vin
T 0 1200 5 8 0 1 0 0 1
pintype=in
}
N 1800 1100 1600 1100 1
^
Again a net, not a pin.
You can add pins in the gschem GUI with
Add - Pin
The accel of this command is [ap].
---)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: creating new symbols
On Mon, Nov 29, 2010 at 16:29, Kai-Martin Knaak kn...@iqo.uni-hannover.de wrote: Micha? Dwu?nik wrote: mic...@jabberwocky:~/pcb$ cat LM1108SF33-1.sym v 20100214 2 B 200 300 1400 1000 3 0 0 0 -1 -1 0 -1 -1 -1 -1 -1 N 200 1100 0 1100 1 This is a net, not a pin. Pin definition lines start with the letter P. Thank you, red squares helped : On the other hand - there's no visible clue in case of such error - segfault does not seem very elegant... M. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: creating new symbols
On Mon, 29 Nov 2010 19:34:36 +0100 Michał Dwużnik michal.dwuznik-re5jqeeqqe8avxtiumw...@public.gmane.org wrote: there's no visible clue in case of such error - segfault does not seem very elegant... You should file a bug report on SF project page. gEDA should not crash. Levente -- Levente Kovacs http://levente.logonex.eu ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: creating new symbols
Levente Kovacs wrote: You should file a bug report on SF project page. gEDA should not crash. This minimum example of a net in a symbol file that shows the same symptoms: /---net_crash.sym v 20100214 2 N 200 0 0 0 1 \ To reproduce: 1) put the file in the local project dir 2) open gschem 3) add the minimum symbol to the schematic 4) try to start a horizontal net at one of red squares gschem segfaults when the mouse cursor starts to move sideways. Vertical nets connect fine. However, if the symbol is rotated by 90°, it is the vertical nets that make gschem go belly up. I guess, the segfaulting piece of code is located in the procedure that tries to unite straight segments of nets. ---)kaimartin(--- -- Kai-Martin Knaak Öffentlicher PGP-Schlüssel: http://pgp.mit.edu:11371/pks/lookup?op=getsearch=0x6C0B9F53 ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
