gEDA-user: Symbol creation
Hi! The included symbol looses its attributes when opened in a gschem window (when I look at main menue EDIT/EDIT) with some other symbols. The symbols from the default libraries do not loose its attributes. Thank you for your kindly treatment to my newbie problems. ostene pgnd-1.sym Description: application/geda-symbol ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Symbol creation
On Fri, 2010-09-24 at 12:30 +0200, Östen Einarsson wrote: Hi! The included symbol looses its attributes when opened in a gschem window (when I look at main menue EDIT/EDIT) with some other symbols. The symbols from the default libraries do not loose its attributes. Thank you for your kindly treatment to my newbie problems. ostene That is NOT a symbol for gschem/gEDA. That file contains a pin, some lines... There is no line starting with C which is the beginning of a Symbol/Component. See http://geda.seul.org/wiki/geda:file_format_spec#component For making symbols I prefer tools like tragesym or djboxsym or similar, these tools give you fine symbols, which can be modified/tuned by gschem. Making new symbols from scratch with gschem may be difficult, I have never done that. Best regards Stefan Salewski ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Symbol creation
Stefan Salewski wrote: That is NOT a symbol for gschem/gEDA. That file contains a pin, some lines... There is no line starting with C which is the beginning of a Symbol/Component. Sorry, that was nonsense, the lines starting with C belongs in the schematic files, not in the sym files. I am still learning the gEDA file format... But my recommendation using tragesym or djboxsym still holds. ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Symbol creation
On Fri, 2010-09-24 at 14:22 +0200, Stefan Salewski wrote:
Stefan Salewski wrote:
That is NOT a symbol for gschem/gEDA.
That file contains a pin, some lines...
There is no line starting with C which is the beginning of a
Symbol/Component.
Sorry, that was nonsense, the lines starting with C belongs in the
schematic files, not in the sym files. I am still learning the gEDA file
format...
But my recommendation using tragesym or djboxsym still holds.
If we compare yours with lm741-1.sym we see that you have refdes inside
of pin, but it should be outside.
ste...@amd64x2 ~ $ cat /usr/share/gEDA/sym/linear/lm741-1.sym attachment.sym
v 20031231 1
T 625 950 8 8 0 0 0 0 1
device=LM741
T 225 350 9 8 1 0 0 0 1
LM741
T 200 900 8 10 1 1 0 0 1
refdes=U?
P 200 200 0 200 1 0 1
{
T 50 225 5 8 1 1 0 0 1
pinnumber=2
T 50 225 5 8 0 0 0 0 1
pinseq=2
}
P 200 600 0 600 1 0 1
{
T 50 625 5 8 1 1 0 0 1
pinnumber=3
T 50 625 5 8 0 0 0 0 1
pinseq=3
}
P 500 200 500 0 1 0 1
{
T 525 50 5 8 1 1 0 0 1
pinnumber=4
T 525 50 5 8 0 0 0 0 1
pinseq=4
}
P 800 400 1000 400 1 0 1
{
T 875 425 5 8 1 1 0 0 1
pinnumber=6
T 875 425 5 8 0 0 0 0 1
pinseq=6
}
P 500 600 500 800 1 0 1
{
T 550 675 5 8 1 1 0 0 1
pinnumber=7
T 550 675 5 8 0 0 0 0 1
pinseq=7
}
L 200 800 200 0 3 0 0 0 -1 -1
L 800 400 200 800 3 0 0 0 -1 -1
L 300 650 300 550 3 0 0 0 -1 -1
L 250 600 350 600 3 0 0 0 -1 -1
L 250 200 350 200 3 0 0 0 -1 -1
L 800 400 200 0 3 0 0 0 -1 -1
v 20091004 2
L 400 800 1000 800 3 0 0 0 -1 -1
L 500 700 900 700 3 0 0 0 -1 -1
L 600 600 800 600 3 0 0 0 -1 -1
P 700 1100 700 800 1 0 0
{
T 700 1100 5 10 0 0 0 0 1
pintype=pwr
T 505 500 5 10 0 1 180 6 1
pinlabel=PGND
T 605 1050 5 10 1 1 180 0 1
pinnumber=1
T 700 1100 5 10 0 0 0 0 1
pinseq=1
T 400 400 5 10 1 1 0 0 1
device=PGND
T 600 1200 5 10 1 1 0 0 1
refdes=P?
}
___
geda-user mailing list
geda-user@moria.seul.org
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Symbol creation
Östen Einarsson wrote:
The included symbol looses its attributes when opened
in a gschem window (when I look at main menue EDIT/EDIT)
with some other symbols.
All attributes in your pgnd.sym file, are associated with the pin. They are
within the pin environment given by curly brackets. Probably they got there
because you selected the pin, typed EE and added the attributes in the
attribute editor. In a sense, your symbol does not loose attributes, but
does not contain any, in the first place.
Attributes of the whole symbol should reside outside any environment. Use
the action Add_Attribute from the Add menu to add them to the symbol.
Shortcut is aa.
Some more notes on your symbol:
* A power symbol needs a net attribute to work as expected.
In your case, it should probably be
net=PGND:1
* A refdes attribute on a power symbol does not make much sense. Power
symbols don't translate to specific footprints in the layout. The symbol
does not represent a physical component.
* The pin number attribute should probably not be visible.
* The pin label and the pin number attributes are rotated by 180 degrees.
There is some evil magic in gschem that prevents them to render upside-down.
Still, there is a difference to upright orientation: The mark of the text
sits on the opposite side of the text. This makes it difficult to align the
text with other strings. My recommendation: Avoid 180° rotation in symbols.
* Your symbol is pretty large -- about three times the size of the power
symbols in the default library. Is this deliberate?
---)kaimartin(---
PS:
/your symbol file with comments by me--
# The version of gschem the symbol was created with
v 20091004 2
# three line statements
L 400 800 1000 800 3 0 0 0 -1 -1
L 500 700 900 700 3 0 0 0 -1 -1
L 600 600 800 600 3 0 0 0 -1 -1
# a pin statement. The attributes of the pin follow in curly brackets
P 700 1100 700 800 1 0 0
{
T 700 1100 5 10 0 0 0 0 1
pintype=pwr
# The pinlabel and the pinnumber are rotated by 180 degrees
T 505 500 5 10 0 1 180 6 1
pinlabel=PGND
T 605 1050 5 10 1 1 180 0 1
pinnumber=1
T 700 1100 5 10 0 0 0 0 1
pinseq=1
# The device attribute is inside the pin environment
T 400 400 5 10 1 1 0 0 1
device=PGND
T 600 1200 5 10 1 1 0 0 1
refdes=P?
}
\---
--
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
gEDA-user: Symbol creation
Here is a symbol I have just created. It is for what Littlefuse / Teccor calls a quadrac which is just a Triac with its own internal trigger Diac. If some possibly interested party would be so kind as to have a look at this little guy, and notify me of any grievous errors; I would be much obliged. Feel free to upload it to gedasymbols if it passes muster. One thing, I made it by copying the symbol for a triac. I did not pay careful attention to pin numbering. Am I going to regret that if I ever decide to do a layout / make a PCB? Here is a link to the dox: http://www.littelfuse.com/data/en/Data_Sheets/Littelfuse_Thyristor_QLTx.pdf -Cullen quadrac.sym Description: application/geda-symbol ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: Symbol creation
One thing, I made it by copying the symbol for a triac. I did not pay careful attention to pin numbering. Am I going to regret that if I ever decide to do a layout / make a PCB? I guess that depends if you got the numbering wrong :P ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: symbol creation - unconnected pin
On Mon, 2007-09-24 at 08:59 +0530, Ramakrishnan Muthukrishnan wrote: Hi, I am trying to create a gschem symbol for an Opamp IC. One of the pins on that IC is usually unconnected, so I didn't have a pin for it in the gschem symbol. But I get a warning from gsymcheck saying tha the number of pins on the symbol and the footprint does not match. How do I insert a pin which is invisible from gschem, but is physically in there? You can't, just ignore the warning from gsymcheck. It is not harmful, just urges you to check you meant what you drew. -- 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!) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: symbol creation
I have followed gEDA/gaf Symbol Creation Documents. After saving the new symbol, when I wish to place it in gschem, it is placed with the whole title-B area. What did I missed? thanks in advance. Yaniv ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: symbol creation
On Tue, 2008-05-13 at 06:39 -0700, Yanivh. wrote: I have followed gEDA/gaf Symbol Creation Documents. After saving the new symbol, when I wish to place it in gschem, it is placed with the whole title-B area. What did I missed? When you're creating a symbol, you need to delete the title block before you symbol translate and save. See the recent geda-user thread: Removing default title box. (Ok guys, I can grant that New-Symbol might be a case where we don't want to include a title block). At the risk of taking this thread off-topic, what about this.. /usr/share/gEDA/default_page.sch (and the various local overrides). Make gschem File-New load that. It is more discoverable, as we could include a menu item Page-Edit Default page or some such. This is a step away from a free-selection of templates, but given gschem doesn't treat title-blocks specially (they are just symbols), template schematic files are probably the best way to implement this. Best regards. -- 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!) ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
Re: gEDA-user: symbol creation
On May 13, 2008, at 9:08 AM, Peter Clifton wrote: On Tue, 2008-05-13 at 06:39 -0700, Yanivh. wrote: I have followed gEDA/gaf Symbol Creation Documents. After saving the new symbol, when I wish to place it in gschem, it is placed with the whole title-B area. What did I missed? When you're creating a symbol, you need to delete the title block before you symbol translate and save. See the recent geda-user thread: Removing default title box. (Ok guys, I can grant that New-Symbol might be a case where we don't want to include a title block). At the risk of taking this thread off-topic, what about this.. /usr/share/gEDA/default_page.sch (and the various local overrides). I like that a lot. Solves several problems with the current approach: the default may differ between projects, and the current code doesn't promote attributes. Make gschem File-New load that. It is more discoverable, as we could include a menu item Page-Edit Default page or some such. But that gets you back to the same problem we have with symbols: when you customize anything from the standard installation, you should be working on a project-local copy, not the installation's copy. This is a step away from a free-selection of templates, but given gschem doesn't treat title-blocks specially (they are just symbols), template schematic files are probably the best way to implement this. Best regards. -- 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!) ___ 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/ [EMAIL PROTECTED] ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
gEDA-user: symbol creation - unconnected pin
Hi, I am trying to create a gschem symbol for an Opamp IC. One of the pins on that IC is usually unconnected, so I didn't have a pin for it in the gschem symbol. But I get a warning from gsymcheck saying tha the number of pins on the symbol and the footprint does not match. How do I insert a pin which is invisible from gschem, but is physically in there? Ramakrishnan ___ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
