Re: gEDA-user: Hi.... first post

[Dan McMahill <dan@xxxxxxxxxxxx>]

Stuart Brorson wrote:

> On Thu, 15 Mar 2007, C P Tarun wrote:
>
> > Can any of you please help me with this question? Why didn't
> > the .cmd file work?
> >
> > Tarun

see below

> > Guys,
> >
> > Can you please help me with one part of my original question?
> >
> > > 1.  When I load the netlist into the PCB program, it gives errors
> > >     saying that it couldn't find pins with the names given in the
> > >     footprints, or some such thing. Just try loading my .pcb file
> > >     first, then try loading the netlist, and you will see what I mean.
> > >
> > >     This problem does not go away even after you
> > >     :ExecuteFile(test-schem.cmd)
> >
> > I believe we have all agreed that the pin numbers in the symbol and
> > the footprint don't match, causing problems with the netlist. However,
> > I did run the test-schem.cmd file after loading the layout into PCB.
> > Shouldn't that have fixed these naming problems?
> >
> > For the set of my files, check
> > http://www.dhandanought.org/tcpip/audio/EXP/geda-probs/


>  Umm, Dan and DJ are the right ones to answer this question.  It's
> possible the renaming functionality hasn't been completely built into
> PCB yet, but they are the experts -- not me.
>
> Meanwhile, just make the symbol pinnumber match the footprint
> pinnumber and forget about the .cmd file.
>
> Stuart

Here is the problem.  In PCB, pins have a name and a number.  The number 
is specific to the package and the name is specific to whats inside the 
package.  Lets take a SO8 package that happens to house an op-amp.

In the schematic you have pin numbers and pin labels.  You might have 
pin 2 labeled as "IN-" and pin 3 labeled as "IN+" and pin 7 labeled as 
"OUT".  When you netlist, you refer to pin numbers.  So for example, 
U1-2 and U1-3 and not U1-IN- and U1-IN+.  The pin numbers define all of 
your connectivity information.  The pin labels are simply informative.

Now you load PCB.  The rat lines key off of the pin number and uses the 
pin number in the netlist.  Pin names are not used at all.

So if pin numbers are broken in your symbol or footprint, thats it, game 
over, things are just broken.

Now that the .cmd file does is it goes through and says "U1-2 (i.e. pin 
#2 of U1) happens to be called the "IN-" pin on this particular op-amp". 
 And it makes all those changes.  Now if you query that pin in pcb, it 
will tell you pin #2 and "IN-".  This is useful when you're working with 
a big part and you don't know the pinout by heart or via the context and 
you want to quickly see the name of the pin you're connecting too.

Thats all the .cmd file does.  If you don't ever load it, nothing bad 
happens other than querying U1 pin #2 will just report "this is pin #2. 
 It is called '2'" instead of ..... It is called "IN-".

Hope this clarifies things.

-Dan









_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user