[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]

Re: gEDA-user: good idea - bad idea ?

On 1/3/07, Andy Peters <devel@xxxxxxxxx> wrote: 
On Jan 3, 2007, at 3:39 PM, John Luciani wrote:

> On 1/3/07, Andy Peters <devel@xxxxxxxxx> wrote:
>> On Jan 3, 2007, at 3:09 PM, John Luciani wrote:
>>
>> > On 1/3/07, Ostheller, Joel A. <JOEL.A.OSTHELLER@xxxxxxxx> wrote:
>> >
>> >> I can not get gsch2pcb / pcb to stop using the M4 library as a
>> >> default.
>> >
>> > What does your gsch2pcb command line look like?
>> >
>> > Are you using the --use-files switch?
>> >
>> > gsch2pcb --use-files --elements-dir ~/YOUR_FOOTRPINT_DIR
>> > SCHEMATIC_NAME
>>
>> --use-files doesn't cause gsch2pcb to ignore the m4 libraries.  Maybe
>> a switch can be added to gsch2pcb: --no-m4-libs ??
>
> It will cause the newlib files to be used first. Wasn't the original
> problem that the M4 libraries were used first?

That seemed to be the problem.  However, --use-files didn't seem to
do what it was supposed to do.  In other words, even though I did

$ gsch2pcb -v --use-files --elements-dir /Users/andy/Library/gEDA/pcb
power.sch

gsch2pcb still searched for m4 libraries first.  I know this because
the spiel from the command would say

____
C11: have m4 element 0805, but trying to replace with a file element.
        Found: /Users/andy/Library/gEDA/pcb/jcl/0805
C11: added new file element for footprint 0805 (value=0.1uF)
____
: have m4 element , but trying to replace with a file element.
        No file element found.
: added new m4 element for footprint    (value=)
----

The unknown entry below C11 is one of the chips that called out that
SOT223- footprint.


I believe that gsch2pcb always searches for m4 lib parts (by running m4 macros)
but will insert newlib parts if the --use-files switch is used and a
newlib file is found
(as is indicated by the C11 message).

If believe the error may be caused by the m4 macro that is called for the SOT223
when gsch2pcb runs. The macro may not like the value of the footprint attribute.
I believe that the macro is in smt.inc


When you delete or move the m4 libraries, running gsch2pcb (with
exactly the same command line), you get an error message saying

/sw/bin/gm4: /sw/share/pcb/m4/common.m4: No such file or directory

which is expected, because it was deleted.  Now gsch2sch doesn't
search the m4 libs and the unknown part is no longer unknown:

____
C11: need new file element for footprint  0805 (value=0.1uF)
        Found: /Users/andy/Library/gEDA/pcb/jcl/0805
C11: added new file element for footprint 0805 (value=0.1uf)
____
U1:  need new file element for footprintf SOT223-230P-650W-356L-4N
(value=LM317EMP)
        Found: //Users/andy/Library/gEDA/pcb/asp/SOT223-230P-650W-356L-4N
U1:  added new m4 element for footprint SOT223-230P-650W-356L-4N
(value=LM317EMP)
----


In this case the macro for the SOT223 is not called since it could not
be found.

So it looks like gsch2pcb doesn't honor --use-files in the expected
manner.


It depends what your expectations are ;-) I think I agree with you here.
I would expect --use-files to look for a newlib file and use it if it is found
and not run any m4 macros. If it is not found then m4 macros would
be run.

(* jcl *)

--
http://www.luciani.org


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