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

Re: gEDA-user: Some problems

Stefan Salewski wrote: 
Dan McMahill wrote:


--skip-m4 really really should have made this problem go away if you're
using the one from geda-20070216.



Seems that you are right.

I just tried this option again and it really solves the problem
resulting from footprint name

SOT23-95P-280L1-5N__LTC_S5_Package

Maybe I have made a typo yesterday or forgot to delete all old files
before launching gsch2pcb again.

Sorry. 

no problem.

But using gsch2pcb-option --use-files does not help.

this is true. --use-files just means to prefer a newlib footprint if it finds one but m4 is still invoked.

What can I do if my schematics contain (newlib) footprints from John
Luciani containing many minus signs (-), but I still need some oldlib M4
footprints. Do I have to rename all newlib footprints which contain
multiple minus signs?

2 things. Strictly speaking John's naming convention is incompatible with the complete gsch2pcb flow... But what you can do is this. If you have a recent version of pcb (basically the 20070208 snapshot or newer from cvs) then all of the m4 generated footprints are also installed as newlib footprints. This gives you all of the m4 footprints but the actual calls to m4 have been moved to compile time instead of run time. So you should be able to just do --skip-m4.

If you have an older pcb or your own custom m4 footprints, I think about your only choice is to renames John's or extract out the m4 ones you need.

Part of how we got in this situation is that the original design of the pcb library mechanism assumed that you only call m4 for a single footprint at a time. That meant problems like the SOT23 part of SOT23-95P.... being expanded simply didn't exist. It wasn't until the birth of gsch2pcb(actually probably the old gschem2pcb) that this problem cropped up.

In terms of a longer term fix for this I think ultimately what needs to happen is for gsch2pcb to not try and directly manipulate .pcb files at all but simply tell pcb "give me a XYZ footprint" and let pcb figure out how to pull it in. But this doesn't exactly help you now.

-Dan


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