kicad-developers team mailing list archive

[Dick Hollenbeck <dick@xxxxxxxxxxx>]

The attached script converts footprints from one library type to another.  The PLUGIN type
defines the library format.

Most any PLUGIN type may be used as a source.  Only writable PLUGINsmay be used as a
destination.

You currently have to edit the plugin types in the script.  (In my last usage of it, I
converted EAGLE to KICADfor testing the EAGLE_PLUGIN.)

Some plugins are read only, sotrying to write to that plugin should not succeed.

Now that the EAGLE_PLUGIN::FootprintLoad() and FootprintEnumerate() functions are
implemented, this brings access to quite a large set of footprints, if you wanted to jump
the gun and convert libraries. 

If you wait for fp_lib_table support, you will not have to convert.

We may want to commit a script like this to the tree somewhere.  Developers may find it
helpful for testing.



#!/usr/bin/python

from __future__ import print_function
from pcbnew import *
import sys

if len( sys.argv ) < 3 :
    print( "usage: script oldLibraryPath newLibraryPath" )
    sys.exit(1)

# 2 libraryPaths.  A lib_path is either a file or directory depending on
# plugin type.

src_lib_path = sys.argv[1]
dst_lib_path = sys.argv[2]

src_plugin = IO_MGR.PluginFind( IO_MGR.EAGLE )
dst_plugin  = IO_MGR.PluginFind( IO_MGR.KICAD )

try:
    dst_plugin.FootprintLibDelete( dst_lib_path )
except:
    None    # ignore, dst_lib_path may not exist if first run

dst_plugin.FootprintLibCreate( dst_lib_path )

list_of_parts = src_plugin.FootprintEnumerate( src_lib_path )

for part_id in list_of_parts:
    module = src_plugin.FootprintLoad( src_lib_path, part_id )
    dst_plugin.FootprintSave( dst_lib_path, module )