kicad-developers team mailing list archive

[Dick Hollenbeck <dick@xxxxxxxxxxx>]

As of 60 seconds ago, there is now

   <kicad_source>/template/fp-lib-table.for-eagle-6.4.0

If you want to try using those many hundreds of eagle footprints, here's how:


1) You need at least testing version 4493, else eagle SMT pads won't show due to a
regression which was fixed in that version 4493.


2) Load fp-lib-table.for-eagle-6.4.0 into a text editor, not a word processor.  Notice the
use of environment variable EGMOD as encoded by ${EGMOD}.  Therefore, to use this table
fragment, you must set that environment variable some way.  I do it on the command line
under linux:

EGMOD=/opt/eagle-6.4.0/lbr pcbnew /i/pcbs/smart-arbitrator/arbitrator.kicad_pcb

all on one line.

EGMOD needs to be set to the lbr directory of your Eagle >= 6.0 install.


3) With the environment variable set, restart kicad and pcbnew.  Within pcbnew, built
(compiled) with USE_FP_LIB_TABLE enabled, pull up fp-lib-table dialog by menu choice

  Preferences | Library Tables


4) We will add the eagle table fragment into "Project Specific Libraries" table.  This can
be temporary or permanent for the project under test. Even if temporary, you will save it
to disk however, and maybe come back later and remove rows as desired.


5) Go to your text editor, and put the entire text of fp-lib-table.for-eagle-6.4.0 onto
the clipboard by copying it there, typically ctl-A followed by ctl-C.


6) In pcbnew, select the "Project Specific Libraries" tab.  Click on add Append Row button
if you already have existing entries in that table, else not.  Make sure your cursor is in
the left most column if there are any rows, and that the cell editor is *not* active.  If
the cell editor is active, the paste to table will not work, you would paste the entire
s-expression into one cell, yuck.  Then press ctl-V or use right click popup menu and
choose "Paste".  The Eagle rows will be appended onto the end of your "Project Specific
Table".

7) Press OK to close the dialog.  Those eagle rows are now appended into a file called
fp-lib-table found in your project directory.


At this point you should have read only access to thousands of footprints.  Note that it
can take a loooong time to load that many footprints of you choose the "List All" option
when picking a footprint within pcbnew, so you are better off using the "List by Browser"
option.  Or do the former and go get a cup of coffee while waiting.


These libraries are opened "read only".  You can drop down a footprint into your board,
but you cannot edit the footprint and put it back into an eagle library, because the
EAGLE_PLUGIN does not support FootprintSave().


Enjoy,

Dick