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
_______________________________________________
Mailing list: https://launchpad.net/~kicad-developers
Post to : [email protected]
Unsubscribe : https://launchpad.net/~kicad-developers
More help : https://help.launchpad.net/ListHelp
