kicad-developers team mailing list archive

[Wayne Stambaugh <stambaughw@xxxxxxxxxxx>]

On 11/20/2013 11:59 AM, Dick Hollenbeck wrote:
> 
> 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().

However, you can do a save library as to either the pretty or legacy
formats, add the new library to the footprint library table, and edit to
your hearts content.

> 
> 
> Enjoy,
> 
> Dick
> 

Excellent work Dick.  Thanks.

Wayne