GERBERS to Footprint

What is the best way to make a footprint file from GERBER data?

I presently have a Planar transformer which will be mounted on a card I am designing and thus I need the pin headers holes to align. Likewise I am designing a daughter card (to help with integration testing, not for the main design) and I would want to pass the outline as a footprint.

Might be the wrong question. You don’t have gerbers yet from the sounds of it. You will have a PCBnew layout?

I have GERBERS for a planar (in fact I physically have them) and I would like to re-use this planar in a new design.

To make use of this I need a footprint to use in the design I am working on right now. The original part and usage was done in Mentor so there isn’t actually any mechanical drawing. Now I could use the GERBERS and extract the centres to make a footprint but I was wondering if there was an easier way since I have these GERBERS

The gerber viewer has an ‘export to PCBnew’. I have NO clue if that would help. If it exported to a graphic or other type drawing that might be useful. I’m not sure if @maui 's step up would help because I doubt Freecad could open the gerber file. Hmm… Searching isn’t showing much hope of getting gerbers to some other graphic format.

Edit. GEDA’s gerber view does do this type of export. I don’t know if they support platforms other than Linux though.

I could use the GERBERS to create a PCBnew then import into freecad, which can create footprints.

This might work. all else fails, ill get the centers thanks

1 Like

an other workaround is to export gerber to dxf and then import dxf in FC.
From there it is possible to export a kicad fp.
No other direct way AFAIK

2 Likes

ok sorted…
so

  1. Load GERBERS in the gerberviewer and export all the key layers to PCBnew

  2. open in PCBnew and clean up any remnant - for me the GERBER have boardoutline on all layers so there were rogue tracks

  3. reposition around the origin by simply taking the average max-y,miny… max-x,minx

  4. export outline as DXF

  5. start footprint and load the DXF onto the silk and fab layer

  6. for each hole in PCBnew, not the xy and place a PTH at the same location

  7. add courtyard and save

Annotation 2020-07-16 173407

As an added bonus, due to this footprint existing and the GERBER PCB, a bit of messing around and a freecad model was created, including the pin headers

Annotation 2020-07-16 173655

thanks all

2 Likes

Glad it worked out for you.

Very nice with the model!

1 Like