I am looking to export a model of the entire pcb, put it into freecad, and have a mechanical engineer move parts to exactly where they need them. Then I want to be able to have them save a file (maybe .step) and be able to import that into kicad and it move the position of my parts accordingly, then just manually reroute the traces where necessary. Is this possible? I am running kicad 5.0.0.
This workflow is not really possible right now.
What you can do is use kicad stepup to get the model into freecad. (This assumes you have step files for the parts of interest already assigned to the footprint. You can have wrl assigned to the footprint as long as the same file name is used for the step file and the step file is in the same folder.)
The mechanical engineer can then move the parts around as need be. After that you can generate a dxf file where you mark down the outline of the parts of interest and re import that into kicad. Use the outlines as a guide for where to put your parts.
You shouldn’t be routing traces before knowing where your mechanical placements for important parts (connectors, large components, heatsinked components, integrated antennas, etc) should go. That’s putting the cart before the horse and a sure fire recipe for duplicated effort. As far as the non mechanically critical components, their placement should be up to the routing demands of the board so the mechanical engineer would have no need for input.
What you can do ATM is sending the STEP model to your MCAD engineer and tell him to detail what he wants to move (3D model) and how (x,y, rotation).
Then you can do it accordingly to your pcb and re-generate your model to give it hime for a second review.
There is a very nice howto about this ECAD-MCAD collaboration process here:
@Rene_Poschl I’ve been thinking of having a push-pull feature for StepUp not only for pcb edge, but also for 3D models… this could be done (not very easily though) but I consider this process not completely comfortable… I normally work like I suggested above… I measure what I need to move and I do it accordingly in pcbnew…
In more complex cases I adopt the technique you suggested:
I export an outline (2D projection as DXF) of the required placement and, after importing it in pcbnew, I move the footprints accordingly.
In general this process is done before routing the board, but after having placed main connectors and parts on pcb to see if they full fit MCAD requirements.
Sometimes a review has to be done even when the board have been routed completely …
this will be a bit harder to fix, but it can be the only route
Thanks for your help. That is the process we have been doing, I was just hoping there might be an easier way. We are on rev 2 of the project, the first revision board worked but with the new mechanical design we need to move parts around and it would have been convenient to just import the new locations. We will continue to use the dxf to get the locations into KiCAD.
now it is possible to keep electrical and mechanical designs in sync also between KC & FC.
Please have a look at the latest StepUp update
This looks awesome! Thanks for doing this, I’m looking forward to trying this out and using it on the next revision.
Hi @pcbman17 have you seen KiCAD StepUp. It is under active develpment:
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.