Kicad StepUp: The Sketcher for Footprint generation


I just made my first footprint with this feature. (See

It was a lot easier then it would have been in kicad. Only problems i encountered is with the text fields (reference and value)
I can’t seem to find how i can set their value and textsizes (by the way this is not really a problem just something that i noticed.)


thx for your positive feedback :smiley:

it is a bit different compared to other items
Editing Label (in Data Tab)

Editing Font Size (in View Tab)

(note: this is adapting font size only in FC, there are only two font size pushed to kicad ATM, but as you already noticed it isn’t a big deal :wink: )



Tech draw does not allow overlaying multiple sketches on top of each other. And dimension between them. (A lot of dimensions are between different kicad layers which all are different bodies when imported using stepup.)

At least i could not find a way to do it a year ago. When i dimension real drawings i use tech draw as it supports more features (like cutout drawings, …)

Should the text contend and the text size be transferred to the kicad footprint?


probably has been updated :smiley:

  • Text Content is transferred to Kicad footprint (the content transferred is the one in the above picture)
  • font size in FC is not a dimension in mm, so for the moment I just transfer 1mm or 0.3mm depending on FC font size. I could add a Dimension Size for Fonts at the end of the reference, as I do for Layers, if you consider this useful.


drawing dimensions is still faster as i can add multiple dimensions one after the other.
In tech draw i need to select both endpoints (unless i want to dimension a line) and then click on the dimension tool. And the select both endpoints step is very hard to pull off if one endpoint involves a center of a small arc.

Hm i do not seem to be able to increase the number of digits shown. For checking courtyard correctness i need at least 3 digits precision. (yes there is an input for number format but it does not seem to work.)

You might want to check the 0.3mm option. The font width might be too large in kicad. (it tells me that it reduced it automatically when i try to edit the field.)


I’m suggesting TechDraw because DrawingDimension is sort of ‘abandoned’ WB
All innovation goes to TD which is in FC main branch.

it should be enough to just zoom in the page

thx I will


I tried it, liked it! The video was a little hard to follow (goes really fast) so I drafted a text-and-photos document of my try at it. Feel free to use it, modify, etc.

Generating a KiCAD Model from 3D Step Data.odt (2.3 MB)


Thx a lot! I will include this at the main repo, so it will be in the Demo help. :smiley:
I really like this kind of support. I know I’m in lacking of documentation and this can help me and users too :smiley:


Hi @Rene_Poschl
I updated the WB adding REF and Value font size as suffix in the FC file

I should have also fixed the REF & Value text exporting to kicad fp …
please have a try


With 1mm text size it might be better to set the text width to 0.15 (or in general text size * 0.15 rounded to two digits)

Also it would be really helpful to have the courtyard rounded to some grid. But to be honest i have no idea how the interface for that could look like. Does freecad support custom fields in sketches somehow? (Maybe a first step could be to round to 0.01mm grid by default.)


ATM it is text size * 0.2 but I can arrange it to 0.15

The origin for sketch is placed to the anchor of the fp … So if you constrain the sketch relatively to the center (0,0) you should be fine.


Great writeup. You are to be commended for your effort. Three comments:

  1. I think that Molex is one (the only?) manufacturer showing footprints in the STEP models. Many other manufacturers don’t.

  2. In order for the footprints to be visible (at least in the Molex-supplied STEP files), don’t you have to check “Enable STEP Compound merge,” accessed in Edit→Preferences→Import-Export→STEP?

  3. I think it may be a good idea, especially newbies, to mention that the footprint-3D alignment procedure, lucidly described after “1. The 3D model now,” applies regardless of how the footprint has been generated.


if the manufacturer will not offer footprint outline as STEP model, a DXF or a pdf should be available… then the route is a bit more complex, but similar.

I’ve added your doc to the Demo files of the latest update… Thx for your contribution :smiley:


I get some python error when generating footprint. I have one complex pad and it seems that if I delete it footprint is generated, but with it, there is error. Could you look if I’m doing something wrong?
SKY13323-378LF.fcstd (10.9 KB)

Edit: I can’t get error text because it shows briefly in freecad window bottom line, and only part of it.

  1. your fp has Pads_TH_SMD with a polyline included
  2. your polyline has arcs inside
  3. your polyline miss the circle reference pad (as it is in kicad polylines)

I’ve updated your FC file:

  1. added a Pads_Poly sketch (copying from Pads_TH_SMD sketch)
  2. removed the ‘arcs’ in poly substituting them with lines
  3. removed polylines from TH_SMD sketch and rectangles from Poly sketch
  4. added a reference circular Pad to Polyline sketch

(You can open the example footprint-template-roundrect-polylines.FCStd in the Demo Menu to have a look in which way Poly are generated)

ATM StepUp doesn’t support ‘custom’ pads with primitive geometry as in latest updates … polyline pads accept only line segments.

Attached the FC file with the correction and the fp for Kicad.
You would need to play with pad numbering and clearance.
SKY13323-378LF.kicad_mod (2.9 KB)
SKY13323-378LF-Lines.fcstd (21.3 KB)

you need to enable the view of ‘Report panel’ in FC through the FC View menu.