Import/Create FootPrint DXF


nice. I got it until the last step where we do ‘discretize’


As in the gif, you need to select ‘Sketch_converted’ (or ‘Shape2DView’) before clicking on the Discretizer…
it seems you have instead selected the 3D shape…


I did…


It is strange… are you on FC0.17 or FC0.18?
Which is your OS?
Would you please post the FC full version (FC Help, About, Copy to clipboard)
would you mind to send me the FC file via PM?
I will have a look at…


OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13522 (Git)
Build type: Release
Branch: releases/FreeCAD-0-17
Hash: 3bb5ff4e70c0c526f2d9dd69b1004155b2f527f2
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: French/France (fr_FR)


I have downloaded .18 I could install this one instead !


FC0.17 is fine for me… I’m on Win1064 same release… very weird your error


I have PMed the file with my 3D model projected and converted to sketch.
It seems your 3D model has some geometry issue that will make the discretization fail… I repaired mine with some tricks before projecting it…


Thanks again :slight_smile:
since the connector will be outside the enclosure/board edge cuts… normally would it be created as a foot print that sticks out from the board ? or only the part that is on the board / silk should be imported… ?


I normally keep also the external outline, to get an overview of the entire system … anyway, everything outside the pcb will be automatically cut by the pcb manufacturer…


I’m going to get annoying lolll. :sweat_smile:
used your file, renamed the layer to FSilks_0.16 ( as in the gif)
used Footprint editor and exporter image
created a file…
back in KiCAD I get



sorry, my fault
the Silk Sketch has to be labelled “F_Silks_0.16
and you need to have also “Ref#_1.0mm” and “Value#_0.8mm” as in the footprint examples…

The following are the reserved Names:

  1. F_CrtYd_0.05 (0.05 is the line width)
  2. F_Silks_0.16 (0.16 is the line width)
  3. F_Fab_0.1 (0.1 is the line width)
  4. Pads_TH_SMD
  5. Pads_NPTH
  6. Pads_Poly
  7. Pads_Round_Rect
  8. Ref#_1.0mm (1.0mm is the text size)
  9. Value#_0.8mm (0.8mm is the text size)


yeayyyy !! I’m now in KiCAD with that footprint :slight_smile:

that video helped a lot. Your Awsome

for the trace and pads, should I use the ‘Sketcher’ tool, draw around the pins and go from there ?


you can use the “footprint_template” in the ksu Demo Menu
There you can find

  1. Pads_TH_SMD to create TH or SMD pads
  2. Pads_NPTH to create NPTH (used for anchor holes)

to get an example …


I guess since we ‘scaled’ the pdf image, can I use the ImagePlane layer again to draw the circles on top of it ?

then the solder pad will depend on how I feel and visual space I have ?


Your two circles look close to me. The PDF drawing is showing a diameter of 1.2mm, and your two circles have 1.22mm diameters. That’s probably close enough for the drill-hit. (Though it would be trivial to actually hit the 1.2mm diameter by changing your radius from 0.61 to 0.60…)

I’d check the KLC for a suggestion for your annular ring in metric. You don’t have to follow KLC, but the suggestions there are based on good manufacturing practices.

Actually, I did just check KLC for you. This section here says that the minimum annular ring must be 0.15mm according to industry standard IPC-2221. Now 0.15mm is very small (5.906mil), depending on your fab house it may actually be too small for their tolerances. Unless you are very good, it is much too small for hand soldering. Think about what size soldering iron you would use for the soldering as a guide for your annular ring, and then see if that would fit along with being able to sneak a trace from pin 5 out of the middle of that connector land pattern.



you need to create constraints to the elements of the sketcher to place the centers of the circles as per the drawing dimensions.
The pdf gives/suggests you only drill dimensions… then for a TH pad, you need to draw two concentric circles, the internal one with a diamenter as the suggested drill, and the bigger one with a diameter that will gie the pad at least a minimum annular, but also a good soldering base…
Pins 1,2,3,4,5 are TH pads, the same for the optional shroud pin.
The other 4 holes (2x2.8 % 2x2.35) will be instead non plated through holes. Then only one circle is fine to describe the hole, inside a NPTH skecth.


The pin 1-5 can have a drill as suggested of 1.2mm because the pins of the 3D models have a diameter of 0.8mm … so there is room to fit the mechanical tolerances.


on spec sheet they mention Wave solder… I was hoping to be able to do it by hand…
note the pin 5 will not be used as I only have 4 pins… pdf share the same drawing for 4 and 5pins connector…

I got that model because the rep came to my office (for a different project) and suggested I use this kind of connector… witch is way more rugged than a green phoenix I originally planed to use.

plus. my good old engineer friend told me to be careful with picking up RF (making a LoRa radio board) and I’m adding 2-3 meter cable for I/O… he suggested a connector to board and adding ferrite on my circuit… so I got that connector… (sheilded cable, shielded connector… and ferrite)

I was to ask about that later in a next post but here I am… :slight_smile:


.21mm should be okay then… … but it looks soo big compared to the pin itself !