OK so after a few hours messing about Iām not too sure if what I want is achievable with custom footprints?
I can create either a DXF, or a FreeCAD sketch, but they both result in a line drawing in the Paste layer when I import them. If I convert my sketch to a surface in order to get the filled area in FreeCAD, I canāt export it.
Am I missing something here ?
This is what I get:
This is what Iām trying to achieve
Then you can use freecad stepup to create a footprint directly from within freecad (click the link or the arrow to read everything. The link gets you to the discussion which might have more information than the initial post):
Well thatās what I have been trying to do. Iāve come to the conclusion that either somethingās broken or Iām having a stupid attack 
Iām sure Iām missing something from the workflow, or Iām not putting in some required information somewhere. Note at this stage Iām not trying to create the whole footprint, just a custom pad.
This is what I do:
I tried auto-constrain after (3), no difference
After my last post I found the āconvert shape to padā option in Kicad, but it doesnāt work. It complains that it needs an anchor point, if I add a small pad as suggested then the error goes but all that happens is the outline disappears.
I thought maybe the fact my shape has 4 segments was causing a problem. But I tried again with just one, same result.
Iām sure Iām missing something very fundamental but I canāt see it, and I canāt see anything from the link posted. What am I doing wrong??
Every polygon pad in kicad needs a so called anchor pad (either a rectangle or circular pad that holds the pad information) So add a circular pad inside the area of the polygon, select both the polygon and pad and then āselect convert shape to padā
Regarding stepup, you also need to tell this tool where the anchor pads are located. Do this by adding a circle to every separate āpadā. Have a look at the demo project ācomplex polygon pad shapeā or ārf-antennaā to see how it is done.
Hi @nali
this is a stress user case! 
The pad could be created like in the following imageā¦ but I have issue on the discretization routineā¦
Unfortunately polyline pads doesnāt support arc ATM, so we need to convert arcs to polyline, but the code need more workaroundsā¦
Iāll have a look later on
A small update 
Now the complex arcs+polylines can be exported as for this user case:
The above looks to work now, but as a general comment, the exact details of the paste-ends, probably do not matter much, as the paste melts and reflows anyway.
I would not fret too much over rounded ends.
Hehā¦ do you mean the user is stress-testing the application, or the application is stressing the user?
I think the fundamental issue here is that I am not at all familiar with the CAD part of the process. I do have FreeCAD but Iāve only used it for importing/exporting files really. I tried a fresh approach this morning to create a simple sketch and how to constain it - then FreeCAD crashed on me, twice. At that point I decided to leave it for a rainy dayā¦
As for my actual footprint - I decided to just use arcs a long time ago. But it annoys the hell out of me when I donāt understand something, especially something that looks as powerful & useful as this.
@maui - do you have any example Freecad file saved anywhere that I or anyone else could try?
Also, I have a small bug to report: I was exporting to a temporary footprint on my desktop and overwriting every time I tried something. When I use the KiCAD export button to save a footprint then select the existing file I get the āAre you sure?ā prompt then āFile saved toā¦ā. But it doesnāt actually overwrite the file! I was trying different things but loading the same old file into KiCAD
This is Win10 x64 and a fresh install of KiCAD 5.0.0 and FreeCAD 0.17.
the file is included in the demo and can be reached through StepUp Demo menu (see the picture above)
Requirements:
Where were you trying to export the footprint to? Windows wonāt let you save to a system folder, for example anywhere in Program Files. I think in this case it might actually save it elsewhere and not let you know, but I forget where.
Also, if you were trying to save your export into the KiCad supplied libraries, DONāT for another reason. The next time you update KiCad the installer will happily overwrite your changes.
Doh! I didnāt notice the menu right in front of my eyes!
Anyways, thatās perfect, just what I needed. The example imported just fine and gave me a working baseline to start with. It looks like my sketch was broken - I used Sketcher to make a simple outline (basically one of the segments) and it worked OK.
Not sure what the naming conventions mean yet āPads_Polyxxxā etc, but thatās sure to be a case of RTFM which I can do at leisure. Right now itās a sunny day and my wife is reminding me I have a house to paintā¦
Thanks for your help & patience!
PS ref the save location - just my desktop which is definitely write-able. I think it may be the fact that something was wrong with the file causing the export to not happen.
If you need help regarding the sketcher, i found a tutorial in the freecad forum:
https://forum.freecadweb.org/download/file.php?id=64732&sid=b487beb523c271f4322e17c947a3a409 (This is a work in progress.)
The discussion thread is found here: https://forum.freecadweb.org/viewtopic.php?f=36&t=30104 (If the file is updated, the new one will appear at that place)
I managed to implement also the recently added primitive geometry (only ācircleā and āpolylineā are supported atm).
Please update your KSU tools.
I updated also the FC demo modelā¦
Looks good! Actually I managed to create my footprint after a few days messing about with FreeCAD. I didnāt get on too well with the Sketcher UI which seemed [to me] to be doing strange things so I just used the macro facility then edited the macro with the values I needed to get the arcs / lines right. Then it was a pretty simple task to export it to a module.
The mic in question was a Knowles SPU0410LR5H, the footprint I made is attached.SPU0410LR5H.kicad_mod (3.4 KB)
Hi @nali
I would suggest you to remove BackCu (selecting Layers to F.Cu) and BackMask (unchecking B.Mask) from the PAD #6 of the footprintā¦ then you will have a full SMD fp as in the data sheet.
Hi @maui
Thanks for the comment. I did ponder whether to make a B.Cu pad, and decided to include it after all. The footprint is SMD, but because it is a bottom-port type microphone a hole is needed anyway, so I thought I might as well include the bottom pad. Itās a GND connection, so I use it to connect to a B.Cu flood fill.
(In reality nothing will be mounted in this area on the underside of the PCB because it normally fits against whatever case the board is mounted in for sound entry.)
I can actually think of a good reason for not allowing that hole to be a PTH. You donāt have to worry about solder getting in the hole and blocking it during manufacture. The solder on the component side around the hole might have a tendency to wick down a plated hole, especially if there is slightly too much solder paste.
+1 ā¦ and some chars
Iām not following that - the solder paste area is a long way from the hole ?
What may be an issue is solder mask ink getting into the hole - a NPTH hole avoids that, but if it is the only NPTH hole, that will cost more.
Careful tune of PADSTACK sizes to avoid both solder and mask-ink issues, should find a PTH solution ?
But it isnāt on the footprint that @nali posted. The 3D view up above is @mauiās example. Here is what @naliās design looks like (front and back) in the 3D viewer:
Though, I suppose a better question to @nali is why his design deviates so much from the originally posted image. Round pads where there should be square, two extra pads, size of the pad around the microphone hole (the OD of your pad is 1.224mm, but the drawing specifies 1.45), pin numbering doesnāt match, etc. Did you upload the right model?
Well, that depends on the manufacturer. More and more board houses now donāt charge extra for NPTH holes.
I donāt know why not having asked them, but I suspect that they expect everyone to have NPTH holes. Thus NPTH holes would already be built into the cost of the board, even if the board design doesnāt use them. For all I know may they have the routing bits and NPTH drill bits all on the same turret and do the routing and NPTH drilling all in one CNC job (probably in the other order, holes then routingā¦). Similarly, per via pricing seems to have also vanished from the industry.
