Step export and StepUp problems

[der.ule]

I’m trying to export a simple board with KiCAD unfortunately it appears that having a big hole in the middle of the board is not supported:

Board:

KiCAD Step Export:

Using StepUp I obtain the correct step file,

however when I try to add a bit of bling to the model (the mechanical guys need to know the copper position to design some brushes) and try to import the copper into the model, the result is not as expected:

@maui Any idea why is this the case ?

The whole procedure already worked correctly once, but I’m not sure what is different now.

[maui]

@der.ule
Which is your StepUp release nbr? and FC full release details?
could you post the board? (or send it to me in PM?)
I’ve tested with the following board without issues…
ruuvitag_revb6.kicad_pcb

[Rene_Poschl]

Make sure your big hole does not exist multiple times and is a closed outline. (Your original board had a simpler hole shape that is less likely to be an invalid polygon. Also note that if the kicad internal exporter fails then there is a high likelihood that your outlines are not quite correct.)

If you run nightly then you can use DRC to check your board outline.

[der.ule]

kicad StepUp version 8.1.0.8

Freecad:
OS: Windows 7
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.12643 (Git)
Build type: Release
Branch: master
Hash: 868d9cc6c215ce3a2ab20d454378ec00e1b9ed26
Python version: 2.7.8
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.1.0
Locale: German/Germany (de_DE)

KiCAD:
Application: kicad
Version: (5.0.2)-1, release build
Libraries:
wxWidgets 3.0.4
libcurl/7.61.1 OpenSSL/1.1.1 (WinSSL) zlib/1.2.11 brotli/1.0.6 libidn2/2.0.5 libpsl/0.20.2 (+libidn2/2.0.5) nghttp2/1.34.0
Platform: Windows 7 (build 7601, Service Pack 1), 64-bit edition, 64 bit, Little endian, wxMSW
Build Info:
wxWidgets: 3.0.4 (wchar_t,wx containers,compatible with 2.8)
Boost: 1.68.0
OpenCASCADE Community Edition: 6.9.1
Curl: 7.61.1
Compiler: GCC 8.2.0 with C++ ABI 1013

Build settings:
USE_WX_GRAPHICS_CONTEXT=OFF
USE_WX_OVERLAY=OFF
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_WXPYTHON=ON
KICAD_SCRIPTING_ACTION_MENU=ON
BUILD_GITHUB_PLUGIN=ON
KICAD_USE_OCE=ON
KICAD_USE_OCC=OFF
KICAD_SPICE=ON

The big holes are couple of arc due to the discontinuities in the perimeter, but I try as best as I could to fit them together (changing the radius of an arc could be a useful feature). Apparently, there is a discontinuity as I am not able to export it anymore directly from KiCAD (the exporter reports an error). With StepUp apparently this is not a problem (Thanks Maui!)

Below I’m attaching the KiCAD project (nothing fancy really) with the 3D models, thanks a lot for your help!

slipring.rar (111.2 KB)

[Shack]

I would recommend Freecad sketcher to draw the outline, and then export it to Kicad from Stepup

EDIT: remember to also remove the Soldermask from the traces

[Rene_Poschl]

You can use stepup to draw your outline and then push it to kicad. This helps a lot for such complex outlines where the kicad internal drawing tools are simply not powerful enough.

[der.ule]

Thanks, but as far as i know it is not possible to remove the soldermask from traces only from pads, my plan was to request the board without solder mask. I just blended out in the 3d viewer.

I believe both of your are right about using StepUp (or FreeCAD) but I told myself that the outline wasn’t complex

[Shack]

@der.ule

Thanks, but as far as i know it is not possible to remove the soldermask from traces only from pads, my plan was to request the board without solder mask. I just blended out in the 3d viewer.

My recommendation:
Select F.Mask layer
Select the circle tool
Draw a circle with the same radius as your copper rings.
Edit the circle and select the line width to the same as your copper rings (perhaps 1.1 instead of the 1.0)
repeat

[der.ule]

Thanks Shack, I was so focus on a parameter of the track that I did not think about this simple method

[maui]

Hi @der.ule
for your user case I would:

1. Design the edge in FC and push it with StepUp
   1alt) Fix your edge simply importing your board in FC with StepUp and push back the automatically fixed-closed edge to pcbnew using again Stepup.
2. For antenna tracks I would create a footprint in FC or in Kicad using a Geometry primitive to create the circles and TH pads.

here my attempt:
slipring-test.kicad_pcb (15.2 KB)
antenna.kicad_mod (1.2 KB)

and the FC files:
ant1.FCStd (13.2 KB)
board.FCStd (25.7 KB)

[der.ule]

Thanks a lot for your support!

I will give it a try with FreeCAD, I still do not feel at home with the UI but I’m sure I will find a couple of good tutorials for the sketcher

Once again, thanks for StepUP, great tool for colaboration!