Application: KiCad
Version: (5.99.0-9785-ga9f86c6f3d), release build
Libraries:
wxWidgets 3.1.4
libcurl/7.74.0-DEV Schannel zlib/1.2.11
Platform: Windows 10 (build 17134), 64-bit edition, 64 bit, Little endian, wxMSW
Build Info:
Date: Mar 14 2021 13:06:59
wxWidgets: 3.1.4 (wchar_t,STL containers)
Boost: 1.75.0
OCC: 7.5.0
Curl: 7.74.0-DEV
ngspice: 34
Compiler: Visual C++ 1928 without C++ ABI
Build settings:
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_PYTHON3=ON
KICAD_SCRIPTING_WXPYTHON=ON
KICAD_SCRIPTING_WXPYTHON_PHOENIX=ON
KICAD_SCRIPTING_ACTION_MENU=ON
KICAD_USE_OCC=ON
KICAD_SPICE=ON
I want to create a footprint with a slotted usb type-c connector.
but, this footprint does not fit into the edge of the PCB, the overlap of the edge.cuts layer and the edge.cuts layer of the circuit board frame will lead to the failure of slotting
Indeed.
I can make some pretty good guesses to your intentions and problems, but I’m not in the mood for guessing and would like some kind of description or question together with your copy & past artwork.
EDIT: Seems like a description of the problem was added to the first post.
The system flagged this first post and held it. I almost deleted it when I saw some Chinese looking characters in the file name. I decided to go with ‘language problem’ as the reason for vagueness because it seemed to be valid except for the lack of a verbal description.
KiCad does not support Edge.Cuts graphics in footprints well.
I think the current state is that it is not “officially” supported at all, and that some graphics can be placed on Edge.Cuts in a footprint itself is just a happy coincidence.
The problem is that graphics on Edge.Cuts must be a bunch of line segments in which the endpoint of a line has (nearly) the same coordinates as the startpoint of the next line segment, and all put together they must form a continuous line.
You want your connector on the edge of the PCB, and therefore you have to integrate the line segments on Edge.Cuts in the footprint with the PCB outline itself. To do that you probably have to edit the footprint itself. Maybe you can move the Edge.Cuts lines from the footprint to Pcbnew directly.
When experimenting with such things, it’s always a good idea to have your custom symbols in a separate editable library.
Make a project specific footprint library (Default libraries are read-only).
Add that library to the library table: KiCad / Preferences / Manage Footprint Libraries / Project Specific Libraries/ +
Copy the footprint into your newly created library.
Update the Footprint library link in Eeschema to use the new library.
Could you use a non-plated hole for that, or multiple of them?
Here is a footprint with a somewhat square hole in it, made with multiple NPTH. It is a bit of a hack to be honest. squarehole.kicad_mod (1.2 KB) The corners are rounded, but they will also be in reality.
Or your could define a layer as coutout layer, add the cutout in your footprint. When producing the PCB tell the manufacturer that this layer is a cutout layer.
I use the layer Eco1.User as cutout layer in my PCBs. KiCad doesn’t know that and therefore the 3D view is not correct, but i rename exported Gerber files accordingly so the the PCBs manufacturer understands it and the PCBs are produced correctly.
Thank you very much for your reply. It seems that this problem is caused by the fact that kicad does not support it. I hope this problem can be solved in the future version!
It is a bit of a hack. You have to ask the PCB manufacturer if they can work with that.
Otherwise you have to define a milling layer and draw a line where the milling/cutout should be, in the correct thickness.
