Footprint with Cutout

[Studio_Pieters]

I hereby certify that I am not simply asking someone else to design a footprint for me.

This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.

Hi all,

I’m designing a new footprint, this footprint needs a cutout. Now I have drawn the cutout using Edge.Cuts. but when I look at the 3D drawing I don’t see the cutout part? Can anybody help me with this problem?

Oh yes I’m using Kicad 5.99

[Joan_Sparky]

Works for me…

Application: Pcbnew

Version: (5.99.0-7479-gddd026da87), release build

Libraries:
wxWidgets 3.0.5
libcurl/7.71.0 OpenSSL/1.1.1g (Schannel) zlib/1.2.11 brotli/1.0.7 libidn2/2.3.0 libpsl/0.21.0 (+libidn2/2.3.0) libssh2/1.9.0 nghttp2/1.41.0

Platform: Windows 7 (build 7601, Service Pack 1), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
Date: Dec 10 2020 22:00:50
wxWidgets: 3.0.5 (wchar_t,wx containers,compatible with 2.8)
Boost: 1.73.0
OCE: 6.9.1
Curl: 7.71.0
ngspice: 32
Compiler: GCC 10.2.0 with C++ ABI 1014

Build settings:
KICAD_SCRIPTING=ON
KICAD_SCRIPTING_MODULES=ON
KICAD_SCRIPTING_PYTHON3=OFF
KICAD_SCRIPTING_WXPYTHON=ON
KICAD_SCRIPTING_WXPYTHON_PHOENIX=OFF
KICAD_SCRIPTING_ACTION_MENU=ON
KICAD_USE_OCE=ON
KICAD_SPICE=ON

[paulvdh]

Have you ran DRC?
It’s got lots of extra checks in V5.99, including checks for malformed PCB outlines.

[Studio_Pieters]

@Joan_Sparky Thank you for your reply, but I’m trying to design a footprint with a cutout design in it, so I don’t have to draw it afterwards in the PCB design.

[Studio_Pieters]

I have added the design once more, maybe it is more clear then what I’m trying to achieve the footprint:

[Studio_Pieters]

The 3D design:

As you can see, is that it doesn’t show the edge.cuts, just the holes. So how do I create this cutout?

[BobZ]

Just to be clear: You are trying to create 2 slots in your footprint. One slot is shaped like a rectangular U with rounded corners. The other slot is more of a V shape with a rounded base and straight at the ends?

[paulvdh]

Again:

@paulvdh

Have you ran DRC?
It’s got lots of extra checks in V5.99, including checks for malformed PCB outlines.

Graphics for Edge.Cuts is pretty finicky. Start point of one vector has to match exactly with the endpoint of another vector, and I can’t see such things on a screenshot, but DRC can check it for you. That is it’s job.

The 3D viewer in KiCad is quite good at rejecting “stuff” on Edge.Cuts that it can not interpret. Because Joan’s desgin looks good in the 3D viewer, and your’s don’t, I suspect you will get “Malformed outline” errors when you run DRC in V5.99, combined with big fat arrows to where the endpoints of the vectors do not line up.

[pedro]

Can you share your footprint? This way we can edit it and find out what’s wrong.

[SembazuruCDE]

Note, these slots will be manufactured with a round milling bit, unless you really want to spend the tooling money to provide them with a custom broach… As such, the squared off ends of your slot will be milled with radiuses, depending on the size of the milling bit the board houses uses the radiuses will either be fillets on the slot or (more likely) fully radiusing the ends.

If you want to fully control what board material is removed and what is left, I’d draw in the fillets and/or fully radius the end. You should also probably bounce the specs for the slot off of your board house to make sure that they have a router bit small enough for your design, and/or find out the size of the router bit that they would likely use for this application and make your drawing fit that tooling.

[BlackCoffee]

Using 5.1.9 (and earlier)

A Few ways to do it - below is perhaps the easist…

• Create the Footprint (and do NPTH or Draw Circles)
• Edit the Footprints .mod file and change Dwg layer to Edge Cuts

Example shows using NPTH holes and original Footprint and added Footprint with the Edited .mod file

Give the video a few moments while it waits for my slow-moving hand…

[Joan_Sparky]

@Studio_Pieters

but I’m trying to design a footprint with a cutout design in it, so I don’t have to draw it afterwards in the PCB design.

That’s why I posted that… it’s a footprint with a cutout in it - the round-cornered rectangle between the solder pads is defined in the footprint on Edge.Cuts.
Depending on where it sits it either creates a hole in the pcb or a piece of pcb when outside.
So it is working.

And I did that in the footprint editor this time, no need for editing the FP file in a text editor to change the layers for those lines.

Here is the file, you can try for yourself:
Display_Nokia5110_BackMount.kicad_mod (7.4 KB)

Have you tried with just one of the two cut outs?
Maybe KiCAD is confused by the amount of them? (a bug then I guess)?
Are you sure the endpoints of those lines that make up your shapes are exactly over each other?
Maybe its because you got PTH/NPTHs in the footprint as well? (another bug)

[Studio_Pieters]

Thank you all I finally got it! thank you all for the great support!

[paulvdh]

Let me guess:
You did a DRC check and it showed a big fat arrow to a location where the end poinds did not line up…

[morganfeldon]

One of the new features of KiCad 5.99 is being able to do Edge.Cuts directly on footprints and not do lengthy workarounds or text editing. Glad to see the OP figured it out – I’m guessing a disconnected endpoint.

[BlackCoffee]

I agree that, for some folks, editing text file is not what they want to do. Thus, I made a Plugin to do it, shown in this video

In followup to that vid post, I made a Pop-Up window with selections. But, though it does reduce the overall window size (as I wanted), I went back to using the Plugins as originally setup (without a Pop-Up)…