V8.0.4 DRC error that didn't happen in earlier versions

[celem]

I have previously used this footprint with multiple versions of KiCad without any problem. Suddenly, with V 8.0.4 the DRC throws an error of “Footprint Component type doesn’t match footprint pads”. This is a hybrid footprint which is a SMD connector plus 2 PTH and 2 NPTH. This never threw DRC errors before 8.0.4. Admittedly, this is a DIY hybrid footprint but I don’t see anything that should choke the DRC. This footprint has been previously built on several functional PCBs that work well - in other words I think that it is a DRC problem, not a footprint problem.

Something in the DRC of KiCad version 8.0.4 has changed. I could exclude this perceived violation but I would rather that the DRC didn’t throw the error.

Any suggestions?

I’ve uploaded a screenshot of what the footprint looks like and also uploaded the footprint file.

My KiCad version information:
Application: KiCad x86_64 on x86_64
Version: 8.0.4-8.0.4-0~ubuntu22.04.1, release build
Libraries:
wxWidgets 3.2.1
FreeType 2.11.1
HarfBuzz 2.7.4
FontConfig 2.13.1
libcurl/7.81.0 OpenSSL/3.0.2 zlib/1.2.11 brotli/1.0.9 zstd/1.4.8 libidn2/2.3.2 libpsl/0.21.0 (+libidn2/2.3.2) libssh/0.9.6/openssl/zlib nghttp2/1.43.0 librtmp/2.3 OpenLDAP/2.5.18
Platform: Linux Mint 21.3, 64 bit, Little endian, wxGTK, X11, xfce, x11
OpenGL: Intel, Mesa Intel(R) HD Graphics 530 (SKL GT2), 4.6 (Compatibility Profile) Mesa 23.2.1-1ubuntu3.1~22.04.2
Build Info:
Date: Jul 17 2024 01:37:25
wxWidgets: 3.2.1 (wchar_t,wx containers) GTK+ 3.24
Boost: 1.74.0
OCC: 7.6.3
Curl: 7.81.0
ngspice: 42
Compiler: GCC 11.4.0 with C++ ABI 1016
Build settings:

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.

MPCIE_MOLEX_0679101002.kicad_mod (15.5 KB)

[paulvdh]

I have seen this same DRC warning before, but maybe the rules of whether a footprint is regarded as either THT or SMT have changed. But it’s just a fabrication attribute. You can set it in: Footprint Editor / File / Footprint Properties. Options are SMT, THT and Unspecified.

I guess that any footprint that has a THT pad is regarded as a THT footprint by KiCad. I am not sure how important these attributes are. As long as you do hand assembly it probably does not matter. When you generate placement files, (With: PCB Editor / File / Fabrication Output / Component Placement there is an option to include only SMD footprints, or to exclude all footprints with THT pads.Changing this fabrication attribute to THT suppresses the DRC warning, but may have unwanted side effects for your placement file. If you want to keep it an SMT part, but not get the warning, then changing the fabrication property of both the THT pads to “heatsink pad” seems to work.

[celem]

Thank you for the reply. I double checked AND the mechanical holes are assigned a pad. All connector pads are SMD. Apparently, with v8.0.4 detects both SMD and THT pads it throws the error despite the footprint being set as SMD in the attributes.

[mf_ibfeew]

As paul said: select both THT-pads and set the fabrication property of these pads == heatsink pad.

[celem]

@mf_ibfeew

select both THT-pads and set the fabrication property of these pads == heatsink pad.

I select both THT-pads and set the fabrication property of these pads == heatsink pad and the DRC error is gone.

[paulvdh]

Instead of adding [Solved] to the title, it is both quicker, simpler and better to click on the “solved” checkbox of the “best” answer.

This also helps others who are searching the forum later to find fitting answers quicker.

[celem]

Selecting both THT-pads in the fabrication property to “heatsink pad” stopped the DRC error.