USB Type C, DRC problems

Hello! I’m new to the forum and have a question about using USB connectors and some DRC problems.

My question concerns the USB Type C connector and the blue holes. Somehow, I think this is causing a DRC error related to hole margin, or something similar. My question is: Is this footprint in the KiCad library incorrect, or are my DRC rules incorrect?

Secondly, I’ve encountered an error regarding thermal relief connections. Can I simply ignore this, or do I need to adjust some configurations regarding how thermal reliefs are applied?

Lastly, there’s an issue with the silkscreen overlapping with the pad, which is giving me some warnings. Is there a way to edit this? It originates from a KiCad footprint as well, so I assume I should edit that footprint. However, if it’s causing an error, should I assume that the footprint itself is also incorrect?

I suppose your rules are incorrect. But some rules can be set at PCB layer and some at footprint and even pad layer. So may be you should change some settings in Board options or in footprint itself. But exact dimensions of pads and holes I suppose are correct. I was not using KiCad for 4 months, I think and don’t have KiCad here to check anything.

There are probably several types of thermal relief errors. If you change settings to make them being not noticed or ignore them the effect will be the same. But there is also possible to change some relief settings to make them being done little different (solid/thermal relief connection, relief track width, relief gap width).

I don’t see it at your picture. You should identify it to decide what to with it.

1 Like

Thanks for your answer! I’ll check everything you said.

There is an image of the silkscreen overlap and the thermal relief:


Silkscreen does not seem to be overlapping the pad in that screenshot.
What is the exact error message, and what is the name of the footprint?

1 Like

For the thermal relief, it’s in the board setup that you can set the minimum number of thermal spoke that you must have.
By default kicad wants 2 spoke, but on a dense board it quite hard to have.
So you can reduce to 1 in the zone setting, or ignore this DRC warning.

1 Like

I missed the thermal relief question…

To get rid of the thermal relief error, you can simply draw a track from the pad into the zone. You can connect it to another nearby GND pad, or lock it in place to prevent it from being moved or deleted by the interactive router. When a manual laid track is present, KiCad assumes you are aware of the reduced thermal relief count and does not issue an error.

I didn’t know that. I’ve just checked. Even your track is ‘hidden’ by relief connection so making no real change the Error is gone.

In KiCad V7 in Board Setup - Design Rules - Constraints for Silkscreen there is parameter “Minimum item clearance:”. I see it being set to 0, but may be if set to higher value it sets the minimum distance between silkscreen item and pad. As silkscreen in theory is the last precision layer in PCB manufacturing so possibility of misplacement should be taken into account.

Thank you everyone for your answers, I really appreciate it. I tried to fix the problems and now I have fewer DRC errors. The only one that seems to appear is the USB error, so I feel my DRC rules are still wrong. I would check it. For any case, I am using JLCPCB Rules.

The error is “Hole clearance violation” (constraints: 0.2mm actual: 0.1944mm)

That is a difference of less then 5 micrometer. I would probably just shift the pads by a tiny amount to get rid of the DRC violation.

Is it a default KiCad footprint? Where does it come from?

There are 26 footprints for USB-C connectors in KiCad’s libraries, and differences are sometimes very small.

Your screenshot also has unusual colors. Purple is used for F.Mask, and that is probably what you are looking at. It’s not copper. (That also explains why the mechanical holes / slots are purple inside).

1 Like

I’ll take your advice. I’ll shift the pads of the footprint a bit to get rid of the DRC.

And yes its from the KiCad library, the name of the footprint is:
I think it’s a very standard USB C footprint because I’ve seen it a lot out there.

I know about the solder mask, sorry about that, I just took the screenshot quickly.
Thanks for your help!

Be very careful with that. There are no standard footprints for connectors. The connectors themselves may be standardized, but their PCB footprints are not. For example, when you look at aliexpress, you can buy assortments of 100+ different USB connectors (Those are popular by people who repair phones and such.) For example, if you compare it with: USB_C_Receptacle_HRO_TYPE-C-31-M-12 then the small pads have the same location, but the big power pads are shifted a bit. This footprint also has a bigger clearance between the NPTH and the pads. There are at least 7 footprints in KiCad’s library that look very similar to the one you use, and that should be enough to ring an alarm bell and look a bit closer.


Alright, I understand. I’m quite a beginner when it comes to designing with USB connectors, so sorry about that. Thanks for the advice. Next time, I’ll double check the footprints!

Buy your USB connectors first (making sure you know how to buy more of EXACTLY the same, should you need more!), and design your PCB to fit. That way you can be sure the connector you buy WILL fit!!!