FEDEVEL
Platform forum

Clarice Starling , 11-16-2024, 06:57 PM

I have a 4 layer board with usb type c connecter.
Altium gives me error for this connector
How can i solve this error? Also, should I connect the shield pins to GND?

QDrives , 11-16-2024, 07:27 PM

Strange... It mentions a coordinate of a pad and not the pad name.
But you just need to repour your polygons to make the short-circuit go away.
As for the shield connection: do you have a chassis ground? Connect it to that. If not, I would just connect it to Gnd.
As a side note, your connector has a (3D) collision too.

Clarice Starling , 11-16-2024, 07:37 PM

am doing repour all but when I do drc check it continues to give the same error. I think I fixed the 3D conflict.

Clarice Starling , 11-16-2024, 07:39 PM

This is my USB layout

QDrives , 11-16-2024, 10:58 PM

What are the holes near A1 and A12? Have you set a clearance on those?

Clarice Starling , 11-20-2024, 08:33 PM

Mechanic Holes. This is the part https://mm.digikey.com/Volume0/opasdata/d220001/medias/docus/5702/USB4105%20-%20Product%20Drawing.pdf

Clarice Starling , 11-20-2024, 08:34 PM

I did not make any special clearance settings.

QDrives , 11-20-2024, 09:20 PM

What are the properties of those holes?
What is your rules for hole to polygon?
Which version of Altium?

Clarice Starling , 11-20-2024, 09:21 PM

Clarice Starling , 11-20-2024, 09:21 PM

v25.0.2

Clarice Starling , 11-20-2024, 09:21 PM

Clarice Starling , 11-20-2024, 09:22 PM

4 Layer PCB for JLCPCB

QDrives , 11-20-2024, 09:26 PM

I assume this is an older design?
Altium added the hole to... clearance rule. In your case it is 0. I have seen this often when opening older designs in newer Altium.
And that can also be seen in the layout where the copper is against the hole.
I still have not updated my Altium to the latest, still on 23.11, and there is a bug.
For you, I hope that when you set the clearance to something like 0.25mm for the hole and repour all polygons, that your short circuit error is gone.

Clarice Starling , 11-20-2024, 09:27 PM

Same clearence error:(

Clarice Starling , 11-20-2024, 09:27 PM

Clarice Starling , 11-20-2024, 09:28 PM

QDrives , 11-20-2024, 09:34 PM

No, it is not the same. First you had short-circuit, now clearance.
Lets see if you have the same bug as I have.
What if you set the clearance for holes to 2mm and do a repour?
Secondly, which distance does it report when you check for the applicable binary rules -> right click the hole, select applicable binary rules, click the hole and click the polygon.

QDrives , 11-20-2024, 09:35 PM

In other words, it may be a bug that you to set a lower clearance as the polygon is created with a fixed low clearance.

Clarice Starling , 11-20-2024, 09:36 PM

I think I made a mistake.
The errors in this picture were for the mounting screw.
I deleted the keepouts around the mounting screw and it was fixed.
Making the hole to polygon distance 0.254 as you said solved the errors in the USB connector.

But now there is an interesting situation.
When I run DRC, I see the x mark on the USB pads even though the error number is 0.

Clarice Starling , 11-20-2024, 09:36 PM

QDrives , 11-20-2024, 09:37 PM

Is that a 3D collision? It usualy is when all pads are colored as an error.

Clarice Starling , 11-20-2024, 09:37 PM

Maybe 3D error ?

QDrives , 11-20-2024, 09:37 PM

It can also be an error because part of the component is outside the board area. Another rule to change.

Clarice Starling , 11-20-2024, 09:39 PM

Yes, it may bleed because it is very close to the edge. I think this small micron protrusion will not be a problem and I can use it as it is.

QDrives , 11-20-2024, 09:42 PM

Can you place components more to the left?
I have seen that when a board is imported from Eagle, it is a the absolute maximum (or minimum?) zero position and nothing can be to the left, or below.
Overhang in that direction would give errors.