FEDEVEL
Platform forum

, 03-31-2025, 08:30 PM

Hello everyone, this is my first Altium PCB design project and I'm quite frustrated with some collision errors I'm getting on the design, even though I think I have the design rules set up correctly. I'm following Robert Fernec's "How to Make Custom ESP32 Board in Altium Designer | Full Tutorial" (https://www.youtube.com/watch?v=KWIzhbQaZZk&t=15633s) and on 4:18:00 where we're supposed to make some Design Rules for 0R's (R1R2, R24R26, R23R25) I already tried doing everything exactly as shown on the video, but I keep getting collision errors no matter what I do. I'm positive my rules have higher priority than the Component Clearance but I keep having collision errors. If someone could offer some guidance I would really appreciate it. Thank you all.

QDrives , 03-31-2025, 09:28 PM

A better way to do it:
1) Select the components in question.
2) Go to Design / Classes
3) Right click "Component classes" and select "Add Class" and give the class a name, like overlapping.
4) Click the icon pointed to in the screenshot below.

QDrives , 03-31-2025, 09:30 PM

5) Click ok
6) Add a new clearance rule
7) Set the 2 matches to component class and select the added component class.
8) Set the horizontal clearance to a **negative value**

QDrives , 03-31-2025, 09:41 PM

It should also be possible to set the component class in the schematic as state here: https://www.altium.com/documentation/altium-designer/classes-schematic-pcb#user-defined-component-class.

QDrives , 03-31-2025, 11:11 PM

You need to make sure that the "User defined classes" are enabled for component.
Project / Project Options
Tab "Class Generation"

QDrives , 03-31-2025, 11:13 PM

Either add a parameter "ClassName" to the component or place a blanket over them and use a "Parameter Set".

Robert Feranec , 04-02-2025, 06:52 AM

did you try to re-run DRC check? Just want to be sure

QDrives , 04-02-2025, 02:49 PM

Setting 0 (zero) gives DRC error, negative disables it.
https://www.altium.com/documentation/altium-designer/pcb-placement-rules#component-clearance

Robert Feranec , 04-04-2025, 05:28 AM

good tip, didnt know that

QDrives , 04-04-2025, 02:05 PM

It used to be 0 to disable.
But it is good that Altium changed it to negative as this also allows 0 as actual clearance, meaning components side-by-side.