Pad near pad error in DRC

Layout
1

I am getting pad near pad error in the DRC check. It is a 4 layer board. Attached is the design rule I set based on the specification. Nothing else is changed from the default.

Can anyone please help?

601Ă—769 48 KB

2

“Pad near Pad” means there are at least two pads that are closer together than the clearance specification for the net class. That’s the “Clearance” column in the “Net Classes Editor” tab.

There are several “default” footprints that you can use that will cause this error with the “default” rules. For example the default clearance is 0.254mm, but on a 0.5mm pitch LQFP you have 0.3mm pads and a 0.2mm clearance. In this case because 0.2mm clearance is smaller than the 0.254mm design rule all of the pads will cause a violation.

Due to rounding errors and parts having been converted between old imperial footprint formats to new metric ones you sometimes get tiny differences (8mil = 0.2032mm so a 0.2mm clearance is still violated) so I often set my clearance to 0.19mm to be sure.

So to make sure you don’t get this error you need to make sure the clearance for all the nets attached to the pad is smaller than the spacing between the pads.

4 Likes
3

Nathan’s explanation is excellent. I have also seen this when I made my own footprints in the past and tried to get around the lack of ability to draw arbitrary polygon shapes for footprints (this may have changed in newer versions?), by placing multiple shapes to make up one “pad”, which each section having the same pin number. This also throws a DRC error, though I’m guessing it’s much more likely that you’re running into the problem that Nathan described.

1 Like
4

excellent information, much appreciation Nathan. I updated my clearance to 0.19mm & no more errors.

5

Hey Chris,
I watched your video where you used Oshpark DRCs in your design and you used 0.254mm as your minimum clearance.

1: I couldn’t see that in Oshpark’s site on here: https://oshpark.com/#support
What am I missing?

2: Can I change the clearance to 0.19mm and still order a board form Oshpark?

Thanx alot for all the info and to Nathan as well.

6

http://docs.oshpark.com/design-tools/kicad/kicad-design-rules/

1 Like