DRC when rotating Package_QFP:TQFP-64_10x10mm_P0.5mm

I have a Package_QFP:TQFP-64_10x10mm_P0.5mm part and in order to get the routing to work I need to orient it at 45 degrees however when I do this I get lots of Pad Too Close DRC errors…

When I orient a 0 degrees I do not get these?

What gives?

This is a stock footprint?

I see… so there is rounding and that is enough to blow up the DRC… For mine it is by netclass…

so it is hidden a bit deeper… but tweakable…

A tolerance would be nice… I imagine it is a pretty small rounding effect.



Can you try the latest stable version? It’s possible that this has been fixed. At least it has been reported before. But it’s also possible that it was fixed in 5.99 only (the feature development version).

It looks very much like:

A fixed tolerance of 1nm was added in may, but the changes has been bumped to V6.0.

1 Like

Yes, it has been fixed in 6.0.

The tolerance is also settable in Advanced Config (a text file) in 6.0. But it should be very rare to need that…

(Note that the DRC system and Zone Filler were completely re-written for 6.0, so there’s no possibility of back-porting these changes to 5.1.)

I cannot really risk moving versions as I am about to send off some boards for manufacture. Will tweak the clearance down to 0.199999 for now and look to move to V6.0 at some point in the future.
Thanks for your interest!

1 Like

The latest stable version is 5.1.7 (one bug-fix version past yours). No one is suggesting that you change to 5.99 (which currently is still pre-alpha release for 6.0, might be up to alpha release by now though), especially since you are using KiCad for production. It should be fairly safe to upgrade from 5.1.6 to 5.1.7 (and I probably would), but only you know your own tolerance for risk.

1 Like

In 4.0.7 without rotation I noticed that if between rectangle pads I have 0.6mm and clearance set to 0.2 I can’t go with 0.2mm track between those pads. Since then I have always clearance set to 0.199.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.