"The routing start point violates DRC"

[ch992319]

I hereby certify that I am not simply asking someone else to design a footprint for me.

This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.

Using KiCad 6.0.8
Package shown here is from the library Housings_QFP:LQFP-208_28x28mm_Pitch0.5mm

Getting this error for these pads shown here:

I saw some other people ask this question and quite frankly were answered with terrible answers. This is a standard package apart of the KiCad library, there is no reducing the distance between these pads. Next question is what is the clearance then? I should simply be able to change the allowable clearance (even though doing this then defeats the entire purpose of the DRC - what I am saying is there should be some sort of exception for footprint clearances that doesn’t affect the clearance of the rest of the layout) - but then I go to the clearance settings of the part itself (going to do of the board as well)

of component:

of board:

Adjusted all these values and nothing changed.

Appears to be something of a non-negotiable default for KiCad layout projects. Any solutions?

EDIT: I also went into violation severity and put clearance violation on ignore which did nothing as well (also defeats purpose of DRC which I don’t want to do either)

[jmk]

Hi @ch992319

I placed that package on a board and performed DRC.

DRC result showed the problem so I changed:

Design Rules > Constraints > Copper > Minimum clearance and also, as DRC shows,
Design Rules > Net Classes > Clearance both to .14mm and DRC stopped complaining.

[ch992319]

Great work, didn’t realize there was another clearance setting in the net classes. This was the fix, appreciate the help!

[straubm]

You also can change the clearance “locally” for this very component in the component’s properties

either for the instance on the board (double click) or in the library (shift-ctrl-E, recommended).
Of course you still have to change the netclass clearance.

[jmk]

@straubm

Of course you still have to change the netclass clearance.

Nearly

You still have to change the Copper Clearance in “Constraints”.

Note: Straubm has shown the 6.99 layout. 6.0.9 layout has some different functions.