I hereby certify that I am not simply asking someone else to design a footprint for me.
Hello everyone,
I am a new user to KiCad and I need some help with a DRC rule error. I have created a custom footprint for a heater PCB I am designing. Now when I place the footprint assigned to a resistor in the schematic I get a DRC error message Error: Clearance violation( netclass “default” clearence 2.000mm; actual 0 ). I understand that something is overlapping but since the footprint is a group how does the pad and the line don’t have clearance? How do I avoid it in general?
Thank you for you time and efforts.
I do not have your footprint, but you probably drew graphic items in your footprint on a copper layer, and this is not the right way.
The proper way is to add the graphics to the pad itself. The way to do this in KiCad V5.1.x is different then in V6.0.0.rc1. I usually default to answering for the stable V5.1.x, but the blue of your screenshot suggests you’re using V6.0.0.rc1.
On top of that, your heater footprint connects two pads. This probably means you should treat it as a “net-tie” in KiCad. Net ties are still a bit of a kludge in KiCad. They currently need the string “net tie” (without quotes) in the keywords section of the footprint.
I cannot upload the footprint itself since I am a new user. But you are correct I drew the footprint shape in a sketch in Fusion360 and then imported it in the copper layer and placed the pads and grouped them.
Yes I do use the newer version even though is not stable, but so far I got only a couple of crashes and the annoying thing that: when I place 3D .stp model for a certain component after a change on the layout or the schematic I lose the directory path to that component for some it’s like it reverts it to an older save for when i got an older model assigned.
“This probably means you should treat it as a “net-tie” in KiCad. Net ties are still a bit of a kludge in KiCad. They currently need the string “net tie” (without quotes) in the keywords section of the footprint.”
Where should I do that in the footprint editor or in the layout? And since I got 17 of these footprints should i do it for everyone individually?
Select a pad, right click and select Edit pad as graphic shapes from the popup menu.
Footprint Editor / File Import Graphics
Or the “Net tie” way of working (It’s either / or, not both methods at the same time).
The “net tie” string is a part of the footprint itself, so you set it in the footprint. After that you have to update the PCB with the modified footprint. The setting is in Footprint Editor / File / Footprint Properties
Below a screenshot of the location of this property for one of the default net-tie footprints.
Thank you very much the “net tie” method worked just fine more than 40 errors disappeared. That’s a nice work around and it helped me even change the footprints geometry a bit and now my board layout is better and I can fit all the components I need.
