I want to have a footprint, that can only be connected on the other side of the board.
Think a resistor, where the body is F.Cu and it can only be connected on B.Cu with traces.
Why?
As I mill my PCBs myself I cant create PTH and only NPTH. When all the components are on one side (F.Cu )it is easy as all connections happen on the B.Cu. But when I flip the components it gets much more prone to errors.
To reduce the error prob I want to create a footprint or better pads of a footprint, which have the property of only being connected on the other side of the board.
Thanks for the replies and yes I have thought long about this, so no need to complain
Use a custom DRC rule with (constraint disallow track) and an F.Cu layer condition and a similar one for disallowing footprint with a B.Cu layer condition.
Thank you. It took me some time to parse the answer. For the ones, who come after @johnbeard meant the following:
Go into the the footprint editor and select the footprint you want to edit.
Select a pad and choose in the context menue “Create from selection → Create rule area”
Uncheck “Delete source objects after conversion” and select the layer you want the rule to apply.
In my case I wanted to keep out tracks on the side of the body of the resistor and have it only connect on the other side.
Select which kind of rule should apply. I recommend checking “Keep out tracks/vias/pads”
Hit apply and save the footprint.
Thanks again @johnbeard for your help
You can apply the “no front copper, no back footprints” rules to the whole board with just two DRC rules and no rule areas needed and no customised footprints.
One rule area on each side, each covering the whole board, with one excluding tracks and one excluding footprints is equivalent if you’d rather have the areas visible in the editor (still no customised footprints required).
I see your point, but than again that was not my problem.
Still want tracks and footprints on Front, but no connections to pads on F.Cu if the courtyard (body) is also on the front. If the courtyard is on back the connections can be on F.Cu.
Maybe I wasnt clear, about my constrains.
Anyways. I needed to be on Footprint level, as I create a library of common footprints and change them to my needs (and to the needs of the CNC Machine). The purpose of the library is that I can give it to friends.
Oh, I see. Then I think your method works. Probably also exclude zones.
The other alternative may be (I can’t check right now) is to create a custom padstack with the front layer removed. So there is only a back pad shape. If I understand your process correctly, this may also reduce isolated dots on the component side that may come away when drilling, and you get some free clearance too.
