I’d like to keep the inside of the courtyard of a mounting hole free of copper which is poured. What is the recommended way to do this?
Eagle has a “Restrict” layer which prevents that copper is poured inside the boundaries of that layer. What is the KiCad equivalent (if any)?
The goal of all this is that a mounting screw could create a short between top and bottom layers. Ideally the mounting hole in the lib should have a copper-free area around the hole, but that doesn’t seem to be the case.
Thanks for trying, but that is not an option in my version of KiCAD (v9.0.1).
I created a circle in layer user.1 and then clicked on “create from selection” in the Properties dialog. Did I miss something?
It looks like you haven’t got the circle selected . . . if you have several objects at the same location it can be difficult sometime to select the one you want, the easiest way I find to get round this is to do a long left click, then you will be presented with a list of what is found at that place, then you can select the circle and not, for example, the footprint.
In your picture you have selected and right-clicked a footprint, not a circle.
You have to select the drawn circle (look in statusbar which item you have selected) to get the “create rule area” option. (the RMB-click context menu is context sensitive).
Additional option:
draw a circle on “margin” layer, this works like a eagle restrict layer. But affects TOP+Bottom+all inner layers at the same time.
the mounting hole is made up from a THT or NPTH pad. You could select exactly that pad and change the pad clearance (for this pad) to 2…4…6…8mm.
note this change can be easily made in the pcb editor - in which case your footprint will be different to the FP stored in the library. Be careful if you later update footprints from library - this change would be reversed. This possibility (change footprints directly in the board view) was not possible in eagle - be careful if you use it the first time.
@ mf_ibfeew Using “Margin” layer doesn’t seem to work as described by you.
The left circle is in the “Margin” layer with all KeepOut settings turned on. The right circle is in the F.Cu and B.Cu layer with the same KeepOut settings. Only the restrictions in the F/B layers seem to have the desired effect.
I created a trace across the restricted areas and only the area surrounded by restrictions in the F/B layer is avoided. The (same) restrictions in the Margin area are ignored by the trace.
Using “Margin” layer doesn’t seem to work as described by you.
Using the workflow with the margin layer is not using the “convert to a rule area” tool. Just draw a circle/rectangle/polygone shape at the margin layer and the zone fill will avoid that shape. Every shape on the margin layer is treated like a board edge (therefore it affects all copper layers together) without really beeing a board edge in the milling file.
With regard to the zone fill this works similar to your known trestrict/brestict layers from eagle.
Since always (= KiCad V4) I am using for it mounting hole footprints.
For example my hole footprint named 32C60 means 3.2mm hole with 6mm diameter free of copper area. It has one NPTH, Mechanical pad with Circular shape and Diameter 3.2 and Hole also circular with Diameter also 3.2. Then in Clearance Overrides I have Pad clearance = 1.4mm ( 2* (3.2/2+1.4) = 6 ).
