Create electrically nonconnected Mounting holes inside a footprint

[robertferanec]

You can also create a mounting hole schematic symbol with 1 pin + footprint and when you use it in schematic, do not connect the pin. That will create a mounting hole which is not connected to nets on your PCB.

[[email protected]]

Aha! Thank you!
Documenting this here for later use:

While in PCB editor I selected: Design/Rules/Design Rules/Mask/Solder Mask Expansion/SolderMaskExpansion
Than I used the Wizzard to create a dummy rule which I edited afterwards with:

• a name "SolderMaskExpansion_NonPlated" ,
• a tag on "Solder Mask From The Hole Edge"
• typing the magic words: (ObjectKind = 'Pad') And (Layer = 'Multi-Layer') And (PadIsPlated = 'False')

Thanks again.

[qdrives]

I assume you want a non-plated through hole.



Oh, and create a special rule for the solder mask expansion too.

[[email protected]]

Electrically not connected mounting holes for M3 studs can be created in PCB layout by using: Tools/Convert/Create board Cutout from selected primitives.
I noticed the following:

• The "Create board Cutout from selected primitives" works for one hole at a time. You cannot apply it to 4 holes at once.
• The "Create board Cutout from selected primitives" is not available when creating a footprint
• The radius of the holes cannot be set afterwards via properties. (The coords can be changed though)

How can I create a hole in the PCB inside a footprint ?