Mounting Hole!

[JohnsonMiller]

Hi Guys,

For higher mechanical strength and longer durability, I am going to use a mounting hole with via drilling around, like this photo:

If I connected a net to it (Earth, in this case), DRC give tons of error! But, without net connection, no DRC error.

Do you know what is the problem, and how to fix it?

Do you have recommendation for mounting hole design?

BR,

[robertferanec]

Please add the picture as attachment. If you add picture directly into the text, the picture will not show up and it will cause problems (our server sees your post then as a very long url - that is then considered to be a suspicious behavior and server will block you out - if you add picture as an attachment, everything will work oki).

[mairomaster]

If your mechanical holes are components (part of schematics) and the footprint contains vias, when you import the footprints to the PCB, the vias will not have net assigned to them, so you will get a clearance violation between the pad/vias. You have to manually assign the net to the vias. The same happens if you have regions connected to a pad in the footprint for example. It's a bit of a bug with Altium, or either lack of sensible funcionality.

[Paul van Avesaath]

just make the footprint with via's in there already. give them a pin name, make sure that pin name is in the schematic symbol and hook it up to GND. then import it as a component and you will have no errors.. also create a clearence rule for those specific components.

[mairomaster]

How do you give the vias a pin name though? They don't seem to have such property.

[Paul van Avesaath]

Sorry should have been more clear.. It should be a through hole pad, the size of your via..

[robertferanec]

As Paul van Avesaath and mairomaster suggested, that is what you will see in many motherboard schematics - a schematic symbol of a mounting hole with pins connected to pads placed around the mounting hole.