pcb holes wthin component footprint

[vixo]

Is it possible to make a hole within a component footprint? The only way I know to make a hole is to make a pad and make the hole as same size as the pad - if I do this I have to label the pad with a number and that means it doesn't pair with the schematic symbol

[trevwhite]

Maybe draw the hole on the mechanical layer that contains the pcb outline. You need to standardise the layer for this.

[T3sl4co1l]

1. Using pad: don't forget to set unplated.  You can use any name you like.  Typically '0' for mechanical holes.

Note that pad names are paired with pin names, so if you only use counting numbers for pin designators, they'll only connect with counting-numbered pads.  You can always edit the pairing on the Pin Map dialog.

2. Using regions: place a board cutout region of the desired shape.  Preferably also copy its outline to the board outline layer, so it shows up on the drawing.

Example: draw the outline on Mechanical 1 (or whatever the board outline layer is).  Select the primitives.  Tools, Convert, Create Board Outline Region (T, V, B).

#1 only allows round or slot holes, or I guess more complicated shapes using the pad library.

#2 allows arbitrary shapes.  Mind to leave an inner corner radius, and minimum slot width, corresponding to the minimum endmill size used for the operation.  Typically 1mm radius.  Smaller radii are available, but the board fab will charge a premium as smaller endmills work slower and have shorter lives.

Tim

[ajb]

You can absolutely make a hole using the pad tool in the component library.  This is entirely normal for components that need unplated mounting holes.

If you need an arbitrarily-shaped milled feature, it doesn't seem like you can fully define that in the PCB lib, at least not in the more modern way that recent versions of Altium favor (by defining a board cutout region), at least as of AD19.1 (it's possible they've fixed this in AD20+).  You can use the older keepout method, though.  If you need any kind of more complex geometry (board cutouts, edge outline features or whatever), then the best method may be to just draw them as a reference geometry in your PCB footprint, and then after placing the part translate that geometry as necessary into the correct primitives on the correct PCB layer.  The translation step might not be necessary in all cases, as long as you have layers set up correctly, not sure on that.