Create a footprint where the pins are shorted with the 3D body

[mrburnzie]

I have a connector which has 4 mounting holes which connect to the casing.
The space between the 2-2 mounting holes is a keep-out-layer, so I can't connect them together on the pcb, BUT the connector is from metal, so technically when mounted, it will connect all of them together, making a connection.

My problem is that altium is giving me an error for of course not connecting it. How do I set a rule which will ignore this?

[T3sl4co1l]

A couple of problems/confusions:
- Datasheets sometimes give "keep out" areas.  This just means they don't want copper (or maybe silkscreen either) there, as there may be projections from the component which could cause short circuits or wear.  A common confusion (I say "common" because I've done this a few times myself, long ago!) is to use an EDA tool's keep-out tools for this.  But a keep-out object may not keep out just the offending material: in the past, Altium had one common keep-out layer, against which all layers collided.  Nowadays, you can set objects by layer, but remember to set every layer you need (probably just top copper, and maybe silk; or multilayer where it really does matter, such as in-board antennas).
- Whether you assign the same pad number/name to a common feature is up to you.  Keeping them distinct is most general, but clutters up the schematic -- you need a symbol with as many pins as the footprint has.  (A multi-pin DFN MOSFET for example ends up looking like a hedgehog this way.)  Making them common is... semantically true enough, but kind of in the opposite way you'd like the EDA tool to understand it.  That is, you make them the same name so they get the same net, which means you must wire them together on the PCB.  If you're going to wire them anyway (to get rated ampacity, to reduce EMI, etc.), done and done.  If you only need one connection, or want to make a through connection (jumper), though -- that's different.  Note that a jumper is really a net split, so should be drawn as such on the schematic -- but you can only do that by splitting up the pins, so you should do that.  Or maybe you only need/want to connect one of the pins (OR instead of AND connectivity of the pads in question), such as for a tactile switch where the pins are in pairs.

Tim

[ajb]

In the PCB footprint, you can set the component type to "jumper" and then assign a common non-zero jumper ID to the pads that should be connected to each other: https://www.altium.com/documentation/altium-designer/creating-pcb-footprint#!working-with-jumper-components

This is intended for things like wire jumpers, but I've tried this for tact switches and it seems to work just fine.  Altium will recognize that the pads are connected via the component and won't generate an unrouted net error for the pads that aren't connected to tracks.  Been a while since I messed with that, though, so YMMV and some experimentation may be required to make sure it works for your needs.

- Whether you assign the same pad number/name to a common feature is up to you.  Keeping them distinct is most general, but clutters up the schematic -- you need a symbol with as many pins as the footprint has.  (A multi-pin DFN MOSFET for example ends up looking like a hedgehog this way.)  Making them common is... semantically true enough, but kind of in the opposite way you'd like the EDA tool to understand it.  That is, you make them the same name so they get the same net, which means you must wire them together on the PCB.  If you're going to wire them anyway (to get rated ampacity, to reduce EMI, etc.), done and done.  If you only need one connection, or want to make a through connection (jumper), though -- that's different. 

Yes, ideally it would be nice to have better control over the mapping between logical pins in the schematic and physical pads on the footprint.  Some way of specifying not just what pins are internally connected (so you could verify that two nets aren't connected improperly) but also which pins must be routed vs which ones are optional would enable the EDA tool to deal with these situations more appropriately -- but that is probably more complexity than the problem really warrants. 

[thm_w]

We have a section: https://www.eevblog.com/forum/altium/ I've asked to move it there.

I don't think you need to change the component type to jumper, just set the jumper ID's and it should work.