Connecting thermal vias to net in footprint

[Araho]

Hi!

I'm designing a footprint for an IC, and the datasheet says thermal vias in the exposed  center pad should be connected to GND.

How can I do this in Altium? As far as I can tell after trying this for a while, I can't connect anything in a footprint to a net at all. Even when adding planes in the stackup editor in a footprint, these can't have nets assigned to them.

One option might be to add the planes, then make the via go from top to GND-plane, but that changes the type to a blind via, doesn't it? And i definitely don't want that.

Anyone have a tip for me on how to do this the proper way?

[8086]

Give the pad a corresponding pin in the schematic part, and then connect it to GND in the schematic.

[gxti]

You can make as many pads as you want with the same designator, and they will all be electrically connected. So in addition to your SMD pad on the top layer add some through-hole pads with the same designator and they will get the correct net when you add the footprint to your PCB.

[Araho]

So basically, the trick is using the Pad-type and not the Via-type for thermal vias. Got it!

[Araho]

So I bumped into another slight problem here. The datasheet of the DRV8811 says that the pads should be connected to a large ground plane underneath the component for heatsinking, which is fine. However, it also says that the thermal pads/vias should not have the standard thermal relief-thingy on the ground plane-layer, to improve heatsinking.

I also understand this very well, as the thermal relief thing is used to simplify soldering to a pad, i.e. lead less heat away from the pad during soldering. But here I want to lead as much heat as possible away from the pads, and neither will there be any soldering on the vias, so the thermal relief-thingys are a no-go.

Does anybody know how to remove these (see photo)?

(Photo 2: Footprint of DRV8811, with thermal vias.)
(Photo 1: Same footprint on GND-plane, with thermal relief-thingys)

[Rufus]

Does anybody know how to remove these (see photo)?

Plane and polygon connect styles are controlled by design rules. You will probably want to devise a rule which matches only those component pads.

[Araho]

Okay, I'll try that. Thanks!

[tesla500]

I just disable thermal reliefs for all vias, keeps it simple. There's no reason for vias to have thermal reliefs, only soldered through hole pads need them.

[gxti]

Which is also what I do, but I just told him to switch from vias to pads so they would get the right net assigned. I think vias are probably the correct component to use there but they may be finnicky about getting the net assigned to them. Normally if you place a via when routing it will take on whatever net is already under your cursor when you click on a trace or pour. Hopefully something similar happens with component vias. It may only happen when you first import/place the component, not later if you try to 'update component footprint in PCB', so try switching back to vias and deleting your existing footprint then re-importing.