Placing a net tie underneath another component without the DRC error?

Question

I'm using Altium Designer 19 and I have a ton of Net Ties many of which I'd like to place underneath other components. My net tie is just 2 6mil pads connected by a trace without any silkscreen or 3d bodies or courtyard or anything... and with the component type set to "net tie (no BOM)". All is well.

However, putting these net ties ( which just looks like a "chunk of trace") under another component I get a DRC collision error. I could ignore these errors, but that seems like bad practice and there are a lot of them. Is there a way to update the library net tie component to tell it that it doesn't have any actual component body and shouldn't generate any collision errors?

Answer 1

You can add another Component Clearance rule under Placement with a custom query such as ComponentType = 'Net Tie', HasFootprint('nettie'), DesignItemID ='nettie' etc.

Set the vertical clearance for that rule to 0 and horizontal clearance to whatever you need.

Set the priority of this rule above the other component rules, so Altium wouldn't complain about it having vertical clearance issues.

Answer 2

If a component has a 3D body, Altium will use that to calculate the component clearance.

The trick to use with net ties, is to make that 3D body be within the PCB.

Set an extruded 3D body to be from -25mil to -20mil for your net tie component. That way it will always be inside the PCB, and more than 20 mil away from your "normal" components.

For the component clearance rule, you may also have to change that rule from All - All to All - HasFootPrint('All')

Answer 3

So while the net ties method from my question works, I don't think it's the best solution here. A better way is to make each component itself "4-wire" in the library footprint. The challenge here is that these components only have 2 connections. I split the pads in half and assigned each one to a different net. This is the right solution for the design/ schematic/ layout and it gets rid of all of the net ties. The board house squawks about the footprint not matching exactly, but since the outline of the 2 pads matches the original single pad size, the assembly works fine. It also connects electrically at the device pad, which is "more 4-wire" than doing it at a nearby net tie on the PCB.

For example a 2-wire through hole sensor:

Becomes 4-wire with split pads:

Similarly, for a surface mount chip, the pads just get split in half, becoming: