Altium: how to assign a net class to unconnected pins?

Question

I have PCB with a clearance rule for nets that can be exposed for higher voltages:

In the schematic I put a blanket around the area I need to be assigned as higher voltages nets (I called this class "Line"):

However the unconnected pin (pin 12 of K2 relay) has no net assigned - no net class consequently. So in the topology the clearance is not corret:

Until I put some arbitrary net label (NC1).

This can be solved for simple cases like mine. But if there will be an IC with many unconnected pins needed to have a net class - it will be a tricky thing.

Any thoughts?

UPDATE

As Matt suggested I tried to put Net Class directive directly to the pin as the following: strange but this didn't work, the pin still has wrong clearance.

Answer 1

Short answer: You can't assign a net class to something that has no net.

But, there are potentially some workarounds; unfortunately, none of them are perfect.

1. Add an additional rule that looks for non-connected pads and give them additional spacing, using the custom query ((Not InAnyNet) And IsPad)¹.

   In addition to this, you could make the first object more specific, such as to a particular net. The downside to this approach is that it will add the additional spacing to ALL the unconnected pads in your board. Is that a big deal? Up to you.

2. As others mentioned (and I think yourself), you could add an arbitrary net to each unconnected pin on connectors you are interested in. In addition, to be a little more elegant, and to catch mistakes, you could add a DRC check that gives you a warning whenever a pin is unconnected - and then for pins you are actually not interested in adding a net or an arbitrary net to, you can place the DRC error nullifier (the red 'X') on those pins.

   In this photo you can see that my connector J24 has unconnected pins 1, 2, 6 and 7. Pad 2 has a non-specific DRC no error marker on it (Red 'X'). See how warnings are thrown for Pins 1, 6 and 7, but now pin 2? The matrix in the photo is found under Project/Project Options/Connection Matrix.

Answer 2

I've had the same problem and the solution is pretty straightforward.

The solution is:

1. As it's shown in the second image the component to be isolated are located inside the "blanket" (it's not necessary to add any specific Net Class directive in the unconnected pins)

2. In the schematic: Project --> Project Options --> Options --> Mark the option "Allow Single Pin Nets"

3. In the schematic update the PCB as: Design --> Update Schematics in "Your_pcb.PrjPCb" and select to include all the "single pin net" in the corresponding class. All the changes can be selected, even though you only interested in a few of them.

With this the single pin will have an associated net, and this net can belong to a class and it will follow all the rules applied to it.