How to create a clearance area around a single PAD in Altium

Question

I'm creating large circular pads (13.5 mm diameter) for some capacitive buttons on ALTIUM.

I want to create a circular clearance non-copper space area around each of these pads (around 1..2 mm) to keep a distance from the ground copper surrounding area around these pads, as recommended below.

My 0.2 mm tracks for each PAD are on the bottom side of the PCB, like this:

I can create this clearance area as a general rule, and it works, but then it's applied to all types of pads in the PCB. I wanted this "rule" to be applied to only a single type of PAD and leave the others out.

Is there a way to do it? I tried changing the paste and solder mask expansions to no difference, and it always end up like this:

My 0.2 mm tracks for each PAD are on the bottom side of the PCB, like this:

As a side question, does it matter to have a hatched ground (as recommended in the picture below) or not around the pad sensors?

I'm doing a hatched one, but I can easily make a solid GND around the pad sensors.

Answer 1

Create a pad class for these pads.

Assign the pads to the pad class.

Make a rule for the pad class to have a much clearance from polygons as you like.

Rebuild all of the relevant polygons.

Answer 2

@The Photons answer is correct.

For the sub question, hatched planes were originally used on inner layers to improve adherence to the prepreg resins. At the time the electroplating process created layers that were very smooth. Currently the inner layers are roughened thus eliminating the need for hatching.

Hatching increases the impedance of the ground plane which is generally undesirable.

Hatching on the opposite layer will reduce the capacitance as opposed to a solid plane.

Hatching on the same layer will change the electric field that that the user's touch is to modify. A solid plane will provide better separation between the pads.

Modern manufacturing processes have eliminated the need for hatched planes in all but very specific cases.

You should ask this as a separate question to attract more focused individuals