The picture looks like a solderpaste stencil. This is typically defined with the paste layer that you already list. Might it be that one of the layers should be copper? (Possibly link to the datasheet of your component)
There is also an alternative to adding one pad per layer. You could calculate the required clearances for past and mask relative to the copper size. This would reduce the workload for you as you only need to set a single value per layer in the footprint settings.
In the datasheet:
Copper, F.Cu, “solderable area” (at least I understand so): 0.28
Solder mask opening, F.Mask: 0.38
Solder paste stencil opening (made with laser in thin metal plate), F.Paste: 0.34
No silkscreen (F.Silk) in specs, it has different purpose.
They suggest soldermask defined pads with the following diameters:
This can be made with the following pads and footprint settings:
All pads get the size of 0.38mm and have F.Cu, F.Paste and F.Mask enabled.
In the footprint settings set soldermask clearance to -0.05mm (yes negative number) and paste clearance to -0.02mm (leave pad clearance and paste ratio clearance alone)
I’m waiting for Rene’s answer, I may have misunderstood the datasheet. Meanwhile, those clearance values should be halved - it’s that value in all sides of the pad and becomes double when measuring the final diameter. Just measure each layer in the footprint editor after setting the values.