Preserving unused via pads on plane layers

[edd]

How do I preserve unused via pads on plane layers? The remove / restore unused pad shapes function appears only to affect signal layers (not plane layers). I'm using Altium Designer 23.2.1.

(In this case, it's a 10 layer board with blind vias (L1-L5 and L6-L10), where L5 and L6 (in addition to L2 and L9) are plane layers (power and ground). The PCB house complained about missing via pads on L5 and L6. Apparently, they would like pads on start / end layers for the blind vias.)

[qdrives]

What export format (Gerber, Gerber X2, ODB++ or IPC2581) did you use?
What is the setting for "Include unconnected mid-layer pads" for that export?

[edd]

Thanks for your response qdrives! My export format is Gerber X2, and "include unconnected mid-layer pad" is checked.

[WhoKnewKnows]

You might want to view the PCB design in 3D view, with the distance between layers expanded and transparency of the fr4 material significantly reduced, and see if the pad being requested is actually appearing in the design. If it is, then "include unconnected mid-layer pad" should retain it in the Gerber output. I'm not certain, but I suspect that when a mid PCB plane layer doesn't connect to a via, there is no pad there to begin with. It simply creates a clearance around the column formed primarily by the drill diameter. Antipad, I think it's called.

Perhaps if you check the via setting? As I recall you can specify whether pads appear on all layers, just top and bottom or individually select. If these settings are correct, then...

Perhaps change the plane layer to a routing layer and see if the missing pads appear. Then place one enormous polygon to replace the plane and see if the pad stays?

[edd]

Thanks WhoKnewKnows!

The via pads on the plane layers are not visible in the PCB editor 2D view, the PCB editor 3D view, nor in the Gerbers.

The "include unconnected mid-layer pads" checkbox in the Gerber dialog is checked.

In the "Remove unused pad shapes" dialog, "vias", "restore unused", and "Preserve pads on start and end layers" are checked.

None of this solved the problem, so I did as you suggested. I replaced the plane layers with signal layers. Problem not solved, but at least bypassed.

[qdrives]

Just did a test with planes, as I don't use them myself.
It seems that Altium does not place pads on unconnected plane layers.
So like WhoKnewKnows mentioned, the solution then is to change the plane layer to a signal layer and place one big polygon.

The "Include unconnected mid layer pads" is only in Gerber (X1) and ODB++. It is missing with Gerber X2.

[edd]

Thanks for confirming this qdrives!