making NPTH Pad hole as blind or back-drilled in Altium

Question

Is it possible to make a mounting pad hole as blind for bottom layer only? If it is possible then how this can be done in Altium?

I am designing a 6-layers PCB and the requirement is that on the bottom layer there should be no holes, I can define vias as blind from top layer to 5th layer in Altium but could not find anything on mounting holes as blind. I have looked into the back-drill option but I do not know that how I can use that and what will be the impact on the bottom layer, therefore I think that the mounting holes should be blind for bottom layer.

Thank you

Answer 1

I am designing a 6-layers PCB and the requirement is that on the bottom layer there should be no holes,

Taken literally, this means you won't have any electrical connection from layer 6 to the other layers. Possibly you can solve this by filling your vias with epoxy, but you haven't made your requirements clear enough to know.

[I] could not find anything on mounting holes as blind.

This is because making a blind mounting hole wouldn't be useful for most applications. The point of a mounting hole is to pass a screw through it to mount the PCB to the enclosure of your system. You can't do this with a blind hole.

The mounting holes may also be used by your assembly (board-stuffing) shop to hold the board in their machinery. If you remove all through mounting holes, be sure to check with your assembly shop whether they need any other design features to compensate.

One solution might be to design your board with break-away tabs, and place any mounting holes required for the manufacturing process in the tabs. Then remove the tabs before using the board in the application where you have the no-through-hole requirement.

I have looked into the back-drill option

This doesn't make any sense. The point of back-drilling is to remove copper plating from parts of a via where it isn't wanted (usually for signal integrity reasons, when you have signals above 5 GHz or so). Since mounting holes aren't plated to begin with, there's no need to back-drill them.

Edit to Add

After seeing your comments, it seems like what you really want is unplated controlled-depth drills.

There's no particular reason this couldn't be done, but it will add cost.

The best way to find out the design rules you'll need to follow for this process is to call your PCB fab shop and ask.

Answer 2

I suggest talking to your fab and asking recommendations for how (and if) they can make something you can use, and then worry about how to specify it.

This does not sound very useful- a shallow hole partially through the board (if the hole is made by a drill bit it will either go completely through some layers of the stackup or will not have a flat end because of the drill point angle (which seems to be 130° for typical PCB drill bits rather than the more usual 118° or 135° for general-purpose drill bits). I suppose you could glue a pin into it or something like that...

You could always specify something like Z-axis milling. Typically you'd add a layer and some notes to tell them which layer to use and how deep to mill (and from which side).

Everything will add cost and time to your order, so it is best discussed with your fab(s) well in advance.