Altium: Blind/Burried vias in footprints?

[TheUnnamedNewbie]

I'm making a HDI project with lots (well actually only) blind and buried vias. In some of the footprints I need to make (RF structures) I need to have blind/buried vias. I cannot for the life of my find how to do this. In the PCB library stackup editor (not the PCB stackup editor itself), it seems like you cannot add any non-through vias.

Is this something Altium simply cannot do, and I have to use another tool, or am i just not seeing the button to do it?

[SerieZ]

As far as I am aware you cannot define Via Types in your Footprint in Altium.

However if I had the same problem you are facing I would give those affected vias a "special" size, impossible for manufacturers (i.e 0.201) and later filter those out (Find Similar) in the Layout and change them all in few clicks to the desired via type previously defined in the Layer Stackup in the Layout itself.

To Clarify:
Select all those Components in the Layout and unlock primitives -> then filter by Find Similar function

[TheUnnamedNewbie]

That is a very nifty work-around. I have currently decided to give Keysight ADS a try for this specific board, since it is just a series of RF structures, but might use this in a next iteration when we add active circuitry to the PCB.

Thanks!

[dstraight]

My workaround: I created my footprint using blind/burried vias in the PCB project document - then I copied the structure into the PCB footprint library. 

I'm not sure if this is the best approach - but this seems to work. 

[free_electron]

The library can store anything that can be created on the pcb. the Library EDITOR is limited in functionality though. for this kind of work : make the structure using the PCB editor first , then copy past into library.

i have been pushing altium to drop the pcb library editor altogether and use the pcb editor instead. instead of saving as a pcbdoc you save as pcblib or pcbpart.

[Gibson486]

I tried doing this the way dstraight did. Did not work. The issue is that you need to define your vias by layers ahead of time. So, if you have a part that was on a 4 layer pcb, then the buried via would get messed up on the 6 layer pcb. The work around is that you can manually make it right by adjusting it after you import the part in, but that kind of beats the whole point.