Choosing drill pairs

[Wesperos]

Regarding Lesson 2 on advanced PCB layout:
In the lesson, Robert selects drill pairs: microvia L1-L2, L2-L3, through via L1-L12 and burried via L3-L10. (Similar on the bottom half).
I just wonder why are we limited in selecting drill pairs. Can't we use any via to connect any two layers we want (in.e.L1 - L3 or L2 - L11)?

[mairomaster]

With micro vias, due to limitation with the manufacturing technology, you must keep the aspect ratio of the via up to 1:1 (height : hole diameter). If you try to connect 2 none-consecutive layers like that, the height of the via would need to be too big, hence the ration will be bigger than 1:1 (unless the diameter of the hole is also bigger, but then it defeats the purpose of using micro vias).

Another thing is that you normally want to keep the micro via drill pairs number to a minimum - the more you have, the more expensive and difficult it is to manufacture the board.

[Wesperos]

Hey mairomaster thanks for the answer. I understand, microvias are tricky, but what about making some other type instead, like blind via or buried via? I see no reason of why not to drill the hole in the layer, laminate them and then plate the via where we want. Or am I missing something? Do you, or anyone esle for that matter, have some reference on different via kinds fabriction?

[mairomaster]

Blind and buried vias you can use to connect any layers. However, the more drill pairs you have the more costly the manufacturing will be. Also often is not really worth it to have drill pairs as L2 - L11 for example, while you can just use a TH via from L1 to L12.

The REX board is a good example of a layer stack and drill pairs use. L1, L3, L10 and L12 are the main signal layers and you have micro vias to go between them. The outermost layers are used for the purpose, since they are close to the surface and easy to reach with micro vias. In the middle of the board you have power planes using TH vias.

Most of the high-speed multi-layer boards use similar stack-up since it is convenient, efficient and cheaper to manufacture.
​

[Wesperos]

L1, L2, L10 and L12 are the main signal layers
​

Do you mean L3 instead of L2?
So all the story about the vias is conveniece and cost? There is no technical limitation on puting vias anywhere actually? I somewhere heard that vias on prepreg layers are kind of impossible, but not sure if that's the truth. I need to learn more about via fabrication..

Btw, on Robert video's cross sections, the microvia is shown as if it is a piece of copper that has been pressed with the needle and bended all the way through the FR4 layer where it's connected to the other copper trace.. is it right?

[mairomaster]

Yes, I meant L3, sorry.

Basically yes, it's mostly about convenience and cost. Having micro/buried/blind vias wherever you want helps to achieve maximum density and saves spaces on some of the layers, but tends to be difficult to manufacture and expensive.

I haven't heard about any limitations with the vias depending on the laminate type (core/pre-preg).

The micro vias look the way you describe them, but they are not manufactured like that. The topic is not perfectly clear to me either, but you can find many useful resources on the web. It is definitely worth understanding the manufacturing process better - that will help you to design better boards in terms of DFM, something very important if working on complex boards.

[robertferanec]

Wesperos, please have a look at the HDI document attached to the lesson 2 (scroll down to Download section). It could help you.

Also, have a look how PCB is manufactured: http://www.fedevel.com/welldoneblog/...r-pcb-is-made/

There are some limitations how you can drill and also how many times the PCB goes through the layer adding process (e.g. to make 12 layer PCB, you may need to do following: put 8 layers together, drill through hole VIAs (these will become buried VIAs), then add two more layers and drill uVIAs, then add two more layers and do uVIAs + drill through hole VIAs .... also do not forget, every time you add VIAs you also need to do plating - adding copper inside the VIAs ... VIAs on more layers = more complex manufacturing process, more times they have to "manufacture" the PCB). If you drill between too many layers PCB may be unnecessary expensive (in reality, you do not really need to drill between many layers).

It is hard to explain. Have a look at the video, you will immediately understand what I mean.

[Wesperos]

please have a look at the HDI document attached to the lesson 2 (scroll down to Download section). It could help you.

Where exactly? I haven't found any section regarding drill-pairing recommendations.

Have a look at the video, you will immediately understand what I mean.

The video confused me even more, since they didn't show how and when drill the via or plate it with the copper But luckily, your description was clear. Now, on the example of iMX Rex module, I imagine the procedure is as follows:

1. Stack up cores named Dielectric 3, 9, 5 and 11 with the pre-preg layers in between and laminate. These are layers L3, L4, L5, L6, L7, L8, L9 and L10. Of course, all before stacking, all the copper traces are etched.
2. Drill the buried vias from L3 to L10. Plate it with the copper.
3. Stack the pre-preg at the top and bottom and copper foil on top of that. Now we have layers L2 and L11.
4. Drill the microvias (pairs L2-L3 and L10-L11). Plate the microvias.
5. Add the core on top and bottom with the coppler layers L1 and L12 and laminate again.
6. Drill the microvia pairs (L1-L2 and L11-L12) as well as TH vias. Plate with copper.
7. Add the solder mask.

If I understand it right, this procedure needs 3 lamination sequences and 3 drill sequences. This is I believe the measure of cost and complexity in PCB manufacture.

[robertferanec]

You have got it. In reality it is probably even more complicated ...