6-layer stackup

Question

Edit 3:

I used the following Stackup - in respect to recommendations provided by my board house and the responses to this question.

This is a 6-Layer, 0.5mm thick, 1 + 4 + 1 HDI board (Copper thicknesses are not correct in the image).

EDIT 2:

As pointed towards in the comments, i had a look at some youtube videos.

Secrets of PCB Optimization - Rick Hartley - AltiumLive 2020 from 1:18:50 anwards gave me a good hint!

Good video for HDI Design Basics

Edit 1:

As further information seems to be helpful: Here it is!

I am working on a very small board (3x7mm) with double sided load.

Packages used are 0201, BGA (0.35mm, 0.4mm and 0.5mm Grid) and 2x2 12-LGA.

This is a "medium frequency (MCU runs at 150MHz)", low power (15mA), purely digital design.

As previous attempts to route the design on 4 layers failed because of "messy results, bad GND-Layers etc. etc." I decided to give 6-Layers a shot.

Stackup:

From Top to Bottom: Signal-GND-Signal-Signal-GND-Signal.

There are no dedicated power planes, as I can decouple each device and there is only little power draw. I used GND planes as sensitive electronics are used (Strictly recommended by IC manufacturer to use multiple GND-Planes).

Issues I am having:

-As I have double sided load, I use plugged through-vias only very carefully and not to break-out the BGAs.

-As this product will be a small lot size, I need a cost effective PCB design.

My current routing:

Currently I plan on routing like this: Fan-Out BGAs on top/bot layer and via Blind-Vias to associated GND plane (1-2 and 15-16) - Caution: The BGAs are 4x4 Grid - therefore, I only need to fan-out 4 signals to the GND plane.

Signals that need to run from TOP to BOT components are routed by means of through vias. As these signals runs all across the board - yes I tried many component orientations and placements - I need to "unravel" these signals on the inner signal layers.

My question is:

-Which via-arrangement will be - in your experience - the most cost effective?

Yes, I talk to my board-house but I like the input from this forum very much!

Original:

I am interested in information regarding the "correct" way to define a 6-layer board.

My objectives are:

• Use the "cheapest" stackup available to fit my requirements
• Be independent of a specific board house

My requirements are:

• 6-layer with vias from 1-2, 15-16 (1=top, 16=bottom, you get the system)

• Option to interconnect 2-15 and 3-14 in some way

What I came up with:

• My first idea is to use the following build-up:

This way, there are three cores (etched, drilled, plated) - then pressed with prepreg and drilled and plated again.

• My second idea is the following stack-up:

This way, there are two cores etched and pressed, then two prepregs pressed, etched, laser-drilled and drilled normally - then plated.

• My third idea is the following stack-up:

This way, there are two cores etched, pressed, drilled and plated - then two prepregs pressed and etched, laser drilled and plated.

My question is:

• What is the most cost-effective and conventional stackup of these three?

Answer 1

None of your proposals is the most conventional and cost effective because they use blind and/or buried vias. Blind and buried vias cost extra. Don't use them unless you actually need them.

https://www.proto-electronics.com/blog/how-and-where-use-vias-in-pcb-design

Just because a via hole goes through the entire stackup doesn't mean it connects to every layer. The via hole is drilled then plated, and only the copper layers that connect to the via have copper foil running right up to the plated wall of the via. Layers that are not connected to the via have a clearance hole etched in the copper foil that the via hole passes through so the copper foil never touches the plated walls of the via.

https://www.allaboutcircuits.com/technical-articles/which-via-should-i-choose-a-guide-to-vias-in-pcb-design/

---

But vias arrangement aside, you shouldn't be trying to overspecify your board layer stackup or determining the order used to fabricate the layers. That's micro-managing. You're trying to tell experts how to do their job when you yourself know very little about what their job entails. Tell them what you need, not how to do it.

The cheapest, least board house dependent thing is to let them do what they want within your requirements and not to micro-manage their process. As soon as you dictate and micro-manage their process it's going to cost more. They know the budgetary aspects of their process and what processes are actually available but you don't try tell them how to do their job.

They have a standard setups which alone reduces the cost by virtue of the fact they are accustomed to it and set up for it. Even if that setup does not have the optimal cost incremental unit for your specific board, unless your board quantity is staggering it would overall cost more to change the process. And if your quantity is staggering they would take it upon themselves to change the process to reduce cost.

Design it to what you actually need and don't put unnecessary restrictions on it so the board house has the freedom to do what they do best (and also to allow different board houses to accommodate themselves). If you are doing a regular commercial order with a board house (where a human actually looks at your board files) you can of course ask a rep if there are possible cost optimizations. Little optimizations aren't likely to be very large though unless your board quantities are very high or your board is super custom with a lot of unusual specifications or requirements.

Answer 2

As others have said, you are describing connections to a via, or the via stack.

In your ECAD software, it is as simple as defining the diameter of your annular ring on that layer. Even if you keep a uniform copper diameter across all layers, your net assignment of the via will define what it connects to electrically.

---

Now for an example:

In Altium, I have used a 6-layer stackup with BGAs on a small PCB, without needing to utilise microvias. The important thing is the BGA pitch - I had a 0.8mm pad-to-pad pitch, which makes it easier to find via space either between, or in pads.

The vias used were 0.2mm drill and 0.45mm diameter copper.

The crucial point is that this was agreed with the manufacturer before significant design work was done, but they are relatively standard sizes.

The vias are all 'full stack', meaning they are all drilled through the entire thickness of PCB, but I get to choose which copper layers they connect to.

I cannot quantify exactly how cheaper it was, but it was certainly easier for the manufacturer to produce.

The overall stackup was as follows:

If I ever start a design with similar constraints, this will likely be my starting point, as I know the manufacturer can produce it, but the best stackup will be design dependent on a case-by-case basis.

Answer 3

To assess the cost of the various buildups, talk to your PCB manufacturers. They will have their own preferences and standard production methods. However, once you are at 6 layers, expect very similar costs.

Often your requirements will push you down one path.

If you use BGAs, then you will generally want micro-vias to get to all the pads. This needs the core board, then the outer layers must be foil on thin prepregs, laser drilled for blind micro-vias.

If you have dense routing issues, then you can use Manhattan routing (up-down on one side, left-right on the other) on a core layer with buried vias.

There is no one-answer-fits-all. Obvious really otherwise PCB manufacturers would not offer all the different options.