Stack up (PCB)

[Rajinder1268]

Hi,
I am trying to understand about PCB layer stack up.
It is a 4 layer PCB, 1oz copper, 1.6mm PCB thickness, FR4 Hi TG, ENIG finish.

The stack up is:
Top solder mask
Top Copper
Prepreg
Inner 1 GND
Core
Inner 2 Power
Prepreg
Bottom.Copper
Bottom solder mask

My question is how to I assign appropriate copper thicknesses for top, inner1/2 and bottom layers? What should the core thickness and prepreg thickness be?

 

[KlausST]

Hi,

if you don´t have any requirement, let the PCB house do the decisions.

But if you need higher current capability, better heat spreading, or need HF design, then you need to decide the stackup and sizes on your own. You may look for ypical values.
It never is a bad idea to talk to the PCBV manufacturer.

Klaus

 

[Rajinder1268]

Hi,

if you don´t have any requirement, let the PCB house do the decisions.

But if you need higher current capability, better heat spreading, or need HF design, then you need to decide the stackup and sizes on your own. You may look for ypical values.
It never is a bad idea to talk to the PCBV manufacturer.

Klaus

I was going to talk to them, but I wanted to understand from my point of view.

For example 1oz - does that mean top / bottom / inner 1 and inner 2 should all be at 35um? I have seen 18um for the top and bottom, then 35um for inner layers? Not sure why?
My other question is, if the PCB thickness is to be 1.6mm, then should the thickness of each layer totalled together be 1.6mm?

How do I know what the prepreg and core thickness should be?

 

[KlausST]

How do I know what the prepreg and core thickness should be?

When you buy tyres for your car. Do you care about the ammount of steel mesh inside, the thickness of the rubber?
If you have special requirements, if you want to goto the limits, or across the limits (this is what you call "my point of view"): you probably do.

But honestly I never did care.

****

The same is with PCBs.
When I have no special requirements: I don´t care. The PCB house should use their standards, and I expect to get a good quality.

As soon as you leave the standards you have to calculate with increased fail rate.

You will find example stackups here in this forum, in the internet, at PCB manufacturers.

My other question is, if the PCB thickness is to be 1.6mm, then should the thickness of each layer totalled together be 1.6mm?

Do you see an option?

****
Standard ouuter layers are laminated with 17-18um Cu. Then during the manufacturing process (plating vias) there adds another 17-18um. This summarizes to 35um.

But you get various Cu thickness, if you need.

**
And if you use a 18um Cu inner layer it won´t get additional Cu, so it stays at 18um.

1 oz equals to 35um Cu.


Klaus

 

[PCBFAE]

Hi,
I am trying to understand about PCB layer stack up.
It is a 4 layer PCB, 1oz copper, 1.6mm PCB thickness, FR4 Hi TG, ENIG finish.

The stack up is:
Top solder mask
Top Copper
Prepreg
Inner 1 GND
Core
Inner 2 Power
Prepreg
Bottom.Copper
Bottom solder mask

My question is how to I assign appropriate copper thicknesses for top, inner1/2 and bottom layers? What should the core thickness and prepreg thickness be?

I was going to talk to them, but I wanted to understand from my point of view.

For example 1oz - does that mean top / bottom / inner 1 and inner 2 should all be at 35um? I have seen 18um for the top and bottom, then 35um for inner layers? Not sure why?
My other question is, if the PCB thickness is to be 1.6mm, then should the thickness of each layer totalled together be 1.6mm?

How do I know what the prepreg and core thickness should be?

Hi,
What Klaus shared are almost the right answer. as an experienced PCB technical guy in PCB industry, I would like to offer much more information to your questions.
1. when define 1oz for both inner and outer layer, the copper thickness should be controlled as following:
inner layer 24.9um(min), typical thickness 28-32um.
top and bottom layer 33.4um(min), typical 35-38um.
refer to copper control defined in IPC 6012E ( default IPC class 2)

when PCB house offer the stack-up for approval , the copper thickness for outer layer don't cover plating copper (average 20um) , this is why you could only see 18um for top and bottom layer in stack-up.

regarding the 1.6mm total thickness , if you could share the stack-up your present PCB supplier offered , I can explain and make your clear if the thickness 1.6mm covers all material like solder mask , plating copper, original copper , prepare and core thickness .
I hope above shares could help you out.

Koen.Hu

 

[marce]

Starting copper weight/thickness will be determined by the size of design features (gaps, trace widths etc.), and current requirements of the layout...
The majority of PCB's are usually around 35um (1oz) inner layers, 18um start for outers plated up to 35um, as shown above 35um inner cores are thinner after processing. They scrub the inner layers, to aid adhesion etc. so some copper is lost.
It is common practice to state required finished copper thicknesses on the PCB manufacturing drawing, and dielectric thickness/type when impedance control or similar is required. This is best done in conjunction with your PCB manufacturer as cost, ease of manufacture etc. need to be considered and they will recommend a stack up using their preferred materials.
Look at doing a CID course from the IPC, it gives a good basic understanding of all the info, standards etc. that you should be using to aid your understanding of PCB design.

 

[kingcrediepcba]

Hi,

Usually, PCB house will use the most economical one like this if you have not any requirement.

Linda