Materiales for Stackup

[Bermell]

How important do you consider the materials for your stackup configuración?

I mean, you don't need to select them for impedance calculations, for example

Thank you very much

[qdrives]

You DO need them for impedance calculation.

[Bermell]

Thank you qdrives for your answer. I calculate the controlled impedance, using the excellent Sierra software.

Please, check the picture attached. As you can see, i can't select the material, in the Sierra program
Thank you very much

[Bermell]

I think the following link can help

https://www.protoexpress.com/kb/pcb-material-selection/

[qdrives]

That is the picture from the presentation.
If you click on the "Try this tool" button and wait for about 1 minute... it opens the tool.

[robertferanec]

I think, you will need to select materials (or predefined / recommended stackups by sierra circuit) somewhere. I tried that tool once a while ago and I think that was the case. As qdrives mentioned, materials need to be specified for impedance calculation.

[binayak]

Bermell,

You can't randomly choose dielectric constant and dielectric thicknesses of cores and prepregs to get controlled-impedance stackup. You need to cross check whether there is material available in the market that matches your requirements.

Otherwise, you will create a great stackup in the tool, but won't be able to manufacture it!

In addition, if it's a high speed board with signal integrity involved, and if you change dielectric constant, dissipation factor, dielectric thickness, etc. at the end due to the fabricator's recommendation (because you the stackup dimension you decided are not available in the market or with the fabricator), all of your signal integrity analysis work has become completely useless.

So it's always better to involve the PCB fabricator from the start, and create stackups based on actual material available to you in the market instead of some random values that give you controlled impedances.

Binayak

[qdrives]

binayak be careful with the terms "controlled impedance" and "controlled stackup" as also explained here: https://www.youtube.com/watch?v=mkf52cOPSRU

For those who did not know, Isola also has calculation tools https://www.isola-group.com/resources/design-tools/
There you can specify how much copper is on a layer and it will calculate how much 'thickness' is lost between the copper. This is especially useful for thicker copper (ie > 2oz).
Limitation is just their materials.

[binayak]

qdrives

I've seen lots of boards where the designer mentions only impedance and let the fabricator do whatever they want. Some call this "the controlled impedance stackup design".

I find the so-called "controlled impedance stackup design" methodology incomplete - something like a half-baked cake. It is the designer's responsibility to engineer the stackup - not the fabricator's. When I mentioned "controlled impedances" in my post, I was NOT referring to that stackup methodology.

What I was saying is that impedance is JUST one of the factors that we have to consider when designing a stackup.

However, stackup design is a holistic process - there are lots of other factors interplaying with each other. It involves a LOT MORE than just impedance.

When you go for high-speed designs, stackup design becomes THE most important piece of engineering work you will do. It will make or break the design!

[qdrives]

binayak I rarely do high speed design. I am more on high voltage and high current. Therefor I am limited on how close two layers can be to each other (>= 0.13mm) and usually do 2oz or more copper thickness.

My remark was as mentioned in the video. In my opinion:
"Controlled impedance" -- here the fabricator 'tweaks' the design to get the impedance correct. A wrong stackup is the fault of the fabricator. A test coupon should be made and tested to verify that the impedance required is reached.
"Controlled stackup" -- the designer specifies what he wants in materials and thicknesses. If he makes a mistake it is his fault.

Perhaps what happens often, as I also think robertferanec does is a bit a mix of the two:
Asking the fabricator what stackup and trace width+spacing is required for a given impedance. Then using those specifications to produce the boards more as a "controlled stackup" way. This means no test coupon and therefor lower cost.

[binayak]

qdrives It is always better if we are in contact with the fab shop throughout the stackup design process.
By interacting with the fab shop early on, we can evaluate their ability against our requirements. If there is mismatch, we can change the fabricator. If we are good with the fab shop, we can sit together and make sure that our PCB stackup requirements are fulfilled with the materials and capabilities available with the fab house.

Consequently, when the stackup is completed, both the designer and fabricator are happy.

[robertferanec]

Perhaps what happens often, as I also think robertferanec does is a bit a mix of the two

- we always design for possibilities to change PCB manufacturer, so designs always need to be done the way pcb stackup can be changed and track width adjusted (different PCB manufacturers use different materials). And that is one of the reasons why I often always route boards with wider tracks and adjust the impedance controlled track width after the board is finished.

Or the other words, I do it this way, because if we need to change a PCB manufacturer and they need to use different materials, they have a lot of flexibility and space (because the board was routed with wider tracks) to adjust track width to meet specific impedance.