I've been working on a four layer board with 100Ω differential pairs. Prototypes were built, impedance was measured, things were fine. But then as I tried to move the production to a different facility, I discovered that some PCB fabs use a much thicker prepreg layer (dielectric between top layer and inner 1 copper).

If you look at specs from MacroFab (https://s3.amazonaws.com/mfprodpublic/datasheets/MacroFab+Stackup+Report.pdf), they use a 0.23mm prepreg layer. OSHPark has an even thinner 0.17mm (6.7mil) prepreg (http://docs.oshpark.com/services/four-layer/). I've seen similar numbers in standard stackups from Chinese manufacturers as well.

But then I encountered a local fab that specified 0.36mm, and looking around I saw that the Eurocircuits standard 4 layer build has a 0.36mm (14mil) prepreg layer (http://www.eurocircuits.com/images/stories/ec09/ec-std-buildups-0-8-layers-english-4-2010-v2.pdf).

I am puzzled as to how this kind of stackup can be useful.

Assuming 0.1524mm (6mil) trace separation, 35µm copper, with a 0.23mm prepreg, I calculated 0.233mm width for 100Ω differential pair (differential microstrip) traces. That's about 9mil, and it's perfectly fine.

But again with a 0.36mm prepreg (same 6mil trace separation) I end up with my differential pair traces having to be 0.32mm wide -- 12.6mil! That seems too wide to be useful, you can't route those traces to 0.5mm pitch ICs. And things get even worse if you need 90Ω (USB).

So, what am I missing? From this point of view, the thick-prepreg stackups of some manufacturers are useless. But they exist (and in fact are standard!) for some reason. How do people use them?


2 Answers 2


So, what am I missing? From this point of view, the thick-prepreg stackups of some manufacturers are useless. But they exist (and in fact are standard!) for some reason. How do people use them?

I think what you're missing is the fact that majority of four-layer boards will not have ANY controlled impedance lines. Therefore, any old prepreg thickness will do.

Other than controlling trace impedances, four layer boards are useful for improving EMI performance by providing better grounding, allowing more dense component placement and simplifying routing.

It would be interesting to know what factors determine the PCB stackup in these cases, though. Maybe it is the ease of manufacture or cost of material?

  • \$\begingroup\$ Ok, I thought the #1 reason for going with a 4-layer board is to get controlled impedance. \$\endgroup\$ Commented Aug 28, 2016 at 10:22
  • 1
    \$\begingroup\$ The #1 reason to go from 2 to 4 layers is to get a continuous ground plane. #2 is to get a continuous power plane. Both can improve power integrity and EMC. Controller impedance is a further step up in complexity, but only useful when high frequency signals are present. \$\endgroup\$
    – The Photon
    Commented Aug 28, 2016 at 15:30
  • \$\begingroup\$ Making some small PCBs with USB or Ethernet (RGMII) that need controlled impedance at some point is not a real step up in complexity compared to improvement of power integrity and EMC of low frequency signals. \$\endgroup\$
    – zeqL
    Commented Aug 28, 2016 at 20:44

There is a lot a parameters to take into account when you make a PCB and with DIY PCB fab, some information may be missing.

For instance MacroFab's stackup state a 1.6 mm PCB thickness, but is this the final thickness, after lamination or before ? Also what's the margin on this thickness.

Also impedance have often a 10% margin to take into account manufacturing process. So you computed a 100Ω impedance and it gave you 6/9mil for a differential pair.

But with a different prepreg you tried to stay at 100Ω, but have you computed the impedance with the 6/9mil differential pair ? If you have 95Ω, it's fine.

You also kept the same trace separation, where you could have changed it.

You're just talking about prepreg thickness, but prepreg can have a different dielectric constant which will also have an effect on impedance. If one prepeg have a dielectric constant of 3.82 and another will have 4.34 but they both will be advertised as "FR-4".

The fact is when you can't define your own stackup with the PCB manufacturer, you will have to change your design, either having different impedance or having different trace size to keep the same impedance.

You need to know that prepreg have fixed sizes from prepreg manufacturer, and they do not provide the same thicknesses for every models. So for instance if you choose Isola's prepreg you may not be able to have the same thickness than from prepreg from Rogers or Panasonic, so it depends of you PCB manufacturer.

Finally, when you look at the core's thickness, it changes between manufacturer. And as you often put GND and Power plane in the inside layers, you will have a natural decoupling effect between them, and the smaller the dielectric thickness between PWR and GND planes, the better the decoupling effect will be.

  • \$\begingroup\$ Well, with the thicker prepreg (0.36mm) I get 113Ω, all other parameters remaining the same. I figured this isn't fine. As for trace separation, I am at 6mil (0.1524mm) and I do not want to go any lower. Increasing trace separation increases the impedance, so my only option is to increase width, which results in really think traces. \$\endgroup\$ Commented Aug 28, 2016 at 10:21
  • \$\begingroup\$ I don't know which software you used for the computation. I run some test with Saturn PCB and clearly it don't see any problem with the Eurocircuit stackup (0.36mm prepreg). You can have 100Ω with a separation of about half the trace width (300µm/150µm for instance). Ok the trace will be wide. But for your 0.5mm pitch component you can use the "neck down" principle : you reduce the trace width near the via/pin to be able to route it. \$\endgroup\$
    – zeqL
    Commented Aug 28, 2016 at 20:51
  • \$\begingroup\$ I normally use the online calculator from Mantaro (mantaro.com/resources/impedance-calculator.htm). I know it produces fairly good results, because I had results measured (results of 102.2Ω, 100.5Ω and 98.9Ω on three test boards). \$\endgroup\$ Commented Aug 29, 2016 at 7:52

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.