I need to specify the construction of a 4-layer PCB with transmission lines on the outer layers and planes on the inner layers. I need to control impedance and propagation speed. The target prepreg thickness is around 0.2mm (7-8mil). I can achieve that with a single ply of 7628 or with two plies of 2113 or 1080.

Most PCB stack-up I have seen use two plies for prepreg layers, even if the same thickness could be accomplished with a single, thicker ply. Why is that? What are the advantages and disadvantages of one versus two plies?

  • \$\begingroup\$ AFAIK, this is a manufacturing question --- like the reason might be your fab shop stocks the thinner material and not the thicker ones. \$\endgroup\$ – The Photon Dec 15 '17 at 1:18
  • \$\begingroup\$ I will definitely compare availability and cost, but I am more interested if there are differences in RF performance (manufacturing tolerances, variability and isotropy of Dk, etc) \$\endgroup\$ – Michael Dec 15 '17 at 2:16
  • \$\begingroup\$ It makes for ease of MFG \$\endgroup\$ – Tony Stewart Sunnyskyguy EE75 Dec 15 '17 at 2:29

What are the advantages and disadvantages of one versus two plies?

For controlled impedance, you get the best performance with zero plies. That is, if you are concerned about a repeatable RF performance between certain layers in a multilayer PCB layup, you should arrange for the impedance critical layers to be separated by core.

If pre-preg between signal and ground is unavaoidable, then arrange for that space to be mostly core, and minimise the pre-preg thickness, so the core dominates the gap.

In your case with inner planes and tracks on the outer layers, it sounds like the PCB fab is trying to sell you a foil-prepreg-core-prepreg-foil arrangement. Ask for a core-prepreg-core quotation. It might be slightly more expensive, but the inner to outer impedance will be better controlled.

If you want the board to be built at any one of several fabs, or are prototyping at one fab then building in volume at another, then it's vital that your controlled impedance layers use core. Because core is built and supplied to a specification, you can control what the fab uses. Even if you specify the pre-preg material, each fab may handle, assemble, press and cure it differently, and even the same fab may do those differently at different times. Using pre-preg for controlled impedance layers is a good way to get unexplained variations in performance between builds.

Most PCB stack-up I have seen use two plies for prepreg layers, even if the same thickness could be accomplished with a single, thicker ply. Why is that?

It's mostly down to the economics of the FAB. I've they've got a good deal on the thin stuff, then they'll use it in preference to the thick. One or two plies, pre-preg is bad for consistency.

In theory, two plies of pre-preg will give you better (less bad) dk isotropy if they are at 45 degrees to each other. Are the fab offering this orientation option, even if at a higher price? Obviously it wastes material for them, and will compromise their standard handling.

You don't say what frequency you're operating at or what tolerance you want to achieve. FR4, core or pre-preg, by the electrical loss of the resin, the coarseness of the glass weave, and the variability of the glass/resin proportions, performs poorly above a few hundred MHz. But core is less bad, it has a much better dimensional and dielectric constant tolerance than pre-preg. Core is made under repeatable conditions, whereas pre-preg is pressed between whatever copper etching you happen to have done.

Remarkably, FR4 is used in WiFi to 2.4GHz, where the designers have used a lot of skill to make the circuit accept the poor tolerance and loss, for the cost benefits. If you are working at 2.4GHz, then using pre-preg rather than core for your FR4 layers is one risk too far.

If you want high tolerance, or are operating in the GHz, then you might want to consider RO4350 for the outer cores, with FR4 pre-preg to join them together. It's more expensive than FR4, but an order of magnitude better on RF tolerance, and better yet on performance. It's compatible with FR4 processing, so can be assembled the same way.

  • \$\begingroup\$ Thanks for the answer. This is for 2.4GHz. Prototypes (from OSH Park) using Isola FR408 2 x 2113 worked well. Now I am trying to have this made in higher volume in China and I suddenly have a choice regarding stack-up. I'll definitely ask about the core-prepreg-core option. Other than that it seems that finer weave is preferable. \$\endgroup\$ – Michael Dec 15 '17 at 6:36
  • \$\begingroup\$ If you're moving between fabs between prototypes and production, then core-prepreg-core is essential. Cores can be specified to be the same between fabs, you just specify the material. Even if you specify the pre-preg material, different fabs may assemble, handle, press, cure differently. It's vital you build, test and debug new prototypes on core-prepreg-core before moving the process to 'somewhere cheaper',otherwise you lose control and are setting yourself up for months or years of grief. \$\endgroup\$ – Neil_UK Dec 15 '17 at 6:47
  • \$\begingroup\$ If you do change to a new stackup or core-p-core, then some parameters will change, you'd expect them to change. This is some voluntary grief you would be pulling down on yourself now. As such, it might be difficult to sell to your bosses. But it's like doing any preparation, it's always more expensive now to do it rather than not do it, but it could avert a disaster in the future. Would you send the design 'out there' to be built with permission to switch to 20% resistor tolerance if they liked? Why do the same with your vital impedances? \$\endgroup\$ – Neil_UK Dec 15 '17 at 7:01

Having spoken to PCB manufacturers here in the US and one in Europe specifically about this issue, I learned the following:

  1. PCB manufacturers control the final thickness of the finished boards as well as the dielectric layers formed using prepreg compression and resin flow. The finished thickness is important for differential pair and other controlled impedance signal lines. To be able to control the thickness, they need some resin to be able to flow out. 7628 is low resin content versus 1080 (see Isola technical prepreg resin content specs). Thus, low resin content prepregs limit thickness control.

  2. Higher flow at the laminate interface tends to lead to better adhesion and lower chances of delamination in the subsequent part population (reflow oven).

  3. Modulus gradient. The gradient in mechanical modulus (change in stiffness) also leads to delamination. Two prepregs back to back will have two very clean prepreg surfaces back to back that bond very well. The difference in modulus between the prepregs and the already cured core is then spread out over two layers of prepreg instead of one. The adhesion between already cured core and prepreg is typically lower than prepreg to prepreg (especially when prepregs are same resin system, CTE, and glass matrix).

  4. Cost: 2 layers costs customer more. 1 layer costs manufacturer more in requiring more engineering time/tighter manufacturing control.

My experience with this issue is in replacing (2 x 106) construction with (1 x 2113) or (1 x 2125). 106 is the most expensive prepreg and highest resin content. 2125 is more common in Europe evidently but similar thickness and usage to 2113. I have heard there is at least one manufacturer that uses 1 x 2113 (external single layer 2113) construction as default or standard construction but have not found it yet.

From contacting Isola, (core and prepreg manufacturer), I learned the 2113 laminate was actually developed over a decade ago (pre 2010) specifically to replace the usage of two prepregs in some constructions.

I have been designed circuitboards for 20+years from 2 to 8 layers.


I don't know of any advantage or disadvantage of using multiple vs. single plies. However, be aware that different glass weaves have different Dk and Df values. You should also be aware that tighter weaves will result in thicker pressed thicknesses compared to looser weaves - resin doesn't flow as easily between tight strands vs. loose strands. This can also impact impedance and propagation delay.

If you knew all this already, I'm sorry. I would ask an FAE from your fab shop, and they should be able to tell you everything. The tips I gave you above came from an FAE I worked with when determining the stackup.

You may find useful these app notes on glass weaves by Altera and Isola Group.

  • \$\begingroup\$ Hi, FYI both your links go to one place - the Altera app note. Therefore it seems that your link to the Isola Group app note is missing. \$\endgroup\$ – SamGibson Apr 14 '18 at 14:29
  • 1
    \$\begingroup\$ Thank you for that correction. I have added the Isola app note. \$\endgroup\$ – FullmetalEngineer Apr 18 '18 at 15:42

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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