How Do you decide Prepreg/Core thickness in 4-Layer Boards

Design and Layout
1

I’m designing a 4-layer PCB with a total board thickness of 1.64 mm, and I’m trying to understand how to approach stackup planning.

Are there standard PCB thicknesses for core and prepreg layers used in multilayer designs? How do printed circuit board manufacturers typically decide or recommend the thickness of each PCB layer?

I’ve seen some 4-layer stackups that use one core and two prepreg layers, while others use two cores and one prepreg. Are both configurations acceptable, or is one preferred depending on the application or fabrication method?

1 Like
2

Although four layers of copper does not sound as though it can make for many ways of implementing a board, the reality is rather different. And the results are not all the same, even if the electrical connectivity and hole and via positions are the same. If the materials are not specified, the separation between layers not stated, and the layer sequence are not provided to the company that makes the bare PCB, you could get almost anything when you receive your boards. It can be enough to make the difference between passing or failing EMC tests. The decisions made are therefore important.

This does not mean that there is only one right answer. There can be quite a few right answers though not all will be good answers. As with many things, it is a question of choosing a good balance.

Suppose you want your board to have USB2 or USB3, these expect a differential impedance of 90 Ohms or 85 Ohms. But you have lots of tracks on the board so you need these differential pairs to be fairly narrow traces with say a 2x trace width gap between them. To do this you need a thin gap (prepreg) between the outer layer (where your signals are) and the reference plane immediately beneath. This favours a thick core at the centre and then a thin prepreg and foil attached to create the top and bottom layers.

If you want some really high frequency differential pairs, one of your main concerns is signal loss. To reduce the loss you need wider traces, but wider traces need a bigger gap between signal layer and plane, so you shift the balance of thicknesses to make the prepreg be thicker (or just use two or three of them).

In general, cores can be very thin, but you can get a whole range of thicknesses up to the thickness of your whole board. Prepregs are always thin. The copper layers can also vary in thickness, 18um and 35um being two of the most common sizes. You could find the data sheets for the PCB materials and work out what combination works best for you; but the better way is to talk to you PCB supplier. If you ask them for their advice on cores and prepregs, and you tell them the things that matter in your design (like perhaps controlled impedance) they will probably suggest a good combination of materials to design with - but better, they’ll do this knowing that they are recommending materials they have in stock and that will probably give you a good price with it.

The last thing about choosing a stack-up is choosing what to put on each layer. With four layers it is tempting to think that the layer allocation should simply be Signal, Power, Ground, Signal; but if you’re using frequencies over say 10 MHz, this stack-up is a poor choice. A much better one is Signal & Power, Ground, Ground, Signal & Power. This is good for medium/high/very high frequency work and done well is excellent for EMI (if you remember the rule that where you put in a via to move you signal between top and bottom layers, add a Ground to Ground via close by. Route the power as a thin signal to begin with, then thicken it using polygon pours. This approach yields surprisingly good performance, and is easy to implement. From experience, this method allows USB2/3/4, PCIe, HDMI to be tracked on 4-layer boards that are regularly 15dB clear of the class B limit lines for radiated emissions, even on peak detect mode (and better on quasi-peak measurements). On the other hand, getting close to this with Signal, Power, Ground, Signal stackup is impossible (or more accurately, I’ve never seen it done).

Key take-away: not all 4-layer boards are created equal, and the differences can be large. For the fine detail, talk to the PCB manufacturing company you want to use and take their advice. Give them more detail in what you’re looking for and you should get a good lead on what you need. Once you’ve got some sort of idea about what you want, look at the Stack-up designer tool on the Sierra website. There are other tools on this site that are available to use as well.

Hope that helps a little.

3 Likes
3

A little? I think that helps A LOT! :grinning_cat:

4

Most FR4 suppliers offer a range of standard core thickness values, often in a set that might progress in steps like 1, 2, 5, and 10 mils. Prepreg thickness, on the other hand, is less fixed because it depends heavily on the resin content and how much pressure is applied during lamination. Because of these variables, it’s essential to know not only which laminate you’re using but also the vendor’s typical process.

To handle this, I usually round the cores to neat 5-mil increments and then adjust the prepreg thickness to complement those values, while noting that the overall board thickness is maintained within an IPC tolerance of about ±10% (with individual layers around ±5 mils). It’s crucial to spell these specifics out on the fabrication drawings and work closely with your manufacturer, especially since some lower-cost fabs might default to their standard recipes, regardless of your instructions.

For designs where precise impedance is critical, It is recommend to oversize the traces (for example, stating that all 11-mil traces should be resized to achieve a 50-ohm impedance within a ±10% tolerance) and then choosing a stackup that accommodates these wider trace requirements. This approach helps maintain signal integrity, particularly on thicker boards with multiple layers.

1 Like
5

One thing worth adding to this discussion is that prepreg thickness doesn’t have a fixed finished value, even if the starting material is known. During lamination, the resin in the prepreg flows and fills voids between adjacent copper layers on each PCB layer. This flow behavior depends on several factors like Copper weight (thickness), Copper coverage/density on each layer and Initial resin content of the prepreg.
As a result, even if two designs use the same prepreg and core materials, the final dielectric spacing between layers can vary due to these copper/resin interactions. This variability is one reason why it’s difficult to define a universal standard prepreg thickness post-lamination. When planning your stackup, this means you can’t just rely on raw material specs, you need to work closely with your PCB fabricator to model actual results based on your layer patterns and impedance requirements. They often simulate resin flow and compression to ensure target thicknesses and impedance values are met.
In terms of stackup choices (1 core + 2 prepreg vs. 2 cores + 1 prepreg), both are valid. The best choice depends on factors like layer symmetry, layer registration needs, total PCB thickness, and whether you want better mechanical stability or specific dielectric thicknesses for impedance control. While datasheets give baseline thickness values, prepreg thickness is not fixed post-lamination, it’s shaped by your copper geometry. Always coordinate with your printed circuit board manufacturers to finalize the stackup based on actual build conditions.

1 Like
6

Using two cores in a 4-layer PCB stackup is unusual and generally not the most cost-effective approach. Cores are fully cured laminates and usually more expensive than prepreg. They also add rigidity and structure to the board, which is useful in complex builds, but in a simple 4-layer stackup, it’s often overkill.

Most printed circuit board manufacturers default to a 1-core + 2-prepreg configuration for 4-layer boards, with copper foil on the outer layers and the core sandwiched in the middle. This structure is both cost-effective and aligned with standard PCB thickness profiles (like 1.6 mm total thickness), and it’s also easier for them to process using well-established lamination cycles.

If you’re specifying a non-standard stackup, like 2 cores and 1 prepreg, you’ll need a very specific electrical or mechanical reason to justify it, and should coordinate closely with your fabricator in advance. Not all shops are set up to run that configuration, and if you don’t clarify your intent, you risk delays or rejections. In general, always work with your board house early in the design phase to ensure your PCB layer configuration fits their processes, available materials, and pricing model.

1 Like
7

When planning a 4-layer stackup, I always start by asking the printed circuit board manufacturers what their standard stackup looks like for that layer count, including materials, copper weights, and thicknesses. Most board houses have standard recipes using readily available cores and prepregs that align with common total thicknesses (like 1.6 mm or 1.64 mm). Starting with their defaults saves time and keeps costs down.

If I’m aiming for a particular impedance, I use that stackup as a first pass to estimate trace geometries to establish a rough baseline before fine-tuning for accuracy. Later, I’ll fine-tune based on actual impedance targets.

Be careful about over-specifying the stackup. Unless you’re designing for controlled impedance or RF, you usually don’t need to dictate exact dielectric thicknesses or material systems. That said, for high-frequency or HDI designs (like blind/buried vias or specific dielectric performance), you do need more control. But again, the process should start with your fabricator not with the stackup tool in your CAD software.

I’ve only had a few RF projects where I fully specified materials and instructed the fab house to follow them exactly, and yes, it was costly. For typical multilayer PCBs, the best approach is to understand what your PCB board manufacturer offers by default and work backwards from there. It’s usually far more cost-effective and avoids surprises during manufacturing.

8

Many PCB websites have example stackups that they typically use for common layer counts. On a 4 layer stackup, many fabs will use a core of around 1mm/40mil thickness and add prepregs to build out to the overall thickness requirements. On Sierra’s site, they have a downloadable stackup guide and also the stackup calculator which can aid in figuring out what to expect.

1 Like
9

Thanks for pointing that out! And here’s the link to our Stackup Designer tool: https://www.protoexpress.com/tools/pcb-stackup-designer/

10

Thanks everyone.