Designing a 4-layer PCB with impedance control (1 signal, 2 GND plane, 3 PWR plane, 4 signal) has raised some questions. While checking the layer stack-up in Altium, the thickness and dielectric constant (dk) appeared incorrect. After consulting with several manufacturers, the confusion only increased.
My background is in low-speed PCBs using 2 layers with FR4 and no impedance control. It seems the dk varies based on material and thickness. When I ask manufacturers about the dk value, they ask, “For what PCB material?” and I don’t know how to respond beyond suggesting FR4.
The first task is to determine the highest frequency traveling through your board. The next is determining how much loss you can tolerate.
If you can use FR4, it’s the lowest cost, easiest to find, probably the easiest to process. The dielectric constant on a piece of FR4 material varies for several reasons. 1) The manufacturers will use slightly different recipes (like most products) and might list the Dk a little higher or lower than another manufacturer. 2) The glass cloth used. There are a dozen or more popular glass fiber weaves in use. Some are basically a tiny weave of loose, pushed together fibers (kind of like placing a thick rope between two strips of a blanket; while others are carefully woven tightly drawn together, or better yet, squished flat. The coarser the weave the more variance in the Dk as the trace runs across the board. Also, the coarser the weave the less fully the epoxy can fill all the little spaces. So a fine weave, spread out, allows the highest percentage of resin and the least changes in Dk. 3) They typically specify no tighter than 10% tolerance for Dk. 4) Sometimes Dk is specified under slightly different conditions (like pre or post lamination. After all that you need to determine what layer spacing will give optimal results as far as a useful, routable, pair of traces. That is, you want a later spacing that won’t demand a 1 mil trace or a 300 mil trace, you want something that works out to 6-12 mils or so.
If you’re doing the really high frequencies then you are usually forced to go to a special, low loss laminate to meet your goals, but it will cost you more.
With your frequencies and other requirements I’m betting you can still use FR4 and get good results unless the board is quite large. Work with your PCB shop - they’ll help you.
If you ask me how much a desk with drawers weighs, I have a general idea for a typical desk, and I probably don’t mind being a little wrong.
If you ask someone who works in a furniture store, they’ll be thinking about dozens of different types of desks, and will be thinking about the differences between them. So they won’t have a single answer at the ready. Maybe they’ll ask what the desk is made of.
Wood? That does narrow it down compared to steel or plastic, but … oak vs pine matters. They might even be thinking of balsawood vs 3-inch thick ironwood.
FR-4 is the “wood” of PCB construction. It is a good default, but there is still lots of variation, and your manufacturer has to pick one (or more) specifically. @allank talked a bit about how to do that, but the “I don’t even know what questions to ask” answer is to ask them what their default stackup is. Then maybe confirm that it will work for your needs. (It sounds like it probably will.) If you want some tools before talking to someone, maybe look at:
FR4 is a composite material that wasn’t originally designed for controlled impedance, which is why its dielectric constant (dk) specifications are somewhat variable. However, it can still be effectively used for GHz designs, such as the 2.45GHz used in WiFi, if the application is sufficiently tolerant. This applies to most applications, including RF or high-speed logic signals between modules and ICs, but not for microwave filters, where a dedicated RF material like RO4350 is recommended.
A practical guideline for achieving 50-ohm microstrip (trace above ground) on FR4 is to make the track width roughly twice the substrate thickness. It’s also advisable to avoid using a pre-preg layer as the substrate because its specifications can be even more variable than FR4. Most board manufacturers may offer a central core with two outer foils as it’s often cheaper, but you should insist on using two cores bonded together. This ensures you have core FR4 between the top signal layer and the ground reference plane below, which is preferable for maintaining controlled impedance.
I appreciate the tip about how to more tightly control impedance, and why someone might prefer the “old” style of two cores. But for the original poster’s actual problem, is it safe to say that they aren’t pushing the envelope hard enough to need special materials or construction?
Yes Jim, you’re correct. Given the original poster’s application, FR4 should be more than sufficient unless there are unusual environmental conditions to consider. Based on the requirements and the details provided, FR4 is a solid choice, and a standard construction should be perfectly adequate without the need for a more complex two-core setup.
For signals below 100 MHz, controlling impedance is less critical, and FR4 material generally works well. The key is to know the dielectric permittivity (εr) of the material and the layer stackup. With this information, you can use tools like the Sierra’s impedance calculator to calculate the impedance for single-ended or differential pairs. You’ll need to know the height above the reference plane and the dielectric constant.
To find the dielectric permittivity and stackup details, you can consult your PCB manufacturer.
For signals in the 30-50 MHz range, as long as traces are kept short and capacitance (from both traces and ports) is managed, you should be fine. Avoiding vias for these signals is also advisable. If reflections become an issue, consider adding a terminating SMT pad for a resistor to mitigate them.