3
\$\begingroup\$

I'm making my first 4 layer PCB (1 signal, 2 GND plane, 3 PWR plane, 4 signal) with impedance control. I was checking the layer stack up for Altium to make sure the thickness and dielectric constant (dk) were correct and I realized they were not. Checking a couple of manufacturers I quickly realized I don't know what I'm doing.

My experience is low speed PCBs that work fine with FR4 on 2 layers and no impedance control. It looks like the dk varies by material and thickness. Asking the manufacturers what dk value their PCB material has just leads to "for what PCB material" question. I don't know, FR4 ok? LOL.

The design I'm working on has an Infineon psoc62, an eMMC memory and a GPS module. The only controlled impedance traces are for the eMMC, GPS antenna (both 50 Ω impedance) and USB 2.0 ports (one on the MCU and another from the GPS module, both 90 Ω impedance). The eMMC will have the highest clock source (from the MCU) at 45 MHz. I see different types of PCB material and their properties but I'm baffled.

How do you know what type of material to use? Is FR4 material ok for the 50 Ω and 90 Ω impedance? Is there a range for the value of the dielectric constant (dk) for a specific material and if so how do I know what to set it up in the stack up?

\$\endgroup\$

2 Answers 2

Reset to default
3
\$\begingroup\$

FR4 material is a composite material, not originally designed for controlled impedance, which is why the dk specifications are somewhat loose. However, it can be used for GHz designs (it's the staple for 2.45GHz WiFi), if the application is tolerant enough. This means almost all applications, so RF or high speed logic signals between modules and ICs. Do not use it for microwave filters, or metrology, for which you would use a proper RF material like RO4350.

A good rule of thumb for 50 ohms microstrip (trace above ground) on FR4 is for the track to be twice as wide as the substrate is thick.

Avoid using a pre-preg layer as the substrate, as if FR4 is poorly specified, pre-preg is even worse. Most board fabs will try to sell you a central core with two outer foils, as it's often a slightly cheaper build. Insist on two cores stuck together, this gives you core FR4 between the top signal layer and the ground reference plane below.

\$\endgroup\$
5
  • \$\begingroup\$ Could you elaborate what you mean with "worse" wrt the prepreg ? E.g. are there dielectric losses or something ? If so at what frequency? Maybe that is even good for EMC ?! \$\endgroup\$
    – tobalt
    Jul 28, 2022 at 10:38
  • \$\begingroup\$ @tobalt Not losses, but larger variations in glass/epxoy ratio. I've had board manufacturers run out of 'this' thickness prepreg, so use two of 'that' thickness instead without telling us. Same nominal height, but quite different epoxy ratios. The thickness is less controlled as well. It depends how much local copper has been etched away nearby how much squidge there is sideways of epoxy. Messy unpredictable business using prepreg for dielectric. \$\endgroup\$
    – Neil_UK
    Jul 28, 2022 at 12:38
  • \$\begingroup\$ Ok I see, so mainly the trace impedance could deviate further from some calculator number. Maybe 20% ? Probably that only really becomes an issue for really long traces or higher frequencies above 100 MHz, because I have used countless cheap China prepreg dielectrics and never had functionality issues. \$\endgroup\$
    – tobalt
    Jul 28, 2022 at 13:51
  • \$\begingroup\$ Using a core instead of the two prepegs? won't that make the PCB a lot thicker than 62mils? 4pcb.com gave me info on the cores and prepegs. The core materials are 39mils thick, the two prepegs make at most 10mils in thickness. So that's 10+39+10 vs 39+39+39? ignoring copper and mask. \$\endgroup\$
    – Rodo
    Jul 29, 2022 at 17:45
  • 1
    \$\begingroup\$ @Rodo You choose core and pre-preg thicknesses to make the board the desired thickness, they're available in a whole range. I've made a 1.6 mm board, and gone from 4, to 6, to 8 layers by changing core and prepreg thicknesses. \$\endgroup\$
    – Neil_UK
    Jul 29, 2022 at 19:27
3
\$\begingroup\$

How do you know what type of material to use?

For sub 100MHz signals it's not as critical to have a controlled impedance and FR4 is fine. zThe main thing is knowing what the dielectric permittivity \$ \epsilon_r \$ of the material is. Once you know what the range AND the layer stackup is you can plug that in to a tool (like saturn PCB toolkit) and calculate impedance for single pair transmission lines or diff pairs. (you need to know the height above the reference and \$ \epsilon_r \$.

You can find the dielectric permittivity and the stackup by asking the PCB manufacturer.

For signals that are in the 30-50MHz you probably won't have to worry much if you keep the traces short and also watch capacitance (of both traces and ports). It's also a good idea to avoid vias with these signals if possible.

If not you may need to leave a terminating SMT pad for a resistor to reduce reflections if you see them on those lines.

\$\endgroup\$
2
  • 2
    \$\begingroup\$ It might be a good idea to put SMT pads for series and parallel connections on a prototype high-speed track, even if one ends up populated with just a 0Ω resistor. Because it's hard to tack these in later if needed. \$\endgroup\$
    – rdtsc
    Jul 27, 2022 at 21:11
  • \$\begingroup\$ Good point, I forgot about series \$\endgroup\$
    – Voltage Spike ♦
    Jul 28, 2022 at 0:29

Your Answer

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

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