I am absolutely new to flex PCBs. I saw some from time to time but never designed one myself.

Now I'd like to get into this topic and the first task would be to create a ~ 10cm board to board interconnect flex PCB with 90 ohm (USB) and 100 ohm (LVDS) controlled impedance traces on it.

I used the KiCAD PCB calculator, asked the PCB manufacturer about the tangent loss (0.01) and dielectric constant (3.3) to calculate trace width and spacing, as I am used to from designing standard PCBs with FR4 material.

KiCAD PCB Calculator

I realized pretty quickly that the trace widths and spacing I'd need to achieve e.g. 45 ohm differential would be way out of spec.

I assume that my assumptions are completely wrong. How do you guys do that? Just ignore the impedance of the flex PCB?

  • \$\begingroup\$ is the thickness of the substrate really 25 µm? 100 to 200 µm would be closer to what I expect. \$\endgroup\$ Apr 18, 2023 at 13:17
  • 1
    \$\begingroup\$ jlcpcb.com/help/newsdetail/… - yes, the Polymide Layer between the 2 Copper layers is spec'ed as 25 um thick ... \$\endgroup\$
    – pm4812
    Apr 18, 2023 at 14:41
  • \$\begingroup\$ and if you check the specs from PCBWay: pcbway.com/pcb_prototype/Stack_up_for_FPC.html - they also spec the thickness of the "polyimide core" with 25um. Seems to be true ... \$\endgroup\$
    – pm4812
    Apr 18, 2023 at 14:49
  • 1
    \$\begingroup\$ You should not be trying to achieve 45 ohm diff impedance, but rather 45 ohms, or 50 ohms single ended impedance on each trace. \$\endgroup\$
    – SteveSh
    Apr 18, 2023 at 15:21
  • \$\begingroup\$ I'll see if I can find the stackup on the last flex design I was involved with for LVDS. \$\endgroup\$
    – SteveSh
    Apr 18, 2023 at 15:22

2 Answers 2


If you need impedance control, don't use such thin core. You can request them to make what you need.

From the PCB Way page you have linked, at the top: "The following is the usual FPC stackup information. If you need custom FPC stackup, please make note and we will manufacture according to your requirement. Polyimide (PI) is the most commonly used thermal curing insulating material in flexible circuit processing. The thickness range of the material is generally 12.5μm (0.5mil) and 125μm (5mil). Divided into with glue and without glue, the DK with glue is 3.5, and the DK without glue is 3.3."

In the past, I have used 0.075mm core for USB flex.

  • \$\begingroup\$ thanks for your answer. I just calculated your example with the KiCAD PCB Calculator, using 75 um core, 0.25mm track width and 0.25 mm spacing and the result is Zodd=~19 Ohm (=> Zdiff=~38 Ohm). Does this mean you simply ignored the impedance requirement for USB and it worked anyway, because the frequency is relatively low (12 Mhz)? \$\endgroup\$
    – pm4812
    Apr 18, 2023 at 15:23
  • \$\begingroup\$ No, do not ignore the impedance requirement. I use Allium for impedance calculations. 0.25/0.25mm seems wrong with this stack-up. 75um core, differential 90R (USB). I get 0.125mm track 0.2mm gap. If your supplier can't make this work, have go with something even thicker then. This was just an example from a real-world design that works at USB 3.0 speeds. \$\endgroup\$
    – Zygis
    Apr 18, 2023 at 15:32
  • \$\begingroup\$ ok, that helped! looks like I can create 90 Ohm and 100 Ohm (both differential) with 100 um core, 0.25mm width and 0.3mm spacing. I guess I start understanding that topic ... \$\endgroup\$
    – pm4812
    Apr 18, 2023 at 15:39

I'm also learning about flex and impedance control. I've asked jlcpcb about their flex service, and they told me that they do not officially support impedance control for flex. Nevertheless, I am guessing that it would be possible with their services under some conditions.

  1. since they are clear that they do not support this, various production batches may have varying materials and thickness, resulting in differences in impedance that is more than 10%.
  2. you can't use a solid reference plane to hit e.g. 90 ohm when the core is only 25um. However, hatch ground planes or co-planar wave guides without a ground plane might work. To calculate the dimensions, you cannot use a simple impedance calculator. You need at least a 2D field solver. Sierra circuits have an online one for coplanar transmission line. It looks possible, but is not something I've tried.

Also, I think that you can ignore impedance mismatch if the traces are short enough (such as a so called lumped circuit). It's difficult to know what "short enough" is though.

  • 2
    \$\begingroup\$ "short enough" is "significantly shorter than a wavelength". \$\endgroup\$
    – Hearth
    Sep 6, 2023 at 21:00

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.