I have been looking into reducing the number of different cables needed for my project: I have a couple of photodiodes on separate boards, with a total of 7 analog outputs. They have signal bandwidths of up to ~1.5GHz. Currently, I am using a separate coax cable with a U.FL connector for each signal. This gives me the required bandwidth, but requires too many cables that need to be routed/plugged in.

I therefore had the idea to combine the cables into a single flex cable (custom flex PCB with the required shape) that fans out to connect to the different photodiodes. The question now is: Can I achieve the required bandwidth with such a cable? What design would I use for the transmission line? Anything else I need to watch out for?

I have tried to find a transmission line calculator that supports the layer stackup of the flex PCB (from JLCPCB): enter image description here

The calculators that I have found so far don't allow the "embedding" layers to be defined (they all assume air).


1 Answer 1


That should work - there's quite a few high-bandwidth applications that use flex PCBs for signal transport, for example the interface between laptop body and screen routed through the hinges.

The problem will be that JLCPCB doesn't seem to provide any data on their substrate ("Polyimide Dk:3.3", I'm going to venture a guess and assue "Dk" stands for "dielectric constant", why ever they didn't use the more common \$\varepsilon_r\$ symbol); without confirmation of dielectric constant applying to the frequencies of your interest, you couldn't design a wave guide.

Regarding the question of bandwidth: you'll need to define that a bit better; with polymers, \$\varepsilon_r\$ often varies quite a bit with frequency, and I have no idea how the situation is for the polyimide they use. If you only care about a narrow bandwidth (say, 1.4 to 1.5 GHz is all that contains useful signal), then that's not going to be a problem; if you're trying to sense things that actually have relevant signal components across 1.5 GHz, you'll see dispersion, and whether or not, and from which length on, that becomes a problem, is up to your application.

The other problem is loss tangent, which might mean more losses than you can tolerate; but that again is pending on what the datasheet of the materials used says. A cursory look for brand-name Kapton tape material suggest we're in the order of \$\tan \delta =10^{-2}\$ at 1 GHz, but this is really just useful as an order of magnitude. Do not that dielectric losses are usually also frequency-dependent.

So, you'll have to ask your board house to give you actual data of the electrical properties of their substrate over frequency (they will very likely have that datasheet at hand). The problem of designing a waveguide in a material isn't impossible to solve; there's very capable tools like MMTL, and the expensive PCB layout tools do have similar functionality as part of EM simulation toolboxes.

EDIT For the interested: a modernized fork of MMTL including a WIP WASM port is available at https://notabug.org/niconiconi/tnt-mmtl , and @比尔盖子 also wrote an explanatory blog post.

  • 2
    \$\begingroup\$ Cross talk might be more serious too. \$\endgroup\$
    – Andy aka
    Apr 16 at 11:39
  • \$\begingroup\$ @Andyaka another good reason to actually simulate using MMTL! \$\endgroup\$ Apr 16 at 11:49
  • 3
    \$\begingroup\$ Dk is a fairly common abbreviation for dielectric constant in PCB manufacturing and materials datasheets. \$\endgroup\$
    – Adam Haun
    Apr 16 at 17:30
  • 1
    \$\begingroup\$ Dk is not Er, Dk is the real part of Er, or Er'. \$\endgroup\$
    – user71659
    Apr 16 at 20:37
  • \$\begingroup\$ @user71659 aha! but that especially means that we can't read losses from Dk \$\endgroup\$ Apr 17 at 7:27

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.