3
\$\begingroup\$

I need to use HMC241AQS16 brand RF SP8T switch on an FR-4 board. The RF ports of this QSOP package integrated circuit have 50 ohms impedance. But there is a problem, the leads of the chip have just 0.41 mm in width. My original 50 ohm transmission lines on a FR-4 are about 3 mm in width. Therefore, I need to design a tapered transmission line as in the following figure, but it must have two ends that have 50 ohms characteristic impedance. The tapered line topics in the literature are generally about matching the lines with two different impedances. How can I handle this problem?

enter image description here

\$\endgroup\$
2
  • 1
    \$\begingroup\$ What frequency are you working at? \$\endgroup\$ Jan 27 at 18:14
  • \$\begingroup\$ The frequency range that I need to work on is 2.4-2.5 GHz. \$\endgroup\$
    – adba
    Jan 29 at 17:33

3 Answers 3

5
\$\begingroup\$

You won't be able to get 50ohm and 0.41 mm wide without changing the dielectric thickness.

Have you reviewed the layout in the datasheet or other application material from the manufacturer?

In the layout in the datasheet they keep the trace width the same until the pin. It is narrower than 3mm, they must have a lower dielectric thickness. You probably need to do the same.

What PCB material and stackup are you currently using?

enter image description here

\$\endgroup\$
4
  • 2
    \$\begingroup\$ 3mm trace width sounds like a 1.6mm pcb thickness. I would suspect he is trying to use a 2 layer pcb. \$\endgroup\$
    – Mike
    Jan 27 at 17:29
  • \$\begingroup\$ They use Rogers 4350 substrate. It has 3.48 dielectric constant. The thickness information of the board is not given but it is not that thin as far as shown in the following photo. Maybe the trick is vias on the board. I need to use FR-4 substrate by the way. My frequency range is 2.4-2.5 GHz. enrgtech.co.uk/product/unclassified/ET13857334/… \$\endgroup\$
    – adba
    Jan 29 at 17:28
  • \$\begingroup\$ @adba - you say FR4 but what PCB stickup are you trying to use? The dense vias are used to ensure that the layer 2 ground plane and the top layer ground are well connected. If you are only working up to 2.4GHz it shouldn't be too difficult, the wavelength is about 5cm. I've done up to 10GHz on FR4 and the project I'm currently involved uses 76GHz on Rogers. \$\endgroup\$ Jan 29 at 17:52
  • \$\begingroup\$ My material is a classical single layer FR4 with 1.6mm thickness as Mike said. \$\endgroup\$
    – adba
    Jan 30 at 9:54
2
\$\begingroup\$

Therefore, I need to design a tapered transmission line as in the following figure, but it must have two ends that have 50 ohms characteristic impedance.

But do you?

Go back to basics, just because the pad is much smaller than the track, do you really need an elegant taper? Maybe it will make matters worse?

As Kevin asked, over what frequency range are you working?

Consider the simple solution - run the fat track up near the pad, then connect it with a thin track. Estimate the effect - a short length of high impedance line will be like a series L, whether it is a problem or not depends on the frequency and impedance. This may well turn out to be better than a longer transition region of non-50ohm track.

If the effect of even a short thin track is bad, then maybe you have to consider using a thinner substrate so you can get 50 ohm tracks up closer to the chip.

Be creative with your layout - there are three tx lines connecting to that side of the chip, if the top one leaves going up, the middle one horizontal and the bottom one going down then you should be able to get them close.

Edit The premise of your question is wrong - there is not way to change the width of the track whilst maintaining 50 ohm impedance. You just have to run 50 ohm tracks as far as you can, then use something smaller, and if you can't make that work, consider changing the substrate thickness.

Simple rough calculation: A 1mm track on 1.524mm FR4 is about 86 ohms. At 2.4GHz, a 5mm length of 1mm track is about 25 degrees. Connecting using this will cost you about 0.25dB in S21 and a return loss of about 12dB. You can improve this if you can manage to squeeze some shunt C at each end of the skinny line.

This is probably too lossy and too narrow band, but \$\lambda/2\$ of any impedance line doesn't change the impedance.

\$\endgroup\$
1
  • \$\begingroup\$ My frequency range is 2.4-2.5 GHz. Actually, I have tried "the fat track up near the pad, then connect it with a thin track" solution but it doesn't work as far as I see in S21 and S11 parameters on VNA. \$\endgroup\$
    – adba
    Jan 29 at 17:32
2
\$\begingroup\$

You might be expecting your reader to be mind-readers of making assumptions on scattering parameters while asking naive questions about "tapered 50 Ohms". The better way is full disclosure of what you expect (scattering parameter plots), do understand and do not understand thus a well-defined question with context to relate with.

Instead you quote this excellent paper which discusses a quarter-wave band-shaping filter with research performed by grad-students authored by the Asst. Prof. They etched this 10% tapered 1/4 wave strip line in the lab but failed to publish dimensions because they were lucky enough (by iteration, I presume) to get a better return loss than predicted simulation with wide tolerance FR4 @ 2GHz 4.3 and must be low loss tangent. When you see such common publications without a table of values and tolerances, BE AWARE. This takes a lot of trial and error to validate Dk otherwise "electrical TDR testing" is done by a fab shop.($$$)

A disclosure of values and tolerances are important to validate their specs. and authenticity of the design It's still a good paper on parasitic surface wave stripline antenna-effects controlled by aspect-ratio of the transmission line and change in effective Dk of the dielectric with some slight change in skin-effects.

I recall in 1st yr physics lab how to compare standard deviation of the theoretic results with actual to rate the quality of the experiment. (yet forgot the equation)

Here's your omission https://link.springer.com/content/pdf/10.1007/s11277-020-07957-0.pdf#page=8&zoom=auto,-49,574

Then you show a wildly tapered photo without any references and ask how do I match it?

enter image description here enter image description here

Aspect ratios of the conductor dielectric geometry determine the impedance changes, so your concept is flawed. Not only is it difficult to get low impedances, but it's also even harder in the double-sided board. In order to mechanical stiffness, the fibreglass resin dielectric must be a couple mm thick overall with copper and in order to get 50 Ohms the trace width to height for most FR4's is 2:1 (h:w) ( lower constant Dk e.g. Teflon demands even lower 1:1 ratio)

Thus with multi-layer boards, it is easier to achieve this aggregate mechanical stiffness while providing thinner dielectric layers to increase the capacitance to achieve the L/C ratio for low controlled impedance.

Impedance is defined by distributed lumped element ratios as \$Z_o=\sqrt{\dfrac{L}{C}}\$

The inductance is geometrically defined by the log of ratio l/w for a straight line roughly. This formula is used by Saturn PCB design.exe (https://welldoneblog.fedevel.com/2021/07/08/pcb-layout-useful-calculations-which-you-maybe-didnt-know-about-with-kenneth-wood/) and also shown in RF-world's calculator

Imagine how you can increase the capacitance by a smaller gap more vertically than horizontally, although both do add. If you chose a very thin board, it would be floppy and possibly break vias, but then you could add an inexpensive stiffener and get away with a 2 layer board. Otherwise, multilayer is the way to go and you mainly pay for the total copper on each layer before processing for high volume orders.

enter image description here

Solution:

The coaxial connector has a large surface area and gap but the ratio is the same as on a PCB (if the Dk was 1). So you must choose this transition in size at the connector interface while maintaining the same ratios. It's a bit more complicated as shown in the formula above, but that's the basic solution and not a tapered track. Don't take my word for it. Look on Google or Baidu "images" for "50 ohm tracks"

\$\endgroup\$
1
  • \$\begingroup\$ Actually, I need to realize my circuit with FR-4 material at 2.4-2.5 GHz. In the following article, it is said that it is possible to do that with a tapered line on the FR-4 substrate (on page 2047). But they didn't give the dimensions of the tapered line. link.springer.com/content/pdf/10.1007/s11277-020-07957-0.pdf \$\endgroup\$
    – adba
    Jan 29 at 17:30

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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