Designing a PCB with 50 ohm impedance

[nrd_au]

Hi all,

I designed my 1st RF PCB for a high pass filter with a bias tee circuit to work in the 1.7GHz - 1.9GHz band inject about 48V-5A DC. It didn't work. It is showing about 20db of insertion loss and the impedance is all over the place (see figures below).




I made the PCB stackup and calculated the race widths according to instructions I read online (many sources) but obviously, I am missing something.

I used PCB-way to manufacture the PCBs so the 4 layer stack is from their website (given below). RF traces were on the bottom layer. L1, L2 and L3 were ground.

Below is the stackup from Altium



I used the impedance calculator in Altium with the trace type selected as "single" which I believe is Microstrip. It gave me a trace width of 6.906mil. Below is the calculation.



Below is the schematic




Below is my layout.








Looking at the design I should have done the following but do not think them alone would explain the results.

1. Via stitching on the ground plane
2. Add teardrop connections for connecting the pads and rf traces

What other things can I do to improve the design?



THANKS!!!

 

[volker@muehlhaus]

Designing a bias tee for 5A is not that simple.

You can test the high pass part and low pass (DC injection) part separately, to see where the issue is. Cut traces to disconnect the other path, and peel of copper if necessary.

For the DC path, you want an open circuit at your RF frequency. One obvious mistake is the large trace width there, which gives a lot of shunt capacitance at the input. This is in parallel to your 50 Ohm lines connecting the high pass section.

 

[vfone]

On top of these statements, due to very thin dielectric layer (0.11mm) you get very narrow 50 ohms transmission lines (0.17mm).
This makes the design very unpredictable due to extra parasitic inductances added to the filter circuit. In this situation, a linear simulator may not be enough, and an EM simulator is required. This in case that the PCB manufacturer can provide the requested trace tolerances (hard to believe that cheap manufacturers can do this).

 

[nrd_au]

Designing a bias tee for 5A is not that simple.

You can test the high pass part and low pass (DC injection) part separately, to see where the issue is. Cut traces to disconnect the other path, and peel of copper if necessary.

For the DC path, you want an open circuit at your RF frequency. One obvious mistake is the large trace width there, which gives a lot of shunt capacitance at the input. This is in parallel to your 50 Ohm lines connecting the high pass section.

Thank you for the reply. Part of the reason for having such a layout was that I wanted to use that particular inductor which has a wired footprint where the 2 pins are on opposite sides. So I will select a different inductor that doesn't require such a big pad.

I will desolder C12 and solder a test cable to isolate the circuit. Hopefully, that would give me a bit more information.

Also, I will make a test board with a few variations to test a few possible solutions like with/without the inductor, microstrip/CPW, and a single trace to see whether the 50 ohms is working.

--- Updated Jul 26, 2021 ---

On top of these statements, due to very thin dielectric layer (0.11mm) you get very narrow 50 ohms transmission lines (0.17mm).
This makes the design very unpredictable due to extra parasitic inductances added to the filter circuit. In this situation, a linear simulator may not be enough, and an EM simulator is required. This in case that the PCB manufacturer can provide the requested trace tolerances (hard to believe that cheap manufacturers can do this).

Thank you for the reply. Yes, 0.11mm is very tight and I am not sure how good their manufacturing process is. However, I did pay a lot extra for their controlled impedance option so...

Since this being a microstrip, I removed all surrounding copper from the layer containing the RF traces. Is this the right thing to do? (because I also read the clearance between the RF trace and surrounding ground plane should be greater than twice the RF trace width).

Later in this design, I need to add a digital step attenuator and an amplifier chip so the layout is going to get dense. In that case, would you recommend a coplanar waveguide instead of a microstrip because I won't be able to keep a large clearance between the RF trace and ground?

Also, can anyone recommend a decent PCB fabrication house?

 

[volker@muehlhaus]

I will desolder C12 and solder a test cable to isolate the circuit. Hopefully, that would give me a bit more information.

I doubt that. The layout is really really bad from an RF perspective.

1) Let me repeat: your very wide pad for DC path at the coax input creates a large shunt capacitance over the entire frequency range. This will damage your response at 1.8GHz.

2) Microstrip without side ground is fine. But to avoid issues with etching precision, you better use wide lines for 50 Ohm, by using another layer for ground that has larger distance = more substrate thickness.

3) You mentioned controlled impedance line, but forget the effect of SMD pads. For thin substrates, these create large shunt C. That's another reason why your layer combination isn't wise.

4) Your air coil sits close above some ground and will have a lot of shunt inductance. Also, it looks suspiciously large (physically) for blocking 1.8 GHz, so you better check the air coil impedance at 1.8GHz.

5) Screenshots show very few vias in the large planes. RF ground planes should connect to other RF ground areas in many places, to avoid resonances.

So there are many details to fix, in my opinion. For injecting DC into an RF line, you might have a look at microwave layout technique: using a lambda/4 line with a radial stub at the end. That's an alternative to the aircoil method, not sure if it can be designed to carry 5 Amps.

 

[G4BCH]

Following on from Volker's advice, try to absorb the parasitic strays in the layout. The layout he is suggesting something like shown in the attached file. This uses a quarter wave length of wire instead of the inductor. The length will need to be adjusted the 37mm does not account for the wire being close to the board or the effective length of the RF decoupling capacitor. My guess is that it will need to be 2 or 3mm shorter to be optimised.
Your circuit has no RF decoupling at the DC only end of the inductor, you do need a low impedance at this point. Choose a capacitor that has a self resonant frequency of about 1.8GHz for this; about 10pF depending on size and manufacturer. You could, following Volker's suggestion use a a radial stub or create a capacitor in the PCB.

I can't find a suitable inductor that will take the current; the Coilcraft 132-03L
https://www.coilcraft.com/en-us/products/rf/air-core-inductors/maxi-spring/132/132-03/
a 4A rated part looks like it would do if you can take the extra temperature rise by using it at 5A.

C12 serves no purpose, C11 blocks the DC from the RF only port.

 

[volker@muehlhaus]

4) Your air coil sits close above some ground and will have a lot of shunt inductance.

I meant shunt capacitance to ground.

 

[nrd_au]

Thanks all.

Since the large pad for the inductor was not underneath the filter circuit, I de-soldered C12 and tested the insertion loss between J4 and C11 by soldering an RF cable to pin 2 of C11. I got about a 12dB improvement on the insertion loss. So now I am making a test board with a few different circuits on it. Hopefully, that would give me a bit more information.

 

[volker@muehlhaus]

I would also check L2. That large 470nH value will have a self resonance below 1.8 GHz and behave very different from the ideal 470nH.

 

[BigBoss]

10uH is an absurd value for 1.7-1.8 GHz @50 Ohm.It should around 47-56nH, not more.
Tapping a component on a Microstrip Line is not a good idea. A small snake coil then main choke coil will be a better solution like that.

 

[nrd_au]

I would also check L2. That large 470nH value will have a self resonance below 1.8 GHz and behave very different from the ideal 470nH.

Yes, these values were taken from a previous design. The next test boards I make will use values taken from this calculator https://rf-tools.com/lc-filter/ Got these values for a 1700MHz cutoff HPF.

--- Updated Aug 3, 2021 ---

10uH is an absurd value for 1.7-1.8 GHz @50 Ohm.It should around 47-56nH, not more.
Tapping a component on a Microstrip Line is not a good idea. A small snake coil then main choke coil will be a better solution like that.

Hi BigBoss,

So the design I have posted here is actually incomplete. In the final design, the transmission line will carry LTE+VHF+DC (see image below). Hence, I will be needing a larger inductor at some point.

I found these inductors from AVX. Although they are not rated for the current I am looking for, I will try them as a proof of concept.

When you said "snake coil" did you mean something like this AVX inductor?

 

[BigBoss]

Snake Coil=Meander Line.
3A is not enough for DC Current Rate ?

 

[nrd_au]

Snake Coil=Meander Line.
3A is not enough for DC Current Rate ?

The original requirement is 10A!

 

[BigBoss]

The original requirement is 10A!

So you will make your own coil by hand using enameled copper wire.I think 7-8 turns over a 5-10mm core diameter air coil will serve you well.For more information, refer to coil calculator on the web.

 

[BigBoss]

I have forgotten to mention that if you have an intention to pass trough this current in a connector, forget about that.You will blow up the connector's inner conductor..