RF Microstrip Design

[vladyslavb]

Hello EEVBLOG community,

I've been messing around with my RF microstrip traces for a while now in an attempt to achieve proper signal quality and I keep coming up short with poor signal quality with every design iteration thus far. I'm beginning to wonder if I have something simple wrong that I am not aware of (some design rule I'm probably overlooking or haven't found so far).

Essentially, the signal chain I have is:

Flat patch 4G LTE antenna, coax cable to u.fl female connector (50Ω) -> u.fl SMD male connector (50Ω) -> Microstrip line RF trace (50Ω, according to JLCPCB impedance controlled design) -> MAIN_ANT pin on a SIM7600E RF module.

I have a strong feeling that my issues lie within my PCB trace layout. I've done a fair bit of experimentation with matching networks (using information gathered using a NanoVNA), various trace widths (as a sanity check test), via placements for grounding, trace lengths (shortest possible) and nothing seems to have done the trick so far.

For reference, I'm including some diagrams of my current trace design (JLCPCB 7628 stack-up https://cart.jlcpcb.com/impedance 4 layer board, 1.6mm PCB thickness, 11.55 mil trace width, 7.1 mil conductor height, FR-4 dielectric).

top_L1.png: Shows the top layer of the PCB, centered around the 3 pin U.FL SMD connector with RF trace going to the MAIN_ANT pin of the SIM7600E.


ground_L2.png: Shows the 2nd layer of the PCB (a full uninterrupted ground pour for the RF microstrip), centered around the 3 pin U.FL SMD connector.




I've done some due diligence (digging around on the EEVblog forums) and found out that the U.FL connector actually has a keep-out layer around the signal pad (which I haven't tried including yet), and some others were also recommending a 3x trace width buffer between the RF trace and the top layer ground pour on either side.

Besides these solutions, is there anything else I'm missing? I'm new to designing with RF and would love some feedback  .

[Marsupilami]

May I ask what the actual issue is?
I'm sure we could start throwing things at your layout but considering how close your connector is I feel like it should mostly work. If you're just fine tuning performance or want to get the maximum sensitivity out of your receiver then yes, probably you should tweak a couple of things, but you made it sound like you're having bigger problems. No?

[hagster]

What you have created is will not work as a microstrip. For a microstrip the RF return path should be underneath the track. In your design the RF return path will mostly be via the top copper pour. The vias you have added will not form part of the circuit as there is no short route back from the vias to the analog ground pin.

My advice would be to use a Grounded Coplaner Waveguide GCPW in this instance rather than a microstrip. But the main thing to consider is the RF return path. At RF the ground plane can not be thought of as solid reference as you can get away with at low frequencies. The return path must have a direct route back to the RF ground connection of your IC.

[vladyslavb]

@Marsupilami

The problem is that I can't get good quality LTE signal, which also corresponds to poor network connectivity with the local 4G LTE providers.

I can verify this through using AT instructions with the SIM7600E RF module. We bought a prebuilt breakout-board with the SIM7600 module on it in early stages of development, and the breakout board has much stronger signal quality and therefore, more networks it can find successfully in the area. I have since designed and redesigned the board a few times, but each time the signal quality was worse than the breakout board.

[vladyslavb]

@hagster

Thank you for leading me into the rabbit-hole that is RF return paths! I found some very informative articles explaining the issue at hand (at RF frequencies, the current follows the path of least INDUCTANCE not RESISTANCE).

From what I understand and what you explained, the ground pour underneath the RF trace must have a direct connection to the ground pin on the IC which receives/drives the RF signals.

So either

1) A via close to the RF trace/AGND IC pin connecting the ground pour on the L2 layer of the board to the L1 top ground pour

2) Isolating the RF ground and treating it separately to the other grounds on the board meanwhile routing the RF ground directly to the IC AGND pins and connecting it to the L2 ground pour with a via

3) Do what you suggested and create a grounded coplanar waveguide, something like


Which would strongly couple the bottom ground pour and the grounds on the sides of the conducting strip, effectively solving my issues and allowing me to keep the ground pours intact on both layers

[Marsupilami]

The problem is that I can't get good quality LTE signal, which also corresponds to poor network connectivity with the local 4G LTE providers.

The reason I'm asking is your trace is so very short that I have a hard time to see how exactly it would mess up your signal.
I did a exaggerated simulation in QUCS:

The trace is represented via a coplanar waveguide to account for the extra capacitance while the two stubs are there to simulate the capacitance of the connector and rf module pads. The two line segments from the ports to ground is to add some effects due to the longer than ideal return paths. (I kept them short as these are actually helping because the rest of the circuit is overly capacitive.) The results show basically negligible effect due to this section of the PCB.
All of this is very inaccurate but the point is that I grossly have to screw this up to see a noticeable loss or matching issue. Even if I use a 2mm wide trace the loss is only about 2dB at 2.5GHz.
Again, surely your design can be improved, but for major issues with performance I would probably look elsewhere. E.g. how is the RF module powered on your custom board. Or if all of its pins grounded properly, etc. etc.

[vladyslavb]

Interesting. So theoretically with the trace so short, the poor design for RF return path shouldn't be destroying my signal quality.

The RF module is currently being powered by a 3.8V regulator that lives on one PCB and the power trace goes through a SMD female-male connector combination to reach the SIM7600E module that is on a separate PCB. We thought having all the regulators on one board made sense, but it's probably better practice to have regulators closer to the modules they power.

Now that I'm thinking about it, with a 2A max current draw from the RF module and a current VIN trace width of 24mil and a total trace distance of a 2-4 inches between both boards, the supply strength could definitely be a problem. Maybe the RF module is not able to source enough current.

I'm not so sure that grounding is an issue, I feel confident that the RF module ground pins have solid connections but it's also probably worth double checking.

[hagster]

As @Marsupilami says, the traces are so short it's unlikely to be an issue, but not impossible at the upper end of the LTE band. It's very hard to guess what the impedance of the arrangement you have actually is. At the top end of the LTE band(2.6GHz) you have about 5 degrees of phase per mm. Your trach looks to be just over 3mm which would be 15degrees. That's enough to make a difference if the characteristic impedance is vastly off target.

Are you using the same antenna as you did with the eval board?

[Marsupilami]

It's very hard to guess what the impedance of the arrangement you have actually is.

That ↑ right there. @vladyslavb do you have equipment to perform wired measurements? One thing I can think of is, since you mentioned NanoVNA, to get an u.fl to SMA pigtail cable and try to measure the input match of your board with the RF module. It's not trivial but maybe doable. If it's bad then that won't help you much, but if the results are not too bad then you'll know for sure you have to look elsewhere.
I suspect the radio module has all sorts of test modes where you can put it in all TX or all RX mode for example. I'd do the latter, set very low source power on the VNA and measure S11 looking into the board.
If you have access to a spectrum analyzer I would hook it up too with a u.fl SMA pigtail just to see the output from the radio module. Does it have adequate power? Does it have a weird flatness problem (e.g. suckout(s) in the middle of the band). Is it at the frequency software says it should be? (Misbehaving reference?)

[vladyslavb]

Are you using the same antenna as you did with the eval board?

I am indeed using the same antennas.

That ↑ right there. @vladyslavb do you have equipment to perform wired measurements? One thing I can think of is, since you mentioned NanoVNA, to get an u.fl to SMA pigtail cable and try to measure the input match of your board with the RF module. It's not trivial but maybe doable. If it's bad then that won't help you much, but if the results are not too bad then you'll know for sure you have to look elsewhere.
I suspect the radio module has all sorts of test modes where you can put it in all TX or all RX mode for example. I'd do the latter, set very low source power on the VNA and measure S11 looking into the board.

I have performed the above test and would like to share my test setup/results for further discussion.

1) Calibration of VNA (open, short and 50 ohm resistor load) to account for coax cable length (solder bridges were used on the impedance matching network pads to create open, short and load tests).

The board in the attached photos is a previous iteration of the board design when I thought I would need an impedance matching network to achieve good signal, which has since been removed as I thought that was what was introducing problems (it wasn't - same signal quality with both boards, with an unpopulated impedance matching network and without). The breakout board does not have an impedance matching network on the antenna pins.

2) 900MHz - 2600MHz sweep test to SIM7600E ANT pin

It appears to me (with my understanding of smith charts) that the results show that I have a z=0, short circuit situation. Switching over to measure the breakout board with verified good signal quality, the results show the same, which is confusing to me. I am unsure if my test setup is incorrect, or there is something else I am doing incorrectly...

One of the test result images shows the 900MHz - 2600MHz sweep, and the other shows a 1900MHz - 2000MHz sweep. Maybe the VNA only has a specific step size that it can accurately show results for, so the 900-2600 is too much for it to handle?

When I did some research about the VNA I purchased off Amazon, it seems that the original NanoVNA manufacturers mentioned that the specific version I got was an unlicensed knockoff NanoVNA (apparently someone stole the design and started manufacturing these units), so I am wary of trusting the specific unit I got since it seems to behave unpredictably.

Unfortunately, I do not have a spectrum analyzer on hand that is capable of showing frequency response curves in the 900MHz - 2.6GHz range.

[hagster]

It looks like a short to me.

[Marsupilami]

Do you have any way of verifying your VNA calibration? E.g. solder a 25Ohm resistor on and measure that.
I would highly suggest getting this thing: https://www.ebay.com/sch/i.html?_from=R40&_nkw=rf+demo+kit+nanovna&_sacat=0&LH_TitleDesc=0&_sop=7
(Despite that I'm not at all sure it would go up to 2.5GHz, it would still give you more confidence than using your own board for cal.)

Assuming your cal is good check for a DC short on that pin with a multimeter, just to rule out the obvious. Then you also have to make sure that the RF module is in some sort of TX only mode. If I remember correctly from the datasheet when I briefly looked at it the other day it can do FDD so that means TX/RX has to be coupled but I can't rule it out that there's a switch still that make the antennal pin look like a short from the outside if not in the right operating mode. (Obviously it has to be powered on for this and make sure that the VNA source power is not too big, as the RF module input is expecting a very low level from an antenna and you don't want to damage it.)

[vladyslavb]

@Marsupilami

I just ordered the VNA calibration board, so we will see what happens upon calibrating/testing.

The antenna pins on the SIM7600 RF module are actually internally "shorted" to ground (as I found out through inspecting my soldering job a while ago). Upon further research, I found:

"Internal to the module, to restrict the spectral shape outputted there are likely to be harmonic filters and these are likely to comprise inductors to ground. They would show up as low ohmic connections to ground. Try searching for images of antenna filters on transmitters and you'll see what I mean."

I couldn't find a proper "RX only" command in the reference manual, as the configurations mostly just allow you to to change "network system modes" i.e

0 no service
1 GSM
2 GPRS
3 EGPRS (EDGE)
4 WCDMA
5 HSDPA only(WCDMA)
6 HSUPA only(WCDMA)
7 HSPA (HSDPA and HSUPA, WCDMA)
8 LTE

etc....

I might try changing it to the "no service" which will hopefully stop the outgoing messages, calibrate the VNA with the u.fl calibration board and give the RF network another test run at various LTE frequencies of interest and read the S11. If that fails or is not as informative as I would hope, I will probably spin another round of boards, this time with a smarter RF return path and more careful attention to the characteristic impedance parameters and also make a GCPW version and send both off to the fab so I have more to test.

Thank you both for your help, I really appreciate it. If there are any other suggestions/tips you might have before I order another round of boards, please let me know!

[cdev]

Every time I looked at that ebay board.  Ive thought that it looked as if it wouldnt last long if used to calibrate a VNA often.

The u.fl connectors aren't robust enough to see much reuse.

OTOH you could make your own, with JLCPCB, if you want. Make a convenient one thats small and handy and you ight be able to sell them. Ive seen them implemented in a little lanyard or similar.

If you have a nanovna2 youre likely to be using the calibration standards that come with it, at least to start. They are pretty idiot proof.

You can also buy or make your own. For Christs sakes its extremely easy to do so.

I got a set of SMAs that provide  "SOLT"

which are simple but work. What would be helpful might be something that held them all together or a combined SOLT like I have seen a few times. One could make one that attached to a lanyard that hug around your neck.

Think convenience and simplicity. Also, no need to spend an arm and a leg. I suspect.

Go easy on the solder if you do plan to hang it around your neck.. because of lead. What I would do is stick the business end of the SMas in a piece of moldable epoxy perhaps. Something not too big and clunky that fit the hand well. Remember youre likely to use it hundreds of times. Bright colors might be handy. So you dont lose it.

[czorgormez]

@vladyslavb

a simple microstrip won't solve your problem. you should do proper impedance matching with your antenna. we always assume antennas and GSM/LTE modems are 50 ohm. but they are not. they have some complex impedances like (35+j10 Ω). things gets complicated when you put your antenna in even a plastic box. so my suggestion is.

- mount your antenna in original box with pcb, all metal parts if you have any, or battery. measure your antenna impedance in interested bands (eg 800-2500 mhz)
- ask your modem manufacturer to real impedance output values of your modem.
- buy some RF inductor and capacitor kits like johanson C603- L603 etc.
- use some software (optenni lab) import your impedance data to the software and choose interested bands, choose your capacitor and inductor kits available.
- let the do software its job and get matching network values, apply and test them in real life.

with this method i solved many poor reception problems with GSM modems.

[cdev]

Test the antenna in its intended design. The SWR should be acceptable or may need a tweaking. Get advice from its oem. Using nanovna 2 you may be able to make a good guess as to optimal positioning. Its worth the trying.

[virtualparticles]

One problem with the supplied calibration pieces for the Nano-VNA. The load has a return loss of about 18 to 20 dB so Return Loss measurements at 10 dB will be +/- 3.3 dB at best. That might be good enough for many projects. A better 50 ohm calibration load is highly recommended though.