Electronics > PCB/EDA/CAD
Measurement of different PCB trace width with R&S ZLNE-3 VNA / JLCPCB
cgroen:
As my Christmas present to myself this year was a brand new R&S ZNLE-3 VNA and a ZN-Z150 calibrator, I thought it would be nice (finally) to measure the impedance of different trace width from JLCPCB.
According to JLCPCB's "impedance calculator" for their JLC7628 stackup, a trace of 11.55 mil should give 50 Ohms.
I made a small 4 layer 1.6mm thick PCB with 4 different traces on it, 8, 10, 12 and 14 mil wide. Each trace was terminated with a 50.3 Ohm resistor (0402, 1%, using thermal relief on GND). All 4 layers had ground pour on them and lots of VIA's.
The clearance around the tracks where 3 times the width of the tracks.
SMA connectors used was Molex: https://www.molex.com/molex/products/part-detail/rf_coax_connectors/0732511150
Cable used was a Minicircuits SMA cable.
As I have not yet received the calibrator for the VNA, I used what I had laying around (open, short and 50 Ohm) of decent quality (I hope..).
Below is the result from 1 MHz to 3 GHz of the 4 different tracks. Now, I'm no RF expert (at all!), so I might have failed in the measurements/setups, if you spot anything strange, please let me know!
It seems that the orange track (10 mil trace) is the one that is least "bad".
Maybe I have had too high expectations, or even more possible, I did something wrong, but I would have guessed that the return loss would have been better ?
EDIT: Smith chart included also
cgroen:
Zoomed in on the smith chart:
thinkfat:
To me it looks like the 10mil trace has the closest match. It has the least wiggles in the logmag graph and also on the smith chart is somewhat straight. However, it is quite obvious from the smith chart that the impedance is mostly inductive capacitive and also quite far from 50 Ohms other than at the very start of the frequency range.
Unfortunately, my RF experience is also quite limited so I don't quite know what this is due to. But it seems really quite odd, the S11 logmag graph should stay below at least -20dB reflected power for most of the range, but instead it rises quickly to be above -10dB. That doesn't look good. I suspect a mistake in your layout somewhere, or in the calibration of the VNA. Could you provide the Gerber files for all 4 layers?
I would, anyway, suggest to drop all the thermal reliefs in the GND pads and make the signal pads for the SMA connectors a lot thinner. Also, put ground vias directly under the connector flanges, not somewhere outside. This all adds inductance.
It would also be quite interesting to see what difference a much wider clearance between the signal trace and the ground fill on the top layer would make and if you were to make another set of boards, have one 10mil trace with SMA connectors on both ends so that you can measure S21 as well.
Putting SMA connectors on both ends would have been the better test setup anyway, IMHO. But I hope someone with more RF experience will take a look as well.
cgroen:
--- Quote from: thinkfat on January 03, 2022, 02:59:28 pm ---To me it looks like the 10mil trace has the closest match. It has the least wiggles in the logmag graph and also on the smith chart is somewhat straight. However, it is quite obvious from the smith chart that the impedance is mostly inductive and also quite far from 50 Ohms other than at the very start of the frequency range.
Unfortunately, my RF experience is also quite limited so I don't quite know what this is due to. But it seems really quite odd, the S11 logmag graph should stay below at least -20dB reflected power for most of the range, but instead it rises quickly to be above -10dB. That doesn't look good. I suspect a mistake in your layout somewhere, or in the calibration of the VNA. Could you provide the Gerber files for all 4 layers?
I would, anyway, suggest to drop all the thermal reliefs in the GND pads and make the signal pads for the SMA connectors a lot thinner. Also, put ground vias directly under the connector flanges, not somewhere outside. This all adds inductance.
It would also be quite interesting to see what difference a much wider clearance between the signal trace and the ground fill on the top layer would make and if you were to make another set of boards, have one 10mil trace with SMA connectors on both ends so that you can measure S21 as well.
Putting SMA connectors on both ends would have been the better test setup anyway, IMHO. But I hope someone with more RF experience will take a look as well.
--- End quote ---
Thanks for input! To be honest, the connectors I used was not what the PCB was laid out for, so it ended up being a compromise...
I have attached the gerbers for the board. I have since changed the layout to the right connector and added a few more things to the board (some experiments with matching circuits etc). This one has also a SMA on one of the "channels", maybe it is better as you write to do this on all of them!
thinkfat:
I have probably misread the smith chart a bit, the impedance is not inductive, it is capacitive. In that case, I guess the problem is that the ground fills are too close to the signal traces.
To give some reference, I've attached some pictures of a resistive power splitter I made for some experiment. The PCB was done not with a specific impedance controlled stack-up, I just calculated some trace widths for standard 1.6mm FR4 PCB. The PCB was manufactured by JLCPCB, though. As you can see, the reflected power is better than -20dB up to 1GHz (I didn't check higher frequency because the target frequency was below 100MHz anyway). Impedance is close to 50 Ohm across the span, slightly inductive for the most part, turning capacitive towards the end of the range. This is how I expected your smith chart to look like, too.
BTW, what is the frequency/div in your plot? I somehow cannot see that from the screenshots.
Navigation
[0] Message Index
[#] Next page
Go to full version