Electronics > RF, Microwave, Ham Radio

JLCPCB Impedance controlled trace is not the right impedance

(1/6) > >>

Xevel:
Hello,

I have a 4 layer PCB with a roughly 16mm feed to a Bluetooth chip antenna on TOP.
I tried to design it to be 50 ohms, but when I started testing the antenna performance it was wildly different from what I was expecting, so I started investigating and it seems to me that the first problem is that my transmission line isn't even close to 50 ohms.

I would be very appreciative if more experienced people could help me understand where I went wrong (if it's at the design stage, or the measurement stage, or something else altogether that I haven't considered).



The PCB : 4 layers, 1mm thick, designed for JLCPCB's impedance controlled stackup JLC7828.
JLC's [url=https://cart.jlcpcb.com/impedanceCalculation]calculator gives 11.55mil / 0.293mm line width for these specifications.
Saturn PCB gives a slightly different answer:
 - Microstrip, 18+18um copper, FR-4 with Er=4,6 (the dielectric constant for prereg 7628 according to JLC's page), conductor height = 0.2mm, F=2400 MHz  ==> about  0.35mm width to get 50ohms
 - Coplanar wave, FR-4 with Er=4,6 (the dielectric constant for prereg 7628 according to JLC's page), conductor height = 0.2mm, Gap = 0.18mm  ==> about  0.34mm width to get 50ohms

I  settled with 0.3mm for the first PCB prototype, since even according to Saturn PCB it gives about 53ohms, not wildly far off, and I would adjust for the next iteration.

That test PCB is aimed at testing the antenna and the effect of the parts around, some which have significant metal pieces (piezo buzzer, speaker), so I added two 0402 footprints to connect the feed + antenna to either where the Bluetooth chip is, or to a U.FL connector.
I realized a little late that the U.FL footprint might not be great with the thermal spokes so small, and on my test board I added a large solder blob on each side of the connector, but that's not the main point I think, since my big question is about the trace impedance.

[attach=1]

So I will spare you most of the confusion of the initial tests and focus on the trace impedance.

After an OSL calibration with a cheap U.FL calibration kit (one on a RF demo kit like the ones people often get with a nanoVNA or similar) on my Siglent SVA1032X (CF=2441MHz, span=390MHz), I tried a sanity check : I cut and removed the trace at the place where it leaves the ground plane to go connect to the antenna (top right), populated the 0402 footprint to connect the U.FL and antenna feed with a 0R (thin film), and soldered a 49.9ohms 1% 0402 resistor  (green on the picture below). I was expecting something not too far from the center of the smith chart but to my surprise it wasn't anyway near (arc on a circle that crossed the horizontal line around 70 ohms, though I did not record that part exactly).

[attachimg=2]


I tried the techniques from this link ( https://chemandy.com/technical-articles/measuring-track-characteristic-impedance/measuring-track-characteristic-impedance-article3.htm ) and this video ( ) to measure the impedance, and both gave roughly 40 ohms.

I cut the side of the PCB to verify the material thickness and measured 0.19 mm, a difference from the 0.2 that should make the impedance greater, not smaller, and only by a couple ohms.
Gnd plane is also well connected (I carved the PCB to make sure vias connected to it).

Any idea why my trace isn't the 50 ohms it should be ? or am I going in a completely wrong direction ?
Thanks in advance.


 


T3sl4co1l:
So you get two different numbers, depending on how you measure it?

How about this, does the circle shrink to zero radius when the trace is terminated with another resistance (say 40 or 70)?  That's pretty characteristic, even if the rest of the system is being weird.

And this is at high enough frequencies where the trace is a wavelength or more, right?  (No scale factor was given, unless I want to compare in units of 0402 or u.FL footprints; and one CF+span was given, but unclear if that's the same for both tests?)

At a glance, I'd guess at 2.45GHz and a handful of 0402s in length, this trace doesn't matter very much.  But I don't know how tolerant your radio is, or how much tuning you expect to do on it.  Could just as well tune the antenna+trace as a whole? -- Which does require assuming your feedpoint is a correct reference (in terms of impedance and grounding), so there is still some value in checking that out, whatever the load or method.

Speaking of grounding, does it change with ferrite beads on the cable or anything?

Tim

ThomasDK:
It's not the trace, it's the connector.

U.FL. connectors have a keepout zone:

Xevel:
Hi, and thank you for the response.


--- Quote from: T3sl4co1l on October 28, 2021, 06:47:14 pm ---So you get two different numbers, depending on how you measure it?

--- End quote ---

I haven't been very clear about that, my bad. When I did the sanity check and read about 70ohms (characteristic impedance), I hadn't played with the port delay at all and the length of the tested transmission line was close to 1/4 period, so maybe it was rotated 180° on the chart ? At that moment there was also the connector and 0R inline resistor in the picture, I might have messed thing up more than I realize...


--- Quote ---How about this, does the circle shrink to zero radius when the trace is terminated with another resistance (say 40 or 70)?  That's pretty characteristic, even if the rest of the system is being weird.
--- End quote ---
interesting test, I will have to try again. The latest tests I did have been a little destructive though, I need to prepare another PCB...


--- Quote ---And this is at high enough frequencies where the trace is a wavelength or more, right?  (No scale factor was given, unless I want to compare in units of 0402 or u.FL footprints; and one CF+span was given, but unclear if that's the same for both tests?)
At a glance, I'd guess at 2.45GHz and a handful of 0402s in length, this trace doesn't matter very much.  But I don't know how tolerant your radio is, or how much tuning you expect to do on it. 
--- End quote ---

Quite the contrary, the line is close to a quarter period (tests made around 2.4GHz so lambda is around 83mm with an assumed velocity factor of 0.66, and the trace I measured is about 16mm of uninterrupted copper, or about 20mm total in the tests with the connector and inline resistor ).


--- Quote ---Could just as well tune the antenna+trace as a whole? -- Which does require assuming your feedpoint is a correct reference (in terms of impedance and grounding), so there is still some value in checking that out, whatever the load or method.
--- End quote ---

Thankfully I am not trying to get a best-in-class performance out of my BLE device, the way it's going to be used it really doesn't make sense that the BLE device and the host it talks to be separated by more than a meter. But I take that opportunity to try to understand a little bit better all that RF stuff.
Right now my problem is that I have multiple designs (physical PCBs on my desk) and I would like to compare them, but if even the most basic stuff (making a 50ohm transmission line) is wildly wrong - or I get wildly wrong results when I try to measure it, which would be even worse - I feel that I need to level up before going forward.




--- Quote ---Speaking of grounding, does it change with ferrite beads on the cable or anything?
--- End quote ---
That part I found out about recently.  :phew:
My first tests I tried with a RG178 cable (SMA to U.FL, 150mm), and indeed I saw measurement changes when I handled the cable or touched the VNA connector. I added a ferrite bead and taped it in place on the cable close to the DUT, negating in large part that effect. However after a few more insertions of the U.FL connector, I realized the female U.FL connector of that cable was damaged (inconsistent results) and got rid of that cable.
Then I changed to a RG 1.13mm cable (SMA to U.FL, 100mm long) and this one did not seem affected. Touching the connector or cable did not show changes in the output anymore, so I did not put the ferrite back.

For the measurement  of the track impedance according to the first method (Chemandy), I used again a RG178 cable,  without connector on the DUT side. For that test I calibrated the VNA at the tip of that cable, with  open, solder blob for short, and 49.9 1% 0402 for load, then soldered directly on the PCB for the measurements(I measured between the 0402 pad at the bottom and the other end of the feed, top right in my first picture).

Xevel:

--- Quote from: ThomasDK on October 28, 2021, 07:25:34 pm ---It's not the trace, it's the connector.

U.FL. connectors have a keepout zone:



--- End quote ---

Urgh, now I feel foolish.. so any test that uses the connector is off, thanks !

With that out of the way, I still have a problem with the trace itself.
I applied the method from https://chemandy.com/technical-articles/measuring-track-characteristic-impedance/measuring-track-characteristic-impedance-article3.htm both on my trace (the largest uninterrupted part, so well away from the connector and its wonky footprint), and did the exact same test with a similar length of RG178 coax cable.
EDIT I used a frequency of 1500MHz for these tests as the length of the trace was about 16mm, and on the first page they make it clear that the frequency and trace length should lead to the trace being close to an odd number of times lambda/8 for accurate results. So I chose 1x lambda/8 as that's the only acceptable value for my setup (VNA goes to 3.2GHz but the RG178 cables are rated to 2.5Ghz). /EDIT

The measurement for the RG178 coax cable came out at 52.3ohms (which is close enough to the theoretical 50 +/-2 ohms of the cable datasheet, considering the errors I introduce at every step [calib with just a resistor or blob, soldering that piece of cable to the original coax cable with dirty pigtails for the braid, shortening of the transmission line when I put a solder blob to short it....]).

[attachimg=1]

The PCB trace came out at 42.7 ohms.
The Saturn PCB computation adjusted with the measured material thickness says my trace should be 52.5 ohms with this geometry and the materials supposedly used by JLCPB in the fabrication of the PCB.


Navigation

[0] Message Index

[#] Next page

There was an error while thanking
Thanking...
Go to full version