¿ªÔÆÌåÓý

ctrl + shift + ? for shortcuts
© 2025 Groups.io
  1. Nanovna-Users
  2. Topics

#measurement #measurement

[email protected]
 

Hi

I have a NanoVNA V2 Plus4.

I am trying to validate a PCB 50 ohm transmission line (trace) to be used for 2.4 GHz Wifi.

I am using a 4 layer stack-up (1.6 mm total) with the following configuration:

L1: Signal + ground pour
Prepreg 0.21 mm
L2: Ground
Prepreg 1 mm
L3: Empty
Prepreg 0.21 mm
L4: Ground

Board is FR-4 with Er = 4.6.

I have calculated the trace parameters using Saturn PCB design as a "coplanar wave" with a plane below.

I have attached 6 board files showing the actual board (board_image.jpg), rendered board (board_render.png) and the four layers (board_lx.png) + a screenshot of the calculations from Saturn PCB (calc.png). I use the following connectors from Molex:

I have calibrated the VNA in frequency range 2 GHz to 2.8 GHz with the provided SMA cable connected, see attached cal_load.jpg and cal_thru.jpg, direct_load.png, direct_thru.png

Now I connect the PCB trace and do a S11 and S21 measurement (see s11_s21.jpg). It seems to me that the result is not particularly good (see trace_thru.png and trace_load.png).

Can any of you spot any issues with the measurement method or configuration of the board? Also, if you can provide some realistic target results for such a configuration (two connectors + 82 mm trace) that would be great.

Any help is highly appreciated.

Thanks

br
Christian

board_l1.png
board_L2.png
trace_load.png
trace_thru.png
direct_load.png
direct_thru.png
board_l3.png
board_l4.png
board_render.png
board_image.jpg
calc.png
cal_load.jpg
cal_thru.jpg
s11_s21.jpg

 

Hi Christian
I do lots of antennas on fiberglass PC Board, and typically the published Er value was measured at 1 kHz,
At 2.4 GHz, Er is going to be in the 3.7-3.8 range.? You can check their spec sheets for Er vs frequency plots, but that data is not commonly provided.

You have to pay BIG Bucks for PCB material that has little change with frequency.
For the record, you have not been able to buy FR-4 for some years.? It contained a Bromide Anti-Flammability compound that was banned by RoHS.??? Yea, lots of similar stuff on the market with slightly different part numbers.?

Best way to measure the Er at 2.4 GHz, bit out of the range for most Nano's, is to design a patch antenna for 2.4 GHz and see what frequency is really resonates at.? Then back into the calculations for a patch antenna using Er's that give you the actual frequency.?? Kent

On Wednesday, July 27, 2022 at 10:49:19 AM CDT, steiniche@... <steiniche@...> wrote:

Hi

I have a NanoVNA V2 Plus4.

I am trying to validate a PCB 50 ohm transmission line (trace) to be used for 2.4 GHz Wifi.

I am using a 4 layer stack-up (1.6 mm total) with the following configuration:

L1: Signal + ground pour
Prepreg 0.21 mm
L2: Ground
Prepreg 1 mm
L3: Empty
Prepreg 0.21 mm
L4: Ground

Board is FR-4 with Er = 4.6.

I have calculated the trace parameters using Saturn PCB design as a "coplanar wave" with a plane below.

I have attached 6 board files showing the actual board (board_image.jpg), rendered board (board_render.png) and the four layers (board_lx.png) + a screenshot of the calculations from Saturn PCB (calc.png). I use the following connectors from Molex:

I have calibrated the VNA in frequency range 2 GHz to 2.8 GHz with the provided SMA cable connected, see attached cal_load.jpg and cal_thru.jpg, direct_load.png, direct_thru.png

Now I connect the PCB trace and do a S11 and S21 measurement (see s11_s21.jpg). It seems to me that the result is not particularly good (see trace_thru.png and trace_load.png).

Can any of you spot any issues with the measurement method or configuration of the board? Also, if you can provide some realistic target results for such a configuration (two connectors + 82 mm trace) that would be great.

Any help is highly appreciated.

Thanks

br
Christian
 

On 7/27/22 9:18 AM, KENT BRITAIN wrote:
Hi Christian
I do lots of antennas on fiberglass PC Board, and typically the published Er value was measured at 1 kHz,
At 2.4 GHz, Er is going to be in the 3.7-3.8 range.? You can check their spec sheets for Er vs frequency plots, but that data is not commonly provided.
Most people do a test coupon, which is essentially what you're doing.


You have to pay BIG Bucks for PCB material that has little change with frequency.
Rogers Duroid(tm) is an example. It also has low loss at microwave frequencies - the issue is the glass in FR-4. Taconic is another brand. You can get them with epsilon all the way from 2 to 10.

For the record, you have not been able to buy FR-4 for some years.? It contained a Bromide Anti-Flammability compound that was banned by RoHS.??? Yea, lots of similar stuff on the market with slightly different part numbers.
Most fab houses still offer FR4


Note the epsilon they give for the various mfrs (3.2 to 3.92)

whether they are brominated, I don't know - there's lots of materials that can make something fire retardant. I don't know that bromine is as much a concern as lead, which is where RoHS gets to be a big deal.




has more info. Polybrominated biphenyls aren't allowed in RoHS, but that might not be a common problem. There are "FR-4 halogen free" materials too.




Best way to measure the Er at 2.4 GHz, bit out of the range for most Nano's, is to design a patch antenna for 2.4 GHz and see what frequency is really resonates at.? Then back into the calculations for a patch antenna using Er's that give you the actual frequency.?? Kent
On Wednesday, July 27, 2022 at 10:49:19 AM CDT, steiniche@... <steiniche@...> wrote:
Hi
I have a NanoVNA V2 Plus4.
I am trying to validate a PCB 50 ohm transmission line (trace) to be used for 2.4 GHz Wifi.
I am using a 4 layer stack-up (1.6 mm total) with the following configuration:
L1: Signal + ground pour
Prepreg 0.21 mm
L2: Ground
Prepreg 1 mm
L3: Empty
Prepreg 0.21 mm
L4: Ground
Board is FR-4 with Er = 4.6.
I have calculated the trace parameters using Saturn PCB design as a "coplanar wave" with a plane below.
I have attached 6 board files showing the actual board (board_image.jpg), rendered board (board_render.png) and the four layers (board_lx.png) + a screenshot of the calculations from Saturn PCB (calc.png). I use the following connectors from Molex:
I have calibrated the VNA in frequency range 2 GHz to 2.8 GHz with the provided SMA cable connected, see attached cal_load.jpg and cal_thru.jpg, direct_load.png, direct_thru.png
Now I connect the PCB trace and do a S11 and S21 measurement (see s11_s21.jpg). It seems to me that the result is not particularly good (see trace_thru.png and trace_load.png).
Can any of you spot any issues with the measurement method or configuration of the board? Also, if you can provide some realistic target results for such a configuration (two connectors + 82 mm trace) that would be great.
Any help is highly appreciated.
Thanks
br
Christian
 

At a glance I noticed the wide traces at the connector pins, which are excess capacitance. Unless there is a compelling reason to do otherwise I tend to select a dielectric material whose 50¦¸ width is slightly larger than the connector pins and component pads I plan on using. It is only necessary to use thin boards such as you are using for very high frequency (>20+GHz perhaps), work, to avoid resonances and radiation. 0.8mm board (or thicker) might be more appropriate.

I also like to pull the solder mask away from the RF traces ideally 2 line widths wide, again to avoid excess capacitance; solder mask has a higher dielectric constant than air. This excess capacitance is particularly problematic in the gaps between RF line and ground of your .

I like to chamfer the corners of the transmission lines and leave a small gap at the connector pin, again to avoid excess capacitance.

Finally, many board houses charge per hole drilled ("hits") and if so, you can drastically reduce the number of vias to a single line on each side of the RF line, with a cluster of vias, or better yet, wraparound grounds (could be copper foil added at assembly), for the connector grounds.

Best regards, Don Brant.
 

ONLY if you test that coupon at 2,400,000,000 Hz!
Testing with the typical C Meter won't do it!?? The usual standard is 1000 Hz.

The Er changes with frequency when you get in the MHz.and up.?? Kent

On Wednesday, July 27, 2022 at 07:04:11 PM CDT, Jim Lux <jimlux@...> wrote:

On 7/27/22 9:18 AM, KENT BRITAIN wrote:
? Hi Christian
I do lots of antennas on fiberglass PC Board, and typically the published Er value was measured at 1 kHz,
At 2.4 GHz, Er is going to be in the 3.7-3.8 range.? You can check their spec sheets for Er vs frequency plots, but that data is not commonly provided.
Most people do a test coupon, which is essentially what you're doing.



You have to pay BIG Bucks for PCB material that has little change with frequency.
Rogers Duroid(tm) is an example. It also has low loss at microwave
frequencies - the issue is the glass in FR-4. Taconic is another brand.
You can get them with epsilon all the way from 2 to 10.

For the record, you have not been able to buy FR-4 for some years.? It contained a Bromide Anti-Flammability compound that was banned by RoHS.??? Yea, lots of similar stuff on the market with slightly different part numbers.
Most fab houses still offer FR4


Note the epsilon they give for the various mfrs (3.2 to 3.92)

whether they are brominated, I don't know - there's lots of materials
that can make something fire retardant. I don't know that bromine is as
much a concern as lead, which is where RoHS gets to be a big deal.




has more info.? Polybrominated biphenyls aren't allowed in RoHS, but
that might not be a common problem.? There are "FR-4 halogen free"
materials too.





Best way to measure the Er at 2.4 GHz, bit out of the range for most Nano's, is to design a patch antenna for 2.4 GHz and see what frequency is really resonates at.? Then back into the calculations for a patch antenna using Er's that give you the actual frequency.?? Kent



? ? ? On Wednesday, July 27, 2022 at 10:49:19 AM CDT, steiniche@... <steiniche@...> wrote:
?
? Hi

I have a NanoVNA V2 Plus4.

I am trying to validate a PCB 50 ohm transmission line (trace) to be used for 2.4 GHz Wifi.

I am using a 4 layer stack-up (1.6 mm total) with the following configuration:

L1: Signal + ground pour
Prepreg 0.21 mm
L2: Ground
Prepreg 1 mm
L3: Empty
Prepreg 0.21 mm
L4: Ground

Board is FR-4 with Er = 4.6.

I have calculated the trace parameters using Saturn PCB design as a "coplanar wave" with a plane below.

I have attached 6 board files showing the actual board (board_image.jpg), rendered board (board_render.png) and the four layers (board_lx.png) + a screenshot of the calculations from Saturn PCB (calc.png). I use the following connectors from Molex:

I have calibrated the VNA in frequency range 2 GHz to 2.8 GHz with the provided SMA cable connected, see attached cal_load.jpg and cal_thru.jpg, direct_load.png, direct_thru.png

Now I connect the PCB trace and do a S11 and S21 measurement (see s11_s21.jpg). It seems to me that the result is not particularly good (see trace_thru.png and trace_load.png).

Can any of you spot any issues with the measurement method or configuration of the board? Also, if you can provide some realistic target results for such a configuration (two connectors + 82 mm trace) that would be great.

Any help is highly appreciated.

Thanks

br
Christian





? ?




 

On 7/27/22 5:25 PM, Donald S Brant Jr wrote:
At a glance I noticed the wide traces at the connector pins, which are excess capacitance. Unless there is a compelling reason to do otherwise I tend to select a dielectric material whose 50¦¸ width is slightly larger than the connector pins and component pads I plan on using. It is only necessary to use thin boards such as you are using for very high frequency (>20+GHz perhaps), work, to avoid resonances and radiation. 0.8mm board (or thicker) might be more appropriate.
As I recall, 50 ohms on 1 ounce copper on an 0.031" board with epsilon=2.5 as microstripline was 0.1" wide. There's countless calculators out there. If you pick the board correctly, a 4 pin SMA solders on very nicely. (the gap between corner pin and center pin is about 1 mm, which is close to 0.039")

I also like to pull the solder mask away from the RF traces ideally 2 line widths wide, again to avoid excess capacitance; solder mask has a higher dielectric constant than air. This excess capacitance is particularly problematic in the gaps between RF line and ground of your .
I like to chamfer the corners of the transmission lines and leave a small gap at the connector pin, again to avoid excess capacitance.
Finally, many board houses charge per hole drilled ("hits") and if so, you can drastically reduce the number of vias to a single line on each side of the RF line, with a cluster of vias, or better yet, wraparound grounds (could be copper foil added at assembly), for the connector grounds.
Best regards, Don Brant.
[email protected]
 

Hi

Thanks a lot for your responses.

Jim, I was not aware that Er would potentially drop significantly by frequency. I will check if data exists for Er vs frequency. Thanks.

Donald, good point on the trace width at the connector pins. I have used the recommended footprint from Molex, but I do see the issue that the pad is part of the trace and does not satisfy the trace width that I calculated. Thanks.

I will order a range of test boards with different trace widths and ground gaps to see if I can get closer.

Do any of you have an idea to what a target S11 / S21 should be for such as trace?

br
Christian
 

If you would take your existing board and use a sharp knife to remove the excess copper you might get a better result, or at least see what changes occur. Trimming the connector pins back will also help reduce THEIR capacitance, as will using minimum solder on the pins.

Of course matching the dielectric constant/height/width to the connector dimensions is the ideal solution. I would do this before going out and fabbing another batch of boards with the same thin dielectric. Thicker boards lalso have larger features so are proportionately less sensitive to mechanical tolerances. The transmission line calculators are accurate, problems with unexpected results are almost always a result of poor layout rather than calculation errors. Trying to compensate by tweaking dimensions instead of making a better layout will not end well, I have been there.

An S11 of -20dB or better is a good result for a length of microstrip or CPWG line plus two connectors/transitions, although I have seen better than -30dB.
The S21 that you are getting where the S11 is good should be achievable across the band, if you get the match fairly good; much of the loss you are seeing is reflection loss due to mismatch, not dissipative loss.
73, Don N2VGU

1 - 8 of 8