Open hardware microwave vector network analyzer

[hendorog]

I've been looking for a looong time for an affordable HP/Wiltron cal kit on eBay and have never seen one for a reasonable price.
There is some sort of pricing mania which affects brand name cal kits. So that leaves the Dr Kirkby ones which are not cheap or DIY.

Considering that, I think the smart option here is for interested parties to setup a calibration club.
Purchase the individual parts, send them to someone who has a calibrated cal kit and get the S-params back along with the parts.
There is code on the net to turn the measured s-params into the model required by a VNA.

[hendorog]

Hi loxodes, I was just about to get some rf bridge pcbs made from the gerbers you have in your vna2 git repo.

However I just saw that the SMA launch pads are very wide where the pin is soldered compared to the transmission line width. I suspect that this would increase the return loss.

My theory is that they should actually be narrower than the the transmission line to compensate for the added thickness of the pin and the solder.
This is what I think is happening in this doc: https://belfuse.com/resources/AssemblyInstructions/JAI026.pdf

The other option is to use a very short pin and keep the trace width constant - e.g. https://belfuse.com/resources/cinch-brochures/CCS%20Johnson%20SMA%20HF%20End%20Launch%20App%20Note.pdf

I'm currently thinking I will get some boards made based on these theories and see what they turn out like, but I am interested to hear your thoughts or anyone else's regardless.

[loxodes]

Hi loxodes, I was just about to get some rf bridge pcbs made from the gerbers you have in your vna2 git repo.

However I just saw that the SMA launch pads are very wide where the pin is soldered compared to the transmission line width. I suspect that this would increase the return loss.

My theory is that they should actually be narrower than the the transmission line to compensate for the added thickness of the pin and the solder.
This is what I think is happening in this doc: https://belfuse.com/resources/AssemblyInstructions/JAI026.pdf

The other option is to use a very short pin and keep the trace width constant - e.g. https://belfuse.com/resources/cinch-brochures/CCS%20Johnson%20SMA%20HF%20End%20Launch%20App%20Note.pdf

I'm currently thinking I will get some boards made based on these theories and see what they turn out like, but I am interested to hear your thoughts or anyone else's regardless.

The vna2 git repo is Henrik's, not mine. If you look at the second layer of his gerber files, he added a cutout on the ground plane below the center pin of the SMA connector to compensate for the increased trace width.

The paper which he based the bridge from uses the same style connectors as the ones you've linked to:
 http://ieeexplore.ieee.org/document/7345756/

I'm in the middle of layout for a board which is mostly a copy of the the IEEE paper. I'll be using Amphenol 901-10512-3 connectors with a footprint which I've tested as working reasonably well out to 12 GHz:

https://raw.githubusercontent.com/loxodes/vna/devel/lib/vna_footprints.pretty/SMA_901-10512_6p7MIL_FR408_CPW_LAUNCH.kicad_mod

[hendorog]

Oh dear that is embarrassing, apologies for my confusion.

I had missed the cutout in my haste as well. Thanks also for the other information and the pointer to your footprint, it is very helpful.

Unfortunately I don't have any access to the IEEE paper mentioned, but have read the Dunsmore paper.
I will get some boards based on Henriks gerbers underway, but will also look at making some based around your tested Amphenol footprint too.

I am interested to see what the effect of different ferrite beads.

[loxodes]

No worries.

I just finished layout of the bridge assuming the OSH Park 4 layer stackup, I'm planning on ordering a set tomorrow after checking over the design.
https://github.com/loxodes/vna/tree/devel/breakouts/coupler_test

Here is a kicad footprint for the bridge with up to 6.1 mm diameter ferrites, no guarantees that it works:
https://github.com/loxodes/vna/blob/devel/lib/vna_footprints.pretty/resistive_bridge_osh_fr408_ustrip.kicad_mod

[hendorog]

Nice, thanks for the heads up.

I will order some of them too, but I will try removing the solder mask on mine around the transmission lines just as an experiment.

Did you happen to do any tests to see if that makes any difference?

[loxodes]

I will order some of them too, but I will try removing the solder mask on mine around the transmission lines just as an experiment.

Did you happen to do any tests to see if that makes any difference?

I'm still trying to build test equipment sensitive enough to measure the difference

A moat of soldermask near the center pin is helpful at stopping solder from wicking down the trace. ENIG plating will add some loss if you remove the soldermask (https://bethesignal.com/wp/2011/09/impact-from-electroless-nickel-on-microstrip-insertion-loss-and-propagation-delay/)
 I haven't measured or simulated which would be better.

[hendorog]

Haha, well you are pretty close

I just ordered some boards with the solder mask removed, and then another set with all of the ground planes added in and via stitched.

Thanks for that info on the effect of nickel. I hadn't come across that before.

[Kilo Tango]

As far as Cal kits I came across this the other day :

I think he sells them thro rfshop.com.au. I don't know how good/bad they are but maybe worth checking out.

Ken

[loxodes]

As far as Cal kits I came across this the other day :

I think he sells them thro rfshop.com.au. I don't know how good/bad they are but maybe worth checking out.

Ken

It looks like his cal kits are only rated to 4 GHz, the sdr-kits kit may be a better better deal. (https://www.rfshop.com.au/sma-cal-calibration-kit.html)

[loxodes]

Haha, well you are pretty close

I just ordered some boards with the solder mask removed, and then another set with all of the ground planes added in and via stitched.

Thanks for that info on the effect of nickel. I hadn't come across that before.

Filling the out ground plane with no soldermask would have been a good idea. I received a set of coupler boards and it looks like copper was routed out along the internal cutout. I was expecting copper to fill right up against the internal edge, but the fab appears to have routed out about 0.5 mm of clearance between pads and the board edge.

There is just enough copper left that I may still be able to make it work..

[hendorog]

Haha, well you are pretty close

I just ordered some boards with the solder mask removed, and then another set with all of the ground planes added in and via stitched.

Thanks for that info on the effect of nickel. I hadn't come across that before.

Filling the out ground plane with no soldermask would have been a good idea. I received a set of coupler boards and it looks like copper was routed out along the internal cutout. I was expecting copper to fill right up against the internal edge, but the fab appears to have routed out about 0.5 mm of clearance between pads and the board edge.

There is just enough copper left that I may still be able to make it work..

Yes mine are exactly the same. I agree, it should be possible to make it work - maybe with a sliver of copper tape to make that copper strip wider to solder the resistors.

[loxodes]

I assembled one of the couplers and took some messy sweeps with a spectrum analyzer/tracking generator.

Insertion loss and coupling are about what I expected, but directivity is only better than 10 dB out to 8 GHz. Maybe adding a top side ground fill or tweaking the resistor values could improve isolation?

[hendorog]

Nice. I have also assembled one and did some quick tests on my 8753 last night.

I will print out some results tonight, but I think the directivity was similar to what you are seeing. I was expecting the directivity to be better than that below 1GHz. I don't know what the problem is there. I did suspect my soldering as the 4 resistors around the coax were quite difficult.

Adding some capacitance with some copper tape or thin metal at both the in and the out ports might improve it a bit more, I was poking at it with my finger and it seemed like I could make it a couple of dB better.

I think I stuffed up and put the beads in the wrong order because I mixed up the test port and the input port. I think the low mu beads should be at the two port end, and the high mu beads at the one port end. That might be affecting performance at the higher frequency end on mine.

[loxodes]

Reducing the resistance between coax shield and ground from ~10.3 ohms to 9.2 ohms didn't appear to improve isolation much.

Attached is a picture of my construction and a revised directivity plot.

Moving the toroids from the one port end to the two port end didn't appear to have much an effect on directivity. (I'm arbitrarily using two Laird 35T0231-00P toroids.)

[hendorog]

With a bit of tweaking - I used some solar tabbing wire - I was able to get worst case directivity very close to 20dB at 3GHz. For the rest of the range it is better than that, up to 6GHz (the limit of my 8753).

I used expensive thin film resistors, mounted them upside down, and used a Vishay FC resistor for the 50 ohm reference resistor. The coax is just cheap RG 405 from China though.

A couple of observations:
The test port return loss isn't so good around 3GHz, which is also where the directivity is at it's worst.
The best directivity is only 26 dB or so even at lowish frequencies sub 1GHz after tuning, which makes me think something is not quite right with my build.

[loxodes]

With a bit of tweaking - I used some solar tabbing wire - I was able to get worst case directivity very close to 20dB at 3GHz. For the rest of the range it is better than that, up to 6GHz (the limit of my 8753).

Nice!

How/where did you use the solar tabbing wire?

It turns out I've been using thick film resistors for the 0402 ~270 ohm and six 0603 62 ohm resistors. I'll order some decent thin film ones..

[hendorog]

Here you go. The 5mm stuff is quite stiff and is what I used. The 2mm is light and flimsy.

https://www.ebay.com/itm/2mm-Tabbing-Wire-5mm-Bus-Wire-Ribbon-Solar-Covered-for-DIY-Solar-Cell-Panel/391316100296?hash=item5b1c41d4c8:m:muMOC6FwYJTtWRe5FDrQ1og

Very handy stuff. The 2mm is a handy no-strip wire alternative/rough as guts transmission line. Solder is impregnated into it already.

I'll try and do pics tonight.

[hendorog]

Here are some pics of the bridge, and test results on the VNA, and then using the SH 124B + TG

I am measuring directivity by normalising with the test port open, attaching a 50 ohm load onto the test port and then making the measurement.

Edit: sorted out the pics, note that I was tweaking the tuning tab all of the time so the images show different tunings.

Bridge pics




Directivity tuned for 6GHz


Directivity tuned for best under 3GHz


Return loss


Difference between open and short



Attached images show the directivity measured on the Signalhound.

[henrikf]

It's quite hard to get better than 20 dB directivity at high frequencies as the output matching needs to be better than directivity. The reflected power from the mismatch reflects in to the coupling port and shows up as worsened directivity. SMA connector layout and impedance of the traces is very important. Also during the measurements S11 of termination needs to be better than directivity or otherwise the reflected power from the termination affects the measurement. It's possible to correct the non-ideal termination in post-processing (http://scikit-rf.readthedocs.io/en/latest/examples/metrology/Measuring%20a%20Mutiport%20Device%20with%20a%202-Port%20Network%20Analyzer.html)

I have found that OSH Park has consistent over etching. 50 ohm microstrip should be 0.34 mm wide, but I measured one 50 ohm line to actually be 0.27 mm on the PCB. This makes the characteristic impedance of the trace to be 57 ohms. Mismatch from 50 to 57 ohms is already -23 dB so it's not surprise if the high frequency directivity is not as good as expected if over etching is not taken into account.

[Odysseus]

Forgive my ignorance, but what is stopping you from using identical reference and DUT impedance/ports/layout? Any mismatch will be shared and cancel to the first order, eliminating deficiencies in the bridge, leaving only your reference terminator as the unknown.

I ask because I recently built such a bridge, and see 50-40dB directivity to 200MHz (limit of my signal generator).

[hendorog]

Forgive my ignorance, but what is stopping you from using identical reference and DUT impedance/ports/layout? Any mismatch will be shared and cancel to the first order, eliminating deficiencies in the bridge, leaving only your reference terminator as the unknown.

I ask because I recently built such a bridge, and see 50-40dB directivity to 200MHz (limit of my signal generator).

In this design the DUT and reference termination cannot be both on SMA connections, as the Zo resistor is not referenced to ground - both ends are 'floating'.

The cool thing about this design is that there is theoretically not much loss in the bridge - only about 1.6 dB.


 

[hendorog]

It's quite hard to get better than 20 dB directivity at high frequencies as the output matching needs to be better than directivity. The reflected power from the mismatch reflects in to the coupling port and shows up as worsened directivity. SMA connector layout and impedance of the traces is very important. Also during the measurements S11 of termination needs to be better than directivity or otherwise the reflected power from the termination affects the measurement. It's possible to correct the non-ideal termination in post-processing (http://scikit-rf.readthedocs.io/en/latest/examples/metrology/Measuring%20a%20Mutiport%20Device%20with%20a%202-Port%20Network%20Analyzer.html)

I have found that OSH Park has consistent over etching. 50 ohm microstrip should be 0.34 mm wide, but I measured one 50 ohm line to actually be 0.27 mm on the PCB. This makes the characteristic impedance of the trace to be 57 ohms. Mismatch from 50 to 57 ohms is already -23 dB so it's not surprise if the high frequency directivity is not as good as expected if over etching is not taken into account.

Thanks, that is a very good tip about the over etching. I did notice that my tuning tab worked best when over the top of the test port microstrip trace. It sounds like you may well have explained why that is. I will have a play around with that trace and see what happens if I e.g. fatten it up with solder and/or put some dielectric on top of it.

[loxodes]

The trace width on my coupler board appears to be correct within about .02mm.

From what I understand OSH Park works with multiple fabs to manufacture their panels, so etching may not be consistent.

[hendorog]

I guess there will be an error in the trace width, dielectric thickness and the Er of the particular batch of dielectric.

The question is how significant is this error considering the traces are quite short.

Here are some more pics after tweaking for best return loss. Directivity is getting quite good now at the high end.
I can't seem to move the lower end much (< 4GHz), possibly a longer coax with more beads would help?


Second image is the open/short balance.


The last image is with my finger carefully placed on the test port, directivity very good