How to properly use these SMA connectors

[Mrt12]

Hey guys,
I have a maybe dumb question. I designed a small mixer+amplifier circuit that works at 23GHz. The prototype PCB that I made works fine, however, for practical use in my application, I need to design it a bit different so I can put it in a metal box for shielding.

For my testing PCB, I have used this connector from Rosenberger 32K243-40ML5

https://mou.sr/3Upb7nE

and I see some people call it "solderless". I am confused, as the Rosenberger datasheet does not give any information about this, I soldered the centre pin in my case. But is this connector really intended to be not soldered at all, i.e. I just make a PCB with gold plating, add this connector and that's it? this would be really nice. But I almost cannot believe this works reliably without soldering.

The other thing that puzzles me already for years is these SMA flange connectors that have this super tiny pin at the end. An example is this one:

https://mou.sr/450J6I9

How are these connected properly to a PCB? this pin is not even long enough to go through some sort of panel. Similar connectors are available that have a flat pin instead of a round one like this:

https://mou.sr/4o4pAD9

it looks to me like this could be connected to some sort of microstrips, but again, the pin is actually too short to go through any sort of panel.

For my current project, I use the HMC977 mixer, and I would like to put it inside a milled aluminium box that has probably ~2..3mm wall thickness, so I need SMA connectors that are properly specified for 23GHz (yes, it's actually 3.5mm connectors....) and that can be mounted on a 3mm panel. But I do not know how these are typically connected to the PCB, so may I get some enlightment here?

thanks!

[Vovk_Z]

That's a good question, definitely not dumb. 23 GHz is sure quite high. I'm interested too, so I'll sit here and wait an answer too.

[shabaz]

I don't know about those particular ones, but generally solderless ones are certainly available and are indeed fully solderless, e.g. this 50-sec video shows an edge launch connector being assembled.



I've only used the vertical-mount solderless versions, and they are really nice. There are different versions, some just press against the conductor, whereas others can even have a little spring internally. The attached photo shows the latter.

The main difficulty with these connectors (apart from that it's easy to lose the screw so you might want to buy spares of those if possible) is the footprint, because not all manufacturers have complete advice there, so it's on you to perform any simulations or test board measurements to know if your proposed footprint will work well or not (sure you'd have to do that with any connector, but at least there are many reference boards/examples for typical soldered connectors, to have a starting point). You may well need to create dozens of possible footprints (and even that may not be enough) on a test board of whatever board you're using so there's that cost too.

[Mrt12]

I don't know about those particular ones, but generally solderless ones are certainly available and are indeed fully solderless, e.g. this 50-sec video shows an edge launch connector being assembled.



I've only used the vertical-mount solderless versions, and they are really nice. There are different versions, some just press against the conductor, whereas others can even have a little spring internally. The attached photo shows the latter.

The main difficulty with these connectors (apart from that it's easy to lose the screw so you might want to buy spares of those if possible) is the footprint, because not all manufacturers have complete advice there, so it's on you to perform any simulations or test board measurements to know if your proposed footprint will work well or not (sure you'd have to do that with any connector, but at least there are many reference boards/examples for typical soldered connectors, to have a starting point). You may well need to create dozens of possible footprints (and even that may not be enough) on a test board of whatever board you're using so there's that cost too.

great, thanks a lot for this! Indeed I also saw these connectors and wondered how they work.
Do they have a little spring contact for the inner conductor on the bottom side, that contacts the PCB?

How would you use these connectors in case you want to mount your PCB in a milled aluminium case. It seems to me the connector itself is very short, so if it goes through 2..3mm of aluminium wall, then there is probably not enough space to actually attach an SMA connector on the outside.

[tszaboo]

great, thanks a lot for this! Indeed I also saw these connectors and wondered how they work.
Do they have a little spring contact for the inner conductor on the bottom side, that contacts the PCB?

How would you use these connectors in case you want to mount your PCB in a milled aluminium case. It seems to me the connector itself is very short, so if it goes through 2..3mm of aluminium wall, then there is probably not enough space to actually attach an SMA connector on the outside.

I think there is just enough compliance in the center pin to make contact to a coplanar waveguide.
Würth has some application notes about them on their website.
https://www.we-online.com/en/components/products/CM_SMA_CONNECTORS_PCB_SOLDERLESS

I ordered a pair of these a week ago, and I'm planning to make a PCB with my regular SMA and these to see if I can measure the difference. I think I'll use these by default on my "throwaway" test boards, as probably I can get a better consistency of the connector than soldering SMA connectors.

[Mrt12]

yes it seems like a good thing, you can prototype stuff and reuse the connectors!

I saw Würth has also a variant of this connector that is intended for striplines (instead of microstrip). The striplines are routed in inner layers of the PC board. I am thinking about if it would be a good idea to try out the striplines, but I never made any striplines at 23 GHz, and I am worrying about the vias needed to go to an inner layer. Do you have experience with this?

I think I will also make a small test board with some through lines and pads for the connectors and order a couple of these connectors and test how it works.

[tszaboo]

yes it seems like a good thing, you can prototype stuff and reuse the connectors!

I saw Würth has also a variant of this connector that is intended for striplines (instead of microstrip). The striplines are routed in inner layers of the PC board. I am thinking about if it would be a good idea to try out the striplines, but I never made any striplines at 23 GHz, and I am worrying about the vias needed to go to an inner layer. Do you have experience with this?

I think I will also make a small test board with some through lines and pads for the connectors and order a couple of these connectors and test how it works.

Yes, I have experience running RF through vias. It was calculating the via characteristics, place it on the board.
Then push my head into the sand like an Ostrich and never measure it and call it probably good enough.
On second though, it is tested, but the testing was RSSI and range testing, and not VNA measurements.

[Mrt12]

Yes, I have experience running RF through vias. It was calculating the via characteristics, place it on the board.
Then push my head into the sand like an Ostrich and never measure it and call it probably good enough.
On second though, it is tested, but the testing was RSSI and range testing, and not VNA measurements.

Cool, I will try this, too. If it is of interest, I could probably post my results here.

By the way, you don't have experience with the other connectors I showed in my original post, do you?

[tszaboo]

Yes, I have experience running RF through vias. It was calculating the via characteristics, place it on the board.
Then push my head into the sand like an Ostrich and never measure it and call it probably good enough.
On second though, it is tested, but the testing was RSSI and range testing, and not VNA measurements.

Cool, I will try this, too. If it is of interest, I could probably post my results here.

By the way, you don't have experience with the other connectors I showed in my original post, do you?

Not yet, I have them, but am still designing the board for it.

[Miek]

The 32K243-40ML5 is not solderless, you do need to solder the centre conductor to make good contact. The Wurth 60312862112552, while it looks the same, is slightly different - its centre conductor is slightly below the plane of the main connector, so when you clamp it all together it presses against the trace and makes good contact without any solder.

[G0HZU]

I've got a few SMA end launch connectors here that bolt to a metal block that then gets screwed to a PCB but they are really only meant to be used up to 18 GHz.

See below for an example of a 2.92mm end launch connector from Southwest. These connectors are used on a wideband MMIC amplifier I have here. It provides about 16dB gain from 2GHz to 24 GHz so it needs to use better connectors than SMA.

There's some additional info about the RF performance of these 2.92mm connectors and how to mount these connectors to a suitable PCB in the doc linked to below:

https://mpd.southwestmicrowave.com/wp-content/uploads/End-Launch-Connectors.pdf

[Mrt12]

Thanks for all the hints so far.
I decided I am going to make a small test board, like in the attachment. As the connectors are solderless, they can easily be recycled, so just 2 connectors is enough to test.
I have several different transmission line types on it, and also the possibility to add shunt or series elements. The short allows for VNA calibration.

What do you guys think about my transmission lines?
I use KiCAD and used the integrated transmission line calculator to verify the width of the microstrips, and the width/gap of the CPWG.

[shabaz]

For what it's worth (not much!) My attempt is shown in the attached photos. This was on FR4,  100 mm length, and was JLC controlled impedance board, and I only did a scalar S21 measurement to 3 GHz, never got around to better testing. I think the approx 2 dB loss at the upper end of the measurements is probably to be expected, but the output was still disappointing enough that I wasn't motivated to do any further tests at the time. You can see from the footprint I tried doing a transition area to get to microstrip. This was on a 4-layer board. The annotated footprint diagram was my notes on all the parameters I wanted to be able to tweak in the CAD footprint (sometimes not easy without warnings from the CAD software).
Incidentally, I reckon the end launch ones may be more practical, because the footprints could be reused at a pinch with normal solderable SMA connectors too. Whereas the vertical connector footprints will only work with that particular SMA.
Anyway, don't assume I know what I was doing, because I didnt; I took a scattergun approach to almost randomly trying different combinations of parameter values, and this seat-of-the-pants approach didn't really work for me, unsurprisingly. Still, it was worth a shot and now I know I would like to try end launch solderless connectors one day too.

[Mrt12]

OK 2dB loss at only 3 GHz is already a lot!
However, if I understood correctly, you use FR4?

I want to try this on a "proper" RF substrate, like Isola I-Tera that is specified to be usable to at least 10GHz. There is no spec at 20GHz, but I assume if it works at 10GHz with a loss tangent of only 0.0031, it possibly also works at 23GHz. I guess I will find out. But thanks for your post, this is indeed very interesting and helpful!

[shabaz]

Hi,
Correct, this was FR4 (my approach wasn't affordable for proper substrate for my purposes, since the test boards were quite large (approx 100x100mm) and I had two different test boards with different lengths of microstrip. I figured if I could get to a somewhat satisfactory state for a few GHz on FR4, then it might be worth attempting the higher end options. But this wasn't work related so I didn't have a goal, so was never prioritised and worked on further.

[Marsupilami]

This is my recent favorite budget option: https://www.digikey.com/short/v4hr4r59
The angled contact digs in well even if your board is not pristine clean or uneven. I'm generally not in good terms with edge launches as it is an ordeal to get the copper reliably close enough to the edge with edge-plating correctly removed. Vertical launches don't have that problem either, but the angled one lets you visually align the pin so it is very user friendly.

On another note add more ground vias. Double what you think is already too much. Especially at the CPWG -> Microstrip transition.
Think of the return current on the ground contacts. You want that transition as graceful as possible and if there is no direct path for the return current between the coplanar ground and the bottom ground plane it will be forced to take a detour impacting performance.


 
HTH

[Mrt12]

Good day dear colleagues
as I promised, I made a little test board for these Würth solderless SMA connectors. See attached a couple pictures.

01: this is the board. I have included several microstrip lines, a CPWG and a pi attenuator. Also there are transmission lines that include vias so I can measure the effects of the vias.

02: connector to CPWG on top layer.

03: connector to via, on the backside is the 50 ohm microstrip.

04: connector to 70 ohm microstrip. The 50 ohm microstrip has the same width as the centre pad of the connector.

05: the board from the backside.

I have used Eurocircuits RF Pool (https://www.eurocircuits.com/services/rf-pool/) with the following stackup:

top Cu layer
core, Isola I-Tera, er=3.45, thickness 0.254mm
inner layer, connected to ground
FR4 core for stability, thickness 0.5mm
inner layer, connected to ground
core, Isola I-Tera, er=3.45, thickness 0.254mm
bottom Cu layer

I will make additional posts to show my results.

[Mrt12]

So I measured the S parameters of the different structures that I have on this board. The VNA was first calibrated, and then I connected the SMA connectors. Then, I mounted the SMA connectors on a short such that I can apply port extension and such compensate for the electrical length of the connectors. (As you may see from my photos, I have a pure short pad on my test PCB).

Using the VNA that is calibrated in this way, I measured all the transmission lines on the little test PCB. Here are my results. For the microstrips that connect on the same side as the connector is mounted, I used these connectors

https://www.mouser.ch/ProductDetail/710-60312872112545

and for the two microstrips that are completely routed on the backside, I used the special "stripline" variant of the connectors

https://www.mouser.ch/ProductDetail/710-60312872112546

(as you can see from the drawings in the datasheet, the microstrip connector has a little "dent" for the feedthrough of the microstrip, whereas the stripline connector does not have this).

ms50.png: this is the "normal" 50 ohm microstrip. The matching is roughly close to 20dB up to 18GHz, and approx -13dB at 23GHz.

ms70.png: 70 ohm microstrip. We can see the mismatch as expected.

cpwg.png: this is the coplanar waveguide. It appears to me like it is a tiny bit better matched than the 50 ohm microstrip.

Now comes the more interesting stuff!

ms50-2vias.png: this is a 50 ohm microstrip couple millimeters on the top layer, then a via, then on the bottom layer, then a via and then back on the top layer. We see the matching is clearly worsre but stays below 10dB.

50r-vias.png: this are the stripline connector, where I have placed a via directly below the connector and the entire microstrip is on the back side. It seems to work somehow, but unfortunately, the matching is not super good. Unfortunately, this was exactly the variant of connector that I planned now to use for my project.

Just for fun, I made also the little 3dB attenuator on the PCB from random 0402 resistors from the junk box. It should be 3dB pi attenuator, with 300 ohm shunt and 18 ohm series. The attenuator S parameters are shown in att.png.


So I know now that in principle the microstrips and CPWG work very good, this is a great achievement. However I don't like the microstrips that go through the via. But, I cannot optimise much the via diameter, as I am already at the smallest diameter that I can do with Eurocircuits RF pool. So I wonder if there is potential to tune this? I cannot make the via hole much smaller, and also of course if it is too large, it will not make proper contact with the connector. So any ideas here?

I am not sure if I can be happy with this as in general, the matching is at least not terrible, or if I shall be super sad as the matching is still quite a bit worse than I expected.

Critiques are welcome.

[tszaboo]

I would try to terminate one of your CPWGs with a Vishay FC series resistor. It's 50 Ohm, about 2-4 EUR. and it's a very high performance RF resistor.

[Mrt12]

sure but I can also use a SMA 50 ohm termination.
However for these measurements the network analyzer ports were connected, so both ports of one transmission line are terminated properly.

[Marsupilami]

Do a time domain conversion on your VNA sweeps and use time gating to separate spatial sections. The most straightforward way to do this is in Metas VNA Data Explorer. That's close to home to you anyway

The stripline via is not guaranteed to be fixable if you're technology restricted. The TDR plots help because you can get some amount of info on whether it is overly inductive or capacitive and you can try to compensate the other way coming out of it, but it's never going to be perfect.

[Mrt12]

Do a time domain conversion on your VNA sweeps and use time gating to separate spatial sections. The most straightforward way to do this is in Metas VNA Data Explorer. That's close to home to you anyway

The stripline via is not guaranteed to be fixable if you're technology restricted. The TDR plots help because you can get some amount of info on whether it is overly inductive or capacitive and you can try to compensate the other way coming out of it, but it's never going to be perfect.

(Attachment Link)

Hmm how is the stripline via supposed to be? if you look at the datasheet of the connector, you see that the centre pin has ~0.5mm diameter, so the vial hole needs to be smaller than that. Or is it intended to be used with blind vias only?

I will try the VNA Tool. I have not used it for a long time so I am not too familiar with the time domain conversion.


In general, the stripline vias, should I make the hole smaller or larger?
I think I can go to 0.2mm but that's the smallest the technology allows.
And much largrer I cannot make it, cause the SMA connector centre pin needs to be larger than the hole, I think.

[Marsupilami]

I would assume that the via pad size should not be larger than the prescribed pad size for the connector.
The proper way to do this, which is economically impossible for hobby use, is to get an (often encrypted) full 3D simulation model for the connector and simulate it with the PCB launch as on the final stackup.

Your starting point could be to take your via and imagine it being a circular coaxial transmission line. (Coax cable) You can easily find a inner and outer conductor diameter ratio that gives you 50 Ohm impedance for the PCB dielectric you're using.

What makes this estimation not all that useful, especially for short/stubby vias, is that the impedance discontunities when transitioning from the connector to the board, or to the trace on the other side, or between layers in case you have mixed dielectrics will likely have a larger negative effect.

What you can do is play with the pad sizes, the antipad sizes and the trace launch geometry. If you can't do full 3D EM simulation on the structure you have to run on guesses and the TDR plot helps a lot with that.


This is the same via test I posted in the previous post but shown in impedance. You can see it starts with perfect 50Ohm, then I have a bit of wiggle; those are coax adapters. The first dip to 47.5Ohm is the connector launch to microstrip, then the dip at 400ps is a via transition to the other side of the board.
The magic is that this is purely done from the capture S-Parameters via an inverse FFT and some simple additional processing.
If you have a VNA with this functionality built in you can look at this plot real time and poke at the circuit to accurately locate features. Typically you take your tweezers and short the trace somewhere and see graph plummet to 0Ohm at that location. If you can only do this in post you can still take such measurements and save the s-parameters to later confirm accurate feature location.
To some extent you can also calculate. Take the velocity factor of your transmission lines then you can estimate spatial location from the travel time. The farther features are separated in space on your board the easier it will be to tell what belongs to what.

To get back to my plot, what that tells me is both my connector launch at 300ps and my via at 400ps are overly capacitive (Z0 < 50Ohm), while my termination at ~480ps is grossly off. That was supposed to be a 50Ohm terminator but it might have a soldering defect or alike.
Let's ignore the termination for now.
Time gating comes in handy to see what to fix. See the image from my last post. You can mask out sections of your time domain response and see what the frequency domain would look like in that case. (Black traces are as is, red is the hypothetical).

If you confirmed that a particular section is influencing your overall response significantly you can try to compensate in the other direction. In my case both the connector launch and the via is overly capacitive. This means there is too much ground copper too close. I can try to make it more inductive by reducing trace width, reducing via diameter, increasing via antipad diameter or increasing coplanar wavegude ground gap, etc. (closer ground -> better capacitor -> lower Z0; wider trace -> bigger capacitor -> lower Z0; etc.)

It's a lot of guesswork even if you are able to simulate it, but some amount of improvement is certainly possible by iteration.

All that being said, your plots are not bad. In many real world cases I would take these results and be happy, but yes, probably it can be improved.

[tszaboo]

So I made a python script that uses SKRF to create a connector model based on measurements and simulations.
The same connector should be soldered on a transmission line, and measured with a VNA, saving S2P ('full_system.s2p').
Then the PCB should be simulated and similarly an S2P file ('ms.s2p' it was a microstrip line for me) created for it.
The script will deembed the PCB and create a model for the connector. Then it will plot some data for visual verification.
I used it to make a model for my ~20 cent connectors with my footprint which seem to follow the measurements. I verified it on another PCB. Now I have a way to compare these.

https://gist.github.com/tszaboo/5c0ba6e8b99e93e384de68f6db674f38

It's somewhat wibe coded with grok.

Code: [Select]

import skrf as rf
import numpy as np
from scipy.linalg import sqrtm
import matplotlib.pyplot as plt

# Load measured S2P file (two SMA connectors + PCB)
full_system = rf.Network('full_system.s2p')

# Load simulated PCB S2P file from QucsStudio
pcb = rf.Network('ms.s2p')

# Get frequency from full_system.s2p
freq = full_system.frequency

# Interpolate pcb.s2p to match full_system.s2p frequency grid
if pcb.frequency != full_system.frequency:
    print("Interpolating ms.s2p to match full_system.s2p frequency grid...")
    pcb = pcb.interpolate(freq)  # Align pcb to full_system frequency

# Verify shapes
print(f"Full system S-parameters shape: {full_system.s.shape}")
print(f"PCB S-parameters shape: {pcb.s.shape}")
print(f"Adapter S-parameters shape: {adapter.s.shape}")

# De-embed the and PCB using SKRF's inv
pcb_inv = pcb.inv          # Inverse of PCB network

# De-embed: Full system = SMA1 + PCB + SMA2
sma_both = full_system ** pcb_inv

# Extract single SMA using matrix square root on T-parameters
sma_both_t = sma_both.t  # Shape: (n_freq, 2, 2)
n_freq = len(freq.f)
sma_single_t = np.zeros((n_freq, 2, 2), dtype=complex)
for i in range(n_freq):
    sma_single_t[i] = sqrtm(sma_both_t[i])  # Compute square root of T-matrix
sma_single_s = rf.t2s(sma_single_t)  # Convert to S-parameters
sma_single = rf.Network(frequency=freq, s=sma_single_s, z0=50)

# Save the de-embedded SMA S-parameters
sma_single.write_touchstone('sma_connector.s2p')

# Plot S12 of the SMA connector in dB using SKRF's built-in method (separate figure)
plt.figure()  # Create new figure for S12
sma_single.plot_s_db(m=1, n=0, label='S12 (dB) SMA')  # SKRF plot for S12
full_system.plot_s_db(m=1, n=0, label='S12 (dB) System')  # SKRF plot for S12

# Plot VSWR for both ports using SKRF's built-in method (separate figure)
plt.figure()  # Create new figure for VSWR
sma_single.plot_s_vswr(m=0, n=0, label='VSWR Port 1')  # VSWR from S11

# Show both plots
plt.show()

print("\nS2P file generated: sma_connector.s2p")

# Print S12 values in SKRF style (frequency in GHz, S12 in dB)
print("\nS12 of SMA Connector:")
for f, s12 in zip(sma_single.frequency.f / 1e9, sma_single.s_db[:, 1, 0]):
    print(f"Freq: {f:.3f} GHz, S12: {s12:.3f} dB")
   
    cascaded = sma_single ** pcb ** sma_single

# Verify shapes
print(f"Full system S-parameters shape: {full_system.s.shape}")
print(f"Cascaded system S-parameters shape: {cascaded.s.shape}")

# Compute maximum S12 difference
s12_diff_db = np.abs(full_system.s_db[:, 1, 0] - cascaded.s_db[:, 1, 0])
max_s12_diff = np.max(s12_diff_db)
print(f"Maximum S12 difference: {max_s12_diff:.3f} dB")

# Plot S12 of full_system and cascaded system (separate figure)
plt.figure()
full_system.plot_s_db(m=1, n=0, label='Full System S12 (dB)')
cascaded.plot_s_db(m=1, n=0, label='Cascaded S12 (dB)')
plt.title('S12 Comparison')


[Roland_W]

Regarding the 23 GHz transition modeling, footprint design, and panel-mount option, here are a few valuable resources that address simulation models and launch tuning:

1. **Multilayer SMA to Microstrip HFSS Simulation:**
   There is an open-source 3D EM model/simulation repository available on GitHub for analyzing SMA transitions on multilayer boards:
   https://github.com/toammann/Multilayer_SMA2Microstrip
   This serves as a solid baseline for simulating S{11} return loss and optimizing launch footprints in HFSS.

2. **Würth Elektronik 3D / HFSS Models for Panel Flange Connectors:**
   Würth provides official 3D EM models (including HFSS format) for their 2-hole and 4-hole WR-SMA flange panel jacks:
   https://www.we-online.com/en/components/products/COAX_SMA_CONNECTOR_PANEL_2-HOLE_AND_4-HOLE_FLANGE#/articles/WR_SMA_PANEL_2-HOLE_AND_4-HOLE_FLANGE_STRAIGHT_JACK
   These models allow you to directly import the connector geometry into your EM solver alongside the milled enclosure geometry to check pin reach, wall tolerance, and cavity resonances.

3. **Transition Tuning & Reflection Minimization (SV Microwave App Note):**
   For optimizing solderless/edge-launch transitions to minimize discontinuity reflections and achieve a smooth S{11} response up to millimeter-wave frequencies, SV Microwave published a detailed application note:
   https://www.svmicrowave.com/images/uploaded/Solderless%20PCB%20Connectors%20Application%20Note.pdf
   It covers tapering techniques, co-planar ground relief, and ground-via placement to optimize transition impedance matching.