Bad Reflection from SMA Board Connector at 4-8 GHz

Question

recently I have tried to design a simple SMA-to-microstrip connector PCB intended for 4-8 GHz. The connectors used are vertical with surface-mounted centerpin (link).

The design idea was to simulate the connector and the transition to the microstrip on the board in CST Microwave Studio and match the transition by finding the best size of a cutout in the groundplane below the point where the center pin meets the microstrip, see pictures (click for higher resolution).

Within the simulation this approach works well, a solution with S11 < -25dB from 4-8 GHz is easily found.

Single connector:

Full board (connector - microstrip - connector) sims with acceptable S11 around -20dB:

So I had a prototype manufactured on 200um FR4 dielectric, the thought being that the S21 losses would be large, but evaluation of the S11 performance should give an idea of how well the design works out in reality.

Sadly the measured reflection is horrible, around -13dB at the worst point:

My questions are now:

• Can I expect a better agreement of simulation and the manufactured board by using a proper HF material instead of FR4?
• Did I do some rookie mistake somewhere?
• Or is this high reflection just unavoidable with these type of right angle connectors? Its surprisingly hard to find any reliable data on this.

Answer 1

In order:

a) Yes.

b) No. A classic would be not realizing how bad FR4 is at 8 GHz, but you've covered that.

c) Yes. Angles of any kind are bad at these frequencies, and while 90's are not the worst, they are a contender.

Note that the microstrip structure is a compromise, and always will perform more worse (?) that a simulation, compared to the Sim/IRW difference of a full stripline design.

Answer 2

FR4 is a bit tricky as you can get different grades of FR4 with very varying RF performance (unfortunately FR4 was originally never meant for RF). FR4 can work higher than most people would think. The normal limit is around 3GHz but I have had circuits working up to about 14GHz albeit with a lot of loss. After 15GHz you start to see sudden dips which makes it unusable but even this depends on the type of FR4. Some will fall over earlier than others.

My advice for measuring connector loss is to first make a few microstrip lines with identical Port1 Port2 connectors. S11 measurements alone have little value as you don't know how much is reflection and how much is loss. The normal method of characterizing connectors is to build two or three lines of different length. Using these you can work out (with S11 and S21) how much is down to losses in the line and how much down to reflection in the connectors. If your VNA has a time domain function you can see this more easily. Even if not you can convert the Sparameter data (using something like Matlab) to time domain reflectometry data (TDR) to see which point along the line dominates the reflections and by how much. The TDR measurements in the Z domain with 50ohm normalization will tell you what you are doing wrong with your connectors. Connector to Line transitions can normally be modeled by an equivalent first order LC circuit. It is normally the case that you either have too much of one quantity (C or L) required for a 50ohm transition. Knowing which one to add (or subtract) you can tailor your transition region appropriately. For example needing more capacitance (hence less inductance) means adding a fatter line region near the connector then tapering this down to 50ohm. Remember you are still less than 1/16th wavelength in the connector region so your fat piece of line will appear almost as a lumped element. You may need to tweak your frequency range for TDR measurements until it shows something sensible and you should see a similar trend with the CST simulations.

Second point is about thickness. The higher frequency you go to the thinner the substrate should be to minimize losses (looks like you are doing this already with 0.2mm).

Third is to follow the land pattern that normally comes with the connector datasheet. I mostly favor edge mount types as these also work for Duroid at higher frequencies. However if your application requires a top mount connector then I suppose this isn't an option.

Hope that helps. Good luck!

Answer 3

You sound like you are measuring the superimposed reflections from two transitions.

Now if both transitions are identical, and if there was negligible loss between them, you may expect those two reflections to cancel at some frequencies, and be 6dB (double voltage) relative to either one at the worst. So you may expect your predicted 25dB to be 19dB on the crests, even if the model was perfect. But it sounds like you are 6dB higher still. So a single connector may be as bad as -19dB return loss.

Does the ripple period correspond to the spacing between the connectors, and a round trip time corrected for effective dielectric constant? If not, this is not the mechanism causing the ripple.

You do not need such a great extra inductance in series or capacitance in shunt to achieve a noticeable extra S11, nor a huge error in the PCB thickness or material composition. It may be useful for you to spend a few minutes estimating those quantities, to see if you are within credible manufacturing variation.