MICRO STRIP TRANSMISSION LINE REVERSE LOSS

[rgarnett1923]

Hi All

I got a reply from Seeed and it seems they have changed their stackup for four layer boards, but they didn't change the specs on the website:  their stackup is now

Top Copper (1oz)
0.12mm Prepreg
Second Copper layer (0.5oz)
1.2mm Core
Third Copper layer (0.5oz)
0.12mm Prepreg
Bottom Copper (1oz)

This explains my problem as I worked on 0.2 mm.  I am sadder, but wiser now. But at least my method was sound. I'm also glad I made the test board.  If I had gone ahead with the radar board and mounted all the bits I would have been in for a big disappointment. My prepreg measurement was pretty close too so the money I spent on the microscope camera is justified.

Seeed said that customers can specify a non-standard stack for an additional $170 or specify impedance control and their engineers will do the calcs and I guess size the tracks.

I suppose all this trouble is part of the rich tapestry of rf design. I knew there was some reason I took it on.

Thanks for all your help. 

Best regards

Rob

[xaxaxa]

seems everybody is moving to 0.1mm prepreg these days to support the high density digital shit; not long ago there was a debate on the JLCPCB forums about switching to 0.1mm (from 0.2mm) and people couldn't come to an agreement; RF engineers wanted 0.2mm (including me) and everyone else wanted 0.1mm. now JLCPCB offers both thicknesses (selectable from the UI).

[xaxaxa]

the rule with >2 layer boards is that if you require a specific stackup, you must inquire about it via email prior to ordering even if it's listed on the website (unless the web UI specifically lets you select from a list of stackups)

[in3otd]

This explains my problem as I worked on 0.2 mm

IMHO not completely. If the mismatch seen in S11 came only from the wrong line impedance it should not rise with frequency and peak close to 0 dB as in your graphs; S11 should oscillate around the return loss corresponding to the actual line impedance (see first graph below).
OTOH, if you (also) had discontinuities at the line ends you will see S11 rising with frequency, as the reflection near the connector will become bigger and not be (much) attenuated with frequency (see second graph below).

[rgarnett1923]

Hi All

Just an update,

I got a test board made up at OSH Park with the correct 0.2 prepreg.  The results were better, but still not acceptable.

I then realised  I had done a silly thing.  I had extended the 0.2mm ground plane under the SMA connector center pin pad.  This area yields about 0.9 pf.  A capacitance this size at 3 GHz will certainly bring the impedance way down and be highly reactive.  I modeled the layout with and without the pads and voila, correct answer.  With the pads, I get a virtually identical S11 response as the OSH Park board. Without the pads, I get the impedance you would expect from the theory.

I modified the board design with keep-outs under the SMA center pin pad.

I am 99% certain that will fix it.

Just an aside I soldered two of the SMA connectors back-to-back and got a very good response.

What a knucklehead!!

That was God punishing me for not using the brain.

[rgarnett1923]

Hi All

The problem was I continued the ground plane under the SMA center pin pad which gives a capacitance of about 1 pf at bot ends of the TLine on my test board.

I have put some keep-outs for the copper pour around the center pin.

I am 99% sure this is the problem and the keep-outs will be the fix.

I have attached the plots for the OSH Park board with the 0.2 mm prepreg with no keep-outs. Better than the other board, but pretty horrible.

I also tested a couple of the SMA connectors back to back (no pc board) and found they have a very good response.  I have attached this.