Impedance calculation for microstrip in middle layer of multi-layer board? - Page 1
Forum section: electronics / rf-microwave

author: wb0gaz
author_rank: Frequent Contributor
timestamp: November 06, 2019, 01:29:10 pm
content: I have designed and built out my first 4-layer board, which includes a few (intended) 50-ohm microstrips in the second-from-the-top layer (ground layers above and below.) From initial testing, the impedance of the microstrip lines may be off (higher than expected insertion loss and roll-off at higher frequencies.) I used an online microstrip calculator to set the with (based on dielectric constant, width/thickness of the strip, and distance to the ground plane), however, I am concerned because I didn't do anything to accommodate the second ground plane (farther away as the thickness of the board material below the microstrip is greater than the thickness of the board material above it.) I also didn't find any calculations to set the (minimum?) horizontal clearance around the microstrip (I picked 0.5mm arbitrarily, but I'd prefer to know if this should be set to some minimum distance.)What is this structure called (microstrip sandwiched between ground planes above and below), and where could I find an online (preferably) calculator (or failing that, the design formulae) for setting the width and (if possible) horizontal clearances?Thanks!

author: Howardlong
author_rank: Super Contributor
timestamp: November 06, 2019, 01:31:05 pm
content: Stripline.

author: ejeffrey
author_rank: Super Contributor
timestamp: November 06, 2019, 05:49:01 pm
content: Specifically asymmetric stripline. Some stripline calculators only handle the symmetric case where the ground planes are equidistant.To ballpark clearance rules for stripline, start with 3-5x the distance to the ground plane.For a more accurate answer look at design calculators for edge coupled striplines. Then you can estimate the actual coupling between adjacent traces for your chosen geometry and compare to your isolation spec.When using stripline you need via fences to tie the top and bottom ground plane together. Otherwise you have very bad crosstalk as the trace will be able to launch waveguide modes across the PCB. I was recently working with a design that looked fine, but there was one small area with inadequate via fencing and unfortunately was right near a connector so there was an impedance discontinuity. That degraded the channel to channel isolation from -60 dB to -15 dB.

author: wb0gaz
author_rank: Frequent Contributor
timestamp: November 07, 2019, 02:47:39 am
content: ejeffery, thank you for much new/useful information - good learning opportunity!Knowing that it's called "asymmetric stripline" was enough to point me to several online calculators, which is exactly what I was looking for (and the drawings there look exactly like the element I'm working on.) I'd not likely have stumbled onto this on my own - thanks!None of the 3 calculators I found in a quick search mention side clearance (between the stripline and the via fence), but the 3x-5x rule-of-thumb gives me a starting point (as there are two ground planes involved with differing distances, I'm thinking base it on the farther of the two ground plane distances, which sounds off the top of my head in the range of what I've already got in place.)As for via fences, I have that in place --- the longest distance between any two adjacent vias is just under 2mm. The application is indeed isolation-intensive (an RF SPDT switch with a need for high port isolation.)Thanks again for the detailed reply - this is certainly enough to get me off to a good (re)start!Dave

author: jhenderson0107
author_rank: Regular Contributor
timestamp: November 09, 2019, 01:37:13 am
content: Quote from: ejeffrey on November 06, 2019, 05:49:01 pmI am currently working on an RFSoC PCB layout in which, due to trace width constraints imposed by my customer, it is only possible to employ embedded microvias connected to just one of the two ground planes sandwiching the stripline along a straight trace segment about 15mm in length. Is the RF stitching seriously undermined if tied to only one of the two surrounding planes?

author: ejeffrey
author_rank: Super Contributor
timestamp: November 09, 2019, 07:27:54 pm
content: I don't understand what the vias are doing if they only connect to one plane. But short answer yes, multiple grounds planes not connected make a waveguide. Long answer is it depends.