50 Ohm Matching microstrip OSH park 4 layer process - Page 1
Forum section: electronics / projects

author: Spikee
author_rank: Frequent Contributor
timestamp: May 06, 2013, 09:28:43 pm
content: In my newest design i need to lay a 50 Ohm? matching microstrip from my gps module to a external antenna socket.But i have never done this before so i would like to know if the following calculations are correct.I am using OSH park new 4 layer stackup:Code:1 oz copper (1.4 mil)6.7 mil prepreg0.5 oz copper (0.7 mil)47 mil core0.5 oz copper (0.7 mil)6.7 mil prepreg1 oz copper (1.4 mil)We’ll also be switching to the high quality FR408 substrate. It has a dielectric constant of 3.66 at 1GHz.My layer stackup:Code:Signal 1groundvccSignal 2The application note about the transmission line: (page 31)http://www.trenz-electronic.de/fileadmin/docs/GlobalTop_Technology/application_notes/Gtop%20Module%20Application%20Note%20-A01%20_MT3339%20series_.pdfMy calculations using Txline 2003: (the line will be on signal 1 layer)Thanks,Spikee

author: nctnico
author_rank: Super Contributor
timestamp: May 06, 2013, 11:00:54 pm
content: Why not go for FR4? If the trace isn't long then it shouldn't matter. Besides that the layer of FR4 between the ground plane and signal plane is very thin so the effect of the FR4 is minimal. IIRC you'll get 0.33mm wide traces on FR4 with the same stack.

author: gxti
author_rank: Frequent Contributor
timestamp: May 06, 2013, 11:33:52 pm
content: You don't get a choice at checkout, all 4 layer orders are FR408 now. But that's a good thing because it's better controlled than FR4.The calculations look fine, although you have "Gold" selected as a conductor. Not sure if that affects impedance calculations, or just loss. The shorter the trace the better, of course. Other layout considerations: make the clearance to the ground fill at least the same width as the trace, ideally 1.5-2x. Use via stitching (but don't go overboard), and make sure the ground plane underneath is totally unbroken. Use curved traces if you can.If you are using external components to supply antenna power, the inductor should be directly on the antenna trace with no "stub". It looks like the module you're using supports supplying power through the module though, so I'm guessing you're using that.

author: Spikee
author_rank: Frequent Contributor
timestamp: May 07, 2013, 08:41:52 am
content: I did the calculation again whit copper conductor instead of gold (because it is copper gold plated) and the values changed a little.Quote from: gxti on May 06, 2013, 11:33:52 pmSo the distance between the ground plane and the trace will be 1.5-2x the width of the conductor on either side.And the via stitching will be every 0.5 inch ? at the edge of the top ground plane to the middle ground plane (layer 2).thanks

author: jahonen
author_rank: Super Contributor
timestamp: May 07, 2013, 09:01:54 am
content: Don't worry about it too much. As long you have return loss of about 20 dB, it is good enough for most purposes (unless you are building a VNA!). Also, there are variables you can't control but will effect your impedance, like tolerances in etching and dielectric thicknesses along with exact composition of the dielectric (but of course it is still useful to try to center on zero error). TXline does not calculate the effect of solder mask but it is usually quite small, few ohms at best.To put in perspective what that 20 dB return loss means in terms of impedance, it means that absolute value of reflection coefficient is less than 0.1. We can thus calculate respective impedances assuming other end is perfect (which it is not). It turns out that whenever your impedance is between 41 and 61 ohms, the above criteria of having reflection coefficient less than 0.1 (or return loss less than 20 dB) is met.Regards,Janne

author: KJDS
author_rank: Super Contributor
timestamp: May 07, 2013, 01:24:50 pm
content: There's no reason why it shouldn't work.In general, I'd far rather a thicker dielectric for general microstrip applications as this will give a wider line with lower conductor losses. It also means that etching tolerances have less effect on a wider line.Remove as much solder resist from the top of the line as you can to also benefit loss. If you've got ground plane at the sides, stitching vias should be at most 0.1 wavelengths apart and more usually every 0.1" Keep the ground plane at least 0.8 * line width, and preferably a whole line width away from the line. Either use an optimal miter on bends or use a curve.