Microstrip, Stripline, Coplanar Waveguide guide - Page 1
Forum section: electronics / general

author: logictom
author_rank: Unknown
timestamp: June 11, 2013, 11:25:53 am
content: I am designing a board with a 50ohm impedance antenna track and I'm having a little difficulty with the terminology.Am I trying to use AppCAD to confirm my track impedance but I'm not sure which calculator to use as it offers Microstrip, Stripline and Colplanar Waveguide.Is there an idiots guide to what setup is classed as what?Am I right in thinking Stripline is a track on an internal layer with planes above and below?Is a Microstrip a track above a plane with nothing to the sides and a Coplanar Waveguide a track with a plane below and to the sides?My board setup is four layers, signal track on the top layer, ground, power then signal below. I have, where possible, ground either side on the top layer. Is this classed as Coplanar or Microstrip?I am using Altium and it has calculated a track width of 0.866mm, however if I put this into either Coplanar or Microstrip in AppCAD I get ~25ohmsIs this due to it only using two layers? Does this matter?Not sure what's right or wrong here

author: KJDS
author_rank: Super Contributor
timestamp: June 11, 2013, 11:47:18 am
content: If the spacing between the line edge and the adjacent ground plane is more than about 0.8W, where W is the line width, then there's very little difference between microstrip and coplaner. If you have the microstrip on the top layer and ground plane beneath it then that layer thickness is what needs putting into the calculators. Make sure the dielectric constant is correct. It may be that Altium is missing one of these bits of info.

author: Rufus
author_rank: Super Contributor
timestamp: June 11, 2013, 11:53:43 am
content: Quote from: logictom on June 11, 2013, 11:25:53 amThe calculators usually have a drawing showing the dimensions you need to enter. If it is asking for dimensions you don't have you chose the wrong one.On 1.6mm FR4 a 50 ohm track against a plane on the other side of the board needs to be about 4mm wide.

author: KJDS
author_rank: Super Contributor
timestamp: June 11, 2013, 12:24:01 pm
content: I've just had a play with appcad for the first time in many years.The easy thing to miss is T, the metal thickness. Accidently left that at its default setting of 2.1, which is fine if it's thou, but not as mil.Once i'd put that right, it came up with a sensible 2.85m giving 50.7ohm on microstrip and 50.2ohms on coplanar where the ground was 2mm away, all on 1.6mm FR4

author: logictom
author_rank: Unknown
timestamp: June 11, 2013, 02:23:57 pm
content: Thanks for the feedback.I have added two images to show what I have setup in Altium and also in AppCAD.Altium has a design rule that the trace has to be 50ohm.Am I doing something daft in AppCAD?

author: KJDS
author_rank: Super Contributor
timestamp: June 11, 2013, 02:51:36 pm
content: your Altium core and prepreg, distance between the top copper and ground plane is 0.58mm. Putting that into Appcad but leaving everything else as it is gives 47ohm, which could be close enough to explain what's happening.

author: logictom
author_rank: Unknown
timestamp: June 13, 2013, 10:57:23 am
content: Thanks KJDS, real face palm moment there