I am currently finishing the design of a board where there are two antenna microstrip on the surface of the top layer. I have a 4 layer PCB. I use FR4,so I suppose dielectric is 4.6. Thickness of the board is programmed to be 1.6mm, with the following stack

enter image description here One is for GPS function and another one is for GSM function.

The manufacturer of the modules specify that control corresponding W and S of 50ohm coplanar waveguide. How do I calculate Track width (W), separation to coplanar ground (S) ? I have saturn pcb software but I don't know if I can achieve this calculation with it ?

When answering, I would really appreciate if you can detailed by a simple 1-2-3 step process, how you process to perform the necessary calculation to determinate those parameters.

  • 1
    \$\begingroup\$ As long as you type the right parameter values, saturn gives the correct result with (1%) tolerance. I use both AWR TX Line and saturn. They are fine. Characteristic impedance calculation can be found on internet: chemandy.com/calculators/… \$\endgroup\$
    – Alper91
    Jun 15, 2016 at 8:19
  • \$\begingroup\$ Altium has an Impedance-Controlled Routing feature, have a look on it. \$\endgroup\$ Jun 15, 2016 at 8:39
  • 1
    \$\begingroup\$ Most flavours of FR4 have a dielectric constant that varies with frequency (3.9 to 4.3 on one variant I use across the range 5G to 100M); some are more tightly controlled than others, so check with your vendor for the specific type of PCB material. \$\endgroup\$ Jun 20, 2016 at 10:10

1 Answer 1


I can recommend MTTL (sourceforge page) which could handle this task. It is a 2D field solver and therefore can cope with many non-standard geometries where the simple empirical calculators cannot deliver an answer. As far as I remember it should give you all parameters required for a CPWG. You could simply play with the parameters until you get the desired impedances. Of course you can use the results of simple empiric calculators as a starting point.

There are also many RF packages out there which could give you the same answers (with a polished interface), but they tend to charge you a lot for them.

Edit: Here is a step by step guide for MTTL (TNT):

  1. choose your unit system (top right), e.g. microns
  2. add a ground plane (New Ground Plane button) and specify the parameters (e.g. 35µm)
  3. add a dielectric (usually FR4, but use whatever you plan to use for your PCB) e.g. 1500µm FR404
  4. add your signal layer ground structure by first adding rectangle GND conductors (button New Rectangle Conductors) e.g. enter as
    • Name GroundSignal,
    • Conductivity: Copper,
    • height: 35µm,
    • width 10000µm,
    • number:2
    • Pitch 15500µm.
  5. add your signal conductor: add rectangle conductor with values

    • Name:Signal,
    • Conductivity:Copper,
    • height: 35µm,
    • width: 1500µm,
    • x offset: 11500µm = 10mm + (5.5mm - 2.5mm)/2 = (left gnd width + (gnd pitch - signal width)/2)
  6. Save your file.

  7. Run the simulation: BEM> Run> Run
  8. Click show results: Find the line

    Characteristic Impedance (Ohms): For Signal Line ::SignalR2= 53.0741

  9. From there adjust the values until you get the desired results.

The results closely match those of the simple calculators (as mentioned by Alper91), but you will be able to also account for special cases not covered by them (e.g. slight asymmetries).


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.