Electrical – How to decide and calculate parameters for track on differential pair

The calculation looks correct, but the tracks are too wide.

For example, a single 0.75 mm track on a 0.36 mm substrate, has an impedance to ground, unbalanced, of about 49 ohms. Thus a "differential pair" any long distance apart will have an impedance of 98 ohms, without any coupling between the lines, i.e. infinite mutual impedance. It only takes a tiny bit of mutual impedance to bring the differential impedance down to 90, which is why your package puts them so far apart.

Hence the warning about spacing/height. You don't really have a differential pair, you have two single-ended lines, which as you say isn't ideal for rejection of coupled interference, or reduction of radiation.

A differential pair should have a significant mutual impedance, at least similar to or smaller than the impedance of each line to ground.

Keeping the final differential impedance constant, you can make each track narrower, raising its impedance to ground, and move them closer together, lowering their mutual impedance. This makes it more like a differential pair, less like two separate lines.

On this thin substrate you need to make the traces a lot narrower, so they can be closer together, so the mutual capacitance dominates the ground capacitance. Try 0.25 mm if your tracks can be this narrow, and see how far apart they need to be to get 90 ohms.

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).