I am a bit lost about how to establish the parameters to establish differential pair routing. I am currently trying to route several differential pair and I am a bit new to this. I have searched online some tutorial but I don't find any really explaining easily and out of the theory with simple succession of steps about how to do it

I have downloaded saturn PCB software to see if it can help but I don't understand well how the soft is working because what it ask me to input is typically what I am searching for (it looks it is reverted... !!!)

Assuming the differential pair I am routing is requiring 90 ohm (this is what the hardware guideline say "Route the USB differential pair on the top layer with a trace width and differential spacing tuned to the PCB stack-up for 90Ω differential impedance ").

So in Saturn PCB I have indicated in target zdiff : 90 Conductor spacing: I don't know (Am I supposed to arbitrary settle this, then accomodate the other parameters ?) Conductor width: same Conductor height: this I suppose I need to check my layer stack up. In this case I suppose I have to decide the spacing between top track and ??? first prepreg or core ?

I would really appreciate if someone who have experience could explain their methodology via a "1./ 2./ 3./ 4./ points methodology" to be able to achieve any differential pair routing.


1 Answer 1


From the text, this appears to be a USB high speed interface.

The signal pair will have very little current, but you need to keep losses to a minimum.

The losses in high speed tracks are dominated by:

Skin Effect. This is because as signal transition rates become faster, the self-inductance of the conductor forms a high impedance in the centre of the conductor. A wider track reduces this loss (but it has diminishing returns above about 8 thou).

Dielectric absorption also causes losses. There is an excellent description of them here.

Another cause of losses is differential to common mode conversion, usually caused by a length mismatch between the pair.

The practical implementation of a controlled impedance pair depends whether you have a plane layer which is immediately below the signals; I will assume for now that you do and it is spaced 5 thou away from the signals (implies a 4 layer or higher PCB). The actual distance is determined by the various requirements of the PCB; a 5 thou core is commonly used (although many thicknesses exist).

I usually use 6 thou tracks for USB high speed (a decent trade-off for skin effect and PCB real estate); the gap between the pair can now be calculated by any number of tools.

For the geometry above, my calculations yield a trace separation of 4 thou using 1 ounce copper (commonly the finished thickness on outer layers).

If you do not have a plane layer, there are other techniques such as differential coplanar waveguide; just what technique I use is determined by the PCB geometries.

There is no one size fits all, but using a 5 thou to 6 thou track width as a starting point helps narrow things down.

  • \$\begingroup\$ Sorry to come back on this. On the calculation link you have indicated, can you please elaborate on the item you selected (is it "Differential Microstrip Impedance Calculator" ?), and then how you entered the values ? does H is the total thickness of the PCB or is it the distance between the top track and another layer (ground, power, bottom layer) ? I am on a 4 layer pcb with FR4 (which i suppose dielectric constant might be 4.6 or 4.4) \$\endgroup\$
    – chris
    Jun 15, 2016 at 6:04

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.