# Differential impedance calculation - which way to go width vs spacing?

In USB2.0 specification, there is a requirement of desigining its data traces to be around 90Ohms +/- 15%.

Using this calculator, based on my earlier question I'll need to make sure to approach 90Ohms with the "Impedance (differential)".

To reach 90Ohms, there are 2 ways (or there is another, please advise!):

1.) Increasing the trace width crazily:

Or

2.) Dramatically decrease the spacing in between differential pairs:

I know:

• This calculator is not exact and precise
• Answer can depend on actual goals

I wish to know in general, is it better practice to increase the data trace widths or decrease the spacing, or 3rd option? (putting "something" in between d+ / d- traces?)

Those two are not the only options. They are the only two options if you have already chosen a PCB structure and material with height between copper planes and dielectric constant Er you can't change, and then that's the problem.

The formulas used by calculators are not valid for any arbitrary parameters, usually the ratio between W and S or maybe even their ratio between H is limited to certain range to give out meaningful results. Which means, the calculators may allow you to input any values, but it does not warn you if the values exceed sensible input range and you get a result you can't trust.

If it is hard to achieve sensible track widths with the H you have, then it means the choice of PCB structure is poor.

The real way to make differential pairs with controlled impedance is to have more than 2 layer PCB which allows you to select a suitable distance H between data wires and ground plane to have sensible track width and spacing, so that tolerances in any of them won't change the impedance too much.

So in general case, you likely need to go to 4 layer board, with a suitable layer structure that allows impedance control.

Even if you calculate and draw the track width and spacing properly to your design, you might not get it properly manufactured due to PCB fab house not knowing what limitations there are to select the PCB material and structure of stack up they happen to have in use. That's why you need to define them when ordering PCBs, sometimes you don't care and sometimes you care how they will manufacture it.

If you give the PCB house instructions that you need impedance control on your USB tracks, then they can fine tune the track width and spacing of impedance controlled lines according to their experience how it will end up in the final PCB, given the properties of PCB material and layer structure. They can also give you feedback if they can't manufacture your PCB with the impedances you request and so they can suggest what to change to make it possible.

So what you must decide, do you really want to pay for that if doing a simple one-off hobbyist product for yourself where the USB traces between connector and MCU are few centimeters and running only at 12 MBps, or should you do it properly if you have a commercial product with long PCB traces running at 480 Mbps.

• Comprehensive description! One suggestion for additional info to last part: as a rule-of-thumb, which trace length can be safe for using without complex impedance matching, but using these "cheap" calculators? I.e. below wavelength / 10? Commented May 14, 2023 at 10:44
• @Daniel Thank you! I am not so sure how to answer that, because these calculators with the help of PCB house can achieve extremely precise impedaces, and the rule of thumb is that for very short trace lengths (like wavelength/10) impedance matching can be simply ignored so you don't need matching. The problem is defining what "electrically short enough" means, as it depends not strictly on wave length, but signal slew rate, i.e. how fast edges are, and how much impedance mismatch and reflections are allowed. Keep in mind also connector wiring and pads are mismatches before the PCB wiring. Commented May 14, 2023 at 11:28