# PCB microstrip width calculator

I am trying to make a PCB that works as a 433mhz amp and filter. However I am having trouble calculating trace widths. I am planning to use an FR4 board. I assume I need to have my signal paths matched to 50$\Omega$?

I was using the following calculator to try and calculate what the thickness needs to be and got a result of approx 1.9mm, this seems very large?

I used the following parameters:

$\epsilon$r = 4.35

Substrate Height = 1mm

Trace Thickness = 35$\mu$m

Frequency = 433.75MHz

Have I made any obvious mistakes or is this actually correct? I have checked on other calculators and obtained the same results.

Many Thanks

• The substrate height you set is 1mm, Why did you pick this value? How many layers is your PCB ? – Abdella Nov 23 '15 at 11:42
• I get 1.8 mm width with the calculator I use (part of the Pulsonix PCB package). Your value seems about right. If the track length is less than 1/10 the wavelength the impedance doesn't really matter and you can use any width. Standard FR4 thickness is 1.6 mm giving 2.9 mm track width. – Leon Heller Nov 23 '15 at 11:52
• I chose 1mm because that is what the thickness of the current PCB I have is. Just shocked me because it would make the width of my tracks wider than some of the components being used. – Stuart Rayner Nov 23 '15 at 12:21
• Double layer PCB? – Abdella Nov 23 '15 at 12:55
• Yeah double layer – Stuart Rayner Nov 23 '15 at 13:22

## 3 Answers

If you want a thinner microstrip, you need to reduce the substrate height using one of the following solutions:

1. Use a thinner 2-layer PCB, for example 0.4mm PCB for a trace width of 0.74mm.

2. Use a 4-layer board so you can achieve h ~= 0.13mm (depends on manufacturer's specs) and you get a trace width of ~0.22mm.

The impedance of your transmission line depends on a wide variety of factors. The main value you want to match is determined by your drivers/receivers. A lot of single-ended drivers shoot for 50Ω but you MUST look at the datasheet for information.

Once you have your target impedance, you need to consider your PCB dimensions. The position of the signal trace with respect to its reference plane greatly affects the impedance, as does the thickness and type of dielectric. You really need to consider the PCB stackup. Rough estimates will not work here. Furthermore, if there are any other traces nearby they will also have an effect on the impedance, as well as their shape and physical size. In my experience all of those calculators out there designed for just one trace are practically useless as they don't take surrounding traces into effect, and the calculated impedance can be off by 10Ω or more just due to surrounding traces.

I was recently introduced to a very powerful tool called HyperLynx which I have found to be extremely useful. It is very expensive (\$18k USD) but there is a free trial that should help you out. I recommend the HyperLynx SI Virtual Lab for your project: https://www.mentor.com/pcb/product-eval/hyperlynx-si-virtual-lab

This software uses Maxwell's equations and a variety of other mathematical formulas to accurately calculate impedance. There is also a tool for checking the coupling between traces and for doing field analysis (to determine if crosstalk would be a problem or not). There is a bit of a learning curve but I highly recommend it. Here are a couple of screenshots:

Differential Impedance:

Single-ended Impedance:

Significant field collisions (bad design--will be too much crosstalk):

In short, do not put much faith in the single calculators you find online. They will often lead you astray, unless you only have one trace on your board, or surrounding traces are a centimeter away.

• If nearby traces are disturbing your microstrip line's impedance, they are also generating and being impacted by cross-talk. Much better to keep other traces at least 5 trace-widths away from your microstrip than to try to adjust the microstrip to achieve matching with the trace too close. – The Photon Nov 23 '15 at 16:36
• @ThePhoton Precisely. However, it's a trade-off as the further away you place traces, the more PCB real estate it takes up and it reduces the density of the board (which in most cases is not desirable). Ideally you'll want to place the traces as close together as possible without causing excessive crosstalk. Finding that sweetspot, however, is very difficult, and the software suggested helps with that. – DerStrom8 Nov 23 '15 at 16:39
• It's certainly a different problem if you're designing a DDR3 interface from feeding a single antenna. – The Photon Nov 23 '15 at 16:51

Polar Instruments Si8000m and Si9000e are widely used in industry to calculate transmission line parameters. Beyond just the usual w, h, and t parameters, Polar will account for etch profile and soldermask overlay effects, for example, to calculate characteristic impedance more accurately than a tool that only considers rectangular geometries and one dielectric layer.

If you aren't able to buy a license for it yourself, but you are using a full-service board fab, your fab may be able to use it to generate trace geometries for you, if you give them your stackup.

Even if you don't use Polar, if you specify impedance control in your fab notes, your board shop is likely to use it (or a similar tool) to adjust your design to achieve the impedance you specified.

For quick and dirty calculations, I have recently been using CGI-Wcalc. Results tend to be within a few per cent of Polar, which is often good enough for the board shop to be able to adjust things to achieve a very good impedance match.

As the comments have said, if your concern is that a 1.9-mm-wide trace is taking up too much real estate, the best solution is probably to use a multilayer board so that you can have a dielectric height on the order of .25 mm (or even thinner if your design requires really high density), and a trace width less than 0.5 mm.