Re: PCB layout at high frequency

Although the trace is short compared to the wavelength of the signal (about 62.5mm on FR4) and short compared with 1/4 wavelength, if it's not a controlled track, there will be some radiation and loss (because you'll have a point impedance mismatch).

If you are not worried about losing some signal, then Leon's comment is the way to go. If it's in a piece of commercial equipment for which you need radiation certifications, it might matter.

The track width and the distance to the ground plane together set the impedance for microstrip (amongst other things, including the dielectric constant of the board).

Assuming this is a single sided board (or single plus ground plane), you are rather limited in your options, though.

A couple of additional comments should you need to do impedance controls on signals at this frequency:

1. 0603 caps have significant parasitics. 0402 are much better (0201 is even better)
2. Commercial fabrication houses can give guidance for track width. Even if you calculate it (I have a perl script at home that does such things), I ask them to calc it, because I am going to hold them to it.

Cheers

PeteS

Hi,

I have a 2.4GHz RF signal (ISM radio) going through an 0603 package capacitor and then a vertical mount SMA connector. I am making the trace as short as possible, but it will be about 0.2" long from the 0603 pad to the SMA pin. For this length of trace is it important to size the width of the trace or will any tracewidth do? For microstrips I read that the signal trace should be approximately 0.1" wide for standard FR4 boards, but I don't have room for that wide of a trace. There is a groundplane on the bottom of the board and the 2.4GHz signal is on the top of the board. Any common sense guidelines for this would be appreciated! :)

cheers, Jamie

My experience is that if the cap width matches that of the microstrip, the parasitics of the cap are negligible.

Sure, a bigger cap has a bigger inductance, but so does the section of microstrip it replaces.

Jeroen Belleman

Leon

I saw some on a board at the NEPCON show a couple of weeks ago.

Leon

Good to see your eyesight is doing so well ;-)

You only need 100mil for 50 Ohms when the the GND is at the other side only. When there is some GND on the same layer, it can be made narrower. This is called coplanar waveguide and is calculated in HP's Appcad, a recommended free package. EG a 30 mil track with a 5mil gap has 51 Ohms on a 1.5mm FR4

Rene

snap

Cheers Terry