PCB layout at high frequency

J

Jamie Morken

Guest
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
 
"Jamie Morken" <jmorken@shaw.ca> wrote in message
news:gayke.1463208$6l.1296816@pd7tw2no...
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! :)
Click to expand...

0.2" is small compared to the wavelength, so it won't matter.

Leon
--
Leon Heller, G1HSM
http://www.geocities.com/leon_heller
 
Jamie Morken wrote:
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
Click to expand...
How long is the trace on the other side of the cap?

Mike Monett
 
PeteS wrote:
The track width and the distance to the ground plane together set the
impedance for microstrip [...]

0603 caps have significant parasitics. 0402 are much better (0201 is
even better)
Click to expand...
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
 
"PeteS" <ps@fleetwoodmobile.com> wrote in message
news:1116931031.559228.7670@g43g2000cwa.googlegroups.com...
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)
Click to expand...
01005 would be better still. :cool:

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

Leon
 
On Tue, 24 May 2005 16:11:06 +0100, "Leon Heller" <leon.heller@dsl.pipex.com>
wrote:

"PeteS" <ps@fleetwoodmobile.com> wrote in message
news:1116931031.559228.7670@g43g2000cwa.googlegroups.com...
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)

01005 would be better still. :cool:

I saw some on a board at the NEPCON show a couple of weeks ago.
Click to expand...
Good to see your eyesight is doing so well ;-)
 
Jamie Morken wrote:

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! :)
Click to expand...
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

--
Ing.Buero R.Tschaggelar - http://www.ibrtses.com
& commercial newsgroups - http://www.talkto.net
 
budgie wrote:
On Tue, 24 May 2005 16:11:06 +0100, "Leon Heller" <leon.heller@dsl.pipex.com
wrote:


"PeteS" <ps@fleetwoodmobile.com> wrote in message
news:1116931031.559228.7670@g43g2000cwa.googlegroups.com...

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)

01005 would be better still. :cool:

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


Good to see your eyesight is doing so well ;-)
Click to expand...
snap

Cheers
Terry
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top