coplanar waveguide

[[email protected]]

Hi gang,
I'm trying to find out why people use CPWs on PCBs.
I'm looking into improving the rise-time performance of a PCB. It is
currently using microstrip on 6.6mils of Rogers 4450B, with a ground
plane right underneath.
We are launching a 50ps step and getting 150ps out at the other end.
The path is about 5 inches long, an 11 mils trace with a nominal
impedance of 50ohms.
The test report from the PCB shop shows we are within 5% of 50ohms.
This is measured, not calculated.
The 150ps figure comes from the lab. Our early simulations showed
there would be rise-time degradation, but not at this level.
So I'm trying to educate myself on CPWs, I'm reading Microwave
Engineering by Pozar.

But I'd like a pre-digested answer like: it makes no difference, it
helps in the high frequencies, your 11mil traces are too thin, etc...
TIA

 

[Bill Sloman]

Hi gang,
I'm trying to find out why people use CPWs on PCBs.
I'm looking into improving the rise-time performance of a PCB. It is
currently using microstrip on 6.6mils of Rogers 4450B, with a ground
plane right underneath.
We are launching a 50ps step and getting 150ps out at the other end.
The path is about 5 inches long, an 11 mils trace with a nominal
impedance of 50ohms.
The test report from the PCB shop shows we are within 5% of 50ohms.
This is measured, not calculated.
The 150ps figure comes from the lab. Our early simulations showed
there would be rise-time degradation, but not at this level.
So I'm trying to educate myself on CPWs, I'm reading Microwave
Engineering by Pozar.

But I'd like a pre-digested answer like: it makes no difference, it
helps in the high frequencies, your 11mil traces are too thin, etc...
TIA

For what it is worth, strip-line - a track routed over ground-plane -
is intrinsically dispersive. Microstrip - a track routed on an inner
layer between two ground planes - is not.

 

[[email protected]]

<[email protected]> schreef in bericht






For what it is worth, strip-line - a track routed over ground-plane -
is intrinsically dispersive. Microstrip - a track routed on an inner
layer between two ground planes - is not.

I think you have your terms backwards there. I use microstrip all the
time (a track routed over the groundplane , but exposed). You can
combine lumped elements to the circuits. All power transistors that I
have used are matched into microstrip circuits.

It is a legitimate , bonified, transmission line, like a coax or
strip line.

 

[[email protected]]

He's right that microstrip is dispersive, but that's not the major
risetime-loss contributor in the op's situation. On a given board
stackup, stripline is generally lossier... the trace will be skinnier,
the dielectric layers thinner, and any pcb dielectric is lossier than
air. Not to mention the vias.

John

Thanks, man. I figured as much on a gut level, but now I have to
figure out the why of the terrible loss.
Then maybe hit up some simulators.

 

[[email protected]]

x-no-archive

But I'd like a pre-digested answer like: it makes no difference, it
helps in the high frequencies, your 11mil traces are too thin, etc...
TIA

50ps corresponds to about 20 GHz.

Sweep your PWB out to 20 GHz and see how much it rolls off at 20 GHz.

This problem may be easier to understand in the frequency domain
instead of the time domain.

Figure out how to reduce losses at 20 GHz, the other posters already
gave some clues.

Mark

 

[[email protected]]

No mystery. The trace is too skinny.

John

Yes the initial simulation (which I now can't find to see who and with
what it was done) showed that.
We were going for 90ps out of the line, which was acceptable for the
application, and I needed the trace width because of
1) density
2) stackup (hands are tied)
.... but we now measure 150ps and I confirmed that to be sure. This is
bad. We are over spec...

So I'll be attacking the problem in a few ways
1) Find out about the adhesion, how is it done? foil type, etc
2) The formulas often used for impedance are empirical approximations
and never give attenuation/inch,
3) Again with the soldermask, I never got a good answer to the
question of removing it: does it change anything? Most of our fast
circuits expose the microstrip to be gold plated. All RF boards I've
seen (eval boards for the chips, etc use this approach as well, but it
looks like hard gold which is a problem in itself)
4) Stackup (thicknesses) can't change since it would be a major re-
spin, so I'm trying to see if re-arranging ground planes will allow
wider traces and not screw up the rest of the design
5) Run away screaming like a girl.

 

[[email protected]]

Rip up a trace (heat it with a soldering iron and peel) and look at
the underside.

Since there isn't much I can do about it, I've elected to email Rogers
and ask their opinion.

TXLINE does, but I don't know that I believe the numbers. And it's
still loss at frequency, which is not risetime.

I'll look into it. You always have the right free tool it seems.

That's the thing to do. Possibly slot out the plane on layer 2...
barely possible.

Yes that's what I'm looking at but it interferes with the transition
from the inner (short) microstrip.
So I'll have to look at the tradeoffs here.

Are you sure the lab's risetime measurement is accurate? I'm guessing
your 150 ps with that skinny trace is real, but you never know. How
are they doing it?

Don't know. The engineer is overworked so I stepped into the lab this
afternoon and will test myself.
It's chaos, there's only one 13GHz infiniium and only one 12GHz probe,
all the other stuff is 6GHz stuff.

Oh, why does the risetime matter? Does it have to be 50 ohms?

It's the spec and yes, it's the spec too.