Impedance of complanar traces on PCB surface?

[Andy]

Hello:

I want to lay out a couple of traces on the FR4 PCB, to provide a
transmission line of specific impedance for a differential-mode signal.

The impedance calculation formulas that I have found so far, for the
common-mode and differential impedance, concern the traces with the
ground plane underneath. I think I don't want the ground plane
underneath, to minimise the common-mode capacitance, and I am looking
for the formula for the coplanar traces on one side of the PCB, with no
metal (copper) in the other PCB layers in the vicinity of the trace.

Can somebody help?

Thank you.

-- Andy

 

[Don Pearce]

Hello:

I want to lay out a couple of traces on the FR4 PCB, to provide a
transmission line of specific impedance for a differential-mode signal.

The impedance calculation formulas that I have found so far, for the
common-mode and differential impedance, concern the traces with the
ground plane underneath. I think I don't want the ground plane
underneath, to minimise the common-mode capacitance, and I am looking
for the formula for the coplanar traces on one side of the PCB, with no
metal (copper) in the other PCB layers in the vicinity of the trace.

Can somebody help?

Thank you.

-- Andy

This is quite normal as there is usually a ground plane somewhere
about - if just the screening box. Make the calculation with the
ground plane at an appropriate distance for this, and all should be
well.

I don't know how tight your coupling is, and the calculations really
aren't terribly good much tighter than about 8dB, but you will
probably need a couple of iterations or a bit of scalpel scraping to
get it right.

d

Pearce Consulting
http://www.pearce.uk.com

 

[Chris Carlen]

This is quite normal as there is usually a ground plane somewhere
about - if just the screening box. Make the calculation with the
ground plane at an appropriate distance for this, and all should be
well.

But some formulas, being approximate models that fit fairly well over a
limited geometrical domain, might deviate too much from meaningful
results when taken far from their intended domain of usefulness.

Might it be better to find expressions for the transmission line
parameters based solely on the adjacent rectangular cross section
conductors that the OP is working with, considering no ground plane?

I don't know how tight your coupling is, and the calculations really
aren't terribly good much tighter than about 8dB, but you will
probably need a couple of iterations or a bit of scalpel scraping to
get it right.

d

Pearce Consulting
http://www.pearce.uk.com

--
_______________________________________________________________________
Christopher R. Carlen
Principal Laser/Optical Technologist
Sandia National Laboratories CA USA
[email protected] -- NOTE: Remove "BOGUS" from email address to reply.

 

[Mark]

You need to think about the common mode impeadance and the differential
impedance. Unless the ground plane is very far away, both will impact
your result.
Consider a thin twisted pair inside a sewer pipe. In most practical
PWB stackups, the common mode impedances dominate because you cannot
get the two differential conductors close enough to each other relative
to their distance from the ground planes.

Mark

 

[Don Pearce]

But some formulas, being approximate models that fit fairly well over a
limited geometrical domain, might deviate too much from meaningful
results when taken far from their intended domain of usefulness.

Might it be better to find expressions for the transmission line
parameters based solely on the adjacent rectangular cross section
conductors that the OP is working with, considering no ground plane?

As I remember it, a distant ground plane was not one of the limit
conditions that gave rise to large errors. Areas of importance are
close traces, and finite thicknesses of traces.

He could always do a finite element analysis based on Laplace's
equation. Most CAD packages offer some sort of field evaluator that
works that way. Mostly they are a bit clunky, and you need to
calculate odd and even modes separately, but they do give the right
answers.

d

Pearce Consulting
http://www.pearce.uk.com

 

[Andy]

As I remember it, a distant ground plane was not one of the limit
conditions that gave rise to large errors. Areas of importance are
close traces, and finite thicknesses of traces.

Thank you. I will try the formulas that are given for PCBs with the
ground plane. But how about the presence of two different materials -
the FR4 and the air?

-- Andy

 

[Don Pearce]

Thank you. I will try the formulas that are given for PCBs with the
ground plane. But how about the presence of two different materials -
the FR4 and the air?

Provided the FR4 is really thin, you can almost ignore it. Performance
is better that way too, as you work in true TEM mode, rather than the
quasi TEM that happens if odd and even mode velocities are not the
same. Most CAD packages will treat mixed mode dielectrics in some
reasonable fashion, though.

d

Pearce Consulting
http://www.pearce.uk.com

 

[John Larkin]

Hello:

I want to lay out a couple of traces on the FR4 PCB, to provide a
transmission line of specific impedance for a differential-mode signal.

The impedance calculation formulas that I have found so far, for the
common-mode and differential impedance, concern the traces with the
ground plane underneath. I think I don't want the ground plane
underneath, to minimise the common-mode capacitance, and I am looking
for the formula for the coplanar traces on one side of the PCB, with no
metal (copper) in the other PCB layers in the vicinity of the trace.

Can somebody help?

Thank you.

-- Andy

Do you have a specific reason to minimize the even-mode capacitance?
In the case of a typical geometry, deleting the bottom ground plane
won't make a lot of difference, unless the board is thin.

To reduce the even-mode capacitance and keep your target differential
impedance, you could just make the traces skinnier and closer
together.

John

 

[Andy]

Do you have a specific reason to minimize the even-mode capacitance?

The signal source is a differential current source, with each output
loaded with a resistance (R) connected to a common DC reference point. I
wanted this combined source see mostly the differential load, with the
impedance Z=2R. A microstrip with a ground plane would present the
differential mode impedance significantly different from two times the
common mode one, unles one distances the strips by several millimeters -
which is not practical in my case. A possibility there is to try to
match the source to the microstrip impedance, by attaching a resistance
between the differential outputs, but I don't like that much as I don't
know what effect this would have on the accuracy of the signal.

In the case of a typical geometry, deleting the bottom ground plane
won't make a lot of difference, unless the board is thin.
To reduce the even-mode capacitance and keep your target differential
impedance, you could just make the traces skinnier and closer
together.

I will study this. But the first try is not promising: with 0.2 mm-wide,
0.2mm-spaced traces with the ground 1.6mm away across the FR4, the
common Z is about 136Ohm, and the differential - 154 ; I need 124 Ohm
differential one.

Thanks.

-- Andy

 

[John Larkin]

The signal source is a differential current source, with each output
loaded with a resistance (R) connected to a common DC reference point. I
wanted this combined source see mostly the differential load, with the
impedance Z=2R. A microstrip with a ground plane would present the
differential mode impedance significantly different from two times the
common mode one, unles one distances the strips by several millimeters -
which is not practical in my case. A possibility there is to try to
match the source to the microstrip impedance, by attaching a resistance
between the differential outputs, but I don't like that much as I don't
know what effect this would have on the accuracy of the signal.


I will study this. But the first try is not promising: with 0.2 mm-wide,
0.2mm-spaced traces with the ground 1.6mm away across the FR4, the
common Z is about 136Ohm, and the differential - 154 ; I need 124 Ohm
differential one.

Thanks.

-- Andy

Cranking up Txline, it recommends 0.32 mm trace widths to get 124 diff
z (62 odd mode impedance), with an opposite ground plane and your
other dims. Even mode impedance is 203 ohms. I doubt that eliminating
the ground plane would change these numbers a lot.

John

 

[lemonjuice]

Hello:

I want to lay out a couple of traces on the FR4 PCB, to provide a
transmission line of specific impedance for a differential-mode signal.

The impedance calculation formulas that I have found so far, for the
common-mode and differential impedance, concern the traces with the
ground plane underneath. I think I don't want the ground plane
underneath, to minimise the common-mode capacitance, and I am looking
for the formula for the coplanar traces on one side of the PCB, with no
metal (copper) in the other PCB layers in the vicinity of the trace.

Can somebody help?

Thank you.

-- Andy

Differential impedance
Assume for a moment that you have terminated both
traces in a resister to ground. Since i1 = -i2, there would be
no current at all through ground. Therefore, there is no real
reason to connect the resisters to ground. In fact, some people
would argue that you must not connect them to ground
in order to isolate the differential signal pair from ground
noise. So the normal connection would be a single resister from Trace
1 to Trace 2. The value
of this resister would be the sum of the odd mode
impedance for Trace 1 and Trace 2, or
Zdiff = 2 * Zo * (1-k) or
2 * (Z11 - Z12)
Calculations:
To say that Zdiff is 2*(Z11 - Z12) isn't very helpful
when the value of Z12 is unintuitive. But when we see that
Z12 is related to k, the coupling coefficient, things can become
more clear. . National Semiconductor
has published formulas for Zdiff that have become accepted
by many.
Zdiff = 2*Zo[1-.48*exp(-.96*S/H)] (Microstrip)
Zdiff = 2*Zo[1-.347*exp(-2.9*S/H)] (Stripline)
where S is the distance between adjacent traces and H is the height of
the board. Zo is as traditionally defined

common mode
impedance differs only slightly from the above. The first
difference is that i1 = i2 (without the minus sign.) Thus Eqs.

V1 = Zo * i1 * (1+k) k is the coupling coefficient
V2 = Zo * i1 * (1+k)
and V1 = V2, as expected. The individual trace impedance,
therefore, is Zo*(1+k). In a common mode case, both trace
terminating resisters are connected to ground, so the current
through ground is i1+i2 and the two resisters appear (to the
device) in parallel. Therefore, the common mode impedance
is the parallel combination of these resisters, or
Zcommon = (1/2)*Zo*(1+k), or
Zcommon = (1/2)*(Z11 + Z12)
Note, therefore, that the common mode impedance is approximately
¼ the differential mode impedance for trace
pairs.

 

[Andy]

...


Cranking up Txline, it recommends 0.32 mm trace widths to get 124 diff
z (62 odd mode impedance), with an opposite ground plane and your
other dims. Even mode impedance is 203 ohms. I doubt that eliminating
the ground plane would change these numbers a lot.

John

I have had a problem with my computer (motherboard failure), back
on-line only recently.

In fact, I cannot approach the required impedance with the ground plane
on the opposite PCB side removed.

A nice program, that Txline.

Thank you!

-- Andy