Building Coaxial transmission line on PCB?

[Geronimo Stempovski]

Thanks for your help, so far. Really appreciate it. I'm already a step
further in my considerations.

Now I'm looking for a diagram like frequency (some MHz to 10 GHz for
example) versus loss tangent and / or epsilon R for FR4. I only found a poor
black-and-white copy from 1991 in a paper which I searched with Google. I
wouldn't have thought it to be so hard to find a graph... Does anybody know
where I can find that?

 

[john jardine]

Hello,

but how about a real closed square shield around the center conductor?

Bye

Would have been ideal. At the time was thinking about a method to do this
and sorted a setup that may have been worth talking to the PCB people about
but a customer was paying to clear down his urgent problem and not to start
up a research project .
No ... I don't remember what I figured out. Ideas are easy, it's the
implementation that's a problem .
No doubt it'll surface again if I'm I'm under pressure.
john

 

[Jim Granville]

Hello,

but how about a real closed square shield around the center conductor?

To do that would need plated slots, and slots have the PCB fabs
luke-warm at best : hard to do cleanly, they also weaken the PCB if
long, and also have minimum router sizes, plus machine time......

A better direction would be thinner laminates, and using the space you
would have lost to the slot anyway, as wider GND webs on the same plane,
coupled with stitching vias (which can be smaller dia than slots)

-jg

 

[Uwe Hercksen]

Now I'm looking for a diagram like frequency (some MHz to 10 GHz for
example) versus loss tangent and / or epsilon R for FR4. I only found a
poor
black-and-white copy from 1991 in a paper which I searched with Google. I
wouldn't have thought it to be so hard to find a graph... Does anybody
know
where I can find that?

Hello,

I am sorry to tell that, but for frequencies of 1 to 10 GHz, FR4 ist not
the right material, there are other PCB materials which are better for
high frequencies, take a look here
http://www.andus.de/Leiterplatten/Impedanz/hfmat.htm
They write there that FR4 may be used up to 4 GHz.

Bye

 

[John Larkin]

Hello,

I am sorry to tell that, but for frequencies of 1 to 10 GHz, FR4 ist not
the right material, there are other PCB materials which are better for
high frequencies, take a look here
http://www.andus.de/Leiterplatten/Impedanz/hfmat.htm
They write there that FR4 may be used up to 4 GHz.

Bye

FR4 can be used at 20 GHz, depending on what you're trying to do.

John

 

[Geronimo Stempovski]

Again, I'm looking for a diagram like frequency (some MHz to 10 GHz for
example) versus loss tangent and / or epsilon R for FR4 or other usual PCB
material. I only found a poor black-and-white copy from 1991 in a paper
which I searched with Google. I wouldn't have thought it to be so hard to
find a graph but as noone replied to my previous question so far it does
seem to be hard!

Does anybody know where I can find that?

Regards Gero

 

[John Larkin]

Again, I'm looking for a diagram like frequency (some MHz to 10 GHz for
example) versus loss tangent and / or epsilon R for FR4 or other usual PCB
material. I only found a poor black-and-white copy from 1991 in a paper
which I searched with Google. I wouldn't have thought it to be so hard to
find a graph but as noone replied to my previous question so far it does
seem to be hard!

Does anybody know where I can find that?

Regards Gero

Google gives lots of hits on stuff like "loss tangent fr4 frequency"

But FR-4 varies a lot, so there's no definitive data.

What are you trying to do?

John

 

[Uwe Hercksen]

FR4 can be used at 20 GHz, depending on what you're trying to do.

Hello,

well, if the transmission line is very, very short.....


bye

 

[Uwe Hercksen]

Again, I'm looking for a diagram like frequency (some MHz to 10 GHz for
example) versus loss tangent and / or epsilon R for FR4 or other usual
PCB
material. I only found a poor black-and-white copy from 1991 in a paper
which I searched with Google. I wouldn't have thought it to be so hard to
find a graph but as noone replied to my previous question so far it does
seem to be hard!

Hello,

look here for FR408
http://www.isola.de/d/ecomaXL/index.php?site=ISOLA_DE_product_additional_information&sid=235&p=10

bye

 

[John Larkin]

Hello,

well, if the transmission line is very, very short.....

Exactly.

John

 

[Geronimo Stempovski]

But FR-4 varies a lot, so there's no definitive data.

What are you trying to do?

Hi John, I'm trying to compare several loss tangent values (I think that's
the decisive parameter..!?) from several materials, FR4-, PE, etc. over the
frequency. But it's hard to find such diagrams.

 

[John Larkin]

Hi John, I'm trying to compare several loss tangent values (I think that's
the decisive parameter..!?) from several materials, FR4-, PE, etc. over the
frequency. But it's hard to find such diagrams.

No, what are you trying to *do*? WHY do you want a "coax on a pc
board"?

John

 

[Geronimo Stempovski]

No, what are you trying to *do*? WHY do you want a "coax on a pc
board"?

Ah, okay, what I am actually trying to find out is what makes FR4 act worse
than e.g. teflon at data rates beyond 2,5 Gbps. Is it the loss tangent or
the epsilon r? How is the frequency-dependent attenuation physically
describable? Where does the energy go? Heat, ...? It was my opinion that
higher frequencies can be transmitted over coax but not over FR4 because of
the geometry. Because in a coax there is (almost) no energy loss because the
TEM wave is "captured" by the outer shield and in a planar setup like
stripline or microstrip there are E-field and H-field lines vanish into the
air environment (or somewhere else...). Therefore I'm trying to design a
coax on a PCB. Am I right with my thoughts, anyway?

 

[John Larkin]

Ah, okay, what I am actually trying to find out is what makes FR4 act worse
than e.g. teflon at data rates beyond 2,5 Gbps. Is it the loss tangent or
the epsilon r? How is the frequency-dependent attenuation physically
describable? Where does the energy go? Heat, ...? It was my opinion that
higher frequencies can be transmitted over coax but not over FR4 because of
the geometry. Because in a coax there is (almost) no energy loss because the
TEM wave is "captured" by the outer shield and in a planar setup like
stripline or microstrip there are E-field and H-field lines vanish into the
air environment (or somewhere else...). Therefore I'm trying to design a
coax on a PCB. Am I right with my thoughts, anyway?

A couple of things make pcb's lossy: the loss tangent of the material
(and FR4 is pretty bad) and the copper losses. Copper loss gets bad on
conventional FR4 boards because

1. FR4's Er is high, so for a given impedance traces are skinny.

2. The underside of the copper is treated to bond to the epoxy/glass,
and the treatment (black oxide or something) greatly increases skin
losses. Peel some up and look... it's gross.

3. In the case of microstrip, the current is concentrated on the
underside (the dirty side) of the trace, so losses are that much
worse... the shiny topside of the copper is underutilized. Stripline
would be better, with balanced current density, except that the trace
will be much thinner, which has its own penalty.


A good microwave pcb has a low Er, low loss dielectric; is thick, for
low current density and wide traces; has very smooth copper, which
means traces and pads peel off easily.

I don't think any simple geometry tricks (ie, emulating coax) will
make FR4 any better, and would probably make it worse. For low losses,
microstrip on a thick board is probably as good as it gets.

John

 

[John Larkin]

A couple of things make pcb's lossy: the loss tangent of the material
(and FR4 is pretty bad) and the copper losses. Copper loss gets bad on
conventional FR4 boards because

1. FR4's Er is high, so for a given impedance traces are skinny.

2. The underside of the copper is treated to bond to the epoxy/glass,
and the treatment (black oxide or something) greatly increases skin
losses. Peel some up and look... it's gross.

3. In the case of microstrip, the current is concentrated on the
underside (the dirty side) of the trace, so losses are that much
worse... the shiny topside of the copper is underutilized. Stripline
would be better, with balanced current density, except that the trace
will be much thinner, which has its own penalty.


A good microwave pcb has a low Er, low loss dielectric; is thick, for
low current density and wide traces; has very smooth copper, which
means traces and pads peel off easily.

I don't think any simple geometry tricks (ie, emulating coax) will
make FR4 any better, and would probably make it worse. For low losses,
microstrip on a thick board is probably as good as it gets.

John

Suppose you did an FR4 pcb with a wide microstrip on the top, then
route out most of the material below the trace, namely route a trench
under the trace, from the opposite side, say 90% of the board
thickness. Now we'd have a sort of suspended substrate trace, much
wider for a given Z, with much lower losses. We could call it
LarkinLine.


-------------- copper trace
=================================================
================== ================= epoxy-glass
================== air =================
------------------ ----------------- copper gnd



I haven't a clue how to calculate the impedance; field solver, like
ATLC maybe?

John

 

[glen herrmannsfeldt]

Ah, okay, what I am actually trying to find out is what makes FR4 act worse
than e.g. teflon at data rates beyond 2,5 Gbps. Is it the loss tangent or
the epsilon r?

It is the imaginary part of the dielectric constant. I believe that
can be described as a loss tangent, though I haven't done that.

> How is the frequency-dependent attenuation physically
describable? Where does the energy go? Heat, ...?

Yes, heat. You can consider it as electrical friction.

It was my opinion that
higher frequencies can be transmitted over coax but not over FR4 because of
the geometry. Because in a coax there is (almost) no energy loss because the
TEM wave is "captured" by the outer shield and in a planar setup like
stripline or microstrip there are E-field and H-field lines vanish into the
air environment (or somewhere else...). Therefore I'm trying to design a
coax on a PCB. Am I right with my thoughts, anyway?

I don't believe that is true. It may be that coax tends to use better
dielectrics. Other than that, even if the wave isn't "captured" as you
say, as long as it doesn't find anything else to induce current into, it
doesn't contribute to loss. (Well, twisted pair cable is twisted to
minimize the radiation. Microstrip isn't twisted. Radiation will be
mostly in the plane of the board, and minimized by keeping the board
thin.) The very low loss coax cables use a spiral dielectric such that
most of the space is air and very little is plastic. There has to be
enough material to hold the center conductor in place.

The other loss increase with frequency is due to the skin effect, where
the current travels in a thin layer on the surface of the wire,
increasing the resistance as seen by the current. I believe FR4
is chosen for its thermal and strength properties, and ability to bind
to metal, all not normally required by a coax cable dielectric.
(And also cost.)

-- glen