grounded co-planar waveguide PCB design advice please

[megoodsen]

Hi,

I'm designing an RF multilayer board that is to work over 10-200MHz.

For the transmission line I'm using grounded co-planar waveguide.

Material is 10 thou Rogers 4350B, with a 50ohm track width of 0.46mm
and a track to top ground gap of 0.146mm.
This is working OK.

I now want to shield the board to prevent crosstalk, but I am
restricted to very little height.

My plan is to get a flat plate of say 1mm material half mm deep etched
with pockets that follow the RF lines and is grounded all elsewhere.

My worry is, will the fairly close proximity (but nearly 4 times the
track to gnd distance) of the metal plate above the transmission lines
cause problems, and/or will I have resonating cavities too?
I can make the cavities be 3 or 4 times wider that the gnd to gnd gap
around the lines if need be.

What do you think?

73

 

[Mark]

how many layers???

why not put the signal on an inner layer with ground plane above and
below?

Mark

 

[tlbs]

Hi,

I'm designing an RF multilayer board that is to work over 10-200MHz.

For the transmission line I'm using grounded co-planar waveguide.

Material is 10 thou Rogers 4350B, with a 50ohm track width of 0.46mm
and a track to top ground gap of 0.146mm.
This is working OK.

I now want to shield the board to prevent crosstalk, but I am
restricted to very little height.

My plan is to get a flat plate of say 1mm material half mm deep etched
with pockets that follow the RF lines and is grounded all elsewhere.

My worry is, will the fairly close proximity (but nearly 4 times the
track to gnd distance) of the metal plate above the transmission lines
cause problems, and/or will I have resonating cavities too?
I can make the cavities be 3 or 4 times wider that the gnd to gnd gap
around the lines if need be.

What do you think?

I designed a multilayer (20 MHz to 1 GHz wideband + digital ECL) RF
board a few years ago using Rodgers material. I just buried the RF
traces on layer 2 under a surface ground plane and a composite
power/ground layer 3.

Even then, there were a few surface layer traces necessary, and they
got covered by a small shielded can. That probably doesn't help you
much. Perhaps there is some portion of the board where the height
requirement isn't so strict. You could place some surface mount
components in that area and cover them.

Good luck,
Tom

 

[John Larkin]

Hi,

I'm designing an RF multilayer board that is to work over 10-200MHz.

For the transmission line I'm using grounded co-planar waveguide.

Material is 10 thou Rogers 4350B, with a 50ohm track width of 0.46mm
and a track to top ground gap of 0.146mm.
This is working OK.

I now want to shield the board to prevent crosstalk, but I am
restricted to very little height.

My plan is to get a flat plate of say 1mm material half mm deep etched
with pockets that follow the RF lines and is grounded all elsewhere.

My worry is, will the fairly close proximity (but nearly 4 times the
track to gnd distance) of the metal plate above the transmission lines
cause problems, and/or will I have resonating cavities too?
I can make the cavities be 3 or 4 times wider that the gnd to gnd gap
around the lines if need be.

What do you think?

73

This will seriously change the impedance, so you'd have to narrow the
trace if Z matters. And the mixed dielectrics (epoxy-glass and air)
will make the calculations a real pain.

John

 

[Fred Bartoli]

This will seriously change the impedance, so you'd have to narrow the
trace if Z matters. And the mixed dielectrics (epoxy-glass and air)
will make the calculations a real pain.

I don't know for a coplanar line, but with a microstrip line, just compute
the impedance with any calculator for a buried line, then multiply the air
side thickness by Er and you'll have the corresponding air thickness,
provided the sidewalls are not too near the line.

Also, why using Rogers4350 at 200MHz? Unless you need it for some other part
of the design, this is overkill.

 

[Ken Smith]

I now want to shield the board to prevent crosstalk, but I am
restricted to very little height.

My plan is to get a flat plate of say 1mm material half mm deep etched
with pockets that follow the RF lines and is grounded all elsewhere.

Just a thought:
If you make the wave guide on the nominal "circuit side" of the PCB you
may be able to make the shield part of the mechanics that holds the PCB in
place. This may save you some height.

My worry is, will the fairly close proximity (but nearly 4 times the
track to gnd distance) of the metal plate above the transmission lines
cause problems, and/or will I have resonating cavities too?
I can make the cavities be 3 or 4 times wider that the gnd to gnd gap
around the lines if need be.

What do you think?

You may want to have a groove for each line and an extra groove between
the lines. I assume the shield will be soldered in place.