1. Home
  2. Electronics Design
  3. grounded co-planar waveguide PCB design advice please

grounded co-planar waveguide PCB design advice please

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
Reply to
megoodsen
Loading thread data ...

how many layers???

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

Mark

Reply to
Mark

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

Reply to
tlbs

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

Reply to
John Larkin

"John Larkin" a écrit dans le message de news: snipped-for-privacy@4ax.com...

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.

--
Thanks,
Fred.
Reply to
Fred Bartoli

In article , megoodsen wrote: [....]

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.

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.

--
--
kensmith@rahul.net   forging knowledge
Reply to
Ken Smith

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.