Why do we have drilled holes along an RF signal trace on PCB?

[venn_ng]

ADC-WB-BB/NOPB Texas Instruments | Development Boards, Kits, Programmers | DigiKey

Order today, ships today. ADC-WB-BB/NOPB – TC1-1-13MA+ series Balun Evaluation Board from Texas Instruments. Pricing and Availability on millions of electronic components from Digi-Key Electronics.

www.digikey.com

If you take a look at the image of this product, you can see there are drilled holes along the trace of RF signal. What's the reason for that? I have always seen this in high frequency PCB boards.

 

[volker@muehlhaus]

Some people create their RF design with grounds on top and bottom side. The vias that you see connect both grounds. There is more ground on the top side, but mostly covered under green solder resist.

 

[venn_ng]

So it's like a ground shied on top/bottom + sides?

 

[FvM]

The transmission line type is coplanar stripline with ground. The main purpose is making a small 50 ohm trace on a thick substrate.

 

[BigBoss]

It's in fact Co-planar Wave-guide. As it sounds, this type of Transmission Line acts as a Wave-guide with grounded holes at both sides.

 

[volker@muehlhaus]

It's in fact Co-planar Wave-guide.

We should use proper names. Co-planar waveguide (CPW) does not have a bottom ground. What we have here is a GCPW with side grounds plus bottom ground.

Sounds like a small difference, but we should use proper names so that people use the correct type in transmission line calculators.

 

[FvM]

I see that different and in part contradictory terms are used in literature.

I like the below shown quite visual terms used by Polarinstruments solver.

The designation of double ground CPW as offset coplanar waveguide is less systematic, I think.

Do you know a comprehensive treatise in paper or text book that covers all PCB transmission line structures?

 

[Azulykit]

Look for books that "speak to you". The Polar Instrument software includes many different transmission line types.


Here are a number of books that I find useful:

T. Moreno, Microwave Transmission Design Data

R. Simons, Coplanar Waveguide Circuits, Components, and Systems

Marcuvitz, Waveguide Handbook

B. Wadell, Transmission Line Design Handbook

Those are a good starting point and there are other useful references. Clayton Paul is another I occasionally find useful. I think of the "drilled holes" you mention as serving two functions. In PCB's where RF and much lower frequency signals are present they give easy access to ground for discrete components, particularly where ground layers are buried in multilayer boards and components are soldered to the top or bottom outside layers. RF usually resides on the outside layers. Looking at the RF transmission line structures the "holes"/ via's are used to change from one transmission line type to another. You might also find it useful to look into blind and buried vias.

The vias/ "drilled holes" make the transmission line (GCPW) look more like a coax equivalent constructed in a layered PCB structure. The figures shown above by FvM do not include vias. Modeling can get very complex depending on your frequency and how far down the Rabbit Hole you want to proceed. In GENERAL, this starts being an issue above 2 GHz and essential at millimeter wavelengths.