Creating a RF PCB, what to consider? Ground planes? Microstrip? Impedance?

[vortexnl]

I'm creating a relatively simple RF transmitter operating at around ~900Mhz, and was wondering what design guidelines I should follow with these speeds. The board will consist mostly of one big IC that does everything and emits the RF signal.
I have read numerous PDF's about RF circuit board design, and I often see the bottom ground plane being solid, and the top layer used for general routing with huge amounts of via's to reduce the inductance for current return paths and stuff like that. However, I'm using another RF board as a design reference here, and I see the top layer being filled with a ground plane as well, I can assume this will affect the impedance of the main RF transmission line running to the SMA connector, and technically this isn't microstrip right because of the capacitance of the top ground plane surrounding the transmission line?

The 1/8 wavelength of 900Mhz is around 40mm, and I think the transmission line to the SMA connector won't exceed 20mm, so in that case I wouldn't need any controlled impedance lines right?

Long story short, if any of you can recommend some good books about RF circuit board design, I would love to read them.

- Nick

[Dago]

However, I'm using another RF board as a design reference here, and I see the top layer being filled with a ground plane as well, I can assume this will affect the impedance of the main RF transmission line running to the SMA connector, and technically this isn't microstrip right because of the capacitance of the top ground plane surrounding the transmission line?

This depends on how close to the microstrip the top layer ground plane goes. If it is far enough it functions as a microstrip and if it is closer (can't remember any rule for it offhand) and you need to take it in to account when designing the microstrip for a specific impedance. I think it is called grounded coplanar microstrip.

[vortexnl]

However, I'm using another RF board as a design reference here, and I see the top layer being filled with a ground plane as well, I can assume this will affect the impedance of the main RF transmission line running to the SMA connector, and technically this isn't microstrip right because of the capacitance of the top ground plane surrounding the transmission line?

This depends on how close to the microstrip the top layer ground plane goes. If it is far enough it functions as a microstrip and if it is closer (can't remember any rule for it offhand) and you need to take it in to account when designing the microstrip for a specific impedance. I think it is called grounded coplanar microstrip.

I did some research and it seems to be called a 'coplanar waveguide', this is probably what I'll be using so I can fill the top layer with a ground plane as well and I can achieve a 50 Ohm impedance with a thinner trace.

[KJDS]

Grounded coplanar waveguide doesn't significan't reduce the line width until the adjacent ground gets very close, at which point be very aware that tolerances of both copper thickness and spacing need to be closely looked at.

The line is probably short enough to not make too much difference, but don't let it stray too far from 50 ohms.

If it's going into volume production then I'd specify the substrate as something decent, probably one of the Isola products.

[LukeW]

A microstrip line (no groundplane surrounding the transmission line on the top layer)  results in the transmission line being several times wider for a given impedance (say 50 ohms) compared to a coplanar waveguide with ground (where a groundplane surrounds the transmission line on the top layer as well as a solid groundplane underneath, and "fence" vias are used). Coplanar waveguide is smaller, among other factors.

The models and equations are different, so different settings in your calculators or software tools need to be chosen.

The spacing between the top layer groundplane and the transmission line is typically very small, as small as you can get in terms of fabrication design rules, say about 6 thou.
http://analoghome.com/articles/an004.pdf

[Dago]

A microstrip line (no groundplane surrounding the transmission line on the top layer)  results in the transmission line being several times wider for a given impedance (say 50 ohms) compared to a coplanar waveguide with ground (where a groundplane surrounds the transmission line on the top layer as well as a solid groundplane underneath, and "fence" vias are used). Coplanar waveguide is smaller, among other factors.

The models and equations are different, so different settings in your calculators or software tools need to be chosen.

The spacing between the top layer groundplane and the transmission line is typically very small, as small as you can get in terms of fabrication design rules, say about 6 thou.
http://analoghome.com/articles/an004.pdf

Thats a very handy pdf, thanks for the link! I've been meaning to make an RF signal gen up to a few gig...

[David Hess]

A microstrip line (no groundplane surrounding the transmission line on the top layer)  results in the transmission line being several times wider for a given impedance (say 50 ohms) compared to a coplanar waveguide with ground (where a groundplane surrounds the transmission line on the top layer as well as a solid groundplane underneath, and "fence" vias are used). Coplanar waveguide is smaller, among other factors.

Doesn't this confuse a conductor-backed coplanar waveguide with a post-wall waveguide?

I usually think in terms of microstrips and coplanar waveguides with or without a ground plane.  The others are too exotic for me.

[penfold]

At 900 MHz with a basic transmitter or receiver, you've just got to be very careful, use a lot of grounding, decoupling and filtering.
Where possible, go for rough rules of thumb for trace impedance and source/sink impedance on board, but remember that your connector to an external antenna will need to be terminated properly and you'll have to take into account the output impedance of the driver on board when calculating your termination resistances

[tggzzz]

I'm creating a relatively simple RF transmitter operating at around ~900Mhz, and was wondering what design guidelines I should follow with these speeds. The board will consist mostly of one big IC that does everything and emits the RF signal.

If you have to ask that question, you should ensure you only "transmit" into a 50 ohm dummy load.

There is far more to RF than PCB layout. Unless you understand concepts such as "intermodulation", "third order intercept point", "phase noise" and many other non-ideal properties of analogue components, you will probably end up splattering a distorted version of your signal across many other peoples' receivers and services.

That can, quite rightly, lead to A Visit From Government Agencies, followed by some detailed questioning.