multi-layer PCB for RF passives

Hi, everyone. I have a question about the multi-layer PCB for RF passives.

Right now I ran out of the space to put my microstrip power dividers and hybrids on a two layer PCB design. And I am thinking whether I can put the power divider into the other layer which is sandwiched by two ground plane as a stripline structure, and use PTH to connect it to the hybrid on the layer on top for microstrip structure. So the structure stack-up is something like this one:

--------- <- hybrid layer
000000 <- dielectric substrate 1
--------- <- GND 1
0000000 <- dielectric substrate 2
--------- <- power divider layer
0000000 <- dielectric substrate 3
--------- <- GND 2

I am wondering whether this idea can work? If yes, what kind of issues should I be aware? And any reference to the multi-layer RF PCB design will be welcomed. Thanks.

This means switching from microstrip to embedded stripline. It has lower radiation losses, but probably higher dielectric and skin effect losses. A dense via grid connecting the two ground planes may be necessary to prevent unwanted modes. Also the layer1-layer3 via connection creates discontinuities.

You don't mention what frequency range your design is going to use. It would also help to know the approximate overall size of your board.

Some general comments:
- The stackup you show is inadvisable for large boards. The asymmetric distribution of layers around the board core tends to cause warping and cupping of the board. You may get away with it if your board is small, or there is dense routing on the signal layers to help offset the solid copper of the planes.
- Placing your stripline between two ground planes will increase the delay along the stripline (higher capacitance).
- The copper losses (including skin effect) won't change if you choose your dielectric thicknesses to keep the trace width the same on inner layers as it is on outside layers.
- Traces on inner layers have higher dielectric loss than traces on outside layers. That should be intuitive since outside layers have air dielectric on one side.
- Unless you're operating at about 6GHz or above, there's no design penalty for placing your RF components on both sides of the board with two internal planes instead of your asymmetric stackup. Use one plane as reference for each side of the board. Losses get harder to control as you go above 6GHz, but they still can be managed in most cases.
- You'll have to design your RF vias with sufficient "blowouts" to minimize capacitance as they pass through the planes.

I aggree with all comments, except for one

- The copper losses (including skin effect) won't change if you choose your dielectric thicknesses to keep the trace width the same on inner layers as it is on outside layers.

Click to expand...

This is unrealistic for the present example, considering a feasible stackup, to my opinion.

I think however, that my first comment neglected an important point. A microstrip has higher copper losses than an embedded stripline, cause the current is concentrated on the bottom side of the strip only. Thus the stripline with symmetric current distribution may be smaller for equal copper losses.

As another point, a symmetric stackup is desirable indeed, but can't be always achieved, respectively would require costly dummy layers. It's also not said, that the suggested unsymmetrical structure must determine the layer usage of the whole board, it may be regional only.

FvM - I said my comments were "general" in the absence of frequency and board information. We don't know what materials he's using, modulation method, frequency, etc, etc.

With regard to the stackup, there are no dummy layers needed. Simply put the two reference planes inside as the core, the two outter layers become copper on prepreg . It is likely he will need/want a power plane in addition to a "ground" plane. Either plane will make a satisfactory reference for RF circuitry on the top and bottom layers. I've designed many commercial RF devices in that manner over the past forty years.

I aggree, that this is a simple and effective design principle, just using a standard 4-layer stackup for two-sided microstrip. The suggested embedded stripline is an option, but I also don't see much sense in discussing it without more detailed specifications.

hi, all. Thanks for your commend. Actually in my design, the frequency range is around 7~9GHz (X-band).

One more question is about the connection between two stripline ground planes. Should I add the plated-thru vias at the edges of the board, or should I add the vias along the stripline trace.

Thanks.