Microstrip, EMI shielding and "mouseholes"

Another problem I am facing currently and I can't get a satisfactory answer on books.

Like I said on another topic, I'm working on a PCB at 5.8 GHz and I am limited to 2 layers (one of them, of course, will be the ground plane). For microwave traces I used microstrip.

Moreover, I will use a tinfoil can as EMI shielding on the top layer. That can will be subdivided in its interior in several subsections (transmitter, low noise amplifier and downconverter). This subsections will be isolated one from another with "walls" of tinfoil.

Problem is I need to route a few microstrip lines from one section to another. This means I need to cut a few "mouseholes" on the "walls".


My question: how large and how high should these "mouseholes" be?

If I make those holes too narrow and too low they will affect stripline impedance.

On the other hand, if I make the holes too big they will render EMI shielding useless.

So, how to compute the dimensions of the hole? Is there a "rule of thumb" that can be used to design those holes wuth, say, 0.1 dB return loss and still effective EMI shielding?

Tinfoil? Sounds pretty funky!

Tinfoil is thin. Since the mousehole will not have any length, it will not attenuate the signal the way a cuttoff waveguide section would. So any mousehole that you put in a wall will act like an Iris would act in a waveguide. An iris typically acts like a shunt reactance to a waveguide.

So, some questions. At 5.8 GHz, are your cavities wide enough to form propagating waveguides (ie wider than λ/2)? If so you will have lengths of propagating waveguide, with iriises in between, which will send energy through unimpeded at some select frequencies-just like a bandpass filter. You can screw around with the iris sizes and the cavity lengths to try to keep them non-resonant at 5.8 GHz. Good luck. If you have big cavities, the better way to fix them is to de-Q them with some sort of absorbing material (ecosorb) on the cover.

If, however, you make sure that all of your cavities are cuttoff waveguide sections at 5.8 GHz, then you have a much better chance of keeping RF from leaking from one section to the next.

As far as making the mouseholes small, I would make the hole 3X the microstrip wide, and keep the mousehole height probably 4X the substrates, as a starting point. It will act to the microstrip line like a little shunt capacitance, with you can tune out by necking down the line slightly.

Rich
www.MaguffinMicrowave.com

Yes, indeed it does. I meant a tin plated can but I wrote tinfoil. This is what happens when I need to write a text in a foreign language without checking with a dictionary. So, the can will be of tin-plated steel. In the first prototype maybe I will use copper or brass, depending on what is available.

Thinking about the shielding can as a waveguide is a nice way to face the problem. Must remeber that. :)

OK, the can will not be as thin as tinfoil, it will be something like 0.9mm thick. Wavelength at 5.8GHz in my 50ohm microstrip lines is about 38mm. This is a ratio of 2.4%. Do you think this is small enough?

Nice tip. Yes, I do have cavities bigger than λ/2. I will check that out.

You are right, but not an option on this design.

Yes, while trying to guess some ballpark values for those holes according to other known good practices of PCB design, layout and microstrip line theory, I thought roughly about the same values as you did. However I still opened yhis thread to hear from more experienced people.


Thank you, Rich! You gave me some very good tips and guidelines. :D

I have used this type of shield on products up to 3 GHz, where I simply ran the trace under the shield rim receptacle, with solder mask on top of the trace and a deliberate little air gap. Unless it is a precision application, that will probably work for you too.

http://www.leadertechinc.com/cbsCBS.shtml