Micro Strip PCBs?

[Mike - K8LH]

What does this term mean fellas? Google didn't help (wrong search criteria?). I've come across it a couple times by manufacturers of antenna switching systems for Ham radio.

TIA, Mike

 

[Nigel Goodwin]

It's basically implementing tuned circuits in the PCB itself, so it's really only a high frequency technique. It's sometimes used at VHF, but more commonly at UHF and above.

 

[RadioRon]

Microstrip is a form of transmission line that is well suited to printed circuit boards. Imagine a length of coax where someone has sliced the outer conductor down two sides and have flattened out that outer conductor. This is sort of like what we call stripline, where you have two flat metal plates on either side of a center conductor. It will still work if you take away one of those flat plates, and we call this microstrip. The width of the ground strip and the "hot" strip are critical in setting the characteristic impedance of the line.

So Microstrip is a transmission line made out of copper on your pcb.

It is used just like any other transmission line. It can transport RF energy from one point to another, just like coax does. It can also be used as a capacitance or inductance at specific frequencies. We call the technique of building filters and couplers out of transmission lines "distributed element" topology. Instead of capacitors and wire inductors, you can use specific lengths of transmission lines instead, using distributed element design. Since the lengths necessary to implement inductors and capacitors are related to the wavelength of the energy, it gets easier to build such things on pcbs as the frequency goes higher, and practically speaking, we see a lot of this above 2 GHz.

Here's your wiki link:
https://en.wikipedia.org/wiki/Microstrip

 

[MrJammin]

RadioRon, can you explain the differences between stripline and coplanar configurations of microstrip?

 

[RadioRon]

We use the word stripline for the configuration where there are two groundplanes, one above and one below the signal conductor. We use the term microstrip to describe the configuration where the signal conductor is on the top surface and there is only one ground plane, beneath it of course. The term microstrip is often used to label all of the different configurations of planar transmission lines, but this is technically incorrect. You can guess that stripline and microstrip are closely related in how they transport energy via TEM mode fields. Stripline is a bit better since it is more shielded than microstrip, but it has the obvious disadvantage of needing three layers of pcb copper, and it is very difficult to modify the signal conductor for prototyping or test purposes. Microstrip is much more convenient and uses less copper layers so it is the more popular. There are a few other multi-layer configurations, for example, if you have a dielectric layer above the signal conductor of a microstrip but no copper, then it is still a kind of microstrip. And then there is the type where you have the signal conductor inside the board, like stripline, but one of the two groundplanes is very close while the other is quite far away. This behaves more like microstrip than stripline.

Well, having said all that, what about co-planar lines. The RF community often calls these "coplanar waveguide". As you might guess, the key difference in construction is that the critical grounds and the signal line are all on one plane, hence the word co-planar. The EM fields exist most strongly in the gap between the signal line and the ground plane next to it. The most common configuration has the edge of a ground plane on either side of the signal conductor, all on top of a dielectric. Variations on this include having a ground plane underneath it as well. You could argue that this is a hybrid betwen a coplanar configuration and a microstrip, and you would be right. The relative spacings determine if it behaves more like one or other other or is a perfect balance. Calculating the characteristic impedance of such lines is a bit of an art form and sometimes requires a bit of trial and error.

Coplanar waveguide offers better RF isolation from other circuits on the same plane because you are guaranteed to have a groundplane in the intervening space. An obvious advantage also is that the CPW only uses one layer of copper, which allows you to pack more stuff in or keep your pcb simpler. This can make a big difference in RF ICs where these lines are printed on semiconductor substrates and in some hybrids and flip chips. In some applications, where you are implementing a grounded stub, you don't need a via hole to ground the end of the line. A disadvantage compared to microstrip is that CPW is usually a bit lossier, mainly because the current is mostly confined to the edges of copper, a small area hence higher resistance. If I remember correctly, the overall size of a CPW is a bit bigger than microstrip because you have more field in the air rather than in the dielectric so the signal conductor tends to be a bit wider.

Coplanar waveguide is less popular than microstrip partly because it is less well understood by users, since they don't use it.

The average cellphone uses all these configurations to some degree as they manage to pack all the rf circuitry into very small areas. A cellphone pcb might be 8 or more layers, and you have rf transmission lines criss-crossing over and under each other. These have to be isolated from each other so you see some pretty interesting things depending on the designer's style.

 

[MrJammin]

Thanks so much, that was a great explanation. I think the main problem I was having was deducing why there were ground strips bordering the conductor but you resolved that question for me.

 

[Mike - K8LH]

Thanks for the great explanations.

Mike, K8LH