2

If I route a 433 MHz AC-coupled RF microstrip trace out of an MMIC such that it's referenced to a Power plane rather than a Ground plane, will that have a significant effect on the impedance of the trace?

I'm designing a 4-layer PCB with a Signal-Ground-Power-Signal stackup which has MMICs on both sides (this amplifier being one example). This makes me want to run microstrip on the bottom such that it's referenced to Power rather than to Ground. I'm aware that this is OK for digital signals (this page from Henry Ott being what finally convinced me of that), and I've read through Microstrip over power plane, but there are a few things that make me leery of blindly applying those conclusions to this situation.

1) This isn't a push-pull driver like the ones in the paper, it's a Class C amplifier (some of the others are Class A). This means it's not symmetric and if I understand right there's likely to be significant inductance from power to collector when compared to emitter to ground.

2) MMICs have a nice big flat low-inductance ground connection through their thermal pad, but typically only a few pins for power. I can only assume any microstrip on-die will be referenced to that ground plane, which I'd imagine would create a discontinuity when transitioning to the PCB microstrip.

3) Eventually this all runs into a coaxial connector whose shield is connected to ground. Unless I connected shield to power (which seems like a terrible idea), wouldn't that create a pretty significant discontinuity as well?

Can someone clarify this for me, ideally with a level of specificity comparable to that Henry Ott paper? I'd really appreciate it!

Community
  • 1
emrlddrgn
  • 21
  • 1
  • Is it reasonable to interrupt your power plane with a piece of ground plane that has many stitching vias to the other ground plane between the MMIC and connector? I have done this to break LVDS signals out of a connector before transitioning to the top side of the board, maintaining ground reference in layers 2 *and* 3. – user2943160 Jun 28 '16 at 20:25
  • I certainly **could** do that, it would just be a fair amount of work and it's frustrating to not know for sure whether or not it's necessary. Plus I generally try to avoid carving up planes if not necessary. – emrlddrgn Jun 28 '16 at 23:26

1 Answers1

1

This isn't a push-pull driver like the ones in the paper, it's a Class C amplifier (some of the others are Class A).

This has nothing to do with the microstrip structure. It's a whole separate issue that you should deal with separately.

MMICs have a nice big flat low-inductance ground connection through their thermal pad, but typically only a few pins for power. I can only assume any microstrip on-die will be referenced to that ground plane, which I'd imagine would create a discontinuity when transitioning to the PCB microstrip.

...

Eventually this all runs into a coaxial connector whose shield is connected to ground. Unless I connected shield to power (which seems like a terrible idea), wouldn't that create a pretty significant discontinuity as well?

Both of these are essentially the same issue. They both mean that your return path will have to find a route between the power plane and the ground plane. You will want to place a bypass capacitor near where these discontinuities occur, giving the return currents a path between the coaxial and on-chip references and the microstrip reference plane. At 433 MHz, this shouldn't create too much trouble if the capacitors are chosen well and not located too far from the discontinuities.

Community
  • 1
The Photon
  • 126,425
  • 3
  • 159
  • 304
  • I see your point. All I was really trying to say with the amplifier comment is that the chip itself doesn't seem to provide a good path from power to ground, but by adding the bypass caps in parallel we should "go around" that inductance. For the bypass caps, am I right in thinking that the largest capacitance with the least parasitic inductance is what I'd be after? I.E., to first order, the largest-value 0402 capacitor? – emrlddrgn Jun 28 '16 at 23:28
  • If your signal is narrowband (like a 20 kHz FM modulation around 433 MHz, for example) then you should probably use a lower value capacitor (like 1 or 10 nF). If it's a broadband digital signal then a 100 nF 0402 part is a common choice. The chip is likely to provide some on-chip bypassing that isn't even mentioned in the datasheet, depending exactly what kind of chip it is. – The Photon Jun 29 '16 at 03:15