Electronics > Projects, Designs, and Technical Stuff
power decoupling myths
Ice-Tea:
What's the target application/frequency for that layout? Seems a bit overkill for a 'regular' board. Not to mention that it will be a total pain for other layers. If you do that for every cap on the board, power planes are going to look like a horror show...
OwO:
Don't use power planes (unless the situation really calls for it, and never as a rule of thumb). That's another myth. This is a 4 layer board and the frequency range is 6GHz. On 4 layers with this stackup (0.2mm prepreg), power planes are completely useless for decoupling. The only potential use case for a power plane is to serve a double purpose of a ground plane that signals can travel against and at the same time deliver power. That's what I did for DDR3 + Zynq on 4 layers, but it's not going to work for RF applications because you'd need a stitching capacitor ever few mm.
Ice-Tea:
Interesting. I was under the impression powerplane/gndplane capacitive coupling was the highest freq/"first line responder". Granted, probably works better if the separation is less than 0.2mm but still.. Any documentation for that?
T3sl4co1l:
--- Quote from: OwO on July 21, 2020, 11:12:17 am ---Don't use power planes (unless the situation really calls for it, and never as a rule of thumb). That's another myth. This is a 4 layer board and the frequency range is 6GHz. On 4 layers with this stackup (0.2mm prepreg), power planes are completely useless for decoupling. The only potential use case for a power plane is to serve a double purpose of a ground plane that signals can travel against and at the same time deliver power. That's what I did for DDR3 + Zynq on 4 layers, but it's not going to work for RF applications because you'd need a stitching capacitor ever few mm.
--- End quote ---
RF applications differ as greatly as any other application does. Approval or dismissal of planes is irrelevant without additional facts.
You wouldn't route RF signals through planes themselves, that's ridiculous. But then, what about the very wide stripline connections to large power transistors? These have line-wave transmission line impedances of a few ohms -- they would be excellent planes for a DDR interface!
Conversely, you would route RF signals over power planes, even gaps between planes. The gaps can be bypassed locally as needed, or differential signals can be used. (Preferably, gaps are avoided, of course.)
--- Quote from: Tomorokoshi on July 20, 2020, 08:33:22 pm ---That is similar to the Hoffman Effect!
https://conradhoffman.com/hoffman_effect.htm
--- End quote ---
Not a very solidly stated thesis, but the result is equivalent I think to noting that, for a C1 || (R+C2) network, R = Xc1 and C2 > 2.5 C1 should be chosen to thoroughly spoil the Q of C1 at the crossover frequency (which is also what gives Xc1).
Tim
Tim
TheUnnamedNewbie:
Ever since I put a number of layouts into actual EM solvers I realized that everyone on the internet who says 'you have to do it this way' is wrong.
The way you have your grounds, and your substrate thickness, and whether or not you cannot have blind vias, all matter and completely change what is the 'best approach'. Not to mention that people often confuse two completely different ideas and don't get that they are two different targets with different ways to get there.
If you really want to understand and know, do yourself a favor: Stop going by some online forum post telling you what to do, and go rent/buy a copy of an EM package for a few weeks, and actually play around in that. Try different substrates, different thicknesses, different types of capacitor, different styles of mounting, etc. Notice how sometimes, it's actually better to just wire to the chip than to try and drop down to a via on a plane, because that added loop area is doing more harm than good. Or that trying to get 10 mOhm supply impedance at 100 MHz is pretty much pointless, because a single bondwire will absolutely destroy your impedance at that frequency.
Sometimes your traget is noise suppression/noise isolation. You want noise from device A not to get to device B. In part by making the power supply able to counter some of the noise, in part by throwing filter caps at it, and in part by reducing the noise in the first place with more capacitance. Applications? LNAs, precision analog, etc.
But other times your target isn't noise suppression, but is actually supply impedance. Getting high performance, high power RF amplifiers and so on to work, often has far less to do with keeping noise in the PA at bay, and much more to do with making sure the PA can draw whatever current it damn well pleases without the supply limiting that.
Some interesting things I found: When working with 2/4 layer PCBs, going to ground plane near chip was pointless, because the via inductance negated any benefit. But on some of the very high frequency boards I'm working, with 50um core's, using blind vias, going to planes actually made my 0402 caps completely unnecessary.
There are also some interesting things when putting caps in parallel - Dell has a patent (US 6,337,798) that claims that putting caps in parallel will actually significantly reduce the efficacy of those caps because of skin effect and current crowding.
This is also why I suspect that OwO's example is actually not useful. The current crowding will just make all but the few outer vias pointless. Might as well get rid of them, your routing, and your wallet will thank you.
I have a bunch of slides that I've been meaning to release about this, but right now they still contain a bunch of unpublished PCBs as examples so I have to wait a few more months before I can.
Another thing I learned: Discrete components are pointless to do any decoupling past a few hundred MHz. Even if you ignore any layout effects, the interal ESL of a 008004 cap makes it's self-resonance frequency be around the 100 MHz range. You just can't get around that without using special bonded capacitors meant for RF/MMIC applications. And to be frank, even if you could, your bond wires will just ruin that too. Just trust that the IC guys know their stuff and take care of decap past 100 MHz.
Navigation
[0] Message Index
[#] Next page
[*] Previous page
Go to full version