Electronics > Projects, Designs, and Technical Stuff
filtering on ground?
Clear as mud:
(? how do you get the pictures to show up in the message - I chose "inline expandable thumbnail, but it still puts them at the end?)
Here is an LT7101-based synchronous switching buck regulator, output 5V at 1A, input will be 36 to 59 volts.
Normally we would want a pretty solid ground, right? I'm not sure the best way to attach PGND to GND. Initially I considered a filter bead like the one I show on the 5V output, I believe it's 100 ohm at 100 kHz. The schematic shows a 0-ohm resistor, which could be a SMD, but I also considered creating a custom footprint that would have a solid copper area on another layer under the whole regulator circuit, connecting to a PGND pad on the input side and a GND pad on the output side.
But, a comment on my first thread led me to consider something completely different: why not filter the ground side symmetrically with the + voltage side? I now believe the comment was geared specifically towards analog inputs, not the switching regulator circuit, but if the output is intended to operate on DC, and inductors and filter beads have very low impedance at DC, why not use them to filter out the high-frequency components from the ground side of the circuit as well as the non-ground side? So, I made this alternative schematic.
The incoming ground is PGND, then PGNDa, then LT_PGND and LT_SGND, then the outgoing ground is just GND. With inductors and filter beads between grounds to match the ones on the positive side. I guess, normally you wouldn't want to do this because if the ground went off-board at all, then someone would probably connect incoming and outgoing grounds externally, so the filtering would be for nothing. And, I do have some off-board LED strips that will be powered from the 5 volts. So: good idea? bad idea? I might simulate both in LTSpice and see what they look like.
T3sl4co1l:
For a regulator, I wouldn't worry about it. I wonder how I'd even construct a setup to measure it. What would be the expected effects? Glitchy timing? Noisy or drifty output (e.g. noise demodulated into control loop)?
With a ferrite bead in there (probably the second example is better), you can at least inject noise to see what happens.
As a policy, I only split grounds when cause can be shown that it is necessary. It is very rare that this occurs in an initial design stage, and I haven't yet had a project where poor grounding has been implicated. (Mind, I haven't done many low noise projects, so don't give too much weight to this opinion with respect to those cases. The plural of "anecdote" is not "data"!)
Tim
Daixiwen:
I usually don't bother either. Just connect the SGND pins directly to the ground plane, and connect together the high power ground pads (PGND, capacitors) with a thick trace, connected to the ground plane in one point, away from high currents.
I have never made the experience either, but I wonder if high frequency potential difference between SGND and PGND will cause higher noise, rather than lower one. I've never seen any dc/dc converter datasheet recommending to filter some ground pins.
Clear as mud:
Sounds like a lot of experimentation would need to be done and actual data gathered, before one could say how filtering the ground might change anything.
I'm OK with skipping all of that and just using a solid ground as recommended. :-+
KT88:
Splitting PGND and SGND on the PCB is usually a terrible idea. The purpose of having different ground pins is to avoid current sharing of noisy and sensitive internal nodes through one bond connection (it's not alway just a wire anymore). This is simelar to ADCs by the way... However it makes sense to treat PGND and SGND differently on the PCB. This means having a parition of the one and only GND on the PCB for PGND and one for SGND. You can find an example in the EVAL-Board layout of the LT7101. The grounds are directly connected but the sensitive signal connections like VFB are separated from the rest of the ground plane. This allows to avoid injecting noise into the fragile parts of the circuit.
It is also a common misunderstanding that a groundplane is able to somehow delete noise that is fed into it... The best results are achieved if no noise is dumped into the ground plane. This can be achieved by taking care of smallest loop areas and proper return paths for transient currents. The most important part is the connection of the input cap for a buck (it would be the output cap for a boost). There is also some significant noise conducted over the winding capacitance of the inductor that has to be taken care of...
If that is done correctly there is not much noise that escapes the regulator circuit....
p.s. The inductor has to be connected with the inner part of the winding to switch node and the outer part will act as a shield connected to the output cap (thus the need for a proper output cap placement and routing...).
Cheers
Andreas
Navigation
[0] Message Index
[#] Next page
Go to full version