Electronics > Projects, Designs, and Technical Stuff
Datasheet layout directions on sense resistor
(1/2) > >>
jmw:
The datasheet for TI's LM5155 switching controller has this PCB layout advice:


* Connect the [current sense] pin to the center of the sense resistor. If necessary,use vias.
* Use a wide and short trace to connect the [power ground] pin directly to the center of the sense resistor.
If you look at the example layouts and evaluation boards, they follow at least the first point closely. They tap the trace from the other side of pad running under the center of the resistor, instead of from the side of the copper pour it is sitting on. I'm struggling to understand the electrodynamics of why it matters where you make the connection. Frequencies seem too low (2.2 MHz max on this controller) for transmission line effects to be significant. What motivates this advice?





Another question: why the distinction between having an "analog ground" for some connections and a "power ground" for others? In these examples, the analog ground is a small copper pour that connects to the power ground under the chip. Why do this instead of having a solid ground plane and dropping vias? The evaluation boards follow this layout even though they have a ground pour on the bottom side. Most of what I have read says that trying isolate one part of your ground plane from the other is bad.
georges80:
For the current sense resistor connections, google "kelvin connections" and toss in resistor as part of the search.

It's not a frequency issue, it's the voltage drop issue of where you take the sense connections from on the current sense resistor. There are also special current sense resistors that have 4 connection points, 2 for the current path and 2 for the sense path.

Separate grounds are to prevent 'switching ground noise' coupling into the sensitive analog sense areas. Stitching one big ground plane together is quite likely to create all sorts of nightmare artifacts.

cheers,
george.
T3sl4co1l:
Kelvin connection, more or less, yes.  It's a little more significant than the basic case, because you want low ESL in the sense path, as well as the correct resistance.  Taking the sense trace back under the resistor maximizes coupling with the resistor (heh, well, if there were no ground plane inbetween; is this 2 or 4 layers by the way?), potentially canceling out some of its ESL.

The ground connection could be made in the same way, though it may be more important to have a wide, low inductance connection there, and simply tolerate what ESL it gives.  It is about as short as can be.

Note that stray inductance is proportional to trace length.  There is a geometry factor, of course: a wide trace has ~proportionally lower inductance than a narrow one.  Also proportional to height over ground plane, so a 4-layer board with closely spaced inner planes (close to the outer layers, that is) is very superior to a 2-layer board, even a fairly thin (say 0.8mm) one.

The same is true of components, so wide-body resistors and capacitors are preferable over their regular lengthwise variants.  Note this isn't a gimme, as resistors are typically trimmed by notching the material with a laser cut; the best current sense resistors are made with multiple cuts, effectively several normal (lengthwise) resistors in parallel on the same chip.  (You can do the same yourself, of course, using multiple long-style resistors in parallel.)



--- Quote from: georges80 on March 29, 2020, 07:55:16 pm ---Separate grounds are to prevent 'switching ground noise' coupling into the sensitive analog sense areas. Stitching one big ground plane together is quite likely to create all sorts of nightmare artifacts.

--- End quote ---

I wouldn't be quite so, alarmist about it... The motivation is to keep switching loop currents, and their associated voltage drops, away from the analog control signals.  That's all.  If you've not put the transistor, diode and cap on that side, there won't be much to worry about.  They're just being careful.

There's nothing wrong with putting that switching loop on the ground plane, without cuts, either.  You just have to take all the signals (input, output, control, whatever) back through a common path and point, so that the voltage drops cancel out.  Add filtering to take care of what's left that doesn't cancel, and you can get quite low EMI levels already, say 40dBuV.  Achieving lower, probably requires shields over the switching nodes/loops anyway; which is maybe not heroic effort, but still a significant step up.

Tim
georges80:

--- Quote from: T3sl4co1l on March 29, 2020, 08:54:43 pm ---

I wouldn't be quite so, alarmist about it... The motivation is to keep switching loop currents, and their associated voltage drops, away from the analog control signals.  That's all.  If you've not put the transistor, diode and cap on that side, there won't be much to worry about.  They're just being careful.

There's nothing wrong with putting that switching loop on the ground plane, without cuts, either.  You just have to take all the signals (input, output, control, whatever) back through a common path and point, so that the voltage drops cancel out.  Add filtering to take care of what's left that doesn't cancel, and you can get quite low EMI levels already, say 40dBuV.  Achieving lower, probably requires shields over the switching nodes/loops anyway; which is maybe not heroic effort, but still a significant step up.

Tim

--- End quote ---

Beg to differ, maybe not in this case (haven't looked through the datasheet), but I've got some experience with LTC (ADI now) switcher IC's (high power LED drivers) and you have to be very careful with where ground paths are, which are tied together with vias and which should be isolated from current paths that could travel through the analog ground floods. Often multilayer is required for these and also care on where the grounding is performed on the sense traces leading back to the switcher controller. You can go from a non-functioning/unstable driver to one that is rock solid, by choice of where the power/analog grounds are cut/isolated and how and where they join together.

What I was stating is that you can't just assume that flooding a big area and calling it ground will lead to a stable implementation of a schematic.

cheers,
george.
T3sl4co1l:
You can't ignore where the currents are flowing, that's for sure.

Tim
Navigation
Message Index
Next page
There was an error while thanking
Thanking...

Go to full version
Powered by SMFPacks Advanced Attachments Uploader Mod