5
\$\begingroup\$

ST L4971 Switching Regulator is the part in question. Figure 1 and 4 both show similar schematics, with Figure 4 being the diagramme as per their evaluation board.

The input capacitor C1, the diode D1, and output capacitor C8 are all connected to the main ground directly, but the low side of the other components are connected to a common reference point which is ultimately connected to the main ground with what looks to be a digital ground symbol.

What is the practical difference compared to just connecting directly to the main ground?

reference design

\$\endgroup\$

3 Answers 3

9
\$\begingroup\$

They provide a high current (low resistance) path for load current to minimize ringing and noise on signal lines (higher resistance). All so they can have a single-sided design.

As OP says, Figure 1 and Figure 4 have a strange layout connection. Also replicated in STEVAL-ISA202V1 - 1.5 A step down switching regulator (VIN = 8 to 55 V) based on L4971:

enter image description here

If you look at sample layout (Figure 5. PCB and component layout of the figure 4.), they show you what they mean: wide ground going from source to load, connecting C1, D1 and C8; a fairly wide ground leaving the main ground and going to all remaining components.

Current will follow the path of least resistance. And since we are talking about electron flow, the majority of current will flow along wide path.

enter image description here

This may have more to do with limiting noise since it is a single-sided design. A similar approach is used on the L4972 2A switcher and the L4973 3.5A switcher (both single-sided). No real explanation is offered in those data sheets.

But if you follow the evolution, you usually can reach the point where the reason for what is commonplace within an organization is explained. For them the reason is too obvious to need explanation!

From Designing with the L296 Monolithic Power Switching Regulator:

enter image description here

LAYOUT CONSIDERATIONS Both for linear and switching power supplies when the current exceeds 1A a careful layout becomes important to achieve a good regulation. The problem becomes more evident when designing switching regulators in which pulsed currents are over imposed on dc currents. In drawing the layout, therefore, special care has to be taken to separate ground paths for signal currents and ground paths for load currents, which generally show a much higher value.

When operating at high frequencies the path length becomes extremely important. The paths introduce distributed inductances, producing ringing phenomena and radiating noise into the surrounding space.

enter image description here

PCB layout for L296 clearly shows what the original designers meant by the ground sketch. Large path for ground (outlined in Red) going from input to output. Skinny path for ground (in Blue) leaving output ground going to rest of circuitry. A definitive low resistance path for load current and a high resistance path for signal current.

\$\endgroup\$
5
  • \$\begingroup\$ Thanks for the detailed explanation. It has been many years since I dealt with switching supplies, usually going with linear regulators. That design note you provided, especially the path length is something I need to be wary of. \$\endgroup\$
    – Usernamed
    Oct 8, 2021 at 22:49
  • \$\begingroup\$ This is not my business, but there does not appear to be a wealth of design data on this switcher, which would be of concern to me! \$\endgroup\$ Oct 8, 2021 at 23:11
  • \$\begingroup\$ It seemed to be similar to some TI designs and didn't look to be the highest risk out there with an ST part + reference board/parts. What sort of design data are you referring to? \$\endgroup\$
    – Usernamed
    Oct 9, 2021 at 1:01
  • \$\begingroup\$ Design info is minimalistic. Absolutely nothing in eval board docs. The paragraphs cited show the complexity of the any switcher design and there is no reference to it in three different switchers. I prefer if they provide all info so I can make informed decisions. If they left that out, what other important info is missing. Just my opinion. \$\endgroup\$ Oct 9, 2021 at 22:02
  • \$\begingroup\$ I have decided not to go with this part, but the information presented was excellent, and certainly made me think a bit more about placement/distance and also the width of the different ground tracks. \$\endgroup\$
    – Usernamed
    Oct 11, 2021 at 10:25
13
\$\begingroup\$

It's a layout suggestion.

In reality, tracks have a resistance and an inductance, and what you should do here is keeping all the signal ground separated from the power ground and only connect both near the load.

That way the signal ground and following, the signal stay clear from rippling ground lifts that stem from high currents through the low but still not neglible resistances and inductances of the power ground path.

It's the same reason why you have Kelvin contacts at low-ohmic measurement resistors.

\$\endgroup\$
9
\$\begingroup\$

Firstly, it's not specifically a digital ground symbol; it's just a ground symbol. Secondly, the ground for the chip and the main power ground are connected by a method known as star-pointing.

Star-pointing prevents power currents (through D1 and C8 and C1 and the actual load) running along tracks for the sensitive areas of the chip such as pin 1. If you did "merge" the grounds, there could be noise voltages forced onto the feedback measurement part of the chip (pin 8 and pin 1) that could make the voltage output a little noisier than what the chip can actually deliver.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.