Feedback needed on switching regulator PCB layout

[floxia]

Hi there!

I need help to review this PCB layout that utilises a TPS563249DDCR, I am aware that switching regulators work properly only if the PCB layout is correct therefore I would need a feedback on whether I have done something incorrect or missed something.

Datasheet: https://www.ti.com/lit/ds/symlink/tps563249.pdf?ts=1741578606771&ref_url=https%253A%252F%252Fwww.ti.com%252Fproduct%252FTPS563249%252Fpart-details%252FTPS563249DDCR

The circuit will only be needed to step down the voltage from 15V (used for another part of my circuit) to around 6V which will feed a SPX3819M5-L-5-0/TR LDO which controls the logic side of my circuit.

I have used WEBENCH to design the circuit and is as follows:



This is the recommended PCB layout from TI:




This is my circuit and PCB layouts:


Is there anything I have done that does not look correct?
Any feedback will be greatly appreciated!

[PGPG]

whether I have done something incorrect or missed something.

You missed to tell us what current your logic side needs.
If it is few mA than using DCDC instead of liner regulator can be doing something incorrect.

In many my designs supplied by 10V..28V I use linear regulators to get 3V3 for logic side.

[mtwieg]

I'm guessing the board is only two layers?

1. Most important current loop to shrink is the one formed by the input bypass caps and the Vin/GND pins of the chip. Looks like your two input bypass caps are both the same footprint, but have very different values. Best practice is to make the smaller value cap a smaller footprint (like 0402 or 0603) and put it that one as close to the chip as possible. Adding another small cap on the bottom side directly below the GND/VIN pins might help as well.
2. Next important loop is for Cboot. Using a 0402 footprint for Cboot would help. Putting Cboot on the bottom side might help as well.
3. Layout shows a single output bypass cap with a small footprint. Typically the output bypass caps are larger than the input bypass caps.
4. Should shrink the area of the SW node, no reason to have a large shape like that.

Higher res images would help.

[floxia]

Thank you all for the kind replies!

whether I have done something incorrect or missed something.

You missed to tell us what current your logic side needs.
If it is few mA than using DCDC instead of liner regulator can be doing something incorrect.

In many my designs supplied by 10V..28V I use linear regulators to get 3V3 for logic side.

Fair call, my logic side is 5V and the current draw is variable and not below 100mA, I have previously used a LM317 on the same circuit but even with heatsink just gets too hot, and if I feed over 7/8 volts to my LDO that one gets too hot, therefore I can only use a switching regulator.

I'm guessing the board is only two layers?

1. Most important current loop to shrink is the one formed by the input bypass caps and the Vin/GND pins of the chip. Looks like your two input bypass caps are both the same footprint, but have very different values. Best practice is to make the smaller value cap a smaller footprint (like 0402 or 0603) and put it that one as close to the chip as possible. Adding another small cap on the bottom side directly below the GND/VIN pins might help as well.
2. Next important loop is for Cboot. Using a 0402 footprint for Cboot would help. Putting Cboot on the bottom side might help as well.
3. Layout shows a single output bypass cap with a small footprint. Typically the output bypass caps are larger than the input bypass caps.
4. Should shrink the area of the SW node, no reason to have a large shape like that.

Higher res images would help.

Yes two layers.


BOM:

CINX C0805 100nF X7R
CBOOT C0603 100nF X7R
CIN C0805 10uF X5R
COUT C0805 22uF X5R
L1 IND-SMD_L7.1-W6.5 1.5uH 9.4A 9.7mOhm
RFBT R0402 100kΩ 1% 100ppm/C
RFFB R0402 10kΩ 1% 100ppm/C

All the components match the BOM provided by TI except for COUT which was supposed to be 0603, but the supplier does not have one with the right voltage rating so I'm trying to avoid paying extended components fees. Although if that one must be 0603 I will change it to 0603.

I will try to reduce the area of SW node, what would you do just make it slightly larger than the inductor's pad?

Sorry for the low res pics I had not noticed that when uploading them, I have attached new ones.

[Whales]

It's worth mentioning the datasheet section 10.1 Layout Guidelines has a list of important items.

Yes reducing the area of the SW node (between inductor and IC) is important.  If you probe it with an oscilloscope you will find it has the biggest voltage waveform, everything else is smoothed by the capacitors.

I am hesitant to recommend 0402 parts unless you're prepared to work with them   Don't go below 0603 or 0805 if you're hand assembling.

Fair call, my logic side is 5V and the current draw is variable and not below 100mA, I have previously used a LM317 on the same circuit but even with heatsink just gets too hot, and if I feed over 7/8 volts to my LDO that one gets too hot, therefore I can only use a switching regulator.

Can you create the 5V directly with your switching regulator, ie get rid of the LDO?

A 1.4MHz switcher is a reasonably high frequency, and the noise it generates will be multiples (1.4Mhz, 2.8Mhz, etc).  You might find LC filters (or similar) better attenuate these frequencies than most LDOs, as LDOs drop off their ripple rejection at higher frequencies.  This may or may not matter to you, I don't know the rest of your circuit or its application looks like

[floxia]

It's worth mentioning the datasheet section 10.1 Layout Guidelines has a list of important items.

Yes reducing the area of the SW node (between inductor and IC) is important.  If you probe it with an oscilloscope you will find it has the biggest voltage waveform, everything else is smoothed by the capacitors.

I am hesitant to recommend 0402 parts unless you're prepared to work with them   Don't go below 0603 or 0805 if you're hand assembling.

Fair call, my logic side is 5V and the current draw is variable and not below 100mA, I have previously used a LM317 on the same circuit but even with heatsink just gets too hot, and if I feed over 7/8 volts to my LDO that one gets too hot, therefore I can only use a switching regulator.

Can you create the 5V directly with your switching regulator, ie get rid of the LDO?

A 1.4MHz switcher is a reasonably high frequency, and the noise it generates will be multiples (1.4Mhz, 2.8Mhz, etc).  You might find LC filters (or similar) better attenuate these frequencies than most LDOs, as LDOs drop off their ripple rejection at higher frequencies.  This may or may not matter to you, I don't know the rest of your circuit or its application looks like

I will look at making the SW node smaller.

I have tried to replicate the PCB as close as possible as what TI shows in their software as I know that PCB layout matters the most with DC-DC converters.

I am getting the PCB manufactured so I am really not worried about small size components, its more like what kind of components the supplier has in stock so that I do not have to pay of extend components fees. The circuit is just a microcontroller and and ADC converter circuit to read loadcell voltage.

I really will have big issues with noise if I am not careful, in my previous iteration I was happy with the low noise LDO that I used and I am worried that by removing that and just use the switching regulator will mess up everything, I have based my circuit on existing scale indicators that I have seen an none use switching regulators, not sure if I am ready to gamble...

It would make my life so much easier to use one regulator.

[mtwieg]

BOM:

CINX C0805 100nF X7R
CBOOT C0603 100nF X7R
CIN C0805 10uF X5R
COUT C0805 22uF X5R
L1 IND-SMD_L7.1-W6.5 1.5uH 9.4A 9.7mOhm
RFBT R0402 100kΩ 1% 100ppm/C
RFFB R0402 10kΩ 1% 100ppm/C

Ok so you should swap the positions of CIN and CINX, and make CINX a smaller footprint (0603).
No reason to make COUT a smaller footprint. In fact I would add another 0805 in parallel just in case you find that 22uF isn't enough. There's plenty of space available there.
Flipping the inductor polarity may also benefit radiated emissions (depending on how it's constructed). Sounds silly but it's actually a thing. Basically has a similar effect to shrinking the switching node area.

I will try to reduce the area of SW node, what would you do just make it slightly larger than the inductor's pad?

I don't see any reason to make that connection with a shape. Just a trace with the same width as the IC's pad will do. It's a short enough connection that width won't really matter for thermal/efficiency reasons.

Anyways to be honest your layout will likely work fine as-is, I would be shocked if it had any issues passing EMC testing. Though depending on the rest of your application, that may not be the primary concern....

[Wolfram]

The chip you proposed is a synchronous, forced CCM controller rated at 3 A. This means you will have a lot of current ripple in your inductor, much more than your mentioned load current. This drastically reduces efficiency and makes noise and EMI harder to deal with, compared to using a controller that is better sized for the load current you need.

Unlike with linear regulators, overdimensioning switching regulators has some real negative consequences, especially forced CCM contollers.

[mtwieg]

The chip you proposed is a synchronous, forced CCM controller rated at 3 A. This means you will have a lot of current ripple in your inductor, much more than your mentioned load current. This drastically reduces efficiency and makes noise and EMI harder to deal with, compared to using a controller that is better sized for the load current you need.

Unlike with linear regulators, overdimensioning switching regulators has some real negative consequences, especially forced CCM contollers.

Good points, I didn't realize this chip used forced CCM. I would use at least a 3.3uH inductor. Depending on what your intended maximum load current is, may want to go even higher.

[floxia]

The chip you proposed is a synchronous, forced CCM controller rated at 3 A. This means you will have a lot of current ripple in your inductor, much more than your mentioned load current. This drastically reduces efficiency and makes noise and EMI harder to deal with, compared to using a controller that is better sized for the load current you need.

Unlike with linear regulators, overdimensioning switching regulators has some real negative consequences, especially forced CCM contollers.

The chip you proposed is a synchronous, forced CCM controller rated at 3 A. This means you will have a lot of current ripple in your inductor, much more than your mentioned load current. This drastically reduces efficiency and makes noise and EMI harder to deal with, compared to using a controller that is better sized for the load current you need.

Unlike with linear regulators, overdimensioning switching regulators has some real negative consequences, especially forced CCM contollers.

Good points, I didn't realize this chip used forced CCM. I would use at least a 3.3uH inductor. Depending on what your intended maximum load current is, may want to go even higher.

You guys had me thinking, since I am not really familiar with swithching regulators perhaps you have a better chip that I could use to drop 15V to around 6V to feed the LDO, something that won't cause much noise and doesn't require too many components? My current load will be between 100mA to 300mA probably most of the time around 150mA at most.

[Kean]

I cut my DC/DC switching converter "teeth" on the ST Micro L5970D many years back based on designs I inherited from a colleague.  Apart from getting some sensible compensation component values, they were very easy to use, and there were some higher current variants (L5972/5973).

Since then I have dabbled with some TI TPS series parts (e.g. TPS54622, TPS54561, TPS562200) but I was finding that some were really not that robust.  I don't recall exactly which ones caused me grief (it was maybe 5 years ago), but I believe it was a lower current part so probably TPS56 something.  Since I switched to some different TI parts (LMR series) I have had no further issues, so I've just stuck with them.  I'm not saying The TPS56 series parts are inherently problematic, but I had a bad experience and tend to stay away from them.

These days I am doing a lot of mixed mains/battery power designs where the currents are not very high but are quite variable, so I mostly use something like the LMR14006/010, or for a little more current the LMR51420/30.  There are a bunch of footprint compatible parts from TI, Richtek, and others vendors.  The newer parts are synchronous and don't need a flyback diode, but if I have space I leave the diode footprint in case I swap parts for later BOM cost savings or due to part shortages.  The final choice of which one to use will depend on your various constraints of board space, input voltage, output current, and quiescent current, but as long as you have a sensible PCB layout you can swap between a bunch these parts and mainly just need to review the inductor sizing, required capacitance, and feedback resistors (some have different reference voltages).

I also do the occasional design where I know there will only be a handful made, and in those cases I might just drop in a Recom (XP Power/Traco/etc) "7805 replacement" style module.

Anyway there are a ton of devices available.  I almost always have a look in TI Webench for recommendations and simulations, but unless there is specific reason to change I stick with what I know and stock.  It sounds like you are on the right track by using Webench and being open to ask others for suggestions.

[mtwieg]

You guys had me thinking, since I am not really familiar with swithching regulators perhaps you have a better chip that I could use to drop 15V to around 6V to feed the LDO, something that won't cause much noise and doesn't require too many components? My current load will be between 100mA to 300mA probably most of the time around 150mA at most.

There are tons of parts which would probably work fine and be a more comfortable fit for your 300mA max load current. TPS560200 for example. Hard to give very specific recommendations without knowing more about your application.

But with regards to "noise," I'll give my typical advice that a well-implemented SMPS isn't nearly as "noisy" as most people think, and adding an LDO on the output of a SMPS isn't the panacea a lot of people expect it to be. Again, hard to give specific recommendations without knowing more about that application.

[CurtisSeizert]

You may be able to use the same controller with a suitably large inductor to keep the current through it from dropping to zero between cycles. Just make sure the SRF of the inductor is >10x the switching frequency and that you keep the bandwidth of the LC network within the datasheet recommended range.

Paralleling multiple values of low ESR capacitors is best avoided in most cases. It can lead to resonant peaks where the supply impedance is particularly high. It is generally better to parallel multiple of the same value of capacitor to avoid this problem. The ESR of electrolytics is generally high enough to damp this out, so bulk capacitors at a different value shouldn’t cause trouble.

For layout, I don’t have much to add other than to emphasize the importance of keeping the input capacitors in tight to both the Vin and GND pins.

[tooki]

Make sure you consider the effects of DC bias derating in multilayer ceramic capacitors: a 100uF 0805 might only have 10uF of capacitance with 15V applied. It depends a lot on the specific capacitor model, and the effect grows more pronounced the smaller the capacitor gets. Note that this is independent of the capacitor’s voltage rating: in the same series of capacitors, if for example 16V and 25V versions of the same size and capacitance are offered, the 25V one can handle higher voltages, but the capacitance loss at, say, 15V will be the same in both versions.

FYI, WEBENCH takes this into account, so its capacitor recommendations are correct, but apply only to the exact capacitor models used. If you go into the component editor, you can see what effective capacitance the software calculated was needed. (For example, it might calculate that it needs an effective capacitance between 92uF and 137uF, and then selects three 100uF caps whose derated capacitance is each 40uF, giving a total effective capacitance of 120uF.) Sadly, WEBENCH’s component library is a bit outdated and many of the caps it simulates are either NRND, EOL, or no longer available, so its good to know how to size capacitors yourself, especially if you want to use smaller-footprint parts than WEBENCH proposes.