LM2679 power supply

Hey there. I’m developing a power supply board for my robot. I require a 5v and 6v rail with 1A and 4A max respectively. After some consideration I’ve decided to go with an LM2679-ADJ switching regulator to give me the 6v rail, and then that feeds into a 5v LDO giving me my logic power.

Generally I used the examples in the LM2679 documentation to make the circuit, and followed the step by step for selecting components. Some components no longer existed, so I had to make some changes with newer ones. For caps I followed the selection guidelines of 1.3 x the voltage, and an RMS of 1/2 the max amperage. With the inductor technically I only need one output stage 560uf cap, but I put the option in for two. The input cap didn’t really have a guideline to follow so I just chose a 100uf cap with the appropriate ratings.

I’m not sure what wattage R2 & R4 should be rated for.
I’m not sure what ohm R3 should be (current limit) as the datasheet for the switching reg is all over the place on this one. As the reg is rated at 5A but can peak to 7A? It’s all very confusing for a hobbiest.

I’ve made a schematic and marked all the parts down that I’m thinking of using and would like some input to see if I’ve made any gross mistakes or if any of my components are not correct. Or any other general wisdom :slight_smile:

Please note the scanned image has grounds marked with blue. The EDA image has them as rat lines. The whole board will have a ground plane so all those GND nets will be connected that way.

Correction: R2 should be 3.92kohms

Critical parts:
2 x RNS1E101MDN1PH
1 x MSS1210-223MEB
2 x 10SEP560M
1 x MBR735PB
1 x LM2679 ADJ

Resistor powers you simply calculate from I^2 R or V^2/R.

Don't try to go near the limits, be conservative in your design. Near the limit you'll have lots of
issues with cooling and inductor saturation, and all sorts.

Your high current traces in the switching loop need to be nice and wide for current handling and to reduce stray inductance. You need to have much more copper area on the device tabs to heatsink.

The datasheet will probably take a few read-throughs - the current limit is probably for protecting
against inductor saturation (very important), so its value depends on the inductor used I suspect.

MarkT:
Resistor powers you simply calculate from I^2 R or V^2/R.

Don't try to go near the limits, be conservative in your design. Near the limit you'll have lots of
issues with cooling and inductor saturation, and all sorts.

Your high current traces in the switching loop need to be nice and wide for current handling and to reduce stray inductance. You need to have much more copper area on the device tabs to heatsink.

The datasheet will probably take a few read-throughs - the current limit is probably for protecting
against inductor saturation (very important), so its value depends on the inductor used I suspect.

Yea definitely need to increase the trace size. I used some online calculator and it said that .7mm was sufficient (which I currently have) but after looking at other implementations they are all rather large. Do you think increasing them to 2mm will be sufficient? and by switching loop you mean from the switch output of the reg to the inductor to the feedback pin?

Further the resistor wattage, I did actually calculate the wattage but something didn't seem right. Do I use the voltage in or the voltage out of the reg as V? Is 5 amps actually going through it? Because if so, take 1kohm resistor thats sqrt(1/2watt resistor / 1000) which is only 22mA. Now I know I'm doing something wrong... All the examples I see online don't have huge resistors or a bunch of resistors in parallel.

Hi,
I would suggest you beef up ALL your tracks, when you get your PCB made don't forget its copper YOU have bought that is getting etched away.

Each solder pad, has a very small footprint adhering it to the PCB, use decent sizes tracks to help the pads keep a grip.

The 7 traces you have going from the interface pins to the sensor pins, would be better if they were as wide as the solder pads they connect, you have the space.

Any trace that is a gnd, make as wide as possible, even shape it around components.
Any trace that is a supply, as wide as possible, especially around filter caps,

Solder pads are providing a physical/mechanical method of keeping you component on the board, so consider any high profile component.

Can I suggest you look at existing PCBs and how they have layed out tracks and how much copper they keep on their surfaces.

For example;

You layout looks nice and clean, no clutter which is good and you have the space to widen your traces.

Tom.. :slight_smile:

That’s a switching supply! Traces between the key components need to be kept as short as possible, not just thick traces.

Also, where is D1? I see the label, but I don’t see the part or connections to it…

DrAzzy:
That’s a switching supply! Traces between the key components need to be kept as short as possible, not just thick traces.

Also, where is D1? I see the label, but I don’t see the part or connections to it…

D1 is the TO-220-2 shottky package (MBR735PB) next to the inductor. I think all the traces on the switching supply are pretty short given the size of the components… I purposely made the feedback one a little longer since it has to be kept away from the inductor flux as per the documentation.

TomGeorge:
Hi,
I would suggest you beef up ALL your tracks, when you get your PCB made don’t forget its copper YOU have bought that is getting etched away.

Each solder pad, has a very small footprint adhering it to the PCB, use decent sizes tracks to help the pads keep a grip.

The 7 traces you have going from the interface pins to the sensor pins, would be better if they were as wide as the solder pads they connect, you have the space.

Any trace that is a gnd, make as wide as possible, even shape it around components.
Any trace that is a supply, as wide as possible, especially around filter caps,

Solder pads are providing a physical/mechanical method of keeping you component on the board, so consider any high profile component.

Can I suggest you look at existing PCBs and how they have layed out tracks and how much copper they keep on their surfaces.

For example;

You layout looks nice and clean, no clutter which is good and you have the space to widen your traces.

Tom… :slight_smile:

Better? :slight_smile:

alex_fagard:
Yea definitely need to increase the trace size. I used some online calculator and it said that .7mm was sufficient (which I currently have)

You are confused by thinking that wide traces are for current carrying capacity - whereas reducing
stray inductance is usually the more important reason, especially in switch-mode stuff.

Wide as fits, plus a groundplane is what to aim for in a switch-mode supply. General power distribution
traces should be wide for low inductance too, especially between the load and the decoupling for it.

Wide trace = low inductance,
wide trace over groundplane = lowest inductance.

MarkT:
You are confused by thinking that wide traces are for current carrying capacity - whereas reducing
stray inductance is usually the more important reason, especially in switch-mode stuff.

Wide as fits, plus a groundplane is what to aim for in a switch-mode supply. General power distribution
traces should be wide for low inductance too, especially between the load and the decoupling for it.

Wide trace = low inductance,
wide trace over groundplane = lowest inductance.

I read an article from maxim on layout for switch mode power supplies and it echoes what you are saying. it also seemed to discourage using a large groundplane, and instead, stated:

it is best to have the grounds for the reg, output, and input caps short and wide, and isolated from the grounds for the analog stuff like the resistor divider.

https://www.maximintegrated.com/en/app-notes/index.mvp/id/2997

Hi,
OPs PCB


Nice I can see you have done a lot of work and it looks much better, I like the labelling to, its not going to cost you extra for the amount of print overlay.

The tag of the TO-220 will probably be connected to one of its leads, so you will need to not let it touch the gnd plane you have made, unless its the pin that is connected to the gnd plane.

Tom.. :slight_smile: