Buck driver design advice needed

kikkoman · 2019-03-25T21:11:27.000Z

Hmmm the first filter was "more correct" but you have to take the 4k7 into account. So R7 would have to be more like 25k. But you can simplify the thing:

P1 and P2 go to a piezo switch. I will test it how it behaves in pull down way

Ah I see. Is it one of those integrated things that need their own supply? Because those I think exist in several variants like open-drain, open-source (or pnp, npn) etc. that dictate how you have to interface them.

OK apparently that's not the case.

stevetto · 2019-03-25T21:32:16.000Z

kikkoman:

Hmmm the first filter was "more correct" but you have to take the 4k7 into account. So R7 would have to be more like 25k. But you can simplify the thing:

P1 and P2 go to a piezo switch. I will test it how it behaves in pull down way

Ah I see. Is it one of those integrated things that need their own supply? Because those I think exist in several variants like open-drain, open-source (or pnp, npn) etc. that dictate how you have to interface them.

OK apparently that's not the case.

Ok. and I can save some space.

stevetto · 2019-03-26T18:17:42.000Z

Is there any more remark, suggestion regarding to this design?
Otherwise I will start wotking on the pcb.

Thank you in advance.

stevetto · 2019-04-08T18:32:34.000Z

I have replaced the FET and the Schottky diode to the same as used on the GT driver.

And have just finished the pcb design. The high and low current part is separeted to the top and bottom side of the pcb.

The bottom side is quite dense, but the pcb is only 26mm.

kikkoman · 2019-04-08T19:08:43.000Z

No objections so far but these few:
Clearance from components to copper areas looks way too low. (This makes it quite hard to tell what’s going on there.) Those from traces to copper look about right. You should check these values against the PCB manufacturer’s guidelines anyway before submitting.
There’s still a few copper islands that could be removed (e.g. under L1) , and conversely, a few pads could have more copper around them. (B- and L- on the FET side look funny)

And are you sure the LM3409 has a good GND connection? It looks kind of boxed in, and I don’t see any vias to the GND plane on the other side. Can’t hurt (for thermals too!)
edit: the ATTiny GND looks like it goes nowhere too…

stevetto · 2019-04-08T20:00:43.000Z

kikkoman:

No objections so far but these few: Clearance from components to copper areas looks way too low. (This makes it quite hard to tell what’s going on there.) Those from traces to copper look about right. You should check these values against the PCB manufacturer’s guidelines anyway before submitting. There’s still a few copper islands that could be removed (e.g. under L1) , and conversely, a few pads could have more copper around them. (B- and L- on the FET side look funny) And are you sure the LM3409 has a good GND connection? It looks kind of boxed in, and I don’t see any vias to the GND plane on the other side. Can’t hurt (for thermals too!) edit: the ATTiny GND looks like it goes nowhere too…

Thank you. I have increased the clearance to 0.5mm between parts and traces to solid regions. I use easyeda to design and I also order the pcb from them. They offer : min. trace 3.5 mil min. space 3.5 mil Unfortunately I can’t remove islands separately in easyeda, I can remove all or keep all. Or I do not know how to do it. I think LM3409 and attiny GNDs are connected. B- and L- looks strange because I used separate GND for the high and low current side and this is the place where these grounds are joined.

kikkoman · 2019-04-09T10:37:18.000Z

stevetto:

Unfortunately I can’t remove islands separately in easyeda, I can remove all or keep all. Or I do not know how to do it.

Yup, I can’t find that either. Though personally, I’d remove them all and patch up where necessary. (i.e. a GND ring on each side, build up the areas I want with polygons)

I think LM3409 and attiny GNDs are connected. B- and L- looks strange because I used separate GND for the high and low current side and this is the place where these grounds are joined.

OK I can see it now. But now you’ve isolated the FET side outer copper pour from GND entirely , you could easily use that and stitch it with a copious amount of vias to the other side. I also think you could put the central GND point opposite right under (or beside) the LM3409, use both planes (remember the 3409 needs heatsinking too), and you could save yourself a lot of convoluted routing. As long as you avoid thin loops it’s okay.
The way it is now, you have those 2 GND connections snaking around the board forever before they reach the node.

Most important issue last, didn’t spot this before, this need to be fixed first: your input caps belong before the sense resistors, you have them after. I wouldn’t take the chance that this works without regulation issues.
On the topic of resistors: there’s 21, 21.5 and 22 mOhm resistors so you could save some real estate there.

Lexel · 2019-04-09T20:38:28.000Z

strange design
did you consider that the LM3409 also produces some heat?
it has for a reason the colling pad this should contain 4 vias and be thermally bounded to ground on bot sides and this ground should also be connected to drivers rim, you insulated it all the way around

I would put it way closer to the boards edge

also your board has no spring pad, usually this also helps with bypassed spring to absorb some heat from the driver

go with all resistors and the small “no power” caps to 0603 size

use a TO277B diode to save some space

do not insulate battery ground from diver edge ground!

you also have your inductor and switching MOSFET on pretty few copper, no viases to get some heat moved to the other side
same with the reverse diode, for god sake connect that ground there to driver rim for heat sinking, especially with significant higher input voltage than LED there is a lot heat produced by this diode

Lexel · 2019-04-09T22:45:40.000Z

I just made a quick design on 26mm with your via power connection

as you can see there are way more efficient variants to trace such a driver, not your spagetti tracing

tried here to explan the wiring and heatflow

of course there is more potential to get the heat paths better

I looked at your design and direct copper heat transfer is very small

stevetto · 2019-04-10T11:44:00.000Z

Thank you very much for the remarks. I will try to redesign my pcb.
But I have a question again.
I was suggested to separate the GND of the high and low current part of the driver.
My idea was to put all high current parts on side of the driver and low current part on the other and finally I joined the GNDs only at the minus battery terminal.
If I use so many vias on the pcb everywhere I will join the GNDs at several locations earlier and not just at the final step.
In this case does it have any sense to separate them?

stevetto · 2019-04-10T19:01:15.000Z

Modified again:

kikkoman · 2019-04-10T19:16:58.000Z

Looks a lot better. Can’t tell for sure about the µC GND and if it’s connected, do you use nets and ratlines at all? It’s unnecessarily hard without.
And again, do the copper fill last after you have figured out all other traces and copper areas and dimensioned them accordingly. It just gets in the way.

stevetto · 2019-04-10T19:28:31.000Z

kikkoman:

Looks a lot better. Can’t tell for sure about the µC GND and if it’s connected, do you use nets and ratlines at all? It’s unnecessarily hard without.
And again, do the copper fill last after you have figured out all other traces and copper areas and dimensioned them accordingly. It just gets in the way.

All traces are conected.

Lexel · 2019-04-10T19:53:32.000Z

if you look on my design the logic ground splits below the LM3409 from the power ground
and I wrote earlier if you don not do that the LDO might freak out

also putting the battery- and L- apart from the input/output cap is a really bad idea

switching node gets heated by the MOSFET, inductor and diode best is here also put viases into a ground polane on the other side
also as the inductors switching node is already heated by the MOSFET its crucial you spread the heat on L+ making that copper area bigger and also get viases to the other side ground plane

so try to get the back side as less populated as possible

stevetto · 2019-08-26T21:54:41.000Z

I did not have time to finish the LM3409 based driver and wanted to give one more chance for the max 16820.

And I have partial success.

This is the schematics:

(R3 and L1 led dependent, neglect the values on the drawing)

I have build 3 drivers, I only changed the current sense resistor and the inductor.

I have 3 modes, 25%,50% and 100%.

1. XM-L2 3,3V 3A

R3=66mOhm L1=3,3 uH (coilcraft XAL7070 332)

This driver works perfectly in every modes. I can change the input voltage and the led current is stable.

The table below shows led current at different modes and input voltages.

2. XHP50.2 6V 3A

R3=66mOhm L1=8,2 uH (coilcraft XAL6060 822)

It also works, but less stable.

3. XHP70.2 6V 4,8A

R3=43mOhm L1=5,6 uH (coilcraft XAL7070 562)

This is the worst one.

If the input voltage is higher than 7,3V the driver switches off regardless of the mode selected.

L was originally 4,7 uH but replaced by a bigger one to see what happens. Nothing, same behaviour.

I also replaced the current sense resistor by a bigger one (2x 43mOhm in series), but it had also no effect. Switches off at around 7,3V input.

https://imgur.com/a/Py3Z17g

Lexel · 2019-08-27T00:42:17.000Z

also the LM3409 has some drift on different voltages, seems the changing switching frequency also plays a role in this

in my spreadsheet with calculations set with fixed current I see the sense resistor value changing a bit

stevetto · 2019-08-27T07:06:24.000Z

Lexel:

also the LM3409 has some drift on different voltages, seems the changing switching frequency also plays a role in this

in my spreadsheet with calculations set with fixed current I see the sense resistor value changing a bit

I can accept this small instability in led current.

The main problem is that one driver switches off at around 7,4V.
And I do not why.
It seems to me that something resets the driver.
When I connect the input voltage the driver starts in OFF state, there is no memory.
My modes are in ascending order, OFF, 25, 50, 100%
When I increase the input voltage the led goes off at around 7,4V and do not switch on automatically if I decrease the input.
But I can switch it on by pressing the button if the input is low enough.

If the input voltage is above 7,4V the led only flashes one but does not remain in ON state.

Any idea?

stevetto · 2019-08-29T18:39:40.000Z

I have made some measurements with a scope and find the followings: The input voltage (output of the max 16820) measured at the pin 8 of the mcu becomes noisy at 7 volts.

Attiny input at 5V input voltage

pwm signal at 5V input

Attiny input az 7V input voltage

pwm signal at 7V input

Lexel · 2019-08-29T18:48:18.000Z

you are not using a low pass for MCU power supply?

stevetto · 2019-08-29T18:54:56.000Z

Lexel:

you are not using a low pass for MCU power supply?

There is only a 1uF capacitor on the input connected to ground.
The datasheet suggested to use it.

analog.com