Buck boost converter confusion / General Science and Electronics / Forums

Forums

4hv.org :: Forums :: General Science and Electronics

« Previous topic | Next topic »

Buck boost converter confusion

previous 1 2 3 4 next

Move Thread

LAN_403

2Spoons

Sat Apr 06 2019, 12:24AM

Registered Member #2939 Joined: Fri Jun 25 2010, 04:25AM
Location:
Posts: 615

For lowest EMI keep the switched node as small as possible. In the application example you posted that would be the junction of M1,M2 and L1.
Also planes are not a panacea for all ills - remember "current flows in loops" so you should always consider the return path of every signal. Sometimes you might want to steer a noisy or large current away from something sensitive, like your current sense amplifier. This can be done by adding slits to the plane in appropriate places.

Inducktion

Sat Apr 06 2019, 12:43AM

Registered Member #3637 Joined: Fri Jan 21 2011, 11:07PM
Location: Buffalo, NY
Posts: 1068

Can you show me an example of what I can do to improve the design?

Does running ground traces around sensitive things help at all?

2Spoons

Sat Apr 06 2019, 02:07AM

Registered Member #2939 Joined: Fri Jun 25 2010, 04:25AM
Location:
Posts: 615

It would help if you post an annotated schematic /pcb so we can see what is where.
The thing to watch out for is the ground plane isn't the same voltage everywhere if there are large currents flowing. So if your feedback needs to be referenced to the 0V leg of the controller chip then your sense amps need to be referenced to that point too, which means you dont want large currents flowing in the copper between the two - you might be better to run a separated ground from the controller to the sense amps.

Running a gnd trace around a sensitive area may be helpful in some cases, but it depends on the nature of the interference you are trying to stop.

Inducktion

Sat Apr 06 2019, 06:12AM

Registered Member #3637 Joined: Fri Jan 21 2011, 11:07PM
Location: Buffalo, NY
Posts: 1068

Here!

I made a schematic and tried annotating the PCB layout a little bit. Link is to a gallery with both shown.

All of the part numbers shown on the schematic image line up with the ones on the PCB; i.e. R5 is R5, C1 is C1, etc.

I know I'm not the best at making schematics so I apologize, but I hope it's readable and understandable.

One other big question, is am I suppose to have my "bulk" capacitance before or after the sense resistor? Or should I realistically have bulk capacitance before AND after?

Additionally, some of the values of components aren't shown; they're likely going to be figured out experimentally.

2Spoons

Sat Apr 06 2019, 09:16AM

Registered Member #2939 Joined: Fri Jun 25 2010, 04:25AM
Location:
Posts: 615

I would put your bulk C before the Isense, otherwise you will be measuring the ripple current from the inductor as well.
Your CV/CC implementation wont work - you have both V and I feedback running to a summing junction - which is not what you want. You need the greater of V or I to control the regulator, not the sum. You need to join the two via precision rectifiers.

I would also allow for a gate resistor on each mosfet - you may not need them, but if you do then having the footprint on the pcb will make life much easier.

You really ought to try simulating the circuit before you build anything. At least do the CC/CV bit.

This is what I mean for the CC/CV combining:

Inducktion

Sat Apr 06 2019, 08:53PM

Registered Member #3637 Joined: Fri Jan 21 2011, 11:07PM
Location: Buffalo, NY
Posts: 1068

Does it need to be a precision rectifier, or would just using two low Vdrop diodes by themselves work?

And I actually do have spaces for gate resistors on two of the fets already, so that's taken care of. I'll add one for the last one too.

And I'll also move the bulk capacitance before the sense resistor.

and I did actually try to do a simulation on LTspice with it, but the output didn't make sense and the entire thing ran INCREDIBLY slowly. It feels very archaic for some reason.

Oh, and should I have the feedback for CV be after or for the sense resistor too? Or does that not overly matter?

Inducktion

Sat Apr 06 2019, 11:24PM

Registered Member #3637 Joined: Fri Jan 21 2011, 11:07PM
Location: Buffalo, NY
Posts: 1068

Updated the PCB. Moved the current sense amp down, farther away from the switching node. Made special care to try to avoid any power ground/signal ground loops with it too.

Added two rectifiers from the CV and CC feedback nodes to the main feedback loop. They're D5 and D7.

Also moved the bulk output cap to a new spot, and added another one for more filtering, and added another plane so the two sides of the PCB conduct current for it.

Added more vias and fixed some layout issues regarding the ground planes; they're more continuous and don't pinch down in any specific spot.

Added a gate resistor to M1.

2Spoons

Sun Apr 07 2019, 01:02AM

Registered Member #2939 Joined: Fri Jun 25 2010, 04:25AM
Location:
Posts: 615

The reason I suggest using a precision rectifier is the temp coefficient of ordinary diodes will screw up your output voltage / current as they heat or cool. A dual opamp for this job is pretty cheap ( it doesn't need to be anything fancy - just unity gain stable) and makes the problem just go away.
I would put Vsense right on the output terminals of your supply, because thats the voltage you are trying to control.

I did a quick and dirty on the power section to show you a more compact way to lay out the heart of the converter. This minimises all the current path lengths, and noisy node areas, and puts all the semis on one side for a single heatsink as suggested by Hen918. The yellow is where the top and bottom layers overlap - its a bit ugly, but you'll get the idea. I haven't tried to route out the gate signals - I wouldn't want to spoil your fun.
I know the sizes of the parts will be wrong but its just conceptual.

Inducktion

Sun Apr 07 2019, 02:18AM

Registered Member #3637 Joined: Fri Jan 21 2011, 11:07PM
Location: Buffalo, NY
Posts: 1068

Ah okay!

That makes sense.

I squeezed in a basic dual op amp right next to the LTC1775;

CqLFnT

Uses an LM2904, really cheap and "internally compensated with unity gain" ? I assume that means it's unity gain stable.

Edit: Just gonna use an LM358 instead. They're a fraction cheaper and from what I read they're unconditionally unity gain stable.

Also uses a really cheap dual common cathode signal diode, so all in all adds a whole 47 cents to the cost. Not bad. If it adds more stability then great.

And I do understand the mounting on one heatsink thing, however I'm kind of smitten with the layout I have... I hope it doesn't cause any issues but we'll see. Plus I actually like being able to use individual heatsinks. I have small ones that work perfectly.

The layout I have is actually pretty similar to the chinese version I'm loosely basing this off of.

2Spoons

Sun Apr 07 2019, 05:28AM

Registered Member #2939 Joined: Fri Jun 25 2010, 04:25AM
Location:
Posts: 615

If you like your layout, then go for it. Engineering is as much art as science.
I'm used to being constrained by things such as budgets or EMC standards, so I tend to optimize for those things automatically - that's what 30 years in the game does to you!

previous 1 2 3 4 next

Moderator(s): Chris Russell, Noelle, Alex, Tesladownunder, Dave Marshall, Dave Billington, Bjørn, Steve Conner, Wolfram, Kizmo, Mads Barnkob