Change Pot in Mini Buck Converter

[rjenkinsgb]

Those inductors look more like RF style, I'd not consider them suitable for a 3A switching power supply. Remember that the main inductor is acting as an energy storage device...

ps. On the circuit board - if you rotated C5 & C7 180', you could eliminate the need for traces on the opposite side.

That would allow a solid ground plane - and then use an array of vias around the ground pin on the IC, to ensure good continuity from there to the rest of the components.
And beef up all the current-carrying tracks!

 

[Diver300]

I would add some ceramic capacitors in parallel with C1 and C2 on the input to the switch. The ESR and inductance of C1 and C2 will lead to voltage spikes as the switching happens, and that can be reduced with some low-ESR capacitors will less inductance.

The same applies to the output capacitors.

The original design seems to use larger value ceramic capacitors. I don't think that you should change to electrolytic capacitors without considering their high-frequency performance.

This is really the point that ThomsCircuit was saying about the ESR of all the big capacitors.

 

[Nigel Goodwin]

I would add some ceramic capacitors in parallel with C1 and C2 on the input to the switch. The ESR and inductance of C1 and C2 will lead to voltage spikes as the switching happens, and that can be reduced with some low-ESR capacitors will less inductance.

You should be aware that adding a ceramic capacitor across the output electrolytic can cause instability (which is why the datasheets generally don't show it). I stuck one across a project of mine, and it completely screwed the power supply up, removing it made it work perfectly.

I agree with rjenkinsb about the inductor, the RF choke he posted the picture of is completely unsuitable.

Here are some I'm playing with at the moment, it's for charging Li-Ion batteries from 12V, the socketed IC is a PIC12F1840 (that does everything), the soldered-in IC is a dual rail-to-rail opamp used to monitor the current and voltage - the test points in the middle are for measuring the outputs of the opamp. The three pin lead feeds an FT232 and connects to a terminal program to display what's going on, and also allows you to make any changes to the charging settings.

The two boards are identical, other than the size of the inductor, evaluating the two coils is the object of the operation, as well as proving the software concept.

​

 

[ThomsCircuit]

Those inductors look more like RF style, I'd not consider them suitable for a 3A switching power supply. Remember that the main inductor is acting as an energy storage device...

So use this type instead.
Can these be soldered with an iron? I do not have a heat gun.

ps. On the circuit board - if you rotated C5 & C7 180', you could eliminate the need for traces on the opposite side.

On this design? I posted two PCB's The first one I posted was suggested that it was poorly laid out. If you wouldn't mind showing me what you mean so i don't get it wrong.
On this board power rails are 25 and signals 15. there will be ground pours on both sides.

Capacitor Type:
A few suggestions about the style of caps im using. The caps i have are (22u / 35v and 47u / 25v) Nichicon. Do you prefer i use something else?

You mention to use an array of vias around the ground pin on the IC, to ensure good continuity from there to the rest of the components. If you could show me what you mean so i can add it properly.

 

[ThomsCircuit]

I would add some ceramic capacitors in parallel with C1 and C2 on the input to the switch. The ESR and inductance of C1 and C2 will lead to voltage spikes as the switching happens, and that can be reduced with some low-ESR capacitors will less inductance.

Im reading about cap types. I understand that in this project low ESR is best. I did not know that electrolytic caps were high ESR. I did find a seller that lists an electrolytic cap as being low ESR but it could not verify it in the datasheet. Ill list it here but ill switch all caps in this project to SMD ceramic caps.

22uF 50V 105C JRB Radial Electrolytic Capacitor​

JB Capacitors | Low ESR | Tolerance: ±20% | Pin Spacing: 2±0.5mm | Tayda
Datasheet

 

[ThomsCircuit]

You should be aware that adding a ceramic capacitor across the output electrolytic can cause instability (which is why the datasheets generally don't show it). I stuck one across a project of mine, and it completely screwed the power supply up, removing it made it work perfectly.

Really like your PCB boards. Nice and neat.
The original designer has a video where he reduces noise by placing a 470uf Electrolytic cap across pin 3 & 4. In his design all his caps are ceramic. I am leaning on changing all caps in this project to ceramic SMD.

 

[Nigel Goodwin]

So use this type instead.
Can these be soldered with an iron? I do not have a heat gun.
View attachment 136122

Yes they can, just needs a little care - the through hole toroidal types are easier though.

 

[Nigel Goodwin]

Im reading about cap types. I understand that in this project low ESR is best. I did not know that electrolytic caps were high ESR.

They aren't, even normal electrolytics are pretty low ESR - but best to use low-esr ones if you can, make sure to use decent quality ones (I like Panasonic or Nichon) - almost all switch-mode PSU faults are down to the use of cheap crappy electrolytics.

 

[rjenkinsgb]

If you wouldn't mind showing me what you mean so i don't get it wrong.

Something like this - the green tracks can then be moved to the other side.

Arrays of VIAs for high current, low impedance or heat transfer though connections; this board has internal ground and power planes which are not selected.

Another example, a small RF board from google images - lines of VIAs to bond the top and bottom layers for low impedance ground around the striplines:

 

[ThomsCircuit]

Yes they can, just needs a little care - the through hole toroidal types are easier though.

Like these. Nice, a bit pricey. Ill get the SMD version, pre solder a slightly modified oversized PCB footprint pad, then apply heat to flow.

 

[Nigel Goodwin]

View attachment 136130
Like these. Nice, a bit pricey. Ill get the SMD version, pre solder a slightly modified oversized PCB footprint pad, then apply heat to flow.

No, those aren't toroidal - those in my pictures above are toroidal.

However, those in your picture work fine, and I've been using then for a while in a number of products we manufacture. The toroids though can handle more power, which is why I'm playing (sorry 'working' ) with them.

BTW, the PCB's of mine above were made by JLCPCB, where I get all my boards manufactured. Takes about a week from order to arrival, depending which day you order, and where the weekend falls. Only drawback is the cost of postage

 

[ThomsCircuit]

BTW, the PCB's of mine above were made by JLCPCB, where I get all my boards manufactured

Cool, That who I use as well.

 

[ThomsCircuit]

Replaced Inductors with SMD. Beefed up tracks. Added ground vias

 

[rjenkinsgb]

Link both inductors directly to C4, and L2 also to C5 (or better, C7), rather than the long track or indirect connections.
The capacitor pins are the "lowest noise" points so you need to minimise track lengths to those, and where possible have in and out connections all to the caps.

Also link all the ground VIAs to the IC ground pin, to be sure they are all seen as the same net.

 

[ChrisP58]

So use this type instead.
Can these be soldered with an iron? I do not have a heat gun.
View attachment 136122

A picture doesn't show any of the important engineering details. Can you provide a part number? Or better yet, a link to it's datasheet?

 

[ThomsCircuit]

A picture doesn't show any of the important engineering details. Can you provide a part number? Or better yet, a link to it's datasheet?

CDRH104RNP-221NC
CDRH104RT125NP-4R7PC

Its an Ebay seller. I know you guys dont like buying components from here but if you dont care for these i can keep looking

 

[Diver300]

You should be aware that adding a ceramic capacitor across the output electrolytic can cause instability (which is why the datasheets generally don't show it). I stuck one across a project of mine, and it completely screwed the power supply up, removing it made it work perfectly.

Was that on a linear regulator or a switch mode regulator?

 

[Diver300]

Im reading about cap types. I understand that in this project low ESR is best. I did not know that electrolytic caps were high ESR. I did find a seller that lists an electrolytic cap as being low ESR but it could not verify it in the datasheet. Ill list it here but ill switch all caps in this project to SMD ceramic caps.

22uF 50V 105C JRB Radial Electrolytic Capacitor​

JB Capacitors | Low ESR | Tolerance: ±20% | Pin Spacing: 2±0.5mm | Tayda
Datasheet

The ESR of electrolytic capacitors is higher than that of ceramic capacitors. Even "low ESR" electrolytic capacitors will have a higher ESR than ceramic capacitors.

The ESR of capacitors isn't always easy to find in datasheets or to compare with other values or other types of component.

In the data sheet that you linked to, the maximum ripple current of those 22uF 35V electrolytic capacitors is quoted as being 35 mA at 120 Hz, with a multiplier of 1.53 at 50 - 100 kHz, so around 50 mA.

This data sheet, https://www.farnell.com/datasheets/2722758.pdf is for a 22uF 35V ceramic capacitors indicates that the capacitor's losses will cause a 10 deg C temperature rise when there is a 3 A ripple current.

Neither of those two figures state the ESR, but the fact that the ripple currents 60 times higher are characterised for the ceramic capacitor would make concerned about swapping to electrolytic capacitors.

For a buck regulator, the input capacitors are where the biggest problem lies. A buck regulator turns the input current on and off, and the inductance of the wires feeding the input will produce big voltage spikes unless there are capacitors to absorb the current, which is why big input capacitors are always fitted. If the wires feeding the regulator are long, the ripple current that the input capacitors are subjected to is approximately the output current of the regulator.

 

[ThomsCircuit]

Link both inductors directly to C4, and L2 also to C5 (or better, C7), rather than the long track or indirect connections.
The capacitor pins are the "lowest noise" points so you need to minimise track lengths to those, and where possible have in and out connections all to the caps.

Also link all the ground VIAs to the IC ground pin, to be sure they are all seen as the same net.

OK I Updated the PCB as directed. Changes to ceramic caps. added vias and connected them to pin4 of IC which is GND.
I made each "VIA" touch each other and the track. LMK if that is how it should be. I DO get design error. "No Spokes" on some of them. Dont know if that's a problem. Seems impossible when there so close to one another. Advise if I need to address this.

 

[ThomsCircuit]

he ESR of electrolytic capacitors is higher than that of ceramic capacitors. Even "low ESR" electrolytic capacitors will have a higher ESR than ceramic capacitors.

The ESR of capacitors isn't always easy to find in datasheets or to compare with other values or other types of component.

In the data sheet that you linked to, the maximum ripple current of those 22uF 35V electrolytic capacitors is quoted as being 35 mA at 120 Hz, with a multiplier of 1.53 at 50 - 100 kHz, so around 50 mA.

I thank you for the formula and the info. It is evident that ceramic is what is needed here. ive updated the project to 0805 style SMDs