3.4V to 12V Boost Convert PCB Review

[Viiux]

Hi everyone,

I’m an electrical engineering college student and this is my second attempt at making a PCB. This is mostly for fun and as a learning experience.
 
I created a 2-layer 3.4/4.2V to 12V Boost Converter using the LM3478. I tried to follow the TI-datasheet/we-bench power designer and evaluation module datasheet/layout as best as I could.

Vin: 3.4-4.2 V
Vout: 12 V
Iout: 1 A

A few questions:

• Every article I read about talks about return currents. I made a big ground pour on the top layer and have all my grounds connected to it. Should I instead individually route grounds?
• I only have 2 signals on the bottom layer. Should I add a ground pour to the rest of the layer?
  
• The diode recommended by WeBench Designer has Io = 2A. The diode I have in my schematic and from the evaluation board has Io = 3A. I want Iout to be 1A. I calculated that the max current to be around 3.7A. Is the diode I have, okay?
• I calculated the inductance for the inductor to be .68uH. WeBench recommended 4.7uH and the evaluation board has 1.8uH. I picked 10uH. Is there a downside to having a bigger inductor besides space/size?

I’m still also learning Altium so if there are any best practices for PCB lay-outing or Schematics, I would appreciate any feedback/advice.

Thank you!

[NiHaoMike]

The pads should have solid connections to the rest of the board. Probably not going to make too much a difference for a 1A converter, but still good practice for power electronics.

I would also add more spots for input and output caps since you have the space, you can always leave them empty if it turns out you don't need them.

The copper area of the COMP pin is bigger than necessary, it looks trivial to pack the components a bit tighter in that area to minimize the area and avoid picking up noise.

[Viiux]

The pads should have solid connections to the rest of the board. Probably not going to make too much a difference for a 1A converter, but still good practice for power electronics.

I'm a little confused on which pads? I removed the thermal reliefs on certain pads but I've heard that increases difficulty soldering the components.

I added extra input and output caps and decreased the copper area with COMP Pin. Is it better to route the traces individually or is the polygon pour acceptable?

I also realized the drain on the MOSFET wasn't connected to the polygon pour.

Thank you!

[Picuino]

My calculations are like this:

Vin_min = 3.4V
Vout =  12 V
Iout = 1 A
L = 10uH

P_out = 12 W
Performance = 0.8 (Estimation)

P_in = 12W / 0.8 = 15 W
I_in_mean =  15W / 3.4V = 4.4 A

Duty cicle
V_in * D = (V_out + Vf) (1 - D)  --> D = (V_out + Vf) / (V_in + V_out + Vf)
D = (12 + 0.32) / (3.4 + 12 + 0.32) = 78%

I_ripple = V_in * D / ( f * L) = 3.4 * 0.78 / (540kHz * 10uH) = 0.49 A

I_in_max = I_L_max = I_in_mean + I_ripple / 2 = 4.4A + 0.25A = 4.65 A

The coil should be able to withstand 5 peak amps.



The same calculations for a 2.2uH coil:
Vin_min = 3.4V
Vout =  12 V
Iout = 1 A
L = 2.2uH

I_ripple = V_in * D / ( f * L ) = 3.4 * 0.78 / (540kHz * 2.2uH) = 2.23 A

I_in_max = I_L_max = I_in_mean + I_ripple / 2 = 5.5 A

The coil should be able to withstand 6 peak amps. And it will be smaller than the previous coil


Edit:
You can estimate the volume of the coil with the maximum energy stored:
E = I^2 · L / 2
10uH 5A coil:  E = 5^2 · 10u / 2 = 125uJ
2.2uH 6A coil:  E = 6^2 · 2.2u / 2 = 40uJ  (3 times smaller)

[Picuino]

Diode: https://assets.nexperia.com/documents/data-sheet/PMEG3030EP.pdf

Circuit Average forward current I_F = 1A
Diode Max Average forward current I_F = 3 A (Enought)

Circuit total Power dissipation = Vf * I_F = 0.32V * 1A = 0.32W
Circuit total Power dissipation = 0.25 W (According graphs)

Diode Max power dissipation = 1.05 W  (Enought)

[mariush]

In my opinion you have too big of a loop where you have the inductor and the mosfet. Maybe rotate the mosfet 90 degrees to the right, bring u1 higher , shift C8 and R1 to the right a bit...

I'm really against those surface mount capacitors like C1 ... especially if it's electrolytic and not polymer.  As your input voltage is up to around 4.2v you can easily get some aluminum polymer capacitor .. example : https://www.digikey.com/en/products/detail/murata-electronics/ECASD40J157M015K00/10413839

They're a bit more expensive but useful if you need low profile.  There's also tantalum-polymer capacitors you could use : https://www.digikey.com/short/p91cjd44

Not so sure how useful those C2 and C9 capacitors would be in that footprint ... you have them at 47uF that's kind of a big value for a ceramic, and if the voltage rating is low, you won't get that capacitance in circuit .. see bias voltage and other stuff : https://www.maximintegrated.com/en/design/technical-documents/tutorials/5/5527.html

No idea why you think you need a via and trace on the back to the gate of mosfet, you could probably route it under the U1 chip and have it come out directly up after you rotate the mosfet 90 degree clockwise.

C5 and C6 ... why the different footprints, why one is so small and the other so big... you telling me you have a hard time finding both 1nF and 22nF in 0402 or 0603 ?
There's 2000 1nF (1000pF) ceramic capacitors in stock on Digikey , 1700+  x5r/x7r/c0g/np0  ... 235 in 0402  and 356 in 0603
There's 908 22nF (0.022uF) ceramic capacitors in stock on Digikey, with above temp coefficient, 110 in 0402 footprint and 158 in 0603

And I really don't see why you'd have to use a small via to for the sensing

You may also want to use 2 resistor footprints in parallel for R3  - if you have a hard time finding exactly 8.45 kOhm, you may be able to parallel  120 kOhm and 9.1 kOhm (both R24 series values) to get 8458 ohm , which would be close enough for your needs.
Or pick a slightly different value for R6 to get some more sane value.

[NiHaoMike]

I'm a little confused on which pads? I removed the thermal reliefs on certain pads but I've heard that increases difficulty soldering the components.

All the ones that deal with high current and/or high frequency. In power electronics, that means the power path (don't forget that the ground is part of the path!) as well as the ground connection to the controller. You will want a decent soldering iron for working on power electronics, something like a TS-100 would be good. The thermal isolation that allows a cheaper soldering iron to be usable adds electrical resistance as well as thermal resistance, very undesirable in power electronics.

I added extra input and output caps and decreased the copper area with COMP Pin. Is it better to route the traces individually or is the polygon pour acceptable?

Just a regular trace is ideal. Note that you can also swap the locations of R4 and C6 if that would make things easier, it would be electrically the same.

[Picuino]

Datasheet: https://www.ti.com/lit/ds/snvs085x/snvs085x.pdf
Vout = 12V
Vreference = 1.26V

Program:

Code: (Python) [Select]

r24 = [1.0,1.1,1.2,1.3,1.5,1.6,1.8,2.0,2.2,2.4,2.7,3.0,3.3,3.6,3.9,4.3,4.7,5.1,5.6,6.2,6.8,7.5,8.2,9.1]
r24 = [r for r in r24] + [10*r for r in r24]

vout_searched = 12
error = 0.1

for r3 in r24:
    for r6 in r24:
        vout = (1.26 / r3) * (r3 + r6)
        if vout < vout_searched + error and vout > vout_searched - error:
            print(f"r3={r3}  r6={r6}  vout={vout:4.3f}")

Result:
r3=1.3  r6=11.0  vout=11.922
r3=3.9  r6=33.0  vout=11.922

[Viiux]

The coil should be able to withstand 5 peak amps.

Thank you for verifying the calculations! So the coil I have right now is rated for 5.2A. I'll stick to the 10uH one for right now.

In my opinion you have too big of a loop where you have the inductor and the mosfet. Maybe rotate the mosfet 90 degrees to the right, bring u1 higher , shift C8 and R1 to the right a bit...

I'm really against those surface mount capacitors like C1 ... especially if it's electrolytic and not polymer.  As your input voltage is up to around 4.2v you can easily get some aluminum polymer capacitor .. example : https://www.digikey.com/en/products/detail/murata-electronics/ECASD40J157M015K00/10413839

They're a bit more expensive but useful if you need low profile.  There's also tantalum-polymer capacitors you could use : https://www.digikey.com/short/p91cjd44

Not so sure how useful those C2 and C9 capacitors would be in that footprint ... you have them at 47uF that's kind of a big value for a ceramic, and if the voltage rating is low, you won't get that capacitance in circuit .. see bias voltage and other stuff : https://www.maximintegrated.com/en/design/technical-documents/tutorials/5/5527.html

No idea why you think you need a via and trace on the back to the gate of mosfet, you could probably route it under the U1 chip and have it come out directly up after you rotate the mosfet 90 degree clockwise.

C5 and C6 ... why the different footprints, why one is so small and the other so big... you telling me you have a hard time finding both 1nF and 22nF in 0402 or 0603 ?
There's 2000 1nF (1000pF) ceramic capacitors in stock on Digikey , 1700+  x5r/x7r/c0g/np0  ... 235 in 0402  and 356 in 0603
There's 908 22nF (0.022uF) ceramic capacitors in stock on Digikey, with above temp coefficient, 110 in 0402 footprint and 158 in 0603

And I really don't see why you'd have to use a small via to for the sensing

You may also want to use 2 resistor footprints in parallel for R3  - if you have a hard time finding exactly 8.45 kOhm, you may be able to parallel  120 kOhm and 9.1 kOhm (both R24 series values) to get 8458 ohm , which would be close enough for your needs.
Or pick a slightly different value for R6 to get some more sane value.

Thank you for the feedback. I decreased the area between the inductor and MOSFET and diode. I also switched out the input capacitor C1 and changed the 47uF caps to 10uF.
You're right I can definitely make everything on one layer without using vias. I ended switching all the components that I can to 0805 footprints.

All the ones that deal with high current and/or high frequency. In power electronics, that means the power path (don't forget that the ground is part of the path!) as well as the ground connection to the controller. You will want a decent soldering iron for working on power electronics, something like a TS-100 would be good. The thermal isolation that allows a cheaper soldering iron to be usable adds electrical resistance as well as thermal resistance, very undesirable in power electronics.

Thank you! I removed the thermal relief from all the high current paths.

Result:
r3=1.3  r6=11.0  vout=11.922
r3=3.9  r6=33.0  vout=11.922

Thank you, I switched out the 8.45k and 1k resistors for 3.9K and 33K. I ended up switching out all resistor values so they are all E24 series.


I attached pictures of the updated schematic/board.

Question:
Since I don't have anything on the bottom layer, should I make it a ground plane? Or does it not make a difference.

[Picuino]

Sorry, I have toggled resistors r3 and r6 inadvertently.
The correct result is:
r3=33.0
r6=3.9 


And corrected Python code:

Code: (Python) [Select]

r24 = [1.0, 1.1, 1.2, 1.3, 1.5, 1.6, 1.8, 2.0,
       2.2, 2.4, 2.7, 3.0, 3.3, 3.6, 3.9, 4.3,
       4.7, 5.1, 5.6, 6.2, 6.8, 7.5, 8.2, 9.1]
r24 = [r for r in r24] + [10*r for r in r24]

vout_searched = 12
error = 0.1

for r3 in r24:
    for r6 in r24:
        vout = (1.26 / r6) * (r3 + r6)
        if vout < vout_searched + error and vout > vout_searched - error:
            print(f"r3={r3}  r6={r6}  vout={vout:4.2f}")

[Picuino]

Question:
Since I don't have anything on the bottom layer, should I make it a ground plane? Or does it not make a difference.

Yes, and you must join together both ground planes with multiple vias.

[mariush]

Looks much better to me but I'm by no means an expert.

One thing that's a concern is how you handle what's under the mosfet ... I think the mosfet has a bottom pad which is connected to the drain pins, so you'll probably want to extend that middle area (where the inductor, mosfet and diode are soldered to) so that the exposed pad is also part of that.
You should also figure out what's up with that island of ground pour right where the C8 text is printed ... there's a tiny sliver of copper between the two pins of the chip which then connects to that area.. you can probably get rid of that.

I also don't like how the trace going to the gate cuts that ground fill (where the C8 text is printed on) cuts that ground. There's really no point in going diagonal with that trace. I'd just make a nice small 45 degree bend and then go straight up until trace comes out from under the chip and then either use vias to jump near the gate of mosfet on the other side,

Also not a fan of the thin vsense via breaking the ground and causing all the stuff to the left of U1 to connect to ground through that thin trace under the R3 resistor
 
Here's a mockup of how I would attempt to do it ... probably screwed up a trace because of my lousy paint skills and there's a via used so I won't break that ground to the left of R7

[Viiux]

Sorry, I have toggled resistors r3 and r6 inadvertently.
The correct result is:
r3=33.0
r6=3.9 

Opps, I didn't catch that either, thank you! I fixed it on schematic/layout.

Looks much better to me but I'm by no means an expert.

One thing that's a concern is how you handle what's under the mosfet ... I think the mosfet has a bottom pad which is connected to the drain pins, so you'll probably want to extend that middle area (where the inductor, mosfet and diode are soldered to) so that the exposed pad is also part of that.
You should also figure out what's up with that island of ground pour right where the C8 text is printed ... there's a tiny sliver of copper between the two pins of the chip which then connects to that area.. you can probably get rid of that.

I also don't like how the trace going to the gate cuts that ground fill (where the C8 text is printed on) cuts that ground. There's really no point in going diagonal with that trace. I'd just make a nice small 45 degree bend and then go straight up until trace comes out from under the chip and then either use vias to jump near the gate of mosfet on the other side,

Also not a fan of the thin vsense via breaking the ground and causing all the stuff to the left of U1 to connect to ground through that thin trace under the R3 resistor
 
Here's a mockup of how I would attempt to do it ... probably screwed up a trace because of my lousy paint skills and there's a via used so I won't break that ground to the left of R7

Thank you! I think I have the drain pins on the MOSFET connected to the drain polygon pour already.
I tried to remove the small ground islands. I rearranged the components so the grounds are more solidly connected.

I also added stitching vias to connect the GND from the bottom layer. I used the default settings on the Altium Stitching Via tool, so I'm not sure if it's too much.

[NiHaoMike]

Remove the thermal isolation on the vias, they're not supposed to be soldered so they would serve no purpose. Also put some on the other side of the break in the ground plane.

[Viiux]

Remove the thermal isolation on the vias, they're not supposed to be soldered so they would serve no purpose. Also put some on the other side of the break in the ground plane.

Thank you. I ended up shifting the feedback via a little more so I could add two columns of ground stitching vias. I wasn't sure how the silkscreen text was going to interact with the vias so I tried to avoid any overlap with them.

I think I'm going to order this revision of the board and I'll post an update once I get it. Thank you everyone for your feedback!

[mariush]

Looking at the feedback, I think you printed R3 and R6 incorrectly.  In your last schematic picture, R3 was between output and the feedback pin.

I was looking at that because I was going to suggest adding a trimpot or resistor footprint in parallel with the R3 resistor (output - feedback), for minor tweaks on the feedback voltage.

For example, it may just happen the chip's voltage reference is on the low side (ex 1.25v instead of 1.26v) and if your two resistors are already chosen for 11.92v, your output voltage may end up too low.

Or you may want to output slightly more than 12v, to account for voltage drop on the cables... ex output 12.1v to get 12v at the connector.

For example, you could replace R3 with a 4.7k resistor and parallel a 47k trimpot  - the middle of the trimpot should give you around 3900 ohm (ex. 4700 ohm and 23k gives you 3902 ohm)