Please critique my PCB design

[darkfenriz]

Hi there

That's my early trial to build a decent self-oscillating PWM amp.
I've designed a rather straightforward PCB so far, but I am not an expert in switching applications.
Any feedback welcome!!
Regards
Adam

[darkfenriz]

Top side ground

[darkfenriz]

And bottom

[darkfenriz]

Is anybody there?

[e_fortier]

Hi,

This is not my cup of tea but it looks like you are missing some info like:

Schematics
Silkscreen

Without these how can someone comment of the PCB layout.

Regards,
Eric

[Eva]

Someone familiar with self oscillating Class D can actually make some comments

- Connections and RF filtering is missing for incoming supply rails.

- Output inductor and capacitor are missing. The switching node is very prone to dV/dt radiation, don't use long wires. Note that you need a very precise sample of the carrier residual from output capacitor at the input of the comparator, so things such as ground loops or long wires are evil. Output capacitor inductance is evil too, self resonance should ideally happen above 1/( twice-the-propagation-delay).

- The inductance from the big electrolytics and the layout will resonate with the SMD ceramics unless you add some smaller electrolytics, whose ESR makes them act as RC dampers (type of capacitor should be found empirically).

- RC snubbers from D to S for damping resonance due to layout and TO-220 inductance and MOSFET die capacitance are missing.

- The inductance from the PCB track that joins the upper source with the lower drain could be reduced. The more inductance, the "stronger" the RC snubbers required and the more heat they dissipate (heat in optimum RC snubbers is directly related to the amount of energy stored in PCB and component parasitics).

[darkfenriz]

Thanks Eva

Great tips from you as usual!

- Connections and RF filtering is missing for incoming supply rails.

Not sure what you mean by RF filtering, will really need a choke at incoming PSU ?

- Output inductor and capacitor are missing.

Inductor is a air core toroid, quite bulky single layer one 40uH, 150mR.
I will connect it between two wire screw clamps as marked at the below image.

- The inductance from the big electrolytics and the layout will resonate with the SMD ceramics unless you add some smaller electrolytics, whose ESR makes them act as RC dampers (type of capacitor should be found empirically).

Yes, well, I will have to experiment a bit. Big electrolytics are planned to be 1500-3300uF high ESR general purpose as an additional filtering. If they make problems I'll throw them away.

- RC snubbers from D to S for damping resonance due to layout and TO-220 inductance and MOSFET die capacitance are missing.

Good comment, thanks for that. At first I was not so sure if I really need snubbers for D-S. Possibly parasitic capacitance from inductor together with output snubber to speaker ground will do
Otherwise I'll experiment with snubbers off the main board. All in all that's a prototype.

- The inductance from the PCB track that joins the upper source with the lower drain could be reduced. The more inductance, the "stronger" the RC snubbers required and the more heat they dissipate (heat in optimum RC snubbers is directly related to the amount of energy stored in PCB and component parasitics).

Corrected that a bit....

Regards
Adam

[darkfenriz]

More about the project...

On the main board there is a IR2110 driving mosfets through ferrite bead (25R/25Mhz;50R/100MHz) and PNP transistor.
Also some positive regulators for driver and for dead time generator both referenced to minus supply.

Input comparator module (installed vertically) will be discrete BJT, basically a long tail pair loaded with current mirror (class AB style).

Comparator output referenced to -V (yes, no level shifters!) drives logic symetrizer/dead time generator (schematic below) already tested and works properly.

Third vertically installed module will be "beta", I would like to test pre and post filter feedback and possibly mixed.

I would like to hear some "good luck" from you

Regards
Adam

[EnvisionAudio]

Originally posted by darkfenriz
Hi there

That's my early trial to build a decent self-oscillating PWM amp.
I've designed a rather straightforward PCB so far, but I am not an expert in switching applications.
Any feedback welcome!!
Regards
Adam

You seem to not be aware of the "polygon" feature of Eagle. Use it to flood the top layer with copper (remember to change the NET name, example N$51 -> GND1).
Then, use TRestrict layer to selectively remove copper.

[darkfenriz]

I've got only top and bottom in "light" edition