Good pcb design

[luka]

Hi

What do I have to watch when making good pcb for ClassD amp?
Loops, ground and where to put (under chips)... that kind of things.

[BWRX]

As with any pcb design, you must be very aware of where currents will be flowing. In the case of a class d amp, the most critical areas are the output stages where there are high voltages and large currents with fast rise and fall times. Grounding, decoupling, keeping loop areas small, keeping sensitive circuitry/traces isolated from potential sources of noise/coupling, etc. all need to be taken into consideration.

Start with a general idea of what board shape/size you want, but do not constrain yourself to set dimensions unless you have to.

Surface mount parts are your friend (and really aren't any harder to solder than through hole parts!).

One layer boards are more difficult to design than two layer boards.

Route the power stage traces first and work backwards (output to input). Power stage traces include VDD, VSS, AND the ground returns!!!

Always be conscious of where ground currents will be flowing if a ground plane is used. Keep low current signal ground currents and ground sense points away from high currents flowing through ground planes.

Don't forget to take part placement into account for proper cooling. For example, TO220 devices will probably need to be attached to a heat sink and are usually positioned at the edge of the board.

There's much more, but that's a start. As has been said many times, pcb design is an exercise in compromise!

[luka]

Hi

Ok I will keep all of this in my mind.
How about placing clock/sawtooth generator under the the comparator that makes PWM? Or should I just put everything on one layer and use other layer ground plane?
Another thing is how/where to connect together power and signal ground and how much apart should they be?
Now I have power coming to amp on each side of the board running almost from start of the board along whole board strait to fets on other side, having logic between them. Is that Ok?
Are only high current with high di/dt problem?

This is how board looks now

[luka]

Hi

And what size of resistors to use. I have experience with SMD's but haven't done any board for myself. Also what else to put in smd, I was thinking of leaving power zener(for +/- voltages for chips) as they are.

[BWRX]

Hi luka. Many questions related to layout depend on other aspects of the design/layout but here are some general answers.

How about placing clock/sawtooth generator under the the comparator that makes PWM?

The quality of the triangle/sawtooth waveform is directly proportional to the quality of the sound. Since this signal is compared to the audio signal you do want it close to the comparator, but you do not want the operation of one component to interfere with the other. For example, do not run the output of the comparator directly next to the input trace carrying the sawtooth waveform or other traces used to generate the sawtooth waveform.

Or should I just put everything on one layer and use other layer ground plane?

You are curently working on a 1 layer design so it may be easier to place all components on one layer and use the other layer as a ground plane. Others have done this with good success. classdfromru has some nice photos of his home etched boards and hand built circuits on his website. If you decide to use one layer as a ground plane remember to think about where ground currents will flow. You don't want a high output current pulse flowing through the same area as a ground sense point.

Another thing is how/where to connect together power and signal ground and how much apart should they be?

Ideally you want power ground and signal ground connected at one point. A good place to do this is near the speaker ground for a single ended design such as yours.

Now I have power coming to amp on each side of the board running almost from start of the board along whole board strait to fets on other side, having logic between them. Is that Ok?

This should be ok. Another good rule to follow is to have power and return traces running side by side, like the two conductors in a speaker cable. And if you must cross power traces with signal traces, cross at 90 degree angles to minimize coupling.

Are only high current with high di/dt problem?

High di/dt and high dV/dt. They often go hand in hand though.

And what size of resistors to use.

Resistor size depends on how much power they will have to dissipate. As far as SMD resistors go, you will generally find that 0603 size resistors will be rated to handle 1/10W, 0805 will be 1/8W, 1206 will be 1/4W, 2010 will be 1/2W, and 2512 will be 1W.

Also what else to put in smd, I was thinking of leaving power zener(for +/- voltages for chips) as they are.

Almost everything is offered in a surface mount package these days. Whether or not you want to use the surface mount version depends on many things: available board space, cooling requirements, cost, rework capabilities, etc.


Also, can you post a schematic of your design?

[luka]

Hi

There it is.

I also have 555 over current limiter on board, not on schema.

[BWRX]

Hi luka. Does the board you have shown in your picture work? If not, what doesn't work?

Also, what is the feedback node connected to? There is only one "FB" label on the schematic.

[luka]

Hi

Sorry my mistake. This FB connects to out, this is post filter feedback. Yes amp works up to around +/-35v signal on output, then is goes crazy and puts +Vcc on output. I asked what could be wrong, and the answer was that it could be bad ground, so pcb badly done. I have +/-0.5v, 250kHz squerewave on supply node of 4060 if I look with scope only for AC signals. This is with no input signal. With input signal, spikes on this node became about +/-4v on top on those 15v even though I have I tantal cap.

[BWRX]

I figured you had used post filter feedback but just wanted to make sure.

That is some really bad ripple on the 15V supply line! Do you see similar ripple on the 10V and 12V supply rails? On the schematic the anodes of the positive regulator zeners and the cathode of the negative reglulator zener are not connected to ground. Are they connected to ground on the board?

The schematic doesn't show it but you should use a larger value electrolytic capacitor on each supply rail near the FETs. It doesn't appear that you are from the pictures. Try using at least 100uF (220uF to 470uF would be better) across each 47V rail close to the output FETs.

[luka]

Hi

Never do things in hury, you will make them wrong. Positive regulator zeners and the cathode of the negative reglulator zener are connected to gnd.

use a larger value electrolytic capacitor on each supply rail near the FETs

You see right. I had no where to put them, so there aren't any. I will put them just to see what will happen to that ripple. Ripple is present on every line, since all of them are elevated xxV from ground. Ground on my board is only about 2cm^2 big, just to have two fastons for supply and speaker