Board Design For STK4040

[aged one]

Hello all

Would you assist me in designing a suitable board for the schematic located at www.users.otenet.gr/~athsam/power_ampl_stk.htm?

I have made several attempts, but they all violate the rules I have read in these threads (grounding, etc).

[aged one]

Oops......The schematic is located at users.otenet.gr/~athsam/power_ampl_stk.htm......sorry for the error.

[aged one]

OK then.......maybe you would comment on my board design?

[carlmart]

It looks OK to me.


Carlos

[dhesing]

it is simple and clear.

[Nostradamus]

hii
this pcb and circuit diagram is it available STK 4040 II ...

[gootee]

I see a few issues that should be improved:

Feedback loop should be made as short as possible, with R9 as close to pin 2 as possible.

All other loops should be as small as possible, enclosing the least possible area.

Capacitors should be as close to chip pins as possible, especially the ones for the power supply pins (C3, C6, C9, C12). Any resistors (or capacitors) that connect to chip pins should be placed right at the pins, or as close as possible. (Place the components first. Then route the traces.)

On the schematic, the ground (0 V) should be cut, just to the left of C12, and the whole "input ground" portion (C1, R2, C13) should have its own separate conductor back to the star ground (stub off of trace between filter caps' gnds in power supply).

On the schematic, the 0V should be cut just below J4 and the "output ground" portion should be wired separately back to the star ground (C8 and speaker ground/J4).

The remaining ground connections should then have a third separate conductor back to the star ground in the power supply (not sure about R10/pin 3 gnd), twisted tightly together with the power + and - wires. Since the board is 2-sided, use a ground plane for those remaining grounds, extending under everything except the input area and the speaker output/zobel areas. That would make the layout MUCH better.

And use a separate section of ground plane for the input signal ground area, extending under all input signal- and ground-connected components. Signal and signal ground inputs should be tightly twisted together all the way to the input jack and the jack should not be grounded. (Alternatively, connect the two jacks' grounds and run a single wire from there to the star ground, and then don't run anything from the pcb input ground area to the star (or to any other) ground.) In any case, the input jacks should be isolated/insulated from the chassis. If shielded twisted pair is used from the jacks to the pcb, the shield should NOT connect to any parts of the input jack, only to the chassis gnd, and should not be connected to anything on the pcb end.

Input signal and input gnd traces should be kept as close together as possible, everywhere. But it would be even better to just use a ground plane, there, on the other side of the board.

Power and output traces should be wider. Ground traces for power and output should be much wider. Use ground planes on bottom of board.

[gootee]

Oops. When I said "bottom of the board", for the ground plane, I meant to say "top". The ground planes would be on the TOP side of the board, for a 2-sided board.

Note that you would have to put trace stubs on the bottom to get out from under flush-mounted components like capacitors with ground pins that needed to be soldered to the top layer, and then solder short pieces of bare wire in the stubs' pads to connect the bottom and top layers (like "vias"), for those types of components. But designing the layout would still be much easier, and it would function much better.

[danielwritesbac]

Ah, well in trying to attach parts to the chip, I got carried away. . .

[danielwritesbac]

The work done above uses the cheats of gel flux and 63/37 solder (notice the big shine on all solder joints because of avoiding 60/40). Although the above is a fair tangle, maybe there is a midway solution. . .

If given the luxury of a circuit board and the simplicity of the monophonic chip, it should be possible to fit all small signal components onto the chip and thus the circuit board doesn't have run power all over small signal.

The big blue chunk up there that filled up the working space too much, is a speaker output component, aka technically a "power" member. It probably should have gone onto the circuit board along with all of the larger power components. Further relief from using the less complicated monophonic chip would then have this job done in minutes. If the pins happen to hang down below the heatsink level, that would increase usable working area and be even easier.

As for installing a good quality discrete amp into a tiny little black box, it seems that STK did a very nice job.