yyes, sry my english its not good enougth, o i mean what i do whit the ground of the entry, how i connect it to the ground of the circuit? whit a capacitor o just in 1 point?
Some update, what do u think now guys?
An externally hosted image should be here but it was not working when we last tested it.
necrofago,
Not too bad.
One probably-significant improvement would be to put the output and Zobel-network ground between the two large electrolytics, because the decoupling caps should usually connect between power pins and load ground.
It should be easy to move C7 toward the left and then turn R7 by 180 degrees, etc. That will also help to make the positive and negative rails closer to the same length, after the large decoupling caps, giving a more-symmetric transient response.
Then you could also make all of the ground plane on the right-most 1/3rd of the board be signal ground.
Regards,
Tom
Not too bad.
One probably-significant improvement would be to put the output and Zobel-network ground between the two large electrolytics, because the decoupling caps should usually connect between power pins and load ground.
It should be easy to move C7 toward the left and then turn R7 by 180 degrees, etc. That will also help to make the positive and negative rails closer to the same length, after the large decoupling caps, giving a more-symmetric transient response.
Then you could also make all of the ground plane on the right-most 1/3rd of the board be signal ground.
Regards,
Tom
Thanks gootee, i migth something like this? or GND Ouput also between C7 and C8?
An externally hosted image should be here but it was not working when we last tested it.
necrofago,
Yes, output ground also between C7 and C8 (or close, and equal distance from both). Sorry, I know that will take a little bit more work. But that's where it should be. (Actually, you will have a lot more layout freedom, with that change.)
I would try to get the Vrail connections for all four of the decoupling caps as close to the chip's Vrail pins as possible, too, and symmetrically distant from them if possible.
But it would be much better to use more than one smaller cap, in parallel, instead of one big one, for each rail. That would make the layout easier, too.
If at all possible, I would use a two-sided PCB, with the top layer as all ground. The connections for the 0.1 uF caps need to be right AT the chip's power pins. And the planar ground would give the lowest inductance and resistance.
The accuracy of the system's transient response (any fast-changing signal currents) will depend on having low-inductance (and low-resistance) decoupling, i.e. very short connection lengths and/or large-size connections to those capacitors, which need to connect between the chip's power pins and the load and power ground.
Big power and ground planes are best, for that. Also, using multiple parallel smaller caps instead of one big one is best for that, with or without planes. (Multiple parallel caps could also make the connection lengths somewhat less critical.)
-----------------------------
See how the music signal IS the capacitor currents:
http://www.diyaudio.com/forums/solid-state/216409-power-supply-resevoir-size-38.html#post3117390
That was showing PSU reservoir caps but the fast transient changes must come from the decoupling caps, near the load, exactly the same way.
The best way to do it would probably be to use a big bank of parallel caps for each rail, like Terry Given suggests, starting at post 1009, here:
http://www.diyaudio.com/forums/power-supplies/216409-power-supply-resevoir-size-101.html#post3154192
Also read more, such as posts 1010, 1016, 1019, 1022, and then also post 1207 (with an example PCB layout) at
http://www.diyaudio.com/forums/power-supplies/216409-power-supply-resevoir-size-121.html#post3166558
and then the second half of post 1214 and all of post 1215, and maybe some others if you still have questions.
Edit: You could put the arrays of decoupling caps on the PCB you are working on in this thread, if you simply used a 2-sided PCB. And that would also enable you to improve a few other minor things in the layout.
Cheers,
Tom
Last edited:
Tom, the power supply for this amp got 10x 1000uf and some ceramic per rail, i think its good enougth.
Ilt ry to move the GND ouput between the caps, but adding more caps in this pcb will be hard cuz the space.
Ilt ry to move the GND ouput between the caps, but adding more caps in this pcb will be hard cuz the space.
Ok, i put 4 more caps, 2 of 1000uf total, and 2 0.1uf smd each, and some rework on layout.
What do u think?
What do u think?
An externally hosted image should be here but it was not working when we last tested it.
It's better. And it's OK.
But if you are feeling motivated, then check the diameter and lead-spacing of 220uF and 330uF and 470 uF caps in that voltage range. If you could replace each (or just one) 1000uF with 2x 470uF, or 3x 330uF, or 5x 220uF, it would be that much better.
You might want to try to pull Cmute in a little. If it's against (or too near) the heatsink, it might age too quickly.
But if you are feeling motivated, then check the diameter and lead-spacing of 220uF and 330uF and 470 uF caps in that voltage range. If you could replace each (or just one) 1000uF with 2x 470uF, or 3x 330uF, or 5x 220uF, it would be that much better.
You might want to try to pull Cmute in a little. If it's against (or too near) the heatsink, it might age too quickly.
Last edited:
Andrew i dont fully understand u my english its not too good.
Tom, ill try to find some smallest capacitor but it ill be hard find good small capacitors, here we got a lot of bad chineese products.
Here is the last pcb whit the Cmute moved were it was at first for anyone who want build this amp, its not tested yet, so check first everything before build it.
Ty Guys for helping me on this pcb.
Tom, ill try to find some smallest capacitor but it ill be hard find good small capacitors, here we got a lot of bad chineese products.
Here is the last pcb whit the Cmute moved were it was at first for anyone who want build this amp, its not tested yet, so check first everything before build it.
Ty Guys for helping me on this pcb.
What do you look for, to find "good" ones? Can you measure ESR of DF? Or do you just go by reputation?
I still say use a 2-sided PCB. The part with the caps won't require extremely-good alignment (which is easy anyway) and the rest can be etched off if you want but I'd use it and re-do the layout. OR, you could just make a separate board or two for the cap arrays, 2-sided. You don't even have to etch the cap array board, except around the holes for one lead of each cap to go through to the other side. So no alignment necessary at all. Other lead of each cap just gets bent and soldered to the surface. A bag of 100uF or 220 uF or 330 uF is probably cheaper than a few big caps, and would work MUCH better. And having so many of them "averages out" any bad ones. And even if all of them were poor quality an array of a lot of them would almost-certainly still be better than a few large good-quality caps. They would also have a lower height, which might help in mounting etc. You could probably even stack two of them and get larger arrays into the same space, over the same part of the main board. Lots of possibilities.
But I guess I would finish what you have, now, first, and then do arrays later, either as a replacement, or an add-on, for the caps on the PCB you have now.
Enjoy.
Saddly i dont got much experience to do a 2-sided pcb thats why i got for a 1 side at first time, and i dont know were to start...
Today my lm3886 have arrived 😀 (and the lm1876 too... which is less powerful and i plan on making a small and pretty 10W@8Ω amp for the miss)
I would expect that so far there would've been a good tried and tested lm3886 pcb, no?
the p2p version that you guys linked to looks good but i am afraid demands delicacy that my butterfingers don't have 🙁
I would expect that so far there would've been a good tried and tested lm3886 pcb, no?
the p2p version that you guys linked to looks good but i am afraid demands delicacy that my butterfingers don't have 🙁
This one is VERY good, as is. The rest of what I have suggested is just like extra icing on a cake. A research project. Go with what necrofago has posted so far. It will be great.
Necrofago, thanks for taking this layout to the next level.
See the pics below to illustrate what Andrew means - you can
allow using different sized capacitors which will make the layout more
flexible.
An externally hosted image should be here but it was not working when we last tested it.
An externally hosted image should be here but it was not working when we last tested it.
Guys, i just build the board in mono stage, and it worked good. Clear sound, no distortions (at least for my ear), sadly i cant test it more in deep today, ill try tomorrow whit the stereo setup.
Just 1 bad thing and its the size of some components, what i have are a little more big than the pcb, but not big deal.
If anyone wanna build this pcb it works rly good.
Cheers.
Just 1 bad thing and its the size of some components, what i have are a little more big than the pcb, but not big deal.
If anyone wanna build this pcb it works rly good.
Cheers.
Great!
Looking forward to the pictures. BTW, there is scope to clean up the power and signal ground traces a bit, but
it dosen't matter too much as those ground areas are filled in correctly when you click on Ratsnest.
Gootee et al - thanks for all the help and handholding you give to folks here, and make this a great forum.
Last edited:
- Status
- Not open for further replies.