Just made PCB layout for single sided LM3886 + power supply 🙂. The circuit is taken from LM4780 data sheet and the parts naming can be refereed to LM4780 Datasheet.
Both the circuits can be easily made on single sided board by DIY laser-toner transfer method
.
PCB and layout is also attached as pdf
Any feedback for improvement is welcome
Both the circuits can be easily made on single sided board by DIY laser-toner transfer method
. PCB and layout is also attached as pdf
Any feedback for improvement is welcome
Attachments
Last edited:
If you're planning to do toner transfer, I suggest beefing up the trace connected to the MUTE pin. It doesn't appear to be more than 8-10 mils wide. At least I have trouble with those tiny traces when doing toner transfer. You have plenty of room. I suggest making it a 15 or 20 mil trace at least.
You don't seem to leave much room for the components. Specifically, Cm is wedged in there and will interfere with the supply cap. The 10R+0.7uH Zobel network will be awkward to fit if it will fit at all. That network is typically built by winding a couple of turns of heavy gauge magnet wire around a 3-5 W power resistor. You'll need to provide space for that.
I suggest using more of a star ground approach as this will cut down hum. Yes! Really! I have measured it and heard it. You could modify your layout fairly easily to accommodate star grounding by having only one ground connection placed right where the ground from the input and feedback come down and meet with the main ground bus. As it is now, the large current spikes charging the supply caps flow right by the very sensitive feedback/input ground. This will induce hum! I guarantee it.
Similarly, I would join the ground for the supply caps on the supply board and bring that common point to the star ground. Grounding is tricky business...
Hope this helps. Good work otherwise. Thanks for sharing!
~Tom
You don't seem to leave much room for the components. Specifically, Cm is wedged in there and will interfere with the supply cap. The 10R+0.7uH Zobel network will be awkward to fit if it will fit at all. That network is typically built by winding a couple of turns of heavy gauge magnet wire around a 3-5 W power resistor. You'll need to provide space for that.
I suggest using more of a star ground approach as this will cut down hum. Yes! Really! I have measured it and heard it. You could modify your layout fairly easily to accommodate star grounding by having only one ground connection placed right where the ground from the input and feedback come down and meet with the main ground bus. As it is now, the large current spikes charging the supply caps flow right by the very sensitive feedback/input ground. This will induce hum! I guarantee it.
Similarly, I would join the ground for the supply caps on the supply board and bring that common point to the star ground. Grounding is tricky business...
Hope this helps. Good work otherwise. Thanks for sharing!
~Tom
The ground copper isn't OK. The signal ground must meet the speaker ground in one point. Now you are going to get currents through the signal ground and this means more hum and possibly more distortion.
it is .4 mm wide and with my toner experiments, i have seen that thinner tracks tends to flat out during pressing and i usually get .5 mm thick track. so its ok. and since there are no much currents flowing, i guess .4-.5 mm is quite good for it.
The output resistor+inductor will be mounted vertically. I tried to optimize its distance from adjoining 1000 muF cap and 2.2R zobal resistor. With vertical mount you will have no problem.
And ya the mute cap is a little offset one, but i didn't want to disturb other components, so the trick is , you solder the mute cap with 3-4 mm above pcb and then slide it to right top corner where it stay as shown in my layout. [/QUOTE]
Ya grounding is a big cat. Here i have already made a small star ground around input signal, Rin and Cl, and then connecting to the main ground plane. Other thing is i am creating the power supply ground in the big ground plane. and connections to both 1000 muF, zobal and pin 7 ina way creates a star grounf only. There is no loop there, which is important.
I have already used same grounding scheme in my Lm4780 PCB, which does not produces any hum or noise.
peranders said:
But i believe that speaker ground should NEVER meet signal ground immediately or with close proximity, coz speaker ground have maximum roughness due to speaker eddy currents and inherent nature of high audio signal current.
And i have already used same grounding scheme in another project without any Hum
Attachments
Last edited:
I'm sorry but you have missed the ground once again. Charge currents from the cap Cs7 passes the signal ground. The signal ground (once again) should meet the speaker ground.
The traces for the signal ground is way too thin. Go for 30-40 mils at least.
The traces for the signal ground is way too thin. Go for 30-40 mils at least.
mmm. Ok, i just take the speaker ground wire from here (shown in pic), i hope this what you are trying to say.
but as a matter of fact in another (LM4780) amp of mine, i have used similar grounding with out any problem
Attachments
Last edited:
I connected my signal ground to board power ground via a 10 ohm resistor. No hum. The speaker ground is connected back to the power supply board which is a star ground.
I wouldn't have the two separate ground tracks on the PSU board. Have one and make the system star point there.
I wouldn't have the two separate ground tracks on the PSU board. Have one and make the system star point there.
yes, i have done the same thing in my earlier project (see the picture in 4# post). This one i have tried something new. i was quite fascinated by BrianGT gainclone design and his carlos power supply. But he has made double sided PCB in a very compact layout and his kit is a reference point.
So in my own DIY way, i have tried to get same layout in single sided including power supply. In fact i want to build the actual prototype and listen to it, but i am quite busy with some other things.
0.4 mm = 15 mil. Yeah, that should be fine. It just looks so skinny on the image.
I have reproduced 0.25 mm (10 mil) traces with toner transfer, but I would not recommend using 10 mil traces on a regular basis if you're using toner transfer.
That'll be a pain if you want to use heavy gauge wire for the inductor part.
Why not rotate it on the PCB and notch the right power bus slightly?
A ground plane is exactly what you DON'T want! And you do NOT have a star ground. What you have done is kept the small ground currents away from the large ground currents - for the most part. This part is good! However, the ripple current through the supply caps will flow right past your input ground. This is NOT good.
First off, repeating a poor practice does not magically turn poor practice into good practice. Secondly, have you looked close enough? I did. See this post as an example of what happens with a poor grounding scheme. Check out the LM3886 grounding thread for how I fixed it. I also used to think that as long as there were no ground loops, everything was good. I have learned through recent experience that this isn't the case and that a good star grounding scheme is the way to go. It would be an easy change on your board so I don't understand your reluctance.
~Tom
New Ground Layout + Ground resistor added
hi, thanks for the feedbacks and i have tried to improve grounding and also added 10 Ohm ground resistor between signal ground path and main ground. Just check this out.
hi, thanks for the feedbacks and i have tried to improve grounding and also added 10 Ohm ground resistor between signal ground path and main ground. Just check this out.
Attachments
Last edited:
Nice. Much better. You might be able to shave a bit off the width of the board by bringing the supply traces in at a 45 degree angle. You could then move the mounting holes down and in. Just a detail.
~Tom
~Tom
First Prototype made
🙂 Just finished one prototype. Will run the amplifier tomorrow. The pads came out to be small and a little trouble with soldering. Will also increase the width to make component layout a little spacious and easy access to audio input and output terminals.
Will update the PCB layout.
More Build pics are here - DIY Audio Amplifier Blog: LM3886 first prototype
🙂 Just finished one prototype. Will run the amplifier tomorrow. The pads came out to be small and a little trouble with soldering. Will also increase the width to make component layout a little spacious and easy access to audio input and output terminals.
Will update the PCB layout.
More Build pics are here - DIY Audio Amplifier Blog: LM3886 first prototype
Attachments
Last edited:
I would like to know if you have the layout as an eagle file.
I think I'll use this simple aproach instead of trying (too hard) to design my own
p.s. sorry for bumping an old thread 😉
I think I'll use this simple aproach instead of trying (too hard) to design my own
p.s. sorry for bumping an old thread 😉
the + & - rails are too far apart.
They will act like an aerial and emit radiation into all the circuits nearby.
Small loop area for circuiting currents is a must.
Since the rails carry half wave rectified copies of the output AC then the power ground must also be included in the small loop area giving a triplet for the cable to the amp and for the traces on the PCB.
They will act like an aerial and emit radiation into all the circuits nearby.
Small loop area for circuiting currents is a must.
Since the rails carry half wave rectified copies of the output AC then the power ground must also be included in the small loop area giving a triplet for the cable to the amp and for the traces on the PCB.
Hey there Andrew,
This is approaching paranoia. AC components on the power rails will be in the audio spectrum mostly, fairly low in amplitude, and sinusoidal. I don't think radiated emissions are much of a concern here.
'looks like a nice layout!
Jim
Ya, its working fine, but i am not using it currently. i already have a LM4780 setup.
Would you like to make it yourself
Last edited:
sorry for the late reply... i just saw it today only.
i don't have eagle layout as i use autocad. But you can have true size PCB layout in pdf format from my blog.
- Status
- Not open for further replies.