The YELLOW color makes it extremely difficult to see! Also, nothing is labeled. A schematic is also needed.
Your 0.1 uF caps are much too far away from the chip pins.
The 1000uF caps are too far away from the chip pins.
Power rails and ground should never have more than the minimum gap between them. I suggest filling ALL open spaces with ground copper, unless you want to spend a lot of time re-routing.
Power rails should be as wide a possible, or at least half as wide as ground rail.
Ground trace is too narrow, in the vertical segment just before it returns to smoothing caps.
Disconnect bottom ground rail from loop, at left end.
The wires connecting the top power rail to the far chip pins might cause noise or hum pickup, since they are not closely paralleled by ground conductors.
Input signal ground must be kept separate from power and all other grounds, all the way back to just after the smoothing caps.
Do you have a center-tapped transformer? If so, the center tap should probably connect at or just before the ground of the first smoothing caps.
I suggest using two stages of smoothing caps. The "star ground" that you need (the one point where the grounds all connect to the chassis) should probably be just after the last set of smoothing caps.
The 0.1 uF caps that parallel the smoothing caps should be removed.
Input signal and input signal ground must have the minimum-possible gap between them, everywhere. It's best to flood the areas around the input conductors and components with the input signal ground copper (while still keeping it separate from all of the rest of the grounds).
It would be better if the two amplifiers were the same distance from the power supply, so they would both see the same power supply and ground rail impedances (which depend on the rail lengths).
Why the 1R that separates the second amp's ground?? It should be removed and the grounds connected fully. (Inpuit signal grounds should remain separate from all other grounds, all the way back to the smoothing caps, anyway. So rather than the 1R, you could just run a wire all the way to just after the smoothing caps.)
There is an acute angle where a smaller ground connects to the larger vertical ground buss, on the left side of each amp. Angles should be 90 degrees or more.
A two-sided board would enable making a much better layout.
Good luck,
Tom
Your 0.1 uF caps are much too far away from the chip pins.
The 1000uF caps are too far away from the chip pins.
Power rails and ground should never have more than the minimum gap between them. I suggest filling ALL open spaces with ground copper, unless you want to spend a lot of time re-routing.
Power rails should be as wide a possible, or at least half as wide as ground rail.
Ground trace is too narrow, in the vertical segment just before it returns to smoothing caps.
Disconnect bottom ground rail from loop, at left end.
The wires connecting the top power rail to the far chip pins might cause noise or hum pickup, since they are not closely paralleled by ground conductors.
Input signal ground must be kept separate from power and all other grounds, all the way back to just after the smoothing caps.
Do you have a center-tapped transformer? If so, the center tap should probably connect at or just before the ground of the first smoothing caps.
I suggest using two stages of smoothing caps. The "star ground" that you need (the one point where the grounds all connect to the chassis) should probably be just after the last set of smoothing caps.
The 0.1 uF caps that parallel the smoothing caps should be removed.
Input signal and input signal ground must have the minimum-possible gap between them, everywhere. It's best to flood the areas around the input conductors and components with the input signal ground copper (while still keeping it separate from all of the rest of the grounds).
It would be better if the two amplifiers were the same distance from the power supply, so they would both see the same power supply and ground rail impedances (which depend on the rail lengths).
Why the 1R that separates the second amp's ground?? It should be removed and the grounds connected fully. (Inpuit signal grounds should remain separate from all other grounds, all the way back to the smoothing caps, anyway. So rather than the 1R, you could just run a wire all the way to just after the smoothing caps.)
There is an acute angle where a smaller ground connects to the larger vertical ground buss, on the left side of each amp. Angles should be 90 degrees or more.
A two-sided board would enable making a much better layout.
Good luck,
Tom
Last edited:
Not a reply to your query, but you might find it easier to modify the Miniref 1.02 schematic and layout posted earlier, to use a single LM4766 instead of the 2x LM1875 it uses now. The miniref already has good ground planes, power and signal isolation.
If you have a source for LM4766s in B'lore, please PM me. I could use about a dozen.
If you have a source for LM4766s in B'lore, please PM me. I could use about a dozen.
You have a thin ground track joining the second amp to the first amp and then to the power supply caps. Ths second amps ground will therfor ne superiposed on any volts drop created by the first amp, better to have each amps returns seperate. A double sided PCB would give you much more scope for a better layout and routing.
Agreed.
At the least, you need to just erase the power supply section and re-do it from scratch. I would change the board shape and put the psu under (or maybe between?) the two amplifiers, so the power and ground connections and their lengths could be much more symmetrical, and shorter, and thicker.
You really DO need a two-sided board.
Also, please research "star grounding".
@gootee, Please check updated layout.
Your 0.1 uF caps are much too far away from the chip pins.
Tried to keep near to the chip pins.
The 1000uF caps are too far away from the chip pins.
Unable to move 1000uf caps near to chip pins. So 10uf added and moved to near the chip pins with 0.1uf ceramic caps.
I suggest using two stages of smoothing caps. The "star ground" that you need (the one point where the grounds all connect to the chassis) should probably be just after the last set of smoothing caps.
Please check the layout for star ground.
Your 0.1 uF caps are much too far away from the chip pins.
Tried to keep near to the chip pins.
The 1000uF caps are too far away from the chip pins.
Unable to move 1000uf caps near to chip pins. So 10uf added and moved to near the chip pins with 0.1uf ceramic caps.
I suggest using two stages of smoothing caps. The "star ground" that you need (the one point where the grounds all connect to the chassis) should probably be just after the last set of smoothing caps.
Please check the layout for star ground.
Look at the PCB in the first post of the thread at
http://www.diyaudio.com/forums/chip-amps/78142-lm4780-ss-pcb.html
It uses a different chip. But do each amp similarly to that one.
If possible, put the two amp layouts side-by-side and put the power supply centered under them.
http://www.diyaudio.com/forums/chip-amps/78142-lm4780-ss-pcb.html
It uses a different chip. But do each amp similarly to that one.
If possible, put the two amp layouts side-by-side and put the power supply centered under them.
You couldn't copy or convert it. I was trying to suggest that you emulate the style and layout characteristics and draw a new layout, that is "similar" to that one, but not exactly the same. Or just study that layout, in order to understand how and why it was done as it was done. I would have added some ground plane around the input signal traces but other than that I think it's a pretty-good layout.
Wow, that is SO much better! Good job!
There are a few changes that need to be made but now we have something much better from which to start.
I need to go find the datasheet and schematic before I can say much more. But I am right in the middle of a network upgrade so my comments and questions might have to be slightly delayed. Sorry.
Turn your caps by 90 degrees, sothe GND pins are facing away from the diodes, run your power direct to the caps. Run the power from E$21 between the pins of E$5. As it is the capacitor return follows a torturous rout around the board and through a high impedance path past the pin of E$20.
Tidy the trace under E$3, currently it is a bad acid trap.
Tidy the trace under E$3, currently it is a bad acid trap.
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.