0R is just to make the connection. i.e a wire link that behaves the same as a wire on the PCB.
1-2R would mean that if there was noise on the star ground due to rectifier currents or even return currents from the output stage. Then the input to output grounds are slightly seperated. i.e the OP ground could move a bit due to large currents on the tracks without upsetting the input ground.
As I said if the amplifier layout is good there should not be any need to do this, but I thought since it was easy to add and you may want to try it out I would put in in.
The best way to see if this works or not would be to do it by listening test since I belive the amplifer will work well without it.
Since you are going to need a PSU you could put it on this PCB, I don't know if you intend to have one PSU for more than one amplifer. If you want to put the PSU on then update your circuit diagram and PCB with the main coupling caps and bridge rectifier. This is a very critical part of the design so you may need further reviews of the PCB.
gootee: You are right since the recifier is not on this PCB the ground returns are less critical. However there will still be some rectifier noise on the local decoupling caps due to the ripple on the main PSU caps so it is just as well to treat them as the main decouplers.
The method used in this design is a star of stars. i.e you group all the similar signals together and try to keep them at equal potential. So all the input signals are grouped together. The amplifer input ground reference is the end of the feedback network and this is grouped with the input filter and input ground referance. Then this group is connected back to the star.
Using a return for all the seperate ground points back to the star will work but as AndrewT pointed out some of those signals don't need to be referanced to the star as much as they need to be referanced to the input ground.
The input filter currents for example should be returned to the input ground as that is their source. i.e any noise filtered off by these caps will flow in the loop from input signal through filter caps and back to the input ground then back down the wire to whatever the noise source was at the other end of the wire. If you connect these to the star ground then the loop area is increased as they have to flow to the star ground and back to the input ground. So more noise is radiated and they might slightly contaminate the star ground (unlikely it would really make much difference but possible).
Regards,
Andrew
1-2R would mean that if there was noise on the star ground due to rectifier currents or even return currents from the output stage. Then the input to output grounds are slightly seperated. i.e the OP ground could move a bit due to large currents on the tracks without upsetting the input ground.
As I said if the amplifier layout is good there should not be any need to do this, but I thought since it was easy to add and you may want to try it out I would put in in.
The best way to see if this works or not would be to do it by listening test since I belive the amplifer will work well without it.
Since you are going to need a PSU you could put it on this PCB, I don't know if you intend to have one PSU for more than one amplifer. If you want to put the PSU on then update your circuit diagram and PCB with the main coupling caps and bridge rectifier. This is a very critical part of the design so you may need further reviews of the PCB.
gootee: You are right since the recifier is not on this PCB the ground returns are less critical. However there will still be some rectifier noise on the local decoupling caps due to the ripple on the main PSU caps so it is just as well to treat them as the main decouplers.
The method used in this design is a star of stars. i.e you group all the similar signals together and try to keep them at equal potential. So all the input signals are grouped together. The amplifer input ground reference is the end of the feedback network and this is grouped with the input filter and input ground referance. Then this group is connected back to the star.
Using a return for all the seperate ground points back to the star will work but as AndrewT pointed out some of those signals don't need to be referanced to the star as much as they need to be referanced to the input ground.
The input filter currents for example should be returned to the input ground as that is their source. i.e any noise filtered off by these caps will flow in the loop from input signal through filter caps and back to the input ground then back down the wire to whatever the noise source was at the other end of the wire. If you connect these to the star ground then the loop area is increased as they have to flow to the star ground and back to the input ground. So more noise is radiated and they might slightly contaminate the star ground (unlikely it would really make much difference but possible).
Regards,
Andrew
gfiandy said:
Hi Andrew,
Thanks for your posts. I have learned some things from them, already.
But, are you saying that it is OK to combine the input section's ground, and the decoupling cap's ground, and the speaker/Zobel's ground, at the local star point, and then have only one ground-return conductor from there to the main star ground point at the power supply?
My suggestions were aimed at using three separate ground-return paths: for the input section's ground reference, for the speaker/Zobel ground-return current, and for the decoupling caps' ground-return currents, each going all the way back to the main star ground point at the power supply (i.e. not meeting at any local star point). Do you think that that is unnecessary?
Sorry completely missunderstood your point thanks for clarifying it. Yes this path is shared and it is not good. Which is why I suggested the PSU should be on the same PCB. However if it is fairly close and if thick wire is used the problem can be minimised for LF large current signals.
Fast transients are likely to flow in the loop with the local decoupling rather than back to the main storgage caps which should solve stability problems. But whatever way you look at it there is a shared path.
I guess I handn't considered a wired star back to the PSU due to the extra complexity but this could be a good solution. I normally just put the PSU on the same PCB so you can define the current paths. I guess this is why AndrewT suggested the resistor to lift the input stage from the return currents.
Regards,
Andrew
Fast transients are likely to flow in the loop with the local decoupling rather than back to the main storgage caps which should solve stability problems. But whatever way you look at it there is a shared path.
I guess I handn't considered a wired star back to the PSU due to the extra complexity but this could be a good solution. I normally just put the PSU on the same PCB so you can define the current paths. I guess this is why AndrewT suggested the resistor to lift the input stage from the return currents.
Regards,
Andrew
Ah. OK. Yes, and that is why I posted the link, in a previous post, to a layout that might solve all of those problems. What do you think of that one?
Here is that link, again:
http://www.diyaudio.com/forums/showthread.php?s=&postid=1387386#post1387386
Post #12, there, has the layout diagrams. And Post #13 has a photo of the finished board.
Here is that link, again:
http://www.diyaudio.com/forums/showthread.php?s=&postid=1387386#post1387386
Post #12, there, has the layout diagrams. And Post #13 has a photo of the finished board.
Hi, Maybee I'm not looking at the right layout but the one shown in post 12 seems to have exactly the same problem in that the path back to the PSU caps that apear to be on another PCB is shared. Did you mean post 1 which shows a seperated path for the input stage, but has other problems.
I think that the post 12 layout has a bit of a problem with the position of the feedback resistor right over the high current power supply feed to the amp. You will probably get away with it but there is definately a risk of parasitic feedback here.
Regards,
ANdrew
I think that the post 12 layout has a bit of a problem with the position of the feedback resistor right over the high current power supply feed to the amp. You will probably get away with it but there is definately a risk of parasitic feedback here.
Regards,
ANdrew
gfiandy said:
Hi Andrew,
There are three diagrams in the image linked from Post #12.
The two smaller ones, on the left, are only the amplifier portion, without the power supply.
The taller PCB pattern, filling the right half of that image, is for both the amplifier and the power supply. That is the one to which I was referring.
The photo, in Post #13, shows the finished result, for two channels.
---
I see your point about the feedback resistor. But that could easily be moved to a somewhat-better location, I guess.
By the way: That layout was not created by me.
Besides the feedback resistor's proximity to the power rails, which I hadn't noticed before, the only possibly-significant helpful changes that I could think of were mainly in the area of tightening-up some things, such as keeping the signal and signal ground traces closer together (and farther from the power rails for as long as possible), trying to get the decoupling caps closer to the chip's power supply pins, and reducing the distance from the power supply to the amp.
danielwritesbac said:
Really? Well, its like 0% harmonic distortion that way.
Oh, I'm sorry. Were you serious?
Or did you mean: "no power supply connected = no distortion" ?
But actually, in that case, if the source was on, then I guess no power = 100% distortion.
Actually, my point was that the power supply is on the same board. And I bet it has a lot less distortion than using a single ground return wire, even though, topologically, they are virtually identical.
Hi again, Sorry again should have looked at the photo as that makes it clearer.
This uses a bit of a brute force method, using alot of copper to try to reduce the impedance between the different parts. However I think it would be better to return the input ground and the power ground to the center point on the main smoothing caps and create a star with a single connection to the thick trace down to the local decoupling caps. This would define the current paths and prevent the output currents sharing a path with the input voltage referance.
Also without the rectifyer bridge on the circuit you could cause problems with the rectifying currents comming to the PCB if the cables arn't kept short and tightly wound together and balanced in length. I would put the rectifier on the PCB so I could balance the current paths and try to shorten the distance from the bulk decouplers to the amplifer. The supply could be fused before the rectifier or not fused at all, the amplfer is protected to some extent byt the sPike protection so fusing shouldn't be needed, this should make it possible to get the parts much closer together.
Having said that I am sure it will work, these amps are fairly forgiving if you have good local decoupling so most solutions will work.
Regards,
Andrew
should have looked at the photo as that makes it clearer.This uses a bit of a brute force method, using alot of copper to try to reduce the impedance between the different parts. However I think it would be better to return the input ground and the power ground to the center point on the main smoothing caps and create a star with a single connection to the thick trace down to the local decoupling caps. This would define the current paths and prevent the output currents sharing a path with the input voltage referance.
Also without the rectifyer bridge on the circuit you could cause problems with the rectifying currents comming to the PCB if the cables arn't kept short and tightly wound together and balanced in length. I would put the rectifier on the PCB so I could balance the current paths and try to shorten the distance from the bulk decouplers to the amplifer. The supply could be fused before the rectifier or not fused at all, the amplfer is protected to some extent byt the sPike protection so fusing shouldn't be needed, this should make it possible to get the parts much closer together.
Having said that I am sure it will work, these amps are fairly forgiving if you have good local decoupling so most solutions will work.
Regards,
Andrew
The other point I should probably make is I normally use double sided PCBs. So I am working a bit outside my normal solution. A double sided PCB enables you to put the +ve and -ve power rails on top of each other, this significantly reduces the high current loop and so reduces any crosstalk from the power rail currents. You can also track the ground close to it an reduce the load return loop as well. However I don't know all the answers and there always seems to be something I haven't taken into account.
Being able to use both sides alows you to slove some of the compromises you have to make with a single sided PCB, like the placemnt of the feedback resistor. I also use SMT parts as their parasitic characteristics are much better and it allows for a smaller tighter design. But this does make, making the PCBs and populating them much more dificult.
Regards,
Andrew
Being able to use both sides alows you to slove some of the compromises you have to make with a single sided PCB, like the placemnt of the feedback resistor. I also use SMT parts as their parasitic characteristics are much better and it allows for a smaller tighter design. But this does make, making the PCBs and populating them much more dificult.
Regards,
Andrew
gfiandy said:Hi again, Sorry again
This uses a bit of a brute force method, using alot of copper to try to reduce the impedance between the different parts. However I think it would be better to return the input ground and the power ground to the center point on the main smoothing caps and create a star with a single connection to the thick trace down to the local decoupling caps. This would define the current paths and prevent the output currents sharing a path with the input voltage referance.
Also without the rectifyer bridge on the circuit you could cause problems with the rectifying currents comming to the PCB if the cables arn't kept short and tightly wound together and balanced in length. I would put the rectifier on the PCB so I could balance the current paths and try to shorten the distance from the bulk decouplers to the amplifer. The supply could be fused before the rectifier or not fused at all, the amplfer is protected to some extent byt the sPike protection so fusing shouldn't be needed, this should make it possible to get the parts much closer together.
Having said that I am sure it will work, these amps are fairly forgiving if you have good local decoupling so most solutions will work.
Regards,
Andrew
Hi Andrew,
Good analysis!
I agree about forming a better-defined star ground point and star ground routing, so the currents have almost no chance to affect the input ground reference. I assume that the speaker/Zobel ground should also be kept separate, until the star point, correct?
Wow! I had been assuming that the rectifier bridge *WAS* on that board!!! I guess I just didn't look closely-enough. Wow. :-o Oh well. That omission could be easily rectified.
)Yeah, I don't like the fuses, there, either. And it could be much more compact, without them.
Just saw your other post: I usually use 2-sided PCBs, too. Many advantages; not many disadvantages that I can think of (except maybe for minor home-fabrication issues), especially with such sparse, small circuits.
Very very thanks to you all I really never thought that the thread will be so big and useful now I have modified my PCB with all of your decisions. I have added two diodes and a MOLEX connector for better flexibility.
Now please read the next...
At first, I thought that I'll use the lm1875 for a centre channel amp and TDA7297 for rear and front channel. NOW, I have changed my decision. I WILL USE FIVE LM1875 FOR FRONT REAR AND CENTER CHANNELs. So, I have to multiply the board into five except the diodes and molex connector. So, I'll made a PCB with five LM1875. you should check it.
Now, Will I have to make five star grounds for each channel and then connect every with a 0 ohm resistance. Please help for finalizing my PCB.
Attachments
Hi,
The diodes you have used will Form a half wave rectifier. You should look up a bridge rectifier which use four diodes and use this solution as it increases efficiency and reduces ripple.
Also you will need much larger smoothing caps to reduce ripple on the supply. I would suggest 4700uF at least. If you are going to run 5 amps from one supply you will need much larger smoothing caps.
Andrew
The diodes you have used will Form a half wave rectifier. You should look up a bridge rectifier which use four diodes and use this solution as it increases efficiency and reduces ripple.
Also you will need much larger smoothing caps to reduce ripple on the supply. I would suggest 4700uF at least. If you are going to run 5 amps from one supply you will need much larger smoothing caps.
Andrew
Hi paswa and others,
I recently finished a LM1875 amp, based on Elliots Project #72 (I think that's what your using too paswa?)
In the thread that you're mentioning Tom I got a lot of feedback from you (and others) and finally came up with this solution:
(See this thread).
It features 3 separate ground return paths; input ground, power ground and speaker/zobel ground. I think Tom would have liked to see the local electrolytics caps even closer to the chip, but still, this solution works really well ( I have rectifyier and 3300uF per rail on another PCB).
At the moment all three ground paths are connected together at the central star ground, but it is nice to have the freedom to reroute them if necessary.
-- hpl
I recently finished a LM1875 amp, based on Elliots Project #72 (I think that's what your using too paswa?)
In the thread that you're mentioning Tom I got a lot of feedback from you (and others) and finally came up with this solution:
An externally hosted image should be here but it was not working when we last tested it.
(See this thread).
It features 3 separate ground return paths; input ground, power ground and speaker/zobel ground. I think Tom would have liked to see the local electrolytics caps even closer to the chip, but still, this solution works really well ( I have rectifyier and 3300uF per rail on another PCB).
At the moment all three ground paths are connected together at the central star ground, but it is nice to have the freedom to reroute them if necessary.
-- hpl
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.