Tough question, and I can argue it either way. Given the low frequencies involved, you don't need a ground plane to insure return currents run parallel and close to their upper traces. You don't have the EMI and loop problems associated with higher frequencies. A ground plane will provide the lowest inductance ground, and helps tremendously with bypassing. OTOH, it can increase stray capacitance to ground through the only so-so dielectric quality of the pcb. It also makes it tougher to insure currents flow where you want them to and circuit blocks don't interact. Even a ground plane has finite resistance. I don't use 'em for audio 99% of the time, but if you tend towards high BW op-amps or unusually high BW discrete designs, there could be benefits. IMO, great amps can be built with or without.
Hi Panson_hk
I would not bother with either ground plane. It is better to direct exclusive ground returns to a specific "low noise" point. This way you can be sure there are no "stray" un-accounted current flows. If you want to; place a thin sheet of metal under the PCB (insulated from the soldered connections and the rest of the case) with a single connection from it to your star ground.
Cheers
Quasi
I would not bother with either ground plane. It is better to direct exclusive ground returns to a specific "low noise" point. This way you can be sure there are no "stray" un-accounted current flows. If you want to; place a thin sheet of metal under the PCB (insulated from the soldered connections and the rest of the case) with a single connection from it to your star ground.
Cheers
Quasi
panson_hk said:
Save your money and go for a single sided PCB.
For audio use, I will agree with Quasi, Hugh and Conrad, you most likely don't need one, and I never put one on the first prototype run of a board. I might add one if I have problems, but they are normally not required, (however, read the component datasheets, some DAC or Class D circuits do require at least a limited GP on part of the board).
Let me dare to say the opposite
If you're skillful enough, you might have good result with single side board. However, too good is never enough. It doesn't hurt to be better.
I always use double-side board, even for prototype board, it's way easier to layout.
But like others have said, stray cap at high impedance point have to be addressed.
If you're skillful enough, you might have good result with single side board. However, too good is never enough. It doesn't hurt to be better.
I always use double-side board, even for prototype board, it's way easier to layout.
But like others have said, stray cap at high impedance point have to be addressed.
Usually, if a circuit is extremely complex, just using a ground plane won't help. It may make the thing even harder to lay out, or you end up with a spidery little bunch of ground plane around all the traces- essentially a randomly wired ground system, rather than a planned one. What is typically done is to go to a 4-layer board. That way you can have your power and ground planes, plus two layers for horizontal and vertical traces. IMO, not really optimal for audio if done in the traditional digital fashion. Good analog design has its own set of requirements unlike just about anything else. The usual way to take care of parasitic capacitance, say around a high value feedback resistor, is to simply void the ground plane underneath the part. Leave a rectangular hole just a bit larger than the part.
Hi,
reading between the lines of this and previous threads on ground planes, I have come to the conclusion that it takes more skill to successfully implement a ground plane than to work without one.
Or put it another way.
If you have to ask, then you don't have the skill to find and eliminate the problems likely to arise as a result of using a badly designed ground plane.
reading between the lines of this and previous threads on ground planes, I have come to the conclusion that it takes more skill to successfully implement a ground plane than to work without one.
Or put it another way.
If you have to ask, then you don't have the skill to find and eliminate the problems likely to arise as a result of using a badly designed ground plane.
A ground plane is really only useful if you're doing controlled impedance work, and that's not gonna happen at audio frequencies.
That said, copper pours are very useful, as they're the lowest impedance way to rout a given net. Same goes with double sided boards - they give you much more opportunity to do a decent low impedance connection, that doesn't snake all over the board. They also allow you to put components on both sides of the board, making the board more compact, again with commensurate gains in connection impedance.
That said, copper pours are very useful, as they're the lowest impedance way to rout a given net. Same goes with double sided boards - they give you much more opportunity to do a decent low impedance connection, that doesn't snake all over the board. They also allow you to put components on both sides of the board, making the board more compact, again with commensurate gains in connection impedance.
All this makes me wonder if I screwed up my latest pcb by adding a ground plane ! It is single sided, but the ground plane was the easiest way to take care of routing the audio ground:
http://www.darkmatter.myby.co.uk/preamp-brd.pdf
and the schematic for those interested
http://www.darkmatter.myby.co.uk/preamp-sch.pdf
The pot is a 100K linear track motorised ALPS potentiometer I salvaged from a mid-80's Pioneer stereo system that the neighbours had thrown away. I plan to use NE5532 for the opamps.
Did I use the ground plane in a Bad Way? I'm still learning how to lay out PCB's well!
http://www.darkmatter.myby.co.uk/preamp-brd.pdf
and the schematic for those interested
http://www.darkmatter.myby.co.uk/preamp-sch.pdf
The pot is a 100K linear track motorised ALPS potentiometer I salvaged from a mid-80's Pioneer stereo system that the neighbours had thrown away. I plan to use NE5532 for the opamps.
Did I use the ground plane in a Bad Way? I'm still learning how to lay out PCB's well!
Hi jaycee
I have done similar in my recent layouts. Try to place all traces on top and a solid ground bottom.
Apart from stray cap, can a ground plane provide protection against interference?
Shall we add a ground (return path) under a high current trace to cancel the generated magnetic field?
panson
I have done similar in my recent layouts. Try to place all traces on top and a solid ground bottom.
Apart from stray cap, can a ground plane provide protection against interference?
Shall we add a ground (return path) under a high current trace to cancel the generated magnetic field?
panson
It is probably well to distinguish "power ground" (the one that cap caps between it and the rails) from "signal return ground" (the one that also can act as a shield to the signal input). In the case of the first, I try to keep it as short as possible taking up little space on the PCB, the leading it away 90 deg from the PCB as quickly as possible and keeping it away from the input signal, etc. I do similarly with the power rails as much as possible.
The quiet ground may have to wander around the PCB. If you limit it so it doesn't get into the output section where there are higher currents, making it copper fill might be OK. (I didn't find it made a noticiible difference but maybe I'm just an insensitive lout.)
The quiet ground may have to wander around the PCB. If you limit it so it doesn't get into the output section where there are higher currents, making it copper fill might be OK. (I didn't find it made a noticiible difference but maybe I'm just an insensitive lout.)
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.