| svemir |
I have drawn aleph X PCB and I am wondering is it ok? Does it have any mistakes or some bad solutions in the layout!
Schem is taken from: http://www.kk-pcb.com/alephx.html
And here is the layout: |
|
|
| svemir |
| And here is Scheme with component markings! |
|
|
| carpenter |
| Are you mounting your power FETs on the pcb? If not, be sure to locate the gate resistor at the FET, and not on the pcb. |
|
|
| svemir |
| Mosfets are going on the PCB board, thanks for the advace obout Gate resistors but i am allready familiar with that. |
|
|
| Francis_Vaughan |
| Nice layout really. My only criticism is really one that is hard to avoid without a double sided board. The attached pic says it all. |
|
|
| carpenter |
Hi Francis,
I'm not following your idea very well. Care to elaborate further? It seems you're drawing electrical loops, but I can't see what's causing them.
The Aleph X is a balanced circuit, so I assumed that electrons flowed evenly from the negative rail towards the positive. Come to think of it, the left and right portions of the pcb could be 180 degrees out of phase (+ and - input and amplification signals). Is this what causes the loops?
John:) |
|
|
| Francis_Vaughan |
Essentially what I'm trying to show is that as the current is steered about you get changes in the flow though the legs. The run across the middle is the speaker load. What I have drawn is an inaccurate extreme (I was too lazy to depict the remaining current in the active load legs - which is still very large). What it is, is an attempt to depict the dynamic current changes. Mirror image it for the other phase of the input cycle.
What you might get is the output coupling back into the circuitry in the middle of the board - especially if there are any reasonably large area loops.
Ugh, I just realised there is a no-no in there too. The drain resistors of the LTP go to different points on the -ve rail. That rail is going to see currents modulated by the signal on the two sides - just as I drew. The voltage drop (and there will be one even across a few cm of track) will leave a signal dependant voltage between the two halves. This is unlikely to help their tracking. They need a private trace between them, which is then connected top the -ve rail at one point only. |
|
|
| svemir |
Like this.
Should I remove R20/R19 and R36/R35 so they are not on the pcb and put them directly on the Gnd of the power suply central point. |
|
|
| Francis_Vaughan |
Yup. That was what I meant.
The principle is important in general. People worry about star grounds, but forget that any other high current leg with any modulation on it has exactly the same problems - and pretty much the same solution. |
|
|
| svemir |
| Ok board is updated I think. |
|
|
| Francis_Vaughan |
OK, so I see you have decided against the output ground resistors.
Now then, two small further thoughts, and one big question.
You have input and ground pads for both + and - inputs - as if you expect a ground to come with each of the balanced input runs. Which seems odd. Rather I would have thought it should be an input for a single twisted pair - and thus the pads would be closer together - with maybe a single pad for a shield ground - although whether that should actually be connected here is another matter. The pad for the external ground link should probably be a little bigger, just to avoid pain later with soldering and unsoldering.
A bigger one. Having avoided the dangers of the current in the -ve rail we can now see the existence of a clear loop (it was always there but now is a separate element.). The common leg just added, the drain resistors, the connections back thought the LTP. Nice big loop. Low Z too, especially when the MOSFETs get biased up. This will couple to those horrid loops I drew. Need to get those drain resistors close together and reduce the area of the loop.
Now the question. It is nice design, but are you wedded to a single sided board? Or would you consider moving to a double sided board if I could convince you it would help yield a superior technical result? |
|
|
| svemir |
| IŽll stick to the one side board. two extra ground pads are here with no special reason it could be said it is the mistake in drowing. Thank you all for sugestions. |
|
|
| svemir |
| Is this a proper way? |
|
|
| carpenter |
| quote: | Originally posted by Francis_Vaughan
...would you consider moving to a double sided board if I could convince you it would help yield a superior technical result? |
Hello Francis,
I'm not trying to hijack this thread, but hope to gain a bit more information regarding pcb layout.
Would you mind sharing your thoughts regarding the double-sided pcb approach? I'm an absolute fan of double-sided boards and generally (after being enlightened by Magura) prefer to use the bottom of the pcb as a ground plane. I allow any SIGNAL component that requires a lead to ground to pick it up directly at the ground plane. I keep the signal portions of the pcb completely separate from the power components. The power components (power resistors, power FETs, output feeds, etc.) may be on the board, but aren't allowed to draw + or - from the pcb power rails. They, the power components, are wired directly to the power supply.
Your thoughts are greatly appreciated.
John :) |
|
|
| Francis_Vaughan |
I'm not actually convinced by arguments for a ground-plane in an audio amplifier. Ground-planes act in specific ways and you need to balance what is happening carefully. What you describe is actually a good compromise, but probably actually too far the other way.
In general:
The return path for any signal must be kept as close to the signal itself as possible (thus keeping that loop minimised.)
Circuits with high frequency energy - where high frequency really means RF - ground-planes work really well. The return path energy naturally confines itself to that part of the ground-plane directly under the signal trace - naturally confining itself to as small a loop area as possible. As the frequencies drop this effect diminishes. Eventually, at audio frequencies, it becomes quite diffuse. You soon run the risk of large currents in the ground-plane naturally setting up areas of varying voltage across the plane, and thus ruining the very effect you were trying to obtain. (Clearly not allowing any power run to even use a trace on the board helps here.)
Anyway, you asked about my thoughts for a double sided board. Trying to reduce the loop area of the big currents is the main goal. On a single sided board you end up with something like the attached variant. It is clearly hard to manage this - and the sketch is really unworkable anyway due to the need to get the power packages mounted in such a manner that they can reach heat-sinking.
But the idea clearly begins to take form if you put the two power rails over one another. This makes for a realisable package layout and significantly reduces the loop area of the power. It is a pity three layer boards are not viable - as we could get the entire high current system into a thin slab with essentially zero external field. It is still possible to get the speaker leads off the board right after the output resistors and dress them over the power traces - getting back a lot of the effect.
The layout has a further advantage. The initial layout had the power entering and exiting at two widely spaced points. This forces the creation of a large loop. Luckily the Aleph has constant power draw with little to no signal on these supplies, but most common amplifier designs would be spraying energy everywhere with such a power feed. Keeping the loops small allows us to keep them small everywhere. Same comment applies for the speaker connections.
This is where point to point really wins. You have the freedom to work in 3-D. Three high current connectors all in a low area run are trivial. |
|
|
| carpenter |
Thank-you Francis, I enjoyed reading your thoughts on the matter.
:) |
|
|
|
