The driver transistors are Q501/Q601. I don't see much benefit to move R505-C503-C502 (+49VDC) and R605-C603-C602 (-49VDC) close to the driver Q601. This will only shorter the trace between Q601/Q501 and the resistors/caps. Unless this is your goal advise...
You have placed the driver filter near the PSU input and then run long tracks to the driver collectors. If you run a THICK ground track over the top of the plus and minus track (the overall loop area will now be very small), you can just tap off the associated power supply track and put the filter cap from after the resistor straight to the thick ground track - you will then have reduced the requirement for separate tracks to the drivers. This frees up the space for the thick ground track, and allows you to couple the plus and minus and ground tracks together to reduce radiated noise.
You’ve still got long traces and large loop areas. Look at the power transistor and associated driver on the right. If you just tapped off the main rail to the power devices near the location of the driver, the total rail loop area is greatly reduced. The decoupling/filter cap ground then goes straight onto the main power ground track. The thick ground track is good but you must place the plus and minus tracks directly over this to keep the loop area small. After this part is done, you have to do the output rail which again has to be close to the plus and minus and the ground return.
I think my English comprehension is the culprit here lol
When you write "tapped off", you mean put the power rail connector right close to the driver transistors ?
So each +/- rails connectors should be close to their respective drivers ? Then a ground trace in the center?
When you write "tapped off", you mean put the power rail connector right close to the driver transistors ?
So each +/- rails connectors should be close to their respective drivers ? Then a ground trace in the center?
If you are restarting, see if it is possible to get the outputs nearer to the middle line of the heatsinks instead of being near to the edge !
For R504 / R604 are you expecting huge amounts of RF power for some reason? By rating them at 5W even though they have 47pF in series, this could be a self-fulfilling prophecy. Use a standard 0.25W size, or 1206 SMD, and their parasitic inductance will be much lower, and you will recover some board space.
R503 / R603 a similar thing. A 2W rating seems excessive for supplying current to the MOSFET gate. Maybe they would get warm in some non-musical stress tests, but for daily driving you risk more if they are too big.
R503 / R603 a similar thing. A 2W rating seems excessive for supplying current to the MOSFET gate. Maybe they would get warm in some non-musical stress tests, but for daily driving you risk more if they are too big.
Last edited:
Honestly I dont remember from where I picked those Power rating! Probably a copy/paste of the Zobel Network from the output. P.S. I dont like SMD...
Same remark as above! The original drawing doesn't have specific Power rating...
I use 1210 1 watt SMD resistors for gate/base stoppers. Place the resistor right next to the gate/base so the connection between the resistor and the gate is as short as possible.
Also if there's transition, this could lead to high frequency spikes. This means you will/can have HF (and associated harmonics) flying around your rails. For that reason it's with having the return rail under the signal/supply rails (as design needs). This will provide a low impedance path and reduce high frequency ground loops. This effect can be in effect quite low in frequency:
This is not my image work, and you should read it's source here: https://incompliancemag.com/alternative-paths-of-the-return-current/
Although you should have only low frequency, the effect can start lower than the simulation images (I can't find the research on that). Just be mindful that high frequency and high frequency harmonics may well be following the least impedance rather than resistance. This includes noise and to make it worse - that low impedance path can be through the components themselves rather than the ground plane you assume.
The big takeaway here is the return path is almost always the lowest impedance path at any given frequency. With fast rise time signals (HF in the context we are talking of here), if you don't provide good coupling between the forward and return paths by locating the traces on top of each other, or at the least, side by side, the result is unnecessarily large loop area that will radiate out and couple to other parts of the circuit causing distortion. At low frequencies where the current levels are normally high, there are also problems with radiated noise.
First let me thank you all for all yours advises. I cannot think of a better place here to learn that much 😎
As said above, I am a French language guy and even if I understand pretty well the English language, sometime I don't interpret the right way some sentence. As a good example, with a physical PCB in mind, and I quote :
There I find this confusing as "over" could be interpreted one trace over the other on the same side or on top of it but on another side of the PCB.
So with these advises above, I did another try, by interpreting that "over" could be on top of but on another layer, and that would mean that the ground plane should be on top of the +/- rails on the components side (Blue traces) while the +/- rails would be on the solder side (Red traces). In the picture below, I stretched the right side of the ground plane to illustrate this. Would it be good this way?
Also, because I want to keep the mounting holes as close as possible to the connectors to have a solid mechanical support when the stress would be put on the screws while tightening them instead of having this stress on the transistors soldered pads, I choose to move the Output MOSFETs in the center available holes to also make the NFB trace shorter between them. This as force me to place the +/- rails connectors aside the Driver transistors, that create this traces layout on either side of the center.
Sevy, here is the generalised idea of what you should try to accomplish
Place the V+ and V- on one side of the board. Place the power ground on the other side and make sure the power ground overlaps the V+ and V- if you can. This now gives you the lowest loop area and lowest radiated noise. Run the speaker output rail on top of the 0V rail and ideally next to the V+ and V- rails as shown. Group the power connectors together and place the speaker return on the other side of the main 0V as shown on the board to minimise common impedance coupling which will cause serious distortion problems and noise. Note how the output coil is oriented - the field lines go out the top and return in through the bottom so that the coupling to other parts of the board is minimised. For the front end, place this well away from the power and speaker connections - so in this depiction, on the left side of the board. Importantly, note how the HBR and feedback+gain resistors are grouped and how the feedback trace and small signal front end ground are kept very close together - again, to minimise noise and distortion due to stray EM pickup. As mentioned before, on a double-sided THP PCB, do not be afraid to use links or thin (1mm) single-core insulated cable to make important small signal connections to maximise your chances of getting a good result.
Place the V+ and V- on one side of the board. Place the power ground on the other side and make sure the power ground overlaps the V+ and V- if you can. This now gives you the lowest loop area and lowest radiated noise. Run the speaker output rail on top of the 0V rail and ideally next to the V+ and V- rails as shown. Group the power connectors together and place the speaker return on the other side of the main 0V as shown on the board to minimise common impedance coupling which will cause serious distortion problems and noise. Note how the output coil is oriented - the field lines go out the top and return in through the bottom so that the coupling to other parts of the board is minimised. For the front end, place this well away from the power and speaker connections - so in this depiction, on the left side of the board. Importantly, note how the HBR and feedback+gain resistors are grouped and how the feedback trace and small signal front end ground are kept very close together - again, to minimise noise and distortion due to stray EM pickup. As mentioned before, on a double-sided THP PCB, do not be afraid to use links or thin (1mm) single-core insulated cable to make important small signal connections to maximise your chances of getting a good result.
Isn't important to keep the current path reaching first physically the 1000uF capacitor (C507/607), than to reach the decoupling capacitor 0.1uF (C506/606) then only after that to reach the Drain MOSFET (Q502/602) so the current at the Drain is filtered from noise?
From the drawing you shared, it look's like the capacitors are connected on each side of the Output Transistors, this imply that the path of the rails will reach first the transistor before the capacitor. Isn't risky?
From the drawing you shared, it look's like the capacitors are connected on each side of the Output Transistors, this imply that the path of the rails will reach first the transistor before the capacitor. Isn't risky?
No - what’s important is the bulk decoupling capacitors are located near the mosfet drains and there is a good thick ground connection nearby. Whether the capacitor is either side of the drain for the power levels and track distances involved in this case makes no difference.