• WARNING: Tube/Valve amplifiers use potentially LETHAL HIGH VOLTAGES.
    Building, troubleshooting and testing of these amplifiers should only be
    performed by someone who is thoroughly familiar with
    the safety precautions around high voltages.

PC board design for PSE amp

Hi,

I want to design a PCB for my PSE amp. Simple circuit, one paralleled driver tube with CCS connected to two paralleled pentodes. I've done a few PCBs in the way past for digital I/O and such but never audio.

Can some of you folks offer advice for what my concerns should be related to signal and power routing?

Is it best to plan on hard wiring the filaments and keep them off the board?

Is it best to have a separate board for the power supply?

Maybe it is best to make them one channel boards with their own power supply?

Any help is greatly appreciated.

Scott

I meant to mention that the design uses a SS power supply.
 
Last edited:
Leave the heaters to off PCB, use twisted wire sets. Space them at least 1/2" off of the PCB., leave tightly twisted up to the socket. I use solid wire to facilitate a tight twist.
Components can be mounted to the top, or the top can be made the bottom depending on where you want them at. I use single sided toner transfer so the ability to swap sides for components is limited by the use of brass eyelets. They are also used for wire connects for mechanical strength. Toner transfer limits my designs to 8.5" x 11" due to limited slick clay paper availability.
Keep the electrolytics on the cool side for their longevity if you decide to mount the power supply on the PCB. I like to use the power supply to separate the 2 channels. The little spud'ed amp uses separate B+ filter strings for the first and second stages, common large cap on the outputs to the transformer center-taps. I like to use diodes for the HV with a large filter cap, through a choke to another large filter cap, through a slow start damper tube to the rest of the circuit. The first few large caps before the damper diode need to be rated for the over-voltage prior to the tubes coming on line.
I use component leads for jumping, stitching the ground plane together over traces. I've found that this method keeps the ground potential more constant to prevent ground loop noise.
You can stack PCB's with standoffs, the standoffs transfer the ground plane. I used the gold plated pins from a DB15 connector to act as interconnects between the PCB's for easy removal. I used heatshrink to cover the female socket of the connector set for more contact force.
Elevate the heaters by 50 volts is also another trick to quieter amps. I use 50 volt zeners to stack to 160V for the screen voltage on some designs. 160 volts is also enough to fire nixie tubes.
 

Attachments

  • keg-ear9.jpg
    keg-ear9.jpg
    798.4 KB · Views: 202
  • keg-ear15.jpg
    keg-ear15.jpg
    479 KB · Views: 188
  • P7070035.jpg
    P7070035.jpg
    983.9 KB · Views: 188
  • spud on bottom.jpg
    spud on bottom.jpg
    712.5 KB · Views: 180
  • spud on top3.png
    spud on top3.png
    857.3 KB · Views: 178
  • P2120279.jpg
    P2120279.jpg
    522.9 KB · Views: 81
Last edited:

artosalo

Member
2010-02-16 9:00 am
I have allways had heaters on the pcb without any problem, but I use double sided PCB. The component side is ground plane.
My last design is two EL509 + driver tubes. Some 5 A all together. And no hum problems.
The track width I use is 2.5 to 3 mm.

Below photos of a 6V6 PP amplifier pcb.

[IMGDEAD]http://kuva.termiitti.com/image/29880.jpg[/IMGDEAD]

[IMGDEAD]http://kuva.termiitti.com/image/29879.jpg[/IMGDEAD]

Heater foils are those two wide ones at the lower part of the pcb.
 

tomchr

Member
Paid Member
2009-02-11 12:58 am
Calgary
www.neurochrome.com
I use double-sided PCBs as well and use 80~100 mil traces for the heaters. Works great.

If you intend to have the tubes poke out the top of the chassis, place the tubes first along with other components that require a mechanical connection to the chassis (like PCB mounting holes). If the board is large (say 4x6 or larger), I'll sometimes put a hole in the center between two tube sockets so the PCB doesn't flex too much when the tubes are inserted.

Run critical signals first. The most critical is the input signal followed by any high-impedance traces. Be mindful of the loop area as this results in inductive coupling to other circuits. Then run the heater traces. Keep them short and avoid vias.

Beware of the breakdown voltage. You need to space high voltage traces away from other traces. I believe the general rule of thumb is about 40 V/mil for a board with solder mask or other conformal coating. For bare FR-4, it's much lower and heavily dependent on humidity.

Whether the supply goes on the amp board or not depends on the complexity of the circuitry. In my Spud, the supply is a rectifier tube (5AR4), two caps, and a MOSFET. That went on the amp board. In my 300B, the supply is about as complex as the amp itself. The supply is on a separate board - with a regulator board on a heatsink on the rear panel of the amp. Either approach is valid.

~Tom
 

tomchr

Member
Paid Member
2009-02-11 12:58 am
Calgary
www.neurochrome.com
Some info about PCB trace spacing for HV circuits can be found here:
PCB Trace Spacing Calculation for Voltage Levels

Another useful tip: Print out the PCB when you're done. Verify that tube sockets, power resistors, etc. will fit before cutting the PCB. I also find that I can spot errors or route optimizations easier on paper than I can on the screen.

~Tom
 
Thanks very much Tom. Great information.

Do you think it will be OK to cross an input signal trace at 90 degrees on the top side of the board in only one place? I'd like to go to the edge of the board to a terminal block. The other option is to just hard wire it and take it directly off the board at the tube socket.

Scott

Some info about PCB trace spacing for HV circuits can be found here:
PCB Trace Spacing Calculation for Voltage Levels

Another useful tip: Print out the PCB when you're done. Verify that tube sockets, power resistors, etc. will fit before cutting the PCB. I also find that I can spot errors or route optimizations easier on paper than I can on the screen.

~Tom
 

tomchr

Member
Paid Member
2009-02-11 12:58 am
Calgary
www.neurochrome.com
Thanks very much Tom. Great information.

You're quite welcome.

Do you think it will be OK to cross an input signal trace at 90 degrees on the top side of the board in only one place?

You mean cross the input and heater at 90 degrees? If the input lines have to cross heaters or signal lines with high voltage swing, keep them perpendicular. It's always better not to cross, but a 90 degree cross is the best you can do when they do cross.

Treat the heater traces as a differential pair. I.e. minimum (or close to minimum) spacing between them. That way, in the ideal world, the EM field from the "forward" current will be tightly coupled to that of the "return" current, and no external field is emitted.

Same goes for the input. Route the input signal and input ground as a differential pair all the way to the tube socket. Recall, the grid stopper is part of this loop. As is the grid leak resistor to ground. Keep the loop area small to minimize inductive coupling.

I'd like to go to the edge of the board to a terminal block. The other option is to just hard wire it and take it directly off the board at the tube socket.

I much prefer to route to a terminal block on the edge of the board rather than tapping off in the middle of the board. The latter just moves the inductive coupling to the wiring harness rather than the board. It's easier to control the loop area on the board than it is to control it in the harness.

~Tom
 
I've got the board about as compact as I can get it, 90x155mm, considering the room taken up by the large coupling capacitor.

I'm using a loop breaker between signal ground and chassis ground. Is it better to connect the top layer ground plane to signal ground or chassis ground?

Do I connect the ground plane at one point only or multiple points?

Thanks,

Scott
 

Attachments

  • 12W6PSE1.jpg
    12W6PSE1.jpg
    204 KB · Views: 83
  • 12W6PSE2.jpg
    12W6PSE2.jpg
    167.7 KB · Views: 79

artosalo

Member
2010-02-16 9:00 am
There is no need to have just a single gnd point on such a small pcb.
I would use the top side copper as a common signal ground and remove all gnd tracks from bottom side.
Then all components that need to be connected to gnd will directly be connected to the top layer gnd via "thru pads".
Then the pcb ground can be connected to chassis ground directly or via the power supply ground.

Make sure that there are sufficient openings at the top copper for the mounting screws to avoid unwanted direct connection to chassis.
 
Thanks artosalo,

This is a little different than point-to-point concerns I guess. I've understood that in point-to-point wiring it is a good idea to have separate ground returns for the preamp and power amp section back to the star point.

I was able to reduce the size to 87.5 x 150mm.

Thanks much,

Scott
 

Attachments

  • 12W6PSE1.jpg
    12W6PSE1.jpg
    272.2 KB · Views: 67
  • 12W6PSE2.jpg
    12W6PSE2.jpg
    288.9 KB · Views: 68