Go Back   Home > Forums > Amplifiers > Tubes / Valves

Tubes / Valves All about our sweet vacuum tubes :) Threads about Musical Instrument Amps of all kinds should be in the Instruments & Amps forum

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 19th April 2013, 09:27 PM   #1
scott17 is offline scott17  United States
diyAudio Member
 
scott17's Avatar
 
Join Date: Aug 2009
Location: JFK
Default 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 by scott17; 19th April 2013 at 09:55 PM. Reason: additional info
  Reply With Quote
Old 20th April 2013, 12:59 PM   #2
roline is offline roline  United States
diyAudio Member
 
roline's Avatar
 
Join Date: Sep 2010
Location: East Tennessee
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.
Attached Images
File Type: jpg keg-ear9.jpg (798.4 KB, 175 views)
File Type: jpg keg-ear15.jpg (479.0 KB, 163 views)
File Type: jpg P7070035.jpg (983.9 KB, 160 views)
File Type: jpg spud on bottom.jpg (712.5 KB, 154 views)
File Type: png spud on top3.png (857.3 KB, 153 views)
File Type: jpg P2120279.jpg (522.9 KB, 66 views)
__________________
SO many tubes, SO little time!!!

Last edited by roline; 20th April 2013 at 01:07 PM.
  Reply With Quote
Old 20th April 2013, 01:31 PM   #3
diyAudio Member
 
artosalo's Avatar
 
Join Date: Feb 2010
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.

Click the image to open in full size.

Click the image to open in full size.

Heater foils are those two wide ones at the lower part of the pcb.
  Reply With Quote
Old 20th April 2013, 08:21 PM   #4
scott17 is offline scott17  United States
diyAudio Member
 
scott17's Avatar
 
Join Date: Aug 2009
Location: JFK
Thank you guys for the replies. Very nice looking boards. The stacking idea is great.

This helps very much. I think I'll give it a go.

I did also find a couple other threads here on the forum that also have good info on this. Here's one:

PCB Trace properties for PP tube amplifier ( 12AQ5, 6v6 etc)

Thanks,

Scott
  Reply With Quote
Old 21st April 2013, 04:37 AM   #5
tomchr is offline tomchr  United States
diyAudio Member
 
tomchr's Avatar
 
Join Date: Feb 2009
Location: Greater Seattle Area
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
__________________
21st Century Maida Regulator, Universal Filament Regulator, Damn Good 300B, Novar Spud, and more...
Neurochrome : : Audio - http://www.neurochrome.com/audio - Engineering : : Done : : Right
  Reply With Quote
Old 21st April 2013, 04:54 AM   #6
tomchr is offline tomchr  United States
diyAudio Member
 
tomchr's Avatar
 
Join Date: Feb 2009
Location: Greater Seattle Area
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
__________________
21st Century Maida Regulator, Universal Filament Regulator, Damn Good 300B, Novar Spud, and more...
Neurochrome : : Audio - http://www.neurochrome.com/audio - Engineering : : Done : : Right
  Reply With Quote
Old 21st April 2013, 07:18 PM   #7
scott17 is offline scott17  United States
diyAudio Member
 
scott17's Avatar
 
Join Date: Aug 2009
Location: JFK
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

Quote:
Originally Posted by tomchr View Post
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
  Reply With Quote
Old 21st April 2013, 08:07 PM   #8
tomchr is offline tomchr  United States
diyAudio Member
 
tomchr's Avatar
 
Join Date: Feb 2009
Location: Greater Seattle Area
Quote:
Originally Posted by scott17 View Post
Thanks very much Tom. Great information.
You're quite welcome.

Quote:
Originally Posted by scott17 View Post
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.

Quote:
Originally Posted by scott17 View Post
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
__________________
21st Century Maida Regulator, Universal Filament Regulator, Damn Good 300B, Novar Spud, and more...
Neurochrome : : Audio - http://www.neurochrome.com/audio - Engineering : : Done : : Right
  Reply With Quote
Old 21st April 2013, 11:40 PM   #9
roline is offline roline  United States
diyAudio Member
 
roline's Avatar
 
Join Date: Sep 2010
Location: East Tennessee
I print out the design and stuff the components into it using florist foam to back it up. I try to design the PCB to be flexible enough that various manufactures product can fit.
Attached Images
File Type: jpg P2110278.jpg (793.2 KB, 27 views)
File Type: jpg spud2.jpg (468.3 KB, 31 views)
__________________
SO many tubes, SO little time!!!
  Reply With Quote
Old 22nd April 2013, 03:34 AM   #10
scott17 is offline scott17  United States
diyAudio Member
 
scott17's Avatar
 
Join Date: Aug 2009
Location: JFK
I really appreciate all of the input from you guys.

I realize this is a very simplistic design, but this is what I came up with for one channel, less power supply.

Scott
Attached Images
File Type: jpg Untitled 1.jpg (225.4 KB, 40 views)
File Type: jpg 12W6PSE.jpg (118.4 KB, 48 views)
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
Tubelab SE board for PSE ystkkmkr Tubelab 12 14th January 2012 07:27 AM
Using PC PSU for Sure 4x100 amp board RhinoDude Power Supplies 2 14th September 2010 05:11 PM
DTA-2 T-amp PC board tresch Parts 3 19th June 2010 04:48 PM
Valve schematic & PC board design Athol Tubes / Valves 2 9th August 2004 08:23 PM
Paralleled LM4780TA PC board design - How's this look? OddOne Chip Amps 17 4th May 2004 01:21 AM


New To Site? Need Help?

All times are GMT. The time now is 06:04 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2