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

[bbuz]

Hello,

I am planning on laying out a couple PCB's for a small PP power amplifier....a la "el cheapo" and "Baby Huey".

Have used the likes of expressPCB and others with success- but strictly for solid state circuits. Designing PCB's for Tube circuits concerns me regarding the trace properties- specifically accommodating the higher voltages and current demands for the tube amplifier.

The company I am most comfortable with describes their traces as:

....."Our laminate is 0.062" FR-4 epoxy glass with 1/2 ounce copper.
We plate an additional 3/4 ounce of copper (totaling 1 1/4 ounce), resulting in a copper thickness of ~0.0017"."


I would imagine the 12aq5 will have the most current demands( as I see less than 5 watts per tube output current and max .225 amps for heater current)....

So, before I start my layout, I am wondering what trace properties people would recommend in light of the mentioned specifications or other pertinent issues others might raise that I have missed.

I am thinking that a .150 trace with 1 1/4 oz copper traces will suffice.. but I do want to get things correct with large enough traces- and yet, hoping the answer will not be "you need 3 inch wide traces" ; )


Thanks!



Thanks!

 

[Nordic]

I would start with googleing for a table of trace spaceing... You may find it quite amazing how large the diffirence is for use at sea level or at altitude...

Currents are not realy an issue with tubes, appart from the heaters... a standard 1.27mm trace can carry enough current for ten tubes and still would not go pow...

So voltage is your enemy, the higher the voltage the greater the required spaceing to prevent arching.

 

[bbuz]

Wow! It is so cool how quickly people reply around this forum : )

I appreciate the other factors to consider( trace spacing,altitude) and will research them further.

So that others don't question my "seach-function abilities" I wanted to mention that I have looked in this forum and google regarding this issue in some depth.

However, I wanted to measure twice and cut once- and as I suspected this forum( already) has provided additional helpful information not found elsewhere.

Thanks!

Bill

 

[Tom Bavis]

For voltage drop, the .150" trace is equivalent to 26 gauge. It can actually carry more current than a 26 guage, since it has three times the exposed surface area (plus conduction into the PCB). 2.5 mm (0.100") should be adequate spacing to 300V. If you are having a circuit board made, I highly recommend solder mask to insulate the surface.

 

[Tubelab_com]

I use a 50 mil (.050) trace all my routing except for the heaters. I will make them 75 or 100 mils depending on current draw and length. I use at least 50 mil trace to trace spacing, and 150 to 300 mil spacing for HV circuitry, more if the board has room. Here in south Florida the humidity can run 90 to 100% for the whole summer. Test boards made at home can show some weird leakages in HV areas with small spacing. Use solder mask to avoid moisture problems on comercially made boards.

Do not put a ground plane under any high impedance runners especially plate and grid runners. Keep ground, and other traces at least 100 mils away from them. The stray capacitances can cause HF rolloff and phase shift.

People claim that PC board technology "kills the sound". This can be true with poor layout and old tech board material. Do not use phenolic boards. FR4 is fine and 1 to 1 1/4 OZ copper is adequate. Some recommend glass teflon boards. It is expensive and too flexible. Traces will break when you change tubes.

 

[nigelwright7557]

I have found just wiring up cvalve amps that you have to be careful running heater wires close to signal wires as you can get a lot of crosstalk.

I also wouldnt run any high power output signals near input signals as you could end up with feedback.

 

[Sherman]

What about not putting heater traces on the board? That way one could tightly twist the heater wires and dress them so that they drop down from the tube socket and away from signal traces. Of course that means at least a bit of P2P hand wiring and soldering.

 

[Tubelab_com]

I routinely put heater traces on the board. They must be kept away from the input and low level signal wiring. They should be routed as a differential pair. Either on top of each other, which is hard to do on a two layer board without cutting the circuitry in half, or right next to each other. I usually put the heater connections on the same edge of the board as the output connections closest to the output tubes since they will be drawing the most current.

For a preamp, convert the AC to DC near the transformer connections and then route DC to the low level tubes. If I wanted to use AC heating on a low level stage, I might use a twisted pair off board. This would require some experiments.

 

[kevinkr]

What about not putting heater traces on the board? That way one could tightly twist the heater wires and dress them so that they drop down from the tube socket and away from signal traces. Of course that means at least a bit of P2P hand wiring and soldering.

This is what I do with the boards I get made by ExpressPCB as space is already quite limited on the standard prototype board they offer at a fixed price, for your project there will be more room as the board will have to be larger. I generally follow the same guidelines in layout as tubelab, and recommend FR4 pcb material.

Make sure that you measure the sockets you are going to use and verify that any patterns you download for sockets match those, or better still make your own library part for each socket type you use - nothing worse than finding your particular part does not fit the part geometry you used.. Don't crowd, and leave plenty of room for power resistors which you may also want to raise above the board surfaces in some instances to improve cooling.