London Power ad

Search the Forum

(Advanced Search)

PCB layout guidelines for audio
Hi Guys

There are a few basic guidelines for laying out audio circuits on PCBs (printed circuit boards):

SAVE a lot - every few operations press SAVE so you do not lose hours of work if the program crashes.

NEVER use the AUTO-ROUTER. The auto-routing function is "a big deal" according to the designers of PCB CAD software, but it is entirely useless when laying out audio circuits as it will destroy the proper order of grounding. Galactic Grounding can be applied to PCBs as well as to hand-wired circuits, and is key to achieving a low-noise assembly. Just as with hand-wiring, the ground and power paths on a PCB must be made manually, or "forced" to go where we want them to. It is often easiest to NOT use the GND symbol to achieve this.

Lay out the schematic with normal orientations for the parts, circuits and symbols:
Positive voltage up
Negative voltages down
Ground symbols (if used) pointing down
Signal coming IN from left
NPN transistors with E pointing down*
N-mosfet with S pointing down*
N-jfet with S down*
PNP transistors with E pointing up*
P-mosfet with S pointing up*
P-jfet with S up*
*sometimes these must be rotated horizontal

Keep the signal path as straight as possible inasmuch as signal flow moves from left to right on both the schematic and the board.

Use proper voltage spacing especially for tube circuits. There are conservative and aggressive guides for this and it is better to err on the side of conservative. a good guideline is:
0.00012 x V
measurement is in inches
solder mask applied
0.001" = 1-mil (milli-inch). The above equation can be done in mils as 0.12 x V = mils. It is easier to refer to a trace width or space as 16-mil, 40-mil, etc.
Without a solder mask (which is pretty unusual today) the equation becomes V / 0.001
When checking the board, turn on the GRID and set it to a small increment and count the divisions between traces, then divide by 0.12 for a spacing in V. For example, a spacing of 40-mil provides 40 / 0.12 = 333V. If you know the voltage spacing you need, multiply V x 0.12 for mils. For example, 500V needs 500 x 0.12 = 60-mils.

Use appropriate track WIDTH. You can select the track WIDTH on the fly, before you lay the trace, or change it afterwards. Track WIDTH determines current capacity and it is surprising how much current a narrow trace will handle.

More to follow.
Hi Guys

DO NOT trust the ERC.

ERC is the check for consistency between the schematic and the board. When you lay out a circuit, you typically draw the schematic first, then press the BOARD button and Eagle asks "Create board (named as your schematic)?". OK produces the empty board outline with a field of parts and flywires to the left.

If you work on the schematic without the board open after this, the two will not be consistent and Eagle will tell you the "Forward and backward annotation will not be performed". You have to go to the board and select ERC to see the error list, which will have WARNINGS that do not mean much and ERRORS which are a problem.

In most cases, the ERC shows issues that are a problem as far as smooth board making goes. However, Eagle's ERC does NOT show all errors, such as traces crossing that should not. Supposedly, the DRC will show this.

DRC is the Design Rules Check, which uses parameters you enter for the project regarding voltage spacing. This is okay when the whole circuit operates from the same voltage, but in a tube amp or preamp there might be different voltages used for different areas. Heater trace spacing can be quite tight since it is only 6V or 12V, BUT those traces must be far from the tube plate since the plate is at high voltage. So, DRC can be cumbersome for true design rule checking but it can keep you from having crossed traces. using DRC just for the latter means you will always have a long list of DRC "errors" that you can generally ignore but should nonetheless verify.
This is great info Kevin! Thanks for sharing!

(09-13-2018, 03:34 PM)soundmasterg Wrote: This is great info Kevin! Thanks for sharing!


I concur. Thanks Kevin!
And so what is the track width rule? Is it as easy as it is to determine the spacing (using your formula)?
Hi Guys

Here is a chart that shows trace width versus thickness (copper weight in ounces) versus temperature rise versus current capacity.

It used to be that 2-ounce copper was standard, but these days you get 1-ounce unless you specify anything else.

I use 2-ounce copper and the 10C temperature rise column.

Have fun

Attached Files Thumbnail(s)
Is it permissible to route a top-surface trace (e.g., from Vpre node to a plate resistor) across a resistor or capacitor? And if so, must the component be lifted off the surface of the PCB?

I have done this on two spots on my PCB (trace crosses two shunt resistors) and I don't notice any problem, even with the resistors resting on the PCB....
Hi jmcd

Yes, absolutely place traces on either side of the board under component foot prints.

The solder mask provides some voltage insulation as does the component body itself. Just follow the voltage spacing guidelines when routing traces near pads or other traces of dissimilar voltages.

Only components that get hot need to be elevated from the board. If you are dealing with voltages over 2kV, then component elevation might be good to do. Since the arc voltage for an EL-34 is 2kV, and this is similar for KTs and other tubes, I make sure there is >2kV spacing around output stage anodes and screens and related components.

There is also no rule about the function of top or bottom traces for audio PCBs. You might see "conventions" followed by people laying out multi-layer boards for computers and similar, but they may have up to 16 layers and need to connect to 1,000 pins (or balls) under a large IC. For them, voltages are extremely low and trace widths will be much smaller than what we use for audio, and especially for tube circuits.

Have fun

oh, and I assume the spacing rules apply to traces on the same layer only, but I want to confirm (or disconfirm).
Hi Guys

Yes, "trace spacing" implies the same layer.

Between the first two layers is the PCB itself, so no worries BUT pads are the same on both sides.

With three or more layers, you would not use such a thing with tube circuits unless you are combining tubes with blue tooth or some other silly thing Smile The tube portion would use only the top and bottom layers and no traces of further layers would be routed in the area. The insulation rating between the 3+ layers is not high, and therefore only suitable to the low-voltage applications it is used for.

Modern PCBs begin as blank fibreglass sheet, which is masked, drilled, holes plated and then copper deposited where required, then solder masked. It is a solder mask upon which the third and fourth layers are applied on opposite sides of the board. Further solder masks insulate these from layers 5 and 6, and so on. The extra layer numbering here may be incorrect, but the basic process of adding those layers is correct. Vias can be added between internal layers and there is certainly a lot for the board designer to keep track of. It is these kinds of assemblies where the Restrict layers in Eagle come into play, where routing has to avoid where other layers may have a blind via, or really, to avoid any via or area of concern.

Forum Jump:

Come in where it's warm!
A warm welcome to tube amp modding fans and those interested in hi-fi audio! Readers of Kevin O'Connor's The Ultimate Tone (TUT) book series form a part of our population. Kevin O'Connor is the creator of the popular Power Scaling methodology for amplifiers.
Please remember these three principles: respect, sharing, community.
Not familiar with The Ultimate Tone book series? See discussion topics, or click here to visit London Power/Power Press Publishing.

Tube Amp Forum Hosted by London Power
London Power logo