PCB Trace widths

[Mark245]

Hey everyone,

I am building a smaller amp with maybe 20 watts per channel. I am routing all of the power traces for 50 mils and the traces I do not expect much power on for 25 mils. Is this a good assumption? I was thinking about going with 75 mils for power. Is this overkill?

Also, I have decided to go with a double sided pcb since I have like 80 parts to route. Basically, the traces I could not fit all on one side I put on the other. Is it ok to do this? Will it cause noise? I have heard some people say to put all power and ground on one side and everything else on the other. Any rule of thumb for this?

Thanks,

Mark

 

[rtarbell]

Generally speaking, yes - the power and ground traces are usually on the bottom of a two-sided PCB - all of your signal traces are on the top. This makes troubleshooting much easier (if you want to probe a certain signal, you don't have to flip the board upside down).

Just another suggestion for you - depending upon what kinds of components you are using (surface mount, lead-less packages, etc.), I would suggest that you do NOT get a solder mask on your board. This way, if your traces are too thin, then you can solder some bus wire right over the top of them to enhance their current carrying capability. If you have a solder mask, you would have to scrape the solder mask away from your traces before doing this.

Do a google search for

pcb trace width calculator

This should get you to several pages that can give you numbers as to how thick a PCB trace should be for a given current.

 

[syn08]

One inch of 50mils 1 oz thick copper has a DC resistance of about 11 milliohm. A 20W amp into 8ohm will have a peak current of 2.2A, hence a voltage drop on critical traces of max 24mV peak per inch. That's way to much to my taste, I would double the high current traces width. Even so, you would still require a good layout to avoid ground loops.

 

[Mr Evil]

Just make the tracks as wide as will physically fit.

If you're using a double-sided board, note that running a track on one side in parallel with one on the other side will capacitively couple them. This is good in some cases, and bad in others.

 

[Steve Dunlap]

One inch of 50mils 1 oz thick copper has a DC resistance of about 11 milliohm. A 20W amp into 8ohm will have a peak current of 2.2A, hence a voltage drop on critical traces of max 24mV peak per inch. That's way to much to my taste, I would double the high current traces width. Even so, you would still require a good layout to avoid ground loops.

I agree with this. Another option is to go with 2 oz copper (or heavier) also. This will make very little difference in price for small runs of just a few pieces.

If you have room, you can go with both our suggestions.

 

[Eva]

Use traces for small signal nodes and polygons for speaker current paths...

Also, double sided PCB calls for a ground plane 😉

 

[east electronics]

you might

also need to be carefull in case your circuit is layout sensitive ....


some amps are some arent that much .... generaly all amps are

also ground plane might be an issue

some manged with it others didnt

regards sakis

 

[nigelwright7557]

If your PCB CAD software allows powerplanes I would use them as much as possible to keep the ground plane as low impedance as possible.

Otherwise fill out tracks the best you can.
I would use a minimum of 75 thou and thicken up where room allows.

I have a 900w amp and use upto 200 thou tracks on high power lines.

An externally hosted image should be here but it was not working when we last tested it.

 

[jackinnj]

See if you can use 100 mils for most of the power and output nodes. Where this isn't workable you can narrow the trace -- I'm lucky to be able to "right-click" to narrow or widen the trace, but ymmv.

When you discover a mistake with a solder mask, just grab the Dremel with a cutting blade.

Audioman45 suggested (in an Application Note) that groundplanes weren't helpful in audio amp circuitry -- so I laid out another board using the LM4702 sans ground plane, using a central locus to bring the signal ground together. The difference was measurable in terms of the THD% being a smidge lower, and by a smidge I mean a tiny but consistently measurable amount.

 

[tinitus]

I dont know
This one has supply caps all the way from bridge to output
Maybe thats slightly different
Oh, connections from power transistors to speaker out will be solid core wire
Well, the whole thing might be hard wired, or just part of it
I should say this too, its a Dx amp

 

[Eva]

Visually symmetric layouts with rails on the sides and small signal stuff in the middle are the worst.

 

[Mr Evil]

Visually symmetric layouts with rails on the sides and small signal stuff in the middle are the worst.

Indeed, you want the two rails as close together as possible, to minimize loop area. However, it is a lot easier to lay out a PCB with one rail on each edge.

 

[GK]

Indeed, you want the two rails as close together as possible, to minimize loop area. However, it is a lot easier to lay out a PCB with one rail on each edge.

That example posted isn’t any good but a rail on each side can be perfectly fine - it's where the power leads terminate and where the current flows that counts. And "visual symmetry" isn't and evil either. There are a number of designs around with both symmetry and rather large “loop areas” (due to mechanical constraints) that still achieve very low distortion.

Also, laying out a class B or AB power output stage with the power supply rails overlayed is often misguided because the field of one half wave will not cancel that of the other.
Same goes for twisting supply rail wires together without the ground return.

 

[east electronics]

from ....a post from user

Eva ....

the ideal pcb will have a small power and ground traces ( lengthwise ) and have this type of stracture :

from left to right ...totally left side the power things outs drivers vbe multiplier ..... in the center ,ground may be power caps ( if no more than 4) and on the totally oposite side right area the small stuff like LTP ccs VAS and goes on ...

ground plane can always be tricky

destroyes your star ground pholosofy
can create capacitance between the other layer

 

[akis]

On a very related subject, once I create a PCB layout, using some appropriate software, currently tinkering with diptrace, how do I go about gettting a PCB created? Is there a service in the UK (actually I do not care where in the world) that would create a PCB for me (even undrilled) ?

 

[tinitus]

Visually symmetric layouts with rails on the sides and small signal stuff in the middle are the worst.

That example posted isn’t any good but a rail on each side can be perfectly fine

Yeah, thats what I have been told numerous times in relation with another design, but it works ok though, as Glen says

Though I wonder if the ground loop issues might be different, when common ground is placed at the end of power supply, close to output stage
Thanks
🙂

 

[tinitus]

Indeed, you want the two rails as close together as possible, to minimize loop area.

However, it is a lot easier to lay out a PCB with one rail on each edge.

That was the point
That the benefits from having supply lines and ground plane end right at the output stage holds enough benefits to override the other issues on hand
And there ought to be some benefits from having no supply wires at all, other than trafo connections

Compromises there will be anyway

Below is from Holton site
Could be an option, but seems to me like there might be other issues with bridge so close to amp curcuit
Additional noise from wire connections etc
Probably works fine though

 

[Mark245]

Thanks everyone for the responses. I will take everything into account as I finalize my PCB layout.

 

[audio845]

On a very related subject, once I create a PCB layout, using some appropriate software, currently tinkering with diptrace, how do I go about gettting a PCB created? Is there a service in the UK (actually I do not care where in the world) that would create a PCB for me (even undrilled) ?

Hi,

I've had good luck with pcbfabexpress.com and custompcb.com.You just send them your gerbers by the web. A lot of people have used olimex with good results - their shipping costs are a little high to the US. Any of these companies will drill them for you so don't worry about that.

If you want to try making your own try http://www.fullnet.com/~tomg/gooteepc.htm where there is an explanation of how to make pcb's using a laser printer. It works quite well for one sided boards. Haven't tried double sided boards yet.

Charlie

 

[nigelwright7557]

On a very related subject, once I create a PCB layout, using some appropriate software, currently tinkering with diptrace, how do I go about gettting a PCB created? Is there a service in the UK (actually I do not care where in the world) that would create a PCB for me (even undrilled) ?
[/UnQuote]

Send your gerber files to this bloke.
I have had excellent PCB's back at good prices.

lorimer888@tiscali.co.uk