Current and PCB Traces

How much current can, in general, a pcb trace withstand? Is there any
general guidelines that I need to be aware of so that I don't end up burning
them up or do i need to measure the resistance and compute the max current?
I plan on using a max of about 2 amps at around 40 volts and I'm wondering
if my pcb can handle it and if I need to worry about the trace width?

Thanks,
Jon

 

The current carrying capacity is going to depend on the trace width,
plating thickness, and allowable temperature rise. As the trace width
and plating thickness go up the resistance goes down and the
temperature rise drops with it. The resistance will be a function of
the (volume) conductivity of copper.

Here is a link to a website that I found with a quick google search:
http://www.geocities.com/CapeCanaveral/Lab/9643/TraceWidth.htm

I don't know how accurate the results are but if you can find a couple
of calculators that agree or find the formulas for copper conductivity
and temperature rise you could verify the results.

 

---
Yes, you need to worry about trace width.

I just posted a nice nomogram for you with the data you need at:

news://

 

Your PCB can certainly handle it but you do need to worry about trace
width

Dan

 

huh?

is this suppose to be a link? Cause its not working...

 

Well, Since 20awg wire can only do about 1 amp(thats what it says on the
insulation of the 20awg wire I have) then it seems that a trace of 0.040in
just falls short(assuming a depth of about 0.005in(a guess but it doesn't
seem that deep on my boards)?

Jon

 

ok.

Thanks,
Jon

 

Well, Since 20awg wire can only do about 1 amp(thats what it says on the

It really isn't that complicated.

The thickness on the boards is based upon the plating thickness in oz
(per square foot I think). You choose the thickness of the plating you
desire, .5oz, 1oz, 2oz, or 3oz and knowing this value you can then
determine the necessary width of the trace to allow X amount of current
at Y temperature rise. If your current draw is operating at a high
frequency you will need to account for skin effect which will decrease
the effective thickness of your copper.

 

There are a lot of variables there. For example, is it an internal or
external trace. How much of a temperature rise do you want on the trace. How
thick is the trace.

For example, a typical temperature rise of 10 degrees Centigrade and at 2
amps:
EXTERNAL TRACE:
1/2 ounce trace -- trace width at least 0.055"
1 ounce trace -- trace width at least 0.028"
2 ounce trace -- trace width at least 0.013"

INTERNAL TRACE:
1/2 ounce trace -- trace width at least 0.205"
1 ounce trace -- trace width at least 0.103"
2 ounce trace -- trace width at least 0.052"

Brian

 

ok... atleast I have some general ideas now.

Thanks,
Jon

 

You're confusing the current rating of the wire's *insulation* with
the thermal characteristics of the bare copper on a PCB. Insulation
melts at a much lower temperature than copper[1].

A given cross section of copper will have a certain temperature
increase for a given current. More current, more heat. More copper,
less heat. You choose a copper size based on how much heat you can
tolerate. For example, in a 70F room with a 110F limit on heat, you
design for a 40F increase in heat due to resistive losses in the
copper.

Wiring is different - it's rated according to how hot it can get
before the *insulation* fails and you get a short.


[1] although I hope you don't design based on the melting point of
copper! There are other considerations, like how hot your ICs
want to get, etc. The melting point of the glue holding the
copper onto the PCB might be a consideration, for example.

 

Get a copy of the old, free PCBTEMP (used to be available from
UltraCAD, but I believe it's no longer available at their site). It's a
handy tool for such things.

Cheers

PeteS

 

Get a copy of the old, free PCBTEMP

http://66.102.7.104/search?q=cache:...abs.com/freesoftware.htm+zzz+zzzz+PCBTemp-zip

 

Ok, I think I understand. Basicaly the in both cases heat will be generated
but in the case of wire the insulation has a lower melting point than on a
PCB(which is due to the type of material and the size?)?

Thanks,
Jon

 

Technically, the insulation has a maximum safe temperature, and your
PCB has a maximum safe temperature, with "safe" defined accordingly
for each. Your project could have a different and unique definition
of "safe" for example. Enclosure temp, thermal cooling of other
components, heatsinks, etc.

But in general, you can't use the current ratings of wires as a guide
to the current ratings of traces.

 

It's a message ID - copy it to your clipboard, migrate to
and paste the message
ID in the appropriate "find message ID" place.

Good Luck!
Rich