Connect with us

Current and PCB Traces

Discussion in 'Electronic Basics' started by Abstract Dissonance, Feb 20, 2006.

Scroll to continue with content
  1. 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
     
  2. Noway2

    Noway2 Guest

    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.
     
  3. John Fields

    John Fields Guest

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

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

    news://
     
  4. Dan H

    Dan H Guest

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

    Dan
     
  5. huh?

    is this suppose to be a link? Cause its not working...
     
  6. 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
     
  7. ok.

    Thanks,
    Jon
     
  8. Noway2

    Noway2 Guest

    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.
     
  9. Brian

    Brian Guest

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

    Thanks,
    Jon
     
  11. DJ Delorie

    DJ Delorie Guest

    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.
     
  12. PeteS

    PeteS Guest

    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
     
  13. JeffM

    JeffM Guest

  14. 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
     
  15. DJ Delorie

    DJ Delorie Guest

    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.
     
  16. Rich Grise

    Rich Grise Guest

    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
     
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-