jump to navigation

## Current vs. Trace Thickness and Temperature vs. Copper DensityDecember 15, 2006

Regarding the PCB Trace Width Calculator [1], Regit asks:

(a.) What is the relationship between current and trace thickness? And, (b.) what is the relationship between temperature and copper density?

Answers:

(a.) The relationship between current and trace thickness is shown in the IPC-2221 formulas under the trace width calculator [1]. With a little algebra, it comes out that current is proportional to thickness raised to the power of c, where c = 0.725. So, per IPC-2221, if the thickness is doubled, the current capacity changes by a factor of 2^(0.725) = 1.65.

A common mistake is to assume that twice the trace thickness should allow twice the current, but it does not. Allowing twice the current for twice the thickness would mean allowing twice the power without any significant improvement in the heat path out of the trace. The heat path out of the trace would not significantly change since the trace still has the same surface area. (Also see comment 4 below.)

(b.) The relationship between temperature and copper density depends on what you mean by copper density. I assume you mean the amount of other copper traces and planes in the board and not the mass per volume of the copper itself. The formulas used in this trace width calculator are empirical relationships stated in IPC-2221.

According to [2], these formulas correlate to a PCB in Euro-Format (Lx=100 mm, Ly=160 mm, D=1.6 mm) made of pure FR4 (conductivity k=0.3 W/m-K, emissivity Îµ=0.9), with one copper trace of length L=100 mm and thickness t=35 Î¼m (=1 oz) on the top face and with a copper layer on the back plane (also of thickness 35 Î¼m, conductivity k=395 W/m-K and with a solder resist with emissivity Îµ=0.9). The ambient condition is that the PCB is suspended in still air by thermally nonconductive straps.

If your board has a different configuration than the above, the actual trace temperature rise and its current capacity will vary from the calculated values and you would have to conduct an analysis as done in [2] to find the relationships for your specific board configuration.

However, some generalizations can be made. Some things will decrease the temperature rise in the trace (and increase its current capacity) such as having more copper in the PCB, more air flow, or the inclusion of the heat path through the mounting hardware. Because of this, the current carrying estimates provided by the IPC-2221 standard are generally considered to be fairly conservative.

[1] PCB Trace Width Calculator
http://circuitcalculator.com/wordpress/2006/01/31/pcb-trace-width-calculator

[2] New Correlations Between Electrical Current and Temperature Rise in PCB Traces, Johannes Adam
http://www.flomerics.com/flotherm/technical_papers/t341.pdf

## Comments

1. shan - March 30, 2007

What is the significance of the track size & copper weight for the different pcb materials and pcb types?

2. Brad - March 30, 2007

Shan,

Track size (width) and copper weight (thickness) effect the resistance of the trace. This in turn effects the heat (power) generated for a given current (P = I^2*R). The different PCB materials and other PCB factors such as board thickness, number of layers, and total copper content by weight are significant because they make up the main path for heat to get out of the trace. Studies have shown that most of a traceâ€™s heat is conducted into the board and then convected into the air through the relatively large surface area of the board. To emphasize the significance of the board - A trace in air (with no board) can be shown to get way hotter than a trace on a PCB. Likewise, different board configurations can have significantly different trace temperature rises at the same current. The trace temperature rise determines the amount of current it can safely carry.

Brad

3. valeri - January 6, 2008

I would like to ask what is the relationship between the temperature for pre curing of PCB from the amount of ink deposited on each trace.

4. gnuarm - January 17, 2008

Part of the explanation above is not correct.

“One may think that twice the trace thickness should allow twice the current, but it does not. This is because the heat path out of the trace has not changed much since the trace still has the same surface area.”

The thickness has little to do with the heat path out of the trace. It reduces the resistance to the current flow and so changes the power generated for a given current. The power for the thickness term is not 1 because the current is not linear to power, but rather runs by the square root of the power, P = I**2 * R. Since the power is constant, twice the thickness of the conductor results in half the resistance and the current can rise by SQRT(2).

You would expect the power of the thickness term then to be 0.5, not 0.7. If you look at a detailed analysis of the data, you will find that the power they end up with is indeed much closer to 0.5. But this is because they separate the thickness from the width while most calculations don’t separate the variables.

See “Temperature Rise in PCB Traces” at http://www.ultracad.com/articles/pcbtemp.pdf for more information on this than you probably want to know…

5. Brad - January 29, 2008

gnuarm,

I revised the paragraph in question to better spell out what I was trying to say. However, you are right in your reasoning and in that the IPC-2221 formulas are not the most accurate model of what is going on in the PCB, but have none the less become an industry standard.

Brad

6. fatima - March 4, 2008

i would like to know how a circuit designer in orcad plans the schematic and layout for the digital, analog, power, low speed high speed portion of the pcbs?

7. Brad - March 7, 2008

fatima,