0
\$\begingroup\$

I'm designing an hot plate made of an aluminum PCB capable to heat up to ~50°C. Having the area I want to heat up and thus the trace length to cover most of it, to determine the track width that I need I used a couple of common online tools (1, 2), which gave me different results.

Then I noticed that one was using IPC2221 (older) and the other was using IPC2152 (newer) as the standard to calculate the result. Reading about it online I found out that IPC2221 was based on 50-years old measurement, and so it would make sense to use the newer IPC2152, but what troubles me is that the Trace Width for external layers (which is what I'm gonna be using) is 1.29 mm for IPC2221 and 3.36 mm for IPC2152: a difference of more than 2x!

How is it possible that they differ by so much? Have people been making inaccurate PCB's the whole time because of IPC2221? Should I use IPC2152 results?

Thanks

enter image description here

\$\endgroup\$
2
  • \$\begingroup\$ Do those standards apply for Alu core PCBs as well? or only FR4? \$\endgroup\$
    – Wesley Lee
    Commented Nov 10, 2022 at 22:08
  • \$\begingroup\$ @WesleyLee that's a damn good point, I haven't checked. Anyway it shouldn't matter because the aluminum pcb would just change the time it takes to heat up (I guess). \$\endgroup\$
    – StefanoN
    Commented Nov 10, 2022 at 22:20

2 Answers 2

2
\$\begingroup\$

The temperature rise is for the copper trace itself sitting on piece of (fairly thermally insulating) FR4. That's why the numbers are different for internal and external layer.

I don't think you can directly apply it in your application. I suggest determining the required power experimentally (find a piece of aluminum of the same thickness and overall dimensions, mount it similarly, and heat it with one or more power resistors bolted to it).

Then you can use the tools to calculate the required trace width for the required resistance at the operating temperature (copper has a positive tempco so you'll need a bit lower resistance at room temperature). There's also a correction for the corners that you may need to apply since current crowds in corners.

Incidentally, 50 year old measurements may well be done better than more current ones. I've often had to look up much older papers to find work done to high standards (for example for magnetic shielding).

\$\endgroup\$
3
  • \$\begingroup\$ Shouldn't the aluminum act as a low pass filter? Meaning that, in an FR4 PCB the traces would heat up and the FR4 not so much, whereas in an aluminum PCB the traces would not heat up as quickly because the aluminum would take the heat away, and by the time the traces have effectively reached the temperature desired the aluminum would be at that temperature as well, effectively achieving the wanted result? \$\endgroup\$
    – StefanoN
    Commented Nov 10, 2022 at 22:35
  • 1
    \$\begingroup\$ You have to separate the heat capacity related transient effects from the thermal conductivity (& radiation & convection) cooling effects. After a long time the temperature of an FR4 PCB will be lower than an alum. PCB but the traces themselves will be hotter. The final temperature will be dependent on the size of the aluminum what is around it & how it is mounted (which affects convection cooling). I think you can assume it to be isothermal if it's not too big & not too thin. That's not true with FR4. You might have to wait 30 minutes for the transient effects to become small enough to ignore \$\endgroup\$ Commented Nov 10, 2022 at 23:49
  • 1
    \$\begingroup\$ The resistance of the copper traces at a known temperature is much easier to calculate accurately than the temperature even of a simple object like a flat plate with a given power dissipation. The heat loss effects are nonlinear and not necessarily intuitive. That's why I suggest finding the required power experimentally. It can be done also with expensive software but most likely you'd still want to verify it experimentally unless you do this sort of thing all the time. \$\endgroup\$ Commented Nov 10, 2022 at 23:53
2
\$\begingroup\$

The IPC-2221 standards were copied from the "Printed Wiring for Electronic Equipment", MIL-STD-275, United States Department of Defense. For example, here is figure 4a "Conductor thickness and width for type 1, type 2, and external layers of type 3 printed-wiring boards" from the MIL-STD-275E (1984) standard:

enter image description here

This plot looks exactly like Figure 6-4 from the IPC-2221A standard. From what I've read (and wish I could remember the reference), these plots may date back to the late 1940's. Nobody seems to remember how they were generated, what the substrate material and thickness was, and how they were verified.

The IPC funded research into this subject because there are a lot of questions that the MIL-STD plots don't address:

  • What happens if I run a plane under my traces? Shouldn't it remove heat allowing me to make my traces narrower?
  • If I switch to a more thermally conducting substrate material (say alumina), does that allow for narrower traces?
  • What if I change trace material (use silk screened silver instead of copper for example)? How should traces be adjusted?

The result of the research was IPC-2152 standard. To answer your second question first:

Yes, you should use the IPC-2152 standard. It incorporates the latest research into this subject.

To your first question, has the IPC-2221 standard (and others) been giving us the wrong answer?

It wouldn't shock me, but it's hard to answer the question of how wide should traces be for all conditions with a couple of plots. In general, if I'm running a 5 A through a trace, the voltage drop per length usually sets the width of my trace, not the temperature rise of the traces. In general, the voltage drop requirements result in traces wider than what the IPC-2221 standard call for.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.