# what is the current limit through a trace?

Similar questions and topics have been asked before such as

I've used PCB Toolkit in the past and I haven't had practical issues, but I also didn't have more than 1A running through signal traces before. What I'm noticing is that there is a difference between some of the calculators. I'd like to know which set of tools is more trusted.

I understand that there are alot of pictures with information all over the pictures, you can skip to the bottom of this question for a summary of the pictures show if that is easier.

# PCB Toolkit

## With IPC-2152 modifiers enabled

The general window looks like this

I've played around with the conductor width until I was able to ~2A. My input settings are the following

I believe my fab house starts with 0.5oz base and then plates up.

Here are the results for external layer

Internal layer (I've updated my conductor width to 22 mils)

If I were to change the option from plane present to no plane present, I get a different set of values.

Keeping the settings for the external layer the same, and changing only plane present: no

## With IPC-2152 without modifiers enabled

From a question I had asked earlier, Will forced air on PCB improve current capacity of trace? , which seems to indicate that heat dissipation improves current limits, then the presence of the plane helps with cooling and therefore can handle higher currents than without.

# CircuitCalculator.com : PCB Trace Width Calculatr

I would have expected that the values to have been similar between the two, but they really are not.

If I were to enter the same values I had entered for the PCB Toolkit (with the exception of the plane present status and base copper and plating copper. I get the following

**Summary**
The following all has a target current of ~2A with a 20C temp rise.
PCB Toolkit with IPC-2152 modifiers           Internal Trace       22 mils
PCB Toolkit with IPC-2152 without modifiers   Internal Trace       55 mils
Circuit Calculator                            Internal Trace       52.6 mils

PCB Toolkit with IPC-2152 modifiers           External Trace       12 mils
PCB Toolkit with IPC-2152 without modifiers   External Trace       36 mils
Circuit Calculator                            External Trace       20.2 mils


So my question is, which is correct because I am also trying to maintain a 50 ohm line if possible ? I'm leaning towards that PCB Toolkit is more accurate, since the online calculator is using IPC-2221A and the website does not appear to have been updated since March 2008 (last blog entry).

In the end, what I am looking for is a smallest external/trace, that can handle 2A without being excessive on copper thickness. Smaller traces make it easier to get 50 ohm line without having to increasing my board thickness.

• A direct comparison of the results would help, because its cumbersome to scroll around, look at the pictures and finding the useful values. – Rev1.0 Apr 14 '15 at 6:52
• @Rev1.0 that's a fair point. Let me merge some of the images together. – efox29 Apr 14 '15 at 6:59
• You seem to have calculated with an AC current at 1MHz in PCB Toolkit, while the CircuitCalculator tool probably assumes DC. I really think you ought to just design conservatively rather than squeezing out the last mil. How many 2A traces do you have on your circuit? Aren't you working too hard to save a dozen-odd mils of board dimension? – Atsby Apr 14 '15 at 7:00
• @Atsby checking the DC option in PCB Toolkit does not change the current. It only affects the Skin depth. I have quite a bit of 2A traces, enough to be concerned with board space. – efox29 Apr 14 '15 at 7:03
• Just out of interest, what is the IPC spec difference between "with and without" modifiers? The difference is massive! – Rev1.0 Apr 14 '15 at 10:56

I'm going to attempt to answer this question from my own research into this.

Many of the online calculators for trace width vs current is derived from a document that was published apparently years ago. Some sources have said it was in the 1950s, but I haven't been able to find the first date it was published. (In fairness, I didn't look that hard either). The IPC-2221 is the Generic Standard on Printed Board Design.

I found a copy of IPC-2221 here [link]

A more modern version of this document exists (I don't have the date), and its the IPC-2152 which has since updated some of the older information of the past. If the original document was published in the 1950s, then PCB design has some a long way, such as the use of planes and multilayer boards.

The PCB Toolkit software uses (by default) IPC-2152 with something called modifiers. I'll get more into that soon. Another website, (http://www.smps.us/) also provides a calculator for trace width vs current and uses the IPC-2152 as the baseline link and the body includes some explanation into the differences with the old and the new.

Until recently, the main source for calculation of the printed circuit board (PCB) trace width for temperature rise were plots derived from the experiments conducted more than half a century ago.

It goes onto say..

The new standard IPC-2152, which is based on the latest studies is much more involved. It provides more than 100 different figures and lets you take into account many additional factors, such as thickness of PCB and conductors, distance to a copper plane, etc.

The rest of the page includes a calculator and some equations and how and why the author did certain things, but one thing he says is

If you have a multi-layer PCB with a copper plane near your conductor, the actual ∆T will be substantially lower. However, for the boards less than 70 mils thick without a plane the temperatures may be higher. Therefore IPC referring to Fig.5-2 as conservative may be misleading. Anyway, to reflect the conditions of a specific application, one can introduce a correction (modifying) factor as the ratio between estimated actual and generic ∆T.

I think this is the modifiers we see with PCB Toolkit. When I plug in the the same values for both PCB Toolkit and this online calculator, I get the same result**

** The internal trace width matches the the revised width of the online calculator.

That document also arbitrarily assumed that internal conductors could carry only half of the current of the outer ones. In reality, as mentioned in the new standard, inner layers may actually run cooler because the dielectric has 10 times better thermal conductivity than air.

I thought this was interesting and according to Wikipedia

Thermal conductivity, through-plane 0.29 W/m·K,[1] 0.343 W/m·K[2]
Thermal conductivity, in-plane  0.81 W/m·K,[1] 1.059 W/m·K[2]


and The Engineering Toolbox at about 20C, thermal conductivity of air is 0.0257 W/m·K

So if you have a plane, the dielectric spreads that heat out, so your trace can actually handle more current than what was previously thought.

TL;DR IPC-2152 is the new standard for trace width vs current, and includes heat dissipation with a plane so that traces can be handle more current, than what was previously thought.

PCB Toolkit (program) and http://www.smps.us/pcb-calculator.html use this new standard. So if you need to squeeze in more traces with a higher current rating, or if you are trying to hit a target impedance and be able to handle a higher load, the IPC-2152 will be able to help. However, if you can go bigger, go bigger because it's better to be conservative, but if you need to squeeze more and be considered "safe", then I think this is the way.

I have used PCB track calculators before but I was not satisfied with the results. The prime reason being the fact that the research done was quite old and second, these calculators abstract you from the research conditions like - what was the safety factor considered at the time of research, what was the condition of operation, what was the PCB quality etc. Besides this, once you get a fully fabricated PCB, it's specifications will be totally different from a theoretical value. For ex - exact conductor thickness will depend upon all the process carried out by the fabrication firm. As such it becomes difficult/inefficient to use a theoretical result in real life scenario.

Getting back to basics, the ampere handling capacity is related to basic physics. Any trace will have finite resistance. When you pass a current under a potential drop, there will be a power dissipation P = V*I in the track. If the track's melting point is reached, your PCB gets damaged. That's it.

I'd suggest a practical approach rather than going into theoretical one. The idea is to get a PCB fabricated with traces made of varying thickness, placed parallel to each other. Also get this board in varying copper thickness (35 microns, 70 microns etc). Use this as a reference board for that particular fabrication house (just to be on the paranoid side). Whenever you want to find the current capacity of a trace width, just apply the signal to a trace which you think will not melt at this current. Let it stay there for a while till the trace reaches stable temperature. Try feeling the temperature with hand (or measure it using a non-contact thermometer or whatever you can use).

Make sure that you do the testing for the worst condition your pcb can get into. After getting the temperature, you can easily decide the trace width to go with.

• I've done a similar-ish test, I had an older board with 10 mil traces, and I fed 3A into it and left it there for about an hour. The area surrounding the trace did get quite hot to touch, felt some measurable pain leaving my finger there for more than 5 seconds. But the trace appeared have been intact. It dropped about ~2V for a 5inch trace, but 3A is more than what I need. But your idea is good to include a board with varying widths and thickness. Unfortunately I don't have access to a non contact thermometer, I'd have to see if I can rent one for a day or two. – efox29 Apr 21 '15 at 23:57
• @efox29 - I don't think you will need an exact temperature value of the trace. You can just feel it with your fingers. You won't be able to tolerate more than 70 degree Celsius easily for more than 5 seconds. So, if the trace temperature feels comfortable to touch then you are good to go. – Whiskeyjack Apr 22 '15 at 7:24
• What about traces you cant touch directly ie, internal traces ? My high current traces are on internal layers and both layers are near solid planes. My current layer stack makes my outer traces 12mils and my internal ones 18 mils in order to achieve 50 ohm impedance. – efox29 Apr 22 '15 at 7:38
• Internal layers can't dissipate heat easily so you need to take a larger safety margin. Alternatively you can simulate internal layer by covering your tracks with another PCB (make sure not to short any connection) and then quickly taking measurements after removing the cover. This will give you a crude understanding of the temperature rise in internal layers. – Whiskeyjack Apr 22 '15 at 7:58
• From what I have read into my investigation, there is greater thermal conductivity in the dielectric than air (assuming convection only). Given greater thermal conductivity and close proximity to a plane, I would think that heat would be spread out more vs concentrated near certain areas. This was one of the differences between IPC-2221 and IPC-2152. Thoughts ? – efox29 Apr 22 '15 at 8:08