Trace Width Question

[bostonman]

Recently I laid out a PCB and accidentally forgot to consider the current on a trace (I did on another trace, but forgot about this one).

Fortunately it's on a RC line where the current will be 1.2A for a short duration; from calculations it will go from 1.2A to 0.75A in 16ms and then continue to drop.

The board is 1oz copper pour and the trace is 0.3mm, which, from research is correct for 1A. The trace would obviously need to be wider if it were carrying a continuous 1A load, but in this case it's carrying it for a short duration.

My question which has somewhat an obvious answer: is it just heat that would cause the trace to fail? Does a chance exist that the surge current would wear out the trace over time?

Also, something else occurred to me. PCB trace size is always a factor based on current, but what about component leads? They are much shorter, but I began to wonder why component lead size isn't a factor too.

[Someone]

Recently I laid out a PCB and accidentally forgot to consider the current on a trace (I did on another trace, but forgot about this one).

Fortunately it's on a RC line where the current will be 1.2A for a short duration; from calculations it will go from 1.2A to 0.75A in 16ms and then continue to drop.

The board is 1oz copper pour and the trace is 0.3mm, which, from research is correct for 1A.

"correct" based on what criteria? IPC2221 for example estimates the 3 way current<>width*height<>temperature_rise tradeoff. 1A 1oz 0.3mm is "correct" for 10 degree rise, 1.2A only changes that to 15 degree rise.

Also, something else occurred to me. PCB trace size is always a factor based on current, but what about component leads? They are much shorter, but I began to wonder why component lead size isn't a factor too.

Fusing current of component leads (or more often bond wires, check out how tiny they are even in power devices) is significantly affected by the temperature at the pad/joint, they sit on a comparatively massive heatsink at either end.

[Smokey]

https://www.eevblog.com/forum/projects/question-about-high-current-pcb-design/msg6197853/#msg6197853

There are multiple aspects to trace current capacity (but they are pretty much all about resistive heating).  The calculators pretty much all assume constant current, so if you have a trace rated for 1A constant current, it can almost certainly do more at lower duty.

One thing you are missing is temp rise.  All the calculators give a current rating for a given trace width at a given temperature rise.  Many of us use about 25C over ambient.  If you can handle more then you get more current for a given width. 

Any airflow over the boards will do a lot to keep the temp down.

If you already have boards get a thermocouple out and see how hot the trace gets under actual load.

[PGPG]

They are much shorter, but I began to wonder why component lead size isn't a factor too.

Typical PCB copper thickness is 35um. Have you seen so thin component leads?

[Doctorandus_P]

When looking at datasheets of newer power MOSfets in TO220, you can find data that claims the die can do 300A (DC!), but the whole device is limited to 150A or so because else the pins of the device melt.

Exploding bondwires is a common cause of failure when you attempt to use chinese resistors at the rating that the numbers printed on their case suggest.

For PCB's current handling capability of tracks is usually based on a 10 degree celcius temperature rise caused by simple track resistance. Such calculations are also not very accurate. If you've got 10 parallel tracks all at their maximum current then the temperature rise will be (a lot) higher in that area. If you have a multi layer PCB with a big fat GND plane directly under the track, then it will spread the heat and the temperature rise will be less.

[bostonman]

Many of us use about 25C over ambient.  If you can handle more then you get more current for a given width. 

I don't see my board being higher than this. Keep in mind, the trace only sees 1.2A of current (we can call it 1.3A to be conservative) for 16ms. If heat is the main factor that can damage a trace, then it should be good. How hot can it get in 16ms or even 100ms?

My thought was to solder wires to all the points, but I think it's overboard.

Typical PCB copper thickness is 35um. Have you seen so thin component leads?

I was thinking a component lead may be equal to a 0.6mm trace wide (2A ?) if you flattened it. Let's assume it was a capacitor that's a short to ground initially. If it doesn't have anything to limit the current, it may see several amps for a brief moment thus exceeding the lead tolerance for such given current.

[Doctorandus_P]

Capacitors can have very high peak currents, especially ceramic SMT capacitors. Putting a 100nF capacitor or so over a switch to "debounce" it (for example common practice with reset pins) can wear out the switch contacts over time.

But for heating it's not a problem. The peak currents can be 10A or more, but the duration is short, and tracks need time to heat up. Short duration high current peaks are rarely a problem on PCB scale. You can calculate the amount of energy in a capacitor, and that's the maximum that can be used to heat up a track.

[Whales]

+1 it will cause no impulse wear to the tracks.  Switch contacts yes, as they make & break contact only a few atoms at a time (which makes them fly off as sparks, wearing away the contacts).  But tracks no.

[tooki]

Many of us use about 25C over ambient.  If you can handle more then you get more current for a given width. 

I don't see my board being higher than this.

You misunderstand. The 25C refers to how large of a temperature rise you are willing to tolerate in the trace. So if your board is at 20C ambient, and you accept a 25C increase, then the trace calculation would crunch the numbers (width or maximum current) that result in the trace heating up by 25C (so the trace would reach 45C in this example).

Typical PCB copper thickness is 35um. Have you seen so thin component leads?

I was thinking a component lead may be equal to a 0.6mm trace wide (2A ?) if you flattened it.

You’re way, way off. 0.6mm is a typical diameter for a component lead, say, for a 1000uF 25V capacitor. Using math, the cross-sectional area is 0.283mm². Dividing that by 35um (0.035mm) gives a trace width of 8.08mm.

Even the dainty, thin leads of a DIP IC (0.455mm x 0.254mm) give a cross-sectional area of 0.114mm², which divided by 35um gives a trace width of 3.25mm.

In other words, the copper cladding of an PCB is far thinner than your gut feeling of it suggests.

[SiliconWizard]

0.3 mm is fine for 1.2 A... but what you need to figure out is whether the temperature increase and voltage drop (depending on trace length) will be acceptable. Now for a very short period of time, temperature should be a completely non-issue, so it's more about the voltage drop.

In terms of "damage" to the trace, pretty much all you need to care about in practice is the fusing current. For a standard copper weight, 0.3 mm trace, at 1.2 A the fusing time is longer than 10 s (but usual models do not cover such long fusing times), so you can safely consider that 1.2 A for just a few tens of ms will not do anything.