pcb trace fusing currents

This one says that for a 10 amp trace, the inner-layer width needs to be 740 mils... 3/4 of an inch!

That's crazy. And they show inner layers needing to be wider than microstrips. Doesn't epoxy-glass conduct heat better than air?

They don't account for heat conduction to inner-layer planes either.

torsdag den 27. juli 2023 kl. 16.48.06 UTC+2 skrev John Larkin:

Entering

1 oz copper 5c rise 10 amps 62 mil pcb thickness 8 mils to a big plane external trace

It claims that I need a trace 1580, or 560, or maybe 440 mils wide.

My private calculation, and experience, says that 100 mils wide would be about right for the 5c temp rise, given that plane 8 mils below. Imagine a trace that's an inch and a half wide for 10 amps!

It also says that internal traces have to be 3x as wide as surface traces.

This is pitiful. The PCB thermal calculators seem to use random number generators.

torsdag den 27. juli 2023 kl. 17.48.00 UTC+2 skrev John Larkin:

copper's resistance + ~0.4% per C so it should be easy enough get some actually numbers with a test pcb and a powersupply

Yes, copper resistance can measure actual trace temps.

I probably have enough old multilayer boards around to do some maybe-destructive testing. Baking a new proto board is a possibility, and I could include some other circuits. I want to test the AP66300 switcher and eval boards can't be had now for some reason.

Yes, it does (air's thermal conductivity is lousy) but that's not the right question. Relatively little heat leaves the board by conduction to air. Most of it leaves via convection (or forced-air).

Equally importantly: the higher thermal conductivity of the epoxy- glass isn't magic. It still adds thermal resistance between the heat source and the outside of the board, in addition to the "surface to ambient" thermal resistance which both internal traces and microstrips have to deal with.

If we neglect the presence of inner-plane flooded layers, then of course the inner traces would need to be wider than the outer, for a given amount of heat dissipation and acceptable temperature rise. The thermal resistance to ambient for an inner layer is going to be higher than that of the outer layers.

Every layer the heat has to go through on its way to ambient is going to add thermal resistance. The thermal resistance to the two sides of the board will combine in the usual parallel-resistance formula. For a trace on the surface, the resulting resistance will be dominated by the direct-to-air resistance on that side, and so it'll be lower than a trace right in the middle.

Now, to add in the "inner layer" effect accurately, you'd have to give an accurate model for the heatsinking ability of those inner planes. What is _their_ thermal resistance to ambient, on a given board? Is there a direct and efficient heat-path from the power and ground planes out to ambient (e.g. big fat power-supply connectors and heavy copper wire to some cold place) or are the power and ground planes thermally "trapped inside" the board and mostly just moving heat around inside the board?

You also would need to consider whether you're trying to get a valid number for a board with just a few traces high-current traces, or for "they're all going to be like this". If it's just one or two traces (hotted up at any given time) you can probably treat your internal planes as something like near-infinite heat-sinks to ambient, and get away with a thinner trace. If you're designing a board which is going to be full of these hot traces operating simultaneously, then you can't make this assumption - the ability of the inner planes to conduct all of that heat out to ambient is likely to be limited and you'll have to limit your heat-generated-per-trace or the board as a whole will cook itself.

I'd guess that the calculators are designed based on some conservative (near to worst-case) simplifying assumptions. "So, you want to fill your whole board with traces like this, and you can't count on your internal planes sinking a lot of heat out to ambient? Do it this way, keep your generated heat down to a minimum, and you can be reasonably confident that the board probably won't cook itself to death before the warranty expires."

If you want a more accurate set of numbers for your own specific board design, you'll probably need to do some finite-element thermal modeling based on your actual board layout, and tune things manually based on your actual trace usage. If you've got 2-3 energized relays on the board at a time, you'll probably like the answers a lot better than if you're expecting to have dozens of relays pulling current most of the time.

If you thermal image the surfaces of a board that has a hot trace inside, the hot area of the board will be wider than the trace. For a narrow trace, much wider. The epoxy spreads the heat and allows the trace to contact a lot more air on both sides.

A full-board ground plane, or better yet a ground plane and a couple of power planes, will spread the heat over the entire board surface.

An inner layer trace could dump heat through thin FR4 layers to thermally conductive planes above and below.

Unless the spreading effect wins. FR4 conducts heat about 12x better than air.

I'll just experimant with a real board. Buying and learning the FEM software would be 50x as hard.

I am disappointed how little that hard numbers are available. And the wild range of calculated results.

If you are pushing the limits of maximum temperature due to thermal expansion and/or the number of temperature cycles, I wonder if placing a number of small round holes in wide traces and planes would help? Not a hole through the fiberglass, just a hole through the copper much smaller than the width of a trace. That would allow resin to flow in and fill the hole during manufacture and should "pin" the trace to resist lateral movement and delamination. Hopefully the loss of electrical performance could be kept small for a substantial increase in the mechanical strength.

Mechanical stresses won't be an issue. Toasting the epoxy-glass will.

I've never seen a board self-destruct from current-induced thermal expansion. They make boats and bathtubs and Corvettes from epoxy-glass.

I have seen a few fused traces.

I was making the assumption that the yield strength of the copper would be greater than the bonding strength of the copper to the substrate so that using the holes to increase the bonding strength of the copper to the substrate would increase the failure strength of the assembly. If they stay bound together then localized bending or curling could relieve some of the stress by spreading it out instead of keeping it localized to pop the copper off the substrate. May not make enough of a difference to matter but it seems a simple, cheap modification to at least try if JL is going to test a few boards to destruction :-).

On a sunny day (Sat, 29 Jul 2023 10:15:18 -0700) it happened John Larkin snipped-for-privacy@highlandSNIPMEtechnology.com wrote in snipped-for-privacy@4ax.com:

Hey, I had some TV sets in for repair that were hit by lightning Several tracks just had evaporated. Managed to fix it.. needed some part replacement too.

Yes

I've seen successfully fused traces, typically where the overload was massive. I've seen many more where the result was a pile of conductive arcing carbon & junk. If you must use a trace as a fuse, I'd at least give it lots of clearance. And don't be surprised by a messy arcing shorting result.

Carl, this is 'cycling', not static stress.

RL

The real problem is likely to be the glass transition temperature of the epoxy resin. The one time I had my nose rubbed in it, the mechanical engineers had used an epoxy with a glass transition temperature of 62C (which is pretty common) to position a pair of electrodes which were supposed to measure the conductivity of a a water-based wash liquid that got up to 85C. None of us were pleased when the electrodes started moving around at 62C.

I found an epoxy resin with a glass transition temperature of 125C which saved the day.

A glass-fibre-epoxy printed circuit board that got hotter than the glass transition temperature of its resin would probably start sagging, and stay permanently sagged when it cooled off.

Getting the copper traces hot enough to melt copper isn't going to be what messes up your board.

Yes, but a lot of materials fail after lots of cycles of stress that is well below the ultimate tensile strength. Steel lasts "forever" so long as you stay below the ultimate tensile, aluminum fails after "some number" of cycles well below UTS. After some number of cycles the bond between copper and substrate will begin to lessen, which eventually will degrade the heat transfer, which will eventually make the trace run hotter, etc. I was thinking more about the total number of use cycles of the product since JL's application is a tester where the current will be cycled frequently, not about prompt failure. I've seen heater controller pcbs with traces carrying a few amps of 110VAC that ran cool when new, then over a few years the fiberglass started to turn brown, and eventually some charred and burnt, all while the current stayed within spec until the final fire. Just thought this might be a way to slow that progression.

I have seen PCB traces used as last-resort fuses. It's not an unreasonable concept, but I was diasppointed to not find any useful references to the appropriate geometry and dimensions.

But polyfuses would be better, if I can fit 48 of them on my board and somehow route the hundreds of fat traces.

Why solve stupid useless puzzles in the back of the New York Times, when PCBs are more challenging?