Will this survive 20A?

[HwAoRrDk]

I am designing a PCB layout where I have a couple of traces that are high-current, but I need to transition the trace between top and bottom layers. I have been trying to figure out whether the via arrangement I have designed will be suitable.

The expected normal current running on these traces will be around 7-8A, but as the circuit is on a 20A fuse, I want to make sure that if a fault condition occurs, the fuse will actually blow rather than my PCB going up in smoke. That is, these traces and vias should never need to handle 20A in normal operation, but I want it to be able to survive a brief 20A peak with no damage.

What I have designed so far is as below:



The trace is approximately 5mm in width for its full length. There are 9 x 0.6mm diameter vias. The PCB will be 2 oz copper.

Is this via arrangement suitable, or will my board catch fire?

[schmitt trigger]

I would do a ""test coupon board" with different configurations, and validate the capabilities with tests.
I would at least repeat the current surge 5 times, with a proper cooling period between surges.

For the configurations that survive, perform a cross section and inspect the copper via with a good optical microscope.

[cowana]

If you 'unrolled' a 0.6mm via, the width would be 1.88mm (the circumference).

Therefore the 9 vias together would be the equivalent of a trace 17mm wide, and the thickness of the plating (typically half the surface thickness). So the resistance of those vias will likely be similar to a 8mm track on the surface.

[Monkeh]

Yes, that should handle 20A - pretty much indefinitely, actually.

[tszaboo]

Copper thickness? How many layer board?
I mean, it will survive. But it will definitely it will be warm.  Satrun gives a 75K temp rise, which will be worse near the vias.

[Monkeh]

Copper thickness? How many layer board?
I mean, it will survive. But it will definitely it will be warm.  Satrun gives a 75K temp rise, which will be worse near the vias.

The trace is approximately 5mm in width for its full length. There are 9 x 0.6mm diameter vias. The PCB will be 2 oz copper.

That'd be 30-40C temp rise at 20A, and less on the vias. Board is pretty visibly two layer.

I see no problems with 8-10A continuous and 20A fault current as long as it's not living inside an oven.

[HwAoRrDk]

Thank you for the input, guys. Looks like what I have is going to be okay.

One further question: does the pattern the vias are arranged in have any effect on the current flow? I mean, say for example I had the vias in two rows (of 4+5) instead of three. Will current flow equally amongst all the vias regardless of layout? Or will certain vias handle more current than others, creating 'hot spots'?

I would do a ""test coupon board" with different configurations, and validate the capabilities with tests.
I would at least repeat the current surge 5 times, with a proper cooling period between surges.

For the configurations that survive, perform a cross section and inspect the copper via with a good optical microscope.

Thanks for the suggestion, but unfortunately I have no means to perform such experiments.

If you 'unrolled' a 0.6mm via, the width would be 1.88mm (the circumference).

Therefore the 9 vias together would be the equivalent of a trace 17mm wide, and the thickness of the plating (typically half the surface thickness). So the resistance of those vias will likely be similar to a 8mm track on the surface.

So if I knew exactly what the through-hole plating thickness would be, it would be possible to work things out more precisely? I suppose I can ask my prospective PCB manufacturer if they have a specification on that.

That'd be 30-40C temp rise at 20A, and less on the vias. Board is pretty visibly two layer.

I see no problems with 8-10A continuous and 20A fault current as long as it's not living inside an oven.

I'm expecting ambient operating temperature to be around 45C at worst - certainly no more than a person could stand to be in, anyway. A brief 40C rise above that is I assume perfectly acceptable for even the cheapest of FR-4 boards?

[Monkeh]

You might want to see if you can find room to fatten up the trace and add a few more vias if you're planning on 40C ambient. 8mm and vias to suit should give you plenty of headroom.

[DerekG]

There are 9 x 0.6mm diameter vias. The PCB will be 2 oz copper.

I would increase the diameter of the vias to 0.9mm or 1.0mm (better). I assume you are having these wave soldered? If so, request that the vias be left open (ie not covered over with solder mask as is becoming more common now). The vias will *mainly* fill with solder during the wave soldering process which will carry a lot more current for you.

For your tracks - why not open up the solder mask on the bottom side so the track receives a coating of added solder during the wave soldering process. This also aids in reducing the operating temperature of the track as it can dissipate the heat to the air much faster. You can also open up the top side solder mask & paste mask & "grid" a pattern of "squares" across the surface to increase the current capability of the top tracks.

If you want some pics of all of the above, just ask & I will post them. We do the above designs on a regular basis for heat dissipation from mosfets etc.

One further question: does the pattern the vias are arranged in have any effect on the current flow? I mean, say for example I had the vias in two rows (of 4+5) instead of three. Will current flow equally amongst all the vias regardless of layout? Or will certain vias handle more current than others, creating 'hot spots'?

The current will take the shortest path until the track (or via) heats & the resistance goes up. The current will then select the next lowest resistance path.

[T3sl4co1l]

So, what's the chip footprint thingy?  Just something off to the side?  Not carrying much current?

What's the current coming from?  The oblong hole, a THT pin?  Why not connect the trace directly up to it, no vias necessary?

As others have covered, a wider trace is probably a good idea.  PCBs get kind of inefficient beyond 10A, at least without additional layers and cooling (forced air, heatsinking pads).  If you don't need anything to cross the connection, you can use both layers in parallel.

As for via capacity, figure the barrel (inner surface) is plated with about 1oz, at the full circumference, and add up circumferences until you have the same cross section as the trace.  It's not rocket science.

Tim

[tszaboo]

Copper thickness? How many layer board?
I mean, it will survive. But it will definitely it will be warm.  Satrun gives a 75K temp rise, which will be worse near the vias.

The trace is approximately 5mm in width for its full length. There are 9 x 0.6mm diameter vias. The PCB will be 2 oz copper.

That'd be 30-40C temp rise at 20A, and less on the vias. Board is pretty visibly two layer.

I see no problems with 8-10A continuous and 20A fault current as long as it's not living inside an oven.

My eyes usually skip through Imperial units...

[schmitt trigger]

Tim;
upon closer inspection, you are absolutely correct.
Where is all the current coming from?

If it is from the oblong hole, then -as you mention- it would make far more sense to connect it directly from the opposite layer.

[HwAoRrDk]

I would increase the diameter of the vias to 0.9mm or 1.0mm (better). I assume you are having these wave soldered? If so, request that the vias be left open (ie not covered over with solder mask as is becoming more common now). The vias will *mainly* fill with solder during the wave soldering process which will carry a lot more current for you.

For your tracks - why not open up the solder mask on the bottom side so the track receives a coating of added solder during the wave soldering process. This also aids in reducing the operating temperature of the track as it can dissipate the heat to the air much faster. You can also open up the top side solder mask & paste mask & "grid" a pattern of "squares" across the surface to increase the current capability of the top tracks.

No wave soldering. Planning on reflow for the surface-mount components, then hand-soldering for the few through-hole components. This is not something that is going to be mass-produced.

I suppose if I really wanted the vias to be solder-filled, I could maybe do it with reflow by leaving them unmasked and adding a dot for each on the paste layer. Would that work? No idea how much paste each via would need relative to it's diameter, though.

This is actually my second revision of the board, and on the first I did actually have it with the tracks un-masked and coated with solder, but that was only because I was being tight-fisted and didn't want to pay for 2 oz copper for the prototype boards. I would prefer not to solder coat, as there is a component that has to sit partially over the tracks, and it sits wonky because of the uneven surface.

The current will take the shortest path until the track (or via) heats & the resistance goes up. The current will then select the next lowest resistance path.

Ah, I see. Makes sense.

So, what's the chip footprint thingy?  Just something off to the side?  Not carrying much current?

What's the current coming from?  The oblong hole, a THT pin?  Why not connect the trace directly up to it, no vias necessary?

It's a 1206 resistor. That and other components just out of shot are a divider/protection/filtering for an input to the micro for detection of when power is applied to that track.

The current is coming from the oblong THT pin on the left. Yes, you may be scratching your head wondering why I don't connect the trace up directly. It's a question of ease of serviceability and access. That pin (as well as others) is a fixed part of the assembly to which the board is attached. The board is installed by dropping it over the pins and soldering it down. Once installed, there is no physical access to the bottom side of the board.

Through experience with my first prototype, where these through-holes are plated, I have found that it makes the board a real bitch to de-solder. The pins are part of what are effectively copper bus bars, and thus a large heatsink. Every time de-soldering I have failed to avoid ripping out at least part of the plating of most holes. By having these pins soldered only on a single side - the accessible top side - it becomes a piece of cake to remove the board.

[Mattylad]

What is the thickness of your hole plating? That is what matters most to be able to calculate how many vias of what size you need for 20A.
You may be better off having them filled by the manufacturer.

[DerekG]

I suppose if I really wanted the vias to be solder-filled, I could maybe do it with reflow by leaving them unmasked and adding a dot for each on the paste layer. Would that work?

My thoughts would simply be to request the board manufacturer to leave the vias open (ie don't close them over with solder mask as is becoming quite common now), then when you manually solder the through hole components, fill up the vias as well. I would use 1.0 to 1.2mm vias in this case or better still, swap them out for some similar sized through hole pads.

[DerekG]

I suppose if I really wanted the vias to be solder-filled, I could maybe do it with reflow by leaving them unmasked and adding a dot for each on the paste layer. Would that work?

My thoughts would simply be to request the board manufacturer to leave the vias open (ie don't close them over with solder mask as is becoming quite common now), then when you manually solder the through hole components, fill up the vias as well. I would use 1.0 to 1.2mm vias in this case or better still, swap them out for some similar sized through hole pads.

[ahbushnell]

http://circuitcalculator.com/wordpress/2006/03/12/pcb-via-calculator/

This is a via current calculator. 

Andy