EEVblog 1559 - PCB Design: Trace Current Rating

[EEVblog]

Dave answers a Twitter question: How should I design a PCB trace to carry 80A of current, and can this be done on one PCB layer? The answer is, well, complicated. Let's go down the PCB design rabbit hole of current rating PCB traces.

PCB Design Video Playlist: https://www.youtube.com/playlist?list=PL8D3B363139B67FF3

00:00 - Twitter question: How should I design a PCB trace to carry 80A of current
01:09 - Ohms law and copper losses
02:06 - PCB Trace calculator
02:45 - The three (four) major factors to PCB current handling calculations
02:54 - Trace Width and Copper thickness (weight) and PCB stackups
04:18 - A trap with Multilayer PCB designs
05:20 - External vs Internal layer matters with thermal design
06:20 - What happens if you exceed the maximum current rating?
07:23 - PCB plating matters
08:12 - Electrical vs Thermal design considerations
09:30 - 1oz copper vs 2oz vs 4oz
10:35 - Solder and tin plated traces
11:37 - Let's look at what a PCB manufacturer offers, HASL, SMOBC, ENIG etc
12:46 - How do you get your PCB traces plated in your design?
14:31 - Those are rookie temperature numbers, you gotta pump those up!
14:51 - The IPC 2152 and IPC 2221 standards are a bit How'ya'Doing
16:30 - The physical and thermal part of your product design matters
16:47 - Thermal conduction to planes matters
19:30 - Does VIA stiching matter?
20:30 - Have you considered a Bus Bar?
21:56 - We can get 80A on a single PCB trace, BUT...
23:18 - Can I interest you in bodge wire Sir? It's complete legit.
24:17 - PCB Standard WARS!
26:19 - Forget about etch factor
27:08 - Internal vs External trace calculations

[jahonen]

Having done plenty of DC drop etc. simulations on HyperLynx and some with Ansys SIWave, I think that the most difficult thing in high current traces/planes is how to get the current into and out of the high current plane/trace without blowing through the roof with the current density where your loads, interconnecting vias and sources are, i.e. how to distribute the current evenly. Even if the plane/trace is very wide, you have a problem how to connect all the current often to a very much smaller area. That tends to create high current densities near the connections.

Also, multiple vias tend to be difficult, since often only the nearest vias facing the incoming current tend to "steal" all the current and rest of them will do pretty much nothing and just increase the cost of the PCB Also, copper thickness in the walls of the vias tend to be quite loosely specified.

Regards,
Janne

[Paul Bryson]

People often make several incorrect assumptions about PCB heat dissipation. Intuition may mislead you.

The #1 misconception:  PCB fiberglass is a good thermal insulator.
In still air, the thermal resistance of the PCB to air is so high that you can almost discount the thermal resistance of the PCB in the vertical dimension. The layers of fiberglass are thin and present relatively low thermal resistance compared to the PCB-air interface.  That means that for copper on the top surface of the PCB, almost as much heat will dissipate through the bottom side of the PCB as off the top.  The case is similar for internal copper layers.

Misconception #2: Nearly all the heat transfer from a PCB is conductive. 
In fact, as much as 40% of the heat can be radiated.  Therefore anything that increases the emissivity of the PCB will help get rid of heat. Shiny metal is your enemy. So adding matte soldermask over the copper may actually significantly increase the heat dissipation!

[thm_w]

The #1 misconception:  PCB fiberglass is a good thermal insulator.
In still air, the thermal resistance of the PCB to air is so high that you can almost discount the thermal resistance of the PCB in the vertical dimension. The layers of fiberglass are thin and present relatively low thermal resistance compared to the PCB-air interface.  That means that for copper on the top surface of the PCB, almost as much heat will dissipate through the bottom side of the PCB as off the top.  The case is similar for internal copper layers.

Yeah. The main reason in current rating difference is outer layers are typically plated to 1oz whereas internal layers are left at 0.5oz unplated.
You can get 2oz outer and 1oz inner, but costs go up. For JLC 4 layer is $7, then if you go 1oz inner $23, 2oz outer or 2oz inner is $40.

A lot of PCB calculators incorrectly tell you that inner layers need to be wider for the same current rating and thickness, as they are based on IPC standards that were pulled out of thin air (no experimental data was used). Saturn calc will now just give you the same rating for internal/external trace.

https://www.signalintegrityjournal.com/articles/1596-internal-trace-temperatures-more-complicated-than-we-think

[richnormand]

Having seen and done several repairs with devices (industrial and some for domestic uses) in the 15 to 20 amp the pcb traces to the solder point was usually at fault.

In many cases where the trace was adequate but the solder point was near the edge of the trace with a puny through hole. Only half of the solder joint was "active" and typically the fire and carbon tracking was from the thin side.
If you used a 1" trace better make sure you have a 1/4 or 1/2" solder point radius.
Worse cases were when a connector was used. Either the solder joint failed from insertion stress or cable induced vibrations in use and that caused the pcb to burn locally and propagate.

Repairs were by cutting all the burned pcb and dead bug with 20A rated copper wires.
One manufacturer kept their design but added a solid copper wire wrapped around the connector pin and along the pcb trace to the other end, all of which was soldered to the trace.
They also did that for the input side too. Never had a failure after that.

Better safe than sorry than cost cutting and finding out..... design with a good safety factor.

 

[EEVblog]

Therefore anything that increases the emissivity of the PCB will help get rid of heat. Shiny metal is your enemy. So adding matte soldermask over the copper may actually significantly increase the heat dissipation!

Yes, I was thinking about doing a custom PCB to measure this under the thermal camera + contact temp probe. Shiny copper has an emissivity bordering on zero.

[SiliconWizard]

How about room temperature superconductor-based traces?

Jokes aside, yes busbars are often a solution for this design problem.
If using through-hole transistors, one approach (that was relatively common in older days) can also be to wire these separately from the PCB altogether. Of course that may add to manufacturing costs though.

[Psi]

Example of 30oz copper, if you have the cash.
Can also be selective, only thick in some sections.

[SiliconWizard]

Now that's thick!

[.RC.]

Just do what I did.   Copper pads cut drilled and soldered on and 3mm thick solid copper wire.

OK for a hobby project, but of course not practical for anything you want to make money from.  (it is an induction heater circuit)

The original board design failed at the original connection (I did not design it).

Yes my soldering skills suck, I know.   

[Psi]

One of the problems you get with thick copper is the bigger track/gap space causing smaller chips like QFN DFN to no longer be possible on that layer. It starts to be a problem at 3oz

You can choose to have your thick copper layers be internal layers and keeping 2oz on at least one outer layer for your QFN/DFN chips. But if you wanted the thick copper for SMT Mosfets then they have to go on the outer layer. So you can end up having to use thin copper just to get the current out of the mosfet and to the via stitching so it can get down to the thick inner layer as soon as possible.

[germitron]

Hi,
Recently I really interested in high current PCBs mixed with low voltage stuff, because I have to design one. The attached image shows an EV charger (Wallbox Pulsar Plus) carrying 3x32A mixed with measurement electronics. It seems that the 3x32A is handled only in internal layers.
I would like to know your thoughts about the layer stackup, insulation between layers and clearance.
Thank you!

[nctnico]

There is no way that board handles 32A. It also is a single phase design...

[germitron]

Sorry, yes, this is just a one phase charger, but there is a more compact design that handles 3x32A:
https://wallbox.com/en_catalog/copper
And possibly a 3 phase energy meter is also integrated, see those CTs.

[BrianHG]

I'm curious.  I know Dave spoke a lot about etching copper away and I know this is a standard PCB process.
But, I though I heard at one of my local fabs where I got a tour decades ago that they use a copper additive process instead of etching.  It this true?  I would suspect that using an additive process would allow for what was shown in Psi's posted image above with the multi-thickness 10/20/30oz  traces.

[coppercone2]

you could make a custom one with bifuricated terminals

[schmitt trigger]

Yes my soldering skills suck, I know.   

If we were making a contest on who makes the most horrible solder joints, I would always end up on the top-3 position. No contest. I possess a 9th Dan black belt in terrible soldering skills.
I hesitate to post a photo because I could be banned for posting obscene images.

Back to topic: I have used the exact same technique for high current devices, whose total production quantities you could count with one hand.

[coppercone2]

copper addition will lead to reverse undercut so you can machine that way. with undercut you would need to weld metal on or something.

[EEVblog]

I'm curious.  I know Dave spoke a lot about etching copper away and I know this is a standard PCB process.
But, I though I heard at one of my local fabs where I got a tour decades ago that they use a copper additive process instead of etching.  It this true?  I would suspect that using an additive process would allow for what was shown in Psi's posted image above with the multi-thickness 10/20/30oz  traces.

Yes, you can plate copper or other materials onto the existing copper.

[floobydust]

Sorry, yes, this is just a one phase charger, but there is a more compact design that handles 3x32A:
https://wallbox.com/en_catalog/copper
And possibly a 3 phase energy meter is also integrated, see those CTs.

That wallbox charger design looks basically terrible - the four relays have 2W coils plus another few watts dissipated in contact resistance - it generates a lot of heat.
It's made as small as possible, I see no cooling fan or ventilation louvers. This is a mistake with high current designs, they aren't going to be small and cute for many reasons.

[thm_w]

I'm curious.  I know Dave spoke a lot about etching copper away and I know this is a standard PCB process.
But, I though I heard at one of my local fabs where I got a tour decades ago that they use a copper additive process instead of etching.  It this true?  I would suspect that using an additive process would allow for what was shown in Psi's posted image above with the multi-thickness 10/20/30oz  traces.

As I mention above, 0.5oz is the typical copper clad laminate thickness. So you etch that and then plate to the final required copper thickness (1oz 2oz). Starting with very thick copper and etching it away is not as economical, and makes it harder to produce small features.

"Boards incorporating heavy copper circuits are produced in exactly the same way, albeit with specialized etching and plating techniques, such as high-speed/step plating and differential etching. Historically, heavy copper features were formed entirely by etching thick copper clad laminated board material, causing uneven trace sidewalls and unacceptable undercutting. Advances in plating technology have allowed heavy copper features to be formed with a combination of plating and etching, resulting in straight sidewalls and negligible undercut."

https://www.pcbway.com/pcb-service.html?step=10#miao10
https://www.epectec.com/articles/heavy-copper-pcb-design.html (this is where the image came from)
https://www.pcbcart.com/article/content/FR4-copper-clad-laminates.html

[Neilm]

I had an e-mail at work this morning from a PCB supplier that does heavy copper PCBS - 5oz. Really heavy copper - 15 oz.
https://www.gspkcircuits.ltd.uk/pages/195/Heavy-Copper-PCBs/

[satyamfifa]

My solution when I did the 60A PCB design was to first of all get like 2 layer both 2 oz copper (reasonably priced) thick pcb. Then just take a thin sheet of copper, simply cut it, and solder that on top of where I need the high current, instead of getting custom busbars made.

https://www.eevblog.com/forum/projects/60-ampere-bldc-pcb-design-and-routing/



it is also to be remembered that high temperature rise at short distances is fine, since the heat will dissipate

[Psi]

My solution when I did the 60A PCB design was to first of all get like 2 layer both 2 oz copper (reasonably priced) thick pcb. Then just take a thin sheet of copper, simply cut it, and solder that on top of where I need the high current, instead of getting custom busbars made.

What voltage/capacitance are those huge ceramic caps? 
Must cost a lot.

[satyamfifa]

Yes indeed, I wanted to as low ESR capacitors as possible, as close to FETs as possible

https://nl.farnell.com/murata/kcm55wr71j226mh01k/cap-22-f-63v-20-x7r-2220/dp/2781467?ost=2781467