EEVblog > EEVblog Specific

EEVblog 1559 - PCB Design: Trace Current Rating

(1/5) > >>

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:

--- Quote from: Paul Bryson on August 11, 2023, 02:14:57 pm ---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.

--- End quote ---

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.

 

Navigation

[0] Message Index

[#] Next page