5. Net Classes
5.2. High Current Traces
"We don't need to worry about this in our design. However, as a rule of thumb, you should consider high currents as anything over 500 milliamperes of current. This is a tad over-conservative, and you might not need special consideration for even a 1-ampere trace, but high currents can create high-heat, which shortens the lifespan of your PCB and components, and it can create fire, so it deserves at least a little of your time and attention."
Printed circuit board traces generate heat when charges travel through them and traces dissipate heat through conduction, convection, and radiation. If the current is constant, the heat sources and the heat sinks will reach equilibrium and the trace will remain at a constant temperature that is above the ambient environmental temperature.
As charges move through a conductor, some of their electrical energy is converted into thermal energy -- you might remember hearing this referred to as Joule heating or Ohmic-heating. The rate of energy conversion is given as P=I²R.
The square of the current is proportional to the heat generated. So for a given trace, a 1-ampere current generates four times as much heat as a 0.5-ampere current. A 2-ampere trace generates sixteen times as much heat as a 0.5-ampere trace. In short, if you aren't paying attention, you can design a board that catches fire with very little effort. This is common for new designers intent on squeezing as many traces as possible into as small an area as possible.
Heat transfers via three methods: Conduction, Convection, and Radiation.
At the temperatures that most PCBs operate, the net radiation flux is not a significant source of heat transfer -- the radiation energy emitted is only marginally greater than the radiation energy absorbed. That leaves conduction and convection as the predominant sources of heat transfer in a printed circuit board.
Conduction requires direct contact between materials to transfer thermal energy. And materials that make good electrical conductors tend to make good thermal conductors. You've likely already realized touching a metal railing on a hot day is much less pleasant that touching a wooden railing -- the metal can transfer energy at a greater rate than the wood. The same is true in a PCB. The metals/conductors (Copper, Silver, Tin, etc...) are able to conduct several orders of magnitude more heat energy than the dielectrics/insulators (FR-4, LPI Solder Mask, etc...), including the air that surrounds the board. Heat energy can move through your board via conduction, but unless your PCB is attached to a metal frame or metal-fin heat-sinks, the heat energy generated inside your board cannot transfer off your board via conduction.
That leaves convection as the predominant source of cooling for most PCBs. In convection, air molecules collide with a high-temperature part of a PCB and a small amount of thermal energy is transferred from the PCB to each of the air molecules. That energy allows the molecules to spread out, decrease density, and get displaced upwards by cooler, less energetic molecules. The PCB transfers thermal energy to the new molecules and the cycle endlessly repeats.
When natural convection isn't enough or isn't available, engineers can resort to heat-pipes, heat-fins, and forced-air to cool their boards (among other things).
If you have high-currents moving through your project, it is important to leave room for airflow inside your enclosure.
Designing for High Current Traces
You should know by the time you complete your schematic whether or not you have any high-current nets. Datasheets indicate the maximum currents your parts might draw, and a detailed power budget can give you a decent idea of what current demands to expect from your power source. You also need to know the operating environment of your board, the material properties of your dielectric, and if there are any heat-sensitive components near your trace. If your trace gets too hot -- it can melt the dielectric material enough to damage it, and even moderate temperature excursions can force you to derate nearby passives or alter sensor readings. So after you know your current requirements, decide what an allowable temperature increase in that part of the PCB might be.
With those details in hand, you can set to work defining the trace specifications.
Option 1: Estimate Using ICP-2152
"Most website trace-width calculators use IPC-2221, which is deprecated, do not use it. IPC-2152 is based on empirically collected data, and offers less conservative results than IPC-2221"
If you have a plain PCB with no attached thermal features, such as pin/fin heat sinks, heat pipes, fans, etc..., convection is available to you, and you aren't in a harsh or high-altitude environment, you might consider the equations available in IPC-2152, and explored at length, by Dr. Douglas Brooks and Johannes Adam in the book PCB Trace and Via Currents and Temperatures: The Complete Analysis. (The chapter Trace Currents and Temperatures Revisited, is available free from Dr. Brook's website Ultracad.com for free.)
In the book, and the article, Drs. Brooks and Adam look at the relationship between current, temperature change, copper-weight, and trace-width. You can use the equations provided to determine suitable trace widths for a variety of copper-weights.
Royal-Circuits took the equations for surface-traces and rearranged them for a variety of temperatures -- you can see the results in the appendix to the blog post: "Copper Trace and Space: Three Factors to Consider." Here's an example graph from that post.
In this graphic, the relationship between copper weight and trace width is shown for a surface trace that is allowed a 20° C temperature increase compared to its neighboring traces. Internal traces or a PCB in a high-altitude environment would see a coefficient less than 215.3, which would shift all curves downward.
A 1-ounce external copper-weight is fairly common for a PCB. Here the graph shows that 1-oz of copper that is ~7 mils wide can handle 1-A of current and only raises the trace by 20° C over ambient temperature.
Option 2: Simulate Using FEA or CFD Tools
Many of the popular 3D cad packages (Solidworks, Autodesk, etc...) come with advanced analysis and simulation tools. Finite Element Analysis can model the conduction of heat around your PCB, while Computational Fluid Dynamics can handle convection.
If you'd like to explore the effect of adding a finned heat-sink to your design, an online simulator such as SimScale (free) might be of interest to you.
This model of convection currents around straight-fin heatsink is from SimScale.com
Option 3: Iterate using Thermocouples or Thermal Camera
There is no amount of simulation that can take into account every possible real-world variable. If you are designing a motor-controller for an electric-vehicle, at some point you need to install your board inside your test vehicle and drive it out to the middle of Death-Valley National Park in the middle of a summer heatwave, point a thermal-imaging camera at it, and see where the hot points are. Then you increase the copper surface area in those parts of the board. Sometimes, it's not possible to put a thermal camera in a position to see a PCB in action, in those cases, engineers will install thermocouples at strategic points on a board, record it under operation, and make adjustments for the next revision.
Your PCB trace-width and copper thicknesses can be increased to handle high-currents. Once you have determined an appropriate trace-width for your designed current, you can define a net-class for that current. Then any nets in your design that must carry that current will be included in any future adjustments. This makes changing copper weights a simple matter.