I am currently designing a PCB for a 10A relay and need guidance on determining the appropriate trace width.
Trace width calculators recommend considering copper thickness, maximum current, and temperature rise. Since I’m aiming for a cost-effective design, I’d prefer to stick with 1oz copper thickness. This leaves temperature rise as the key variable to adjust.
Using a calculator with 10A current, 1oz copper, 1 in trace length, and a 10°C temperature rise, I get a 283 mil trace width, which is too wide.
Increasing the temperature rise to 100°C results in a much more manageable 70mil trace width.
My question is: How do you determine an acceptable temperature rise for a PCB trace? Are there any general guidelines or factors to consider when making this decision?
Additionally, why is the temperature rise inversely proportional to trace width?
To determine an acceptable temperature rise for a PCB trace, consider factors like the operating environment and reliability requirements. If the temperature rise is too high, the PCB will get too hot, potentially affecting other components nearby. This could lead to shorts or even damage. So, it’s crucial to keep the temperature rise within safe limits.
General guidelines suggest keeping temperature rise within reasonable limits to avoid issues like signal distortion, component degradation, or even safety hazards. Factors such as airflow, ambient temperature, and nearby heat sources also play a role.
As for why temperature rise is inversely proportional to trace width, it’s because wider traces have lower resistance and consequently generate less heat when current flows through them. Thicker traces offer better thermal conductivity, effectively dissipating heat more efficiently, thus leading to lower temperature rise.
To further reduce trace width without sacrificing performance, you can use multiple layers on the PCB. By splitting the trace into multiple layers and adding via stitching, you distribute the current flow across parallel traces, reducing the overall current density and allowing for narrower individual traces. This helps optimize space usage and minimize manufacturing costs while meeting design requirements.
There are a lot of variables to consider! The junction temperature of any local ICs for good reliabilty is 150°C but if you are running the PCB in the artic only the ambient is generally -10°C so a rise of 160 is acceptable, but if run in the sahara at 50°C then you only have 100° to lay with. Generally a 5 or 10° is used. Consider that the bab of an auto can hit 100 on a hot day. Engine compartment can get to 130 easily. A cat hits 400 to 500°C
Deciding how fat your trace needs to be has been an ongoing debate for decades. The factors going into the decision are 1) Desired trace width, 2) allowable temperature rise, 3) length, 4) location, 5) trace thickness, 6) allowable voltage drop
If you’re dealing with sensitive circuits where the exact amount of voltage is a primary requirement you’re Fairly limited. If the allowable temperature rise is your concern there’s more wiggle room. Here’s why.
If you have a very short trace, especially between two thru-hole components, you have much greater leeway as the component leads and bodies will provide a lot of heatsinking compared to the trace. So the shorter the better if you have a choice. Inner layers will also allow higher currents for the same reason. And if you’re not concerned about the voltage drop you only need to deal with temperature. Let’s say you had a ceramic substrate - you could let it get pretty hot (as long as nothing else is too close). If you board has lots of heatsinking and cooling you may be able to go much hotter. So some of these are trade-offs the designer can make. You said cost was important and were holding it to one ounce copper. Find out how much two ounce copper will add - it may not need to be that much when you consider the PCB shop can either buy it that way or plate it up to two ounce. Then specify HASL as a finish which will probably add another half ounce or so. If you look at the fusing current for various trace sizes you’ll see there quite a bit of headroom. More voltage drop or higher temperature might be acceptable for your case.
As for your last part, just imagine it. If you have a lot of current in a fine wire (think toaster here) it glows red hot. Start adding more “meat” to the wire and the heat is spread out and no longer red hot. Check our website for a trace calculator and look at IPC-FC-217.
Dear Rachel, answering the basic question. You are asking in Trace width. Think Traces are like round conductors but flat. So your 283mil externally are not two wide, they are what they are because you are using 1oz. Use 2oz and it will be half (142mil) because you increase the height (t) so the width went down but the area (t)xW is about the same. For DC, this one flows through the entire conductor, So what’s important is the area, just as any round conductor with AWG # and minimum and maximum current. So in Traces, the Copper has an average thickness (t) and a Width(W) so you know what’s the area equivalent for a circular conductor. Now, what you need to consider is that you do not want the trace to be hot or warm because heat will travel through the board. I used a place slot in the PCB to prevent heat traveling (conduction). from high current traces. Now, Inside traces will be about twice the width of the outside layers because we want to reduce the heat. So to trace Power traces, the best is to route them externally, and use 2oz or more, you are trying to mimic a conductor. If you need the entire board with 1oz, your traces will be wide, inside will be twice wide. Talk to the fabricator to see how specific traces can be added copper to make them thick while the rest of the board is thinner. I heard it is possible. But 10A traces don’t allow more than 10-15deg rise above ambient because you must consider the Operating temperature of the end device. If your equipment is 60deg Max, you will have traces running at 75deg. I have done a Board that replaces just Plan cables, but the minimum Cu layers used are 2 oz and multi-layer 10-12, so yes!! very thick board. There are some online calculators and if they say they use IPC equations is about the same equations found in IPC -2152. The curves there for internal or external sources are based on Cross-Section in Squre-mil, a terminology for Round conductors.