How to Design Thermal Reliefs with Minimal Manufacturing Issues

October 15, 2016 , in Blog

Thermal Relief Pads

Electronic components become smaller and smaller every year; the market, in turn, demands electronics with ever-shrinking form factors. PCBs with dimensions under an inch are commonplace, and their surfaces are growing more tightly packed with placements. Some designers, in the interest of squeezing slightly more space out of a small area, are leaving out thermal reliefs — but this can be a bigger mistake than it seems.

A thermally relieved pad is an SMT pad with the copper around it removed (“relieved”) except for 2–4 traces. Adding thermal relief to pads that will have components soldered to them is crucial in directing and controlling the flow of heat through your board during reflow. Pads with poor thermal relief may not heat evenly in the reflow oven and cause tombstoning, no-connects, or poor solder joints, which require manual rework. Rework is then impeded by a lack of thermal relief as well. Adding thermal relief to your design can reduce quality problems as well as the time needed to repair them.

The use of thermal relief for these pads will make rework easier and quicker by eliminating the higher conductivity and time it takes to heat up all or most of a copper pour, as with a solder mask defined pad. A single pad with thermal relief will reach the correct temperature much more quickly. If there are component pads next to each other that share the same copper pour, it can be very time-consuming to heat up a pad, even for experienced technicians. In some cases rework may not be possible due to the amount of heat and time it takes to bring a pad up to temperature without thermal relief — components and/or the board’s surface can easily suffer damage from the extended use of a soldering iron. Thermal relief for pads is easy to implement, and strongly recommended for any electrical component that doesn’t require a high voltage current. With higher copper weights, thermal relief may save hours of rework time and also help ease the initial soldering process.

Formulae for designing thermal reliefs

This is the suggested formula for designing thermal reliefs that we use at Tempo Automation, which follows IPC-2222 standards.

Thermal connecting trace width:

X = Overall length of the X or Y-axis of an SMT Pad (Imperial / metric).

Y = Quantity of thermal connecting traces.

T = 60% of the pad size.

Z = Trace width ( T / Y )

(X * 0.60) / Y = Z

Example:

We have a .040” x .040” SMT pad, so we will take the length of either the X- or Y-axis and plug it into ‘X’. (For this example, we take the X-axis length.) We need 4 thermal connecting traces, so ‘Y’ will be 4.

(.040 * .60 ) / 4 = Z

.024 / 4 = Z

.006” = Z

Thermal relief size:

X = Overall length of the X- or Y-axis of an SMT Pad (imperial / metric).

TR = Distance from thermal relief pad to copper pour (this must not exceed the minimum of .005”)

X * .25 = TR

Example:

We have a .040” x .040” SMT pad, so we will take the length of either the X- or Y-axis and plug it into ‘X’. ( For this example, we take the X-axis length.)

.040 * .25 = TR

.010” = TR

 

The latest PCB news delivered to your inbox.

Search Sign In
[[]
[[]
[").replace(/[]]
[").replace(/[]]
[?&]
[?&]
[^&#]
[^&#]
[name="email"]
[name="email"]
[w-.]
[w-.]
[w-]
[w-]