Thermal Relief Pads: Spokes, Soldering and Current

A thermal relief is a small piece of geometry that decides whether a component can be soldered at all. It is the difference between a pad that is connected to a copper plane by four narrow spokes and a pad that is welded to that plane with a full ring of copper, and it is one of the few layout choices that has a direct effect on the assembly line.

What a Thermal Relief Is

When a pad sits on a copper plane, the tool has to decide how to connect them. A solid connection fills the whole area around the pad with copper, so the pad is surrounded by metal on all sides. A thermal relief keeps the same pad but connects it through a small number of narrow spokes, with the remaining space around the pad left as bare laminate.

The pattern is usually four spokes at right angles, though three or two are possible where the pad is close to other features. The spokes are sometimes called webbing or legs, and the clearance ring around the pad is the air gap or thermal gap. Together they form a pad that is electrically connected to the plane but thermally only loosely coupled to it.

The name describes the purpose. The connection is a compromise between electrical and thermal behaviour, and the geometry is a deliberate heat break rather than a manufacturing convenience. It is also one of the most commonly misused features on a board, because it is applied by default in many tools without anyone deciding whether it belongs there.

Why It Exists

The problem is heat sinking. A copper plane is an excellent conductor of heat, and a pad welded to one behaves as though it is attached to a block of metal with a large thermal mass. When a soldering iron touches that pad, the heat flows out of the iron into the plane faster than the iron can supply it, and the joint never reaches soldering temperature. The result is a cold joint, a lifted pad, or a component damaged by a long dwell time with a hot iron.

The same effect appears in wave soldering, where a through hole pad connected solidly to an internal plane can stay below the solder temperature for the short time the board is over the wave. It shows up again in reflow on boards with thick copper, where the plane pulls heat away from the joint during the ramp so the paste on that pad does not fully melt even though the rest of the board does.

A thermal relief solves all three cases with the same mechanism. Four narrow spokes have a much higher thermal resistance than a solid ring, so the plane cannot draw heat away quickly, and the pad reaches soldering temperature in a normal time with a normal tip. The electrical connection is preserved because the spokes are copper and the path to the plane still exists.

When a Solid Connection Is Better

The relief is a compromise, and there are cases where it should not be used at all.

The first is current. Four spokes of a given width carry far less current than a solid ring, and the spokes have a higher resistance. On a power rail, a ground return carrying several amps, or a pad for a high current connector, a thermal relief adds resistance exactly where the design cannot afford it, and it can become the hottest point on the board. High current designs usually specify a solid connection with the plane flooded around the pad, and the assembly process is then adjusted instead, through a longer preheat, a higher peak temperature or a selective soldering step.

The second is thermal performance. A pad that connects a power device to a plane is often the device heat sink. A thermal relief there is a deliberate thermal bottleneck that raises the junction temperature, and the whole point of the plane connection is to conduct heat away. Where the pad is a thermal path rather than an electrical one, the connection should be solid, or made with a via array under the pad.

The third is reflow only assembly. Where every joint on the board is made in a reflow oven and the profile is tuned for the assembly, the heat sinking penalty is smaller, because the whole board is at temperature and the plane is part of the same thermal system. Plenty of designs run solid connections on surface mount pads and reflow them without trouble, particularly where the copper is thin.

There is also a signal integrity angle. A thermal relief pattern is a small local change in the return path geometry, so it adds a little inductance and a little resistance at the pad. At high frequency the spokes can look like a discontinuity. On RF boards, and on fast digital nets where the via and pad are part of a controlled impedance transition, the common practice is to use a solid connection or a tightly spaced via pattern rather than a relief with wide air gaps.

Sizing the Pattern

The pattern is defined by three parameters, and the values that most fabricators and assembly houses see as normal are reasonably consistent.

• Spoke width: typically 0.3 mm to 0.5 mm, and never below the minimum trace width the board is specified for.
• Air gap: the clearance between the pad and the plane is usually 0.25 mm to 0.5 mm, sized to the same rule as the board minimum clearance.
• Number and angle: four spokes at 90 degrees is standard, and rotating them to 45 degrees is common on round pads to improve symmetry.

Two details matter more than the numbers. First, the air gap must not become a thin sliver of laminate that peels during thermal cycling; a gap that is much smaller than the board minimum clearance is a defect waiting to happen. Second, the spokes should not be so narrow that they cannot be etched reliably on the copper weight in use. On a 2 oz outer layer, a 0.3 mm spoke is straightforward; on a heavy copper board it may not be, and the wider spokes then reduce the thermal benefit of the whole pattern.

On through hole pads the relief is applied on the layers where the pad meets a plane, which means the pattern may exist on inner layers and not on the outer face. That is useful, because a pad can have a solid outer face for easier soldering and a relieved connection to the plane underneath. Most tools let the pattern be defined per layer, and it is worth checking that the setting applied to the outer layers is the one you intended.

Thermal Relief or Via Array

The two features solve different problems and are often confused.

A thermal relief controls how much heat flows from a pad into a plane. It is used when that flow is inconvenient, which usually means during soldering.

A thermal via array is the opposite: a group of small vias under a pad that deliberately increases heat flow from a component into the board. It is used when the component needs to be cooled, and it is normal under a power device, a ball grid array with a large thermal pad, or an LED.

Putting a relief pattern around a pad that also has a thermal via array is contradictory, and it is one of the more common layout errors on power boards. If the pad is meant to conduct heat away, the plane connection should be solid and the vias should be there to move the heat into the layers below. If the pad is a signal pad that happens to sit on a plane, the relief is appropriate and the vias are not needed.

Where a design genuinely needs both, the usual answer is a solid connection with a via array for thermal conduction, and a process that can handle the heat load. That is a decision for the thermal design rather than for the layout alone.

Matching the Pattern to the Process

The right choice depends on how the joint will be made, and the same design can call for different answers at different stages of its life.

For hand soldering and rework, reliefs are almost always correct. Any pad an operator may have to touch with an iron is easier to solder with a relief, and rework is where solid plane connections cause the most damage.

For wave and selective soldering, reliefs on through hole pads connected to internal planes remain important, because the thermal mass of the plane can hold the pad below the solder temperature. Wider spokes and a smaller air gap are sometimes used to keep some thermal coupling while retaining solderability.

For reflow of surface mount parts, the picture is different. The assembly is heated as a whole, so the heat sinking effect is reduced, and many designs run solid connections on surface mount pads by preference, because they are better electrically and thermally. Where a reflow joint does suffer, the fix is usually a profile change rather than a layout change.

Design Checklist

• Decide per pad, not by a global default, whether the plane connection should be solid or relieved.
• Use reliefs on through hole pads tied to internal planes, and on any pad that may be hand soldered or reworked.
• Use solid connections on power and ground pads carrying significant current, and on pads that conduct heat into the board.
• Keep spoke width at or above the minimum trace width, and the air gap at or above the board minimum clearance.
• Check the pattern on inner layers separately, because a pad can be solid on the outer face and relieved underneath.
• Review the setting again after any plane is added or re-poured, since a plane edit can silently re-apply the default pattern.

It is also worth telling the fabricator and the assembly house what you intend. A board with solid plane connections and a low thermal mass can be produced without comment, while a board that mixes solid and relieved pads in the same area is easier to build when both parties know which joints are expected to be difficult.

FAQ

• Are thermal reliefs required for all plane connected pads? No. They are a soldering aid, and where the joint is reflowed and the design needs the current or the heat flow, a solid connection is better.
• How many spokes should a relief have? Four is standard. Fewer spokes are used in tight areas but increase resistance and reduce symmetry.
• Does a relief affect the electrical performance? Slightly. It adds a small resistance and inductance at the pad, which matters on power nets and at high frequency.
• Do relieved pads overheat? They can, if they carry a lot of current. Where a pad is expected to run warm, the connection should be solid.

Summary

A thermal relief is a heat break that keeps a plane connected pad solderable. Four narrow spokes and a clearance ring raise the thermal resistance enough for an iron, a wave or a reflow ramp to bring the joint to temperature, while preserving the electrical path to the plane. It is the right choice on through hole pads, on anything that may be reworked, and anywhere the soldering process is marginal.

It is the wrong choice on power pads, on ground pads carrying heavy current, and on pads that exist to move heat out of a component. There, a solid connection plus a via array does the job, and the process is adjusted to suit. Since a high current design and a hand soldered prototype can share the same layout region, the decision belongs at the pad level and should be reviewed during the layout check rather than left to a tool default.