PCB thermal relief helps a pad reach soldering temperature without losing excessive heat into a large copper plane. However, the same spokes that improve solderability also increase electrical and thermal resistance.
Therefore, designers should not apply thermal relief to every pad, via, and plane connection. Ordinary soldered pads often benefit from spokes, while high-current terminals, thermal vias, exposed thermal pads, RF grounds, and non-soldered vias may need solid copper connections.
The correct choice depends on what the connection must carry during operation and how the PCBA manufacturer will solder it.
What Is PCB Thermal Relief?
PCB thermal relief connects a pad to a copper plane or pour through several narrow copper spokes.
Without the relief pattern, copper surrounds the pad and conducts heat away during soldering. Consequently, the pad and component lead may heat more slowly than the soldering process expects.
A thermal relief reduces that heat flow while maintaining electrical continuity.
The pattern normally includes:
- A component pad or plated hole
- A copper-free relief gap around the pad
- Two, three, four, or more copper spokes
- A surrounding plane or copper pour
PCB design software may call this feature:
- Thermal relief
- Thermal connection
- Relief connect
- Spoke connection
- Thermal spokes
- Plane thermal
Although four spokes provide a common starting pattern, they do not represent a universal rule.
Thermal Relief Vs Thermal Pad Vs Thermal Via
These three terms describe different PCB functions.
| Feature | Primary Purpose | Normal Thermal Direction |
|---|---|---|
| Thermal Relief | Restrict Heat Loss During Soldering | From Pad Into Plane |
| Exposed Thermal Pad | Transfer Operating Heat From A Component Into The PCB | From Component Into Copper |
| Thermal Via | Transfer Heat Between PCB Layers | Through The Board |
| Copper Heat Spreader | Distribute Heat Across A Larger Area | Along The Copper Layer |
A PCB thermal relief intentionally increases thermal resistance around a soldered pad.
In contrast, an exposed thermal pad under a QFN, regulator, MOSFET, or power amplifier normally needs low thermal resistance. Therefore, designers often connect it directly to copper and thermal vias.
Likewise, thermal vias usually need solid connections to internal planes. Adding spokes to these vias can restrict the heat path that the designer created them to provide.
Texas Instruments specifically recommends full-circumference plane connections for PowerPAD thermal vias and advises against spoke connections that obstruct heat transfer in its PowerPAD layout guidelines.
Consequently, designers should never treat “thermal relief” and “thermal dissipation” as the same function.
Why Does PCB Thermal Relief Improve Soldering?
Solder must heat the pad, component termination, and solder alloy above the required process temperature.
A large copper plane acts as a heat sink. It draws energy away from the joint and spreads it across the PCB.
As a result, a solid plane connection can cause:
- Slow solder melting
- Incomplete wetting
- Insufficient through-hole fill
- Cold or disturbed joints
- Longer soldering contact time
- Excessive local rework heat
- Uneven heating between component pads
- Higher dependence on preheating
PCB thermal relief reduces the copper cross-section between the pad and plane. Therefore, the soldering process can raise the pad temperature more quickly.
However, the relief does not replace a suitable thermal profile, solder alloy, flux, preheat setting, or soldering tool.
IPC identifies J-STD-001J as the current consensus standard for soldered electrical and electronic assemblies. The assembly drawing should also define the required product class and any customer-specific acceptance criteria.
PCB Thermal Relief Vs Solid Connection
The correct connection depends on solderability, current, operating heat, impedance, and mechanical requirements.
| Design Condition | Normal Starting Choice | Main Reason |
|---|---|---|
| Ordinary Through-Hole Ground Pin | Thermal Relief | Improves Heating And Hole Fill |
| Small SMT Pad Connected To Large Pour | Thermal Relief | Balances Pad Heating |
| QFN Exposed Thermal Pad | Solid Connection | Preserves Heat Transfer |
| Thermal Via | Solid Connection | Reduces Through-Board Thermal Resistance |
| Ground Stitching Via | Solid Connection | Reduces Electrical Inductance |
| High-Current Terminal | Solid Or Custom Wide Spokes | Preserves Current Capacity |
| Press-Fit Pin | Solid Or Application-Specific | No Soldering Benefit From Relief |
| RF Ground Connection | Solid Or RF-Specific Geometry | Reduces Inductance |
| Hand-Soldered Connector | Thermal Relief | Reduces Required Heating Time |
| Test Via Without Soldering | Solid Connection | Relief Provides Little Benefit |
This table provides a starting point rather than a universal rule. Component datasheets, current requirements, PCB materials, and the actual assembly process take priority.
How Spoke Width Affects PCB Thermal Relief
Spoke width creates the main tradeoff in PCB thermal relief design.
Narrow spokes:
- Reduce heat flow into the plane
- Make the pad easier to solder
- Increase electrical resistance
- Reduce current capacity
- Increase manufacturing sensitivity
Wide spokes:
- Carry more current
- Transfer more operating heat
- Reduce connection impedance
- Make the pad harder to heat during soldering
Therefore, designers should not select spoke width only from a CAD software default.
The KiCad PCB Editor documentation allows designers to control spoke width and relief gap separately. It also distinguishes thermal connections from solid zone connections.
Does Four Spokes Equal A Trace Of Four Times The Width?
Not exactly.
Four equal spokes provide four parallel copper paths only when the current distributes evenly among them. Pad geometry, current entry direction, nearby copper, layer connections, and plane shape can produce unequal sharing.
In addition, each spoke remains short and connects to a much larger copper area. Therefore, its temperature behavior does not exactly match a long isolated PCB trace.
Nevertheless, the combined copper width provides a useful first screening check.
For example, four 0.25 mm spokes provide 1.00 mm of nominal parallel width. However, the designer must still evaluate:
- Copper thickness
- Spoke length
- Current direction
- Plane geometry
- Temperature rise
- Fault current
- Number of connected layers
- Manufacturing tolerance
Our PCB trace width article explains why current capacity depends on the complete conductor path rather than one nominal width.
How Relief Gap Affects Thermal Performance
The relief gap separates most of the pad perimeter from the surrounding copper plane. Consequently, the gap controls the length of the thermal spokes.
A larger gap generally creates longer spokes and greater thermal isolation. However, it also consumes more copper area and may weaken the electrical connection.
A smaller gap creates shorter spokes and lower resistance. Nevertheless, the surrounding plane can then remove more heat during soldering.
The designer must also confirm that the relief gap does not create:
- Copper slivers
- Narrow plane necks
- Insufficient spacing to another net
- Broken spokes
- Unwanted plane islands
- Reduced current paths around nearby pads
Therefore, spoke width and relief gap should form one coordinated design rule.
How Many Thermal Relief Spokes Should You Use?
Four spokes provide a symmetrical pattern and remain common for round through-hole pads. However, pad shape and nearby copper may prevent the CAD tool from generating all four.
A PCB thermal relief may contain:
- Two spokes in a constrained area
- Three spokes for improved connectivity
- Four spokes for a balanced general connection
- More than four spokes for a large pad or high-current connection
- Custom wide sectors instead of conventional spokes
More spokes generally reduce electrical and thermal resistance. However, they also transfer more heat into the plane during soldering.
The final filled copper geometry matters more than the selected software setting. A designer may request four spokes, while clearances around nearby vias or pads leave only one or two in the exported data.
Consequently, refill every copper zone and inspect the actual Gerber or ODB++ output before release.
PCB Thermal Relief For Through-Hole Components
Through-hole pins often connect to copper planes through the plated barrel and internal-layer pads.
If every connected plane uses a solid connection, the combined copper mass can remove substantial heat during wave, selective, or hand soldering.
Possible results include:
- Incomplete vertical solder fill
- Poor wetting on the component side
- Longer solder contact time
- Excessive preheating
- Difficult rework
- Damage to nearby materials or components
Therefore, ordinary through-hole ground and power pins often benefit from PCB thermal relief on connected plane layers.
Heavy Copper Through-Hole Boards
Heavy copper increases both current capacity and thermal mass. Consequently, a connection that solders easily on a 1 oz board may become difficult on a 3 oz or 4 oz PCB.
The designer may need:
- Wider thermal spokes
- More spokes
- Relief on selected layers
- Solid connections on high-current layers
- Higher preheat
- Longer selective-solder contact
- A custom soldering nozzle
- A verified thermal profile
The PCB copper thickness article explains how heavy copper changes etching, current capacity, drilling, and assembly.
Connectors And High-Current Terminals
A connector pin may need both reliable solder fill and high current capacity.
Instead of choosing between very narrow spokes and a complete solid connection, designers can use:
- Wider spokes
- Additional spokes
- Multiple connected layers
- Parallel pins
- Larger copper areas
- Local preheating
- A customized selective-soldering process
This combined approach often produces a better result than applying one default rule to every connector pin.
PCB Thermal Relief For SMT Pads
SMT components experience a different soldering process because the reflow oven heats the complete assembly.
Nevertheless, unequal copper connections can make component pads heat at different rates.
For example, one end of a small resistor may connect to a large ground plane while the other connects to a narrow trace. This imbalance can contribute to:
- Tombstoning
- Rotation
- Uneven solder melting
- Inconsistent wetting
- Joint-shape variation
Therefore, a PCB thermal relief can help balance the two pads.
However, stencil design, paste volume, component placement, pad dimensions, surface finish, and reflow profile also affect the result. Thermal relief alone cannot correct every tombstoning problem.
A production-representative PCB reflow soldering process should confirm the final behavior.
When Should SMT Pads Use Solid Copper?
Some SMT pads need direct copper connections because they carry heat, current, or high-frequency energy.
Examples include:
- QFN exposed pads
- Power MOSFET tabs
- Voltage-regulator thermal lands
- LED thermal pads
- RF grounding pads
- High-current shunt resistors
- Power-module terminals
For these components, the datasheet and package application note should control the land pattern and copper connection.
Analog Devices notes that exposed-pad packages depend on the PCB connection for heat dissipation and advises designers to confirm the pad’s required electrical potential in its exposed-pad design note.
Therefore, do not add thermal-relief spokes under an exposed pad unless the component manufacturer specifically supports that geometry.
Do Vias Need PCB Thermal Relief?
The answer depends on the via’s function.
Thermal Vias
Thermal vias transfer heat from a surface pad into internal or bottom copper layers. Therefore, they normally need solid plane connections.
Thermal spokes would increase the resistance of the heat path.
Ground Stitching Vias
Ground stitching vias connect ground structures and reduce transition impedance. They also normally use solid connections because they do not require component soldering.
Ordinary Signal Vias
Signal vias normally connect traces or pads rather than a large plane. Therefore, a thermal-relief rule may not apply.
Via-In-Pad Structures
A via inside a soldered component pad affects solder paste and assembly. Filled and capped via-in-pad structures normally maintain a solid copper connection, while open vias may draw solder away from the joint.
The via treatment, rather than thermal relief alone, controls this risk.
Test Vias
A test via may need solder access during debugging or repair. However, automated probing does not require the via to heat like a component pad.
Therefore, choose the connection according to the actual test and repair process.
PCB Thermal Relief For Wave And Selective Soldering
Wave and selective soldering heat through-hole leads from the solder-contact side.
Large copper planes can prevent the barrel and component-side land from reaching a suitable temperature before the solder contact ends.
Therefore, PCB thermal relief often provides substantial value for these processes.
A process review should consider:
- Board thickness
- Copper weight
- Number of connected plane layers
- Hole diameter
- Lead-to-hole clearance
- Component thermal mass
- Preheat temperature
- Flux activity
- Solder alloy
- Contact time
- Nozzle access
- Nearby heat-sensitive parts
Selective soldering can apply heat more locally than wave soldering. However, it still needs a stable process window.
Our selective soldering article explains nozzle access, preheating, dwell time, and through-hole fill in more detail.
When Should You Avoid PCB Thermal Relief?
Avoid or reconsider thermal relief when the connection must provide:
High Current
Narrow spokes can become the smallest part of the current path. As a result, they may create voltage drop, temperature rise, or a fusing point.
Low Inductance
RF grounds, switching-current loops, shield connections, and high-speed return paths often need short, wide copper connections.
Maximum Heat Transfer
Exposed thermal pads and thermal vias should move heat into large copper areas rather than restrict it.
Mechanical Strength
Press-fit connectors and high-insertion-force terminals may need a robust pad and plane structure.
High Fault Current
Protective-earth, surge, battery, and power-input connections may carry short-duration currents far above normal operation.
In each case, a custom wide-spoke pattern may provide a compromise. However, the assembly supplier must confirm that the soldering process can handle the resulting copper mass.
PCB Thermal Relief And Copper Pour Settings
A PCB thermal relief depends on the surrounding PCB copper pour.
The design rules should define:
- Connected net
- Pad connection mode
- Spoke quantity
- Spoke width
- Relief gap
- Minimum copper width
- Copper-pour priority
- Island-removal rule
- Plane clearance
- Layer-specific exceptions
After changing routes, pads, vias, or component placement, refill the zones. Otherwise, the design display or output may contain an outdated relief pattern.
In addition, check that polygon priority does not allow another zone to remove part of the intended connection.
Manufacturing Risks In PCB Thermal Relief
The PCB factory must reproduce every spoke within its imaging and etching capability.
Spokes Below Minimum Copper Width
A narrow spoke may over-etch or break. Consequently, the pad can lose part or all of its plane connection.
Spokes That Meet Only At A Point
Poor polygon geometry can create a fragile point connection instead of a full-width copper path.
Acute Copper Slivers
Relief gaps and nearby clearances can leave thin copper fragments that etch unpredictably.
Copper Weight Changes
A spoke suitable for standard copper may not work with heavy copper because thicker copper requires different etch compensation.
CAM Modifications
A CAM engineer may widen, remove, or reshape a spoke to meet factory rules. However, this change can affect current capacity, heat flow, or solderability.
Therefore, the manufacturer should obtain approval before changing critical thermal connections.
How To Specify PCB Thermal Relief
Do not rely only on a drawing note that says “use thermal relief where required.”
Instead, define:
- Which pad or net classes use relief
- Which pads require solid connections
- Minimum finished spoke width
- Spoke quantity where critical
- Relief-gap requirement
- Copper weight
- Connected plane layers
- High-current exceptions
- Thermal-pad exceptions
- RF-ground exceptions
- Press-fit exceptions
- Applicable assembly process
- Required IPC class
- First-article inspection criteria
In addition, provide component datasheets for unusual power, thermal, RF, or press-fit connections.
The PCB designer, fabricator, and assembly supplier should approve the same geometry before production.
How To Verify PCB Thermal Relief During First Article Inspection
First-article inspection should confirm both the fabricated copper and the soldering result.
Bare-PCB Review
Inspect:
- Spoke presence
- Finished spoke width
- Plane connectivity
- Copper breaks
- Slivers
- Etch quality
- Annular ring
- Layer-specific connections
Assembly Review
Evaluate:
- Solder wetting
- Through-hole fill
- Component-side fillet where required
- Tombstoning
- Pad heating balance
- Rework time
- Thermal profile
- Joint appearance
Electrical And Thermal Review
For high-current or thermal connections, also measure:
- Voltage drop
- Temperature rise
- Operating temperature
- Current sharing
- Fault-current behavior
- Component junction or case temperature
A solder joint can look acceptable while narrow spokes still create excessive electrical resistance during operation.
PCB Thermal Relief Decision Checklist
Before releasing the layout, confirm:
- Does the pad connect to a large copper plane or pour?
- Will the assembly process solder this pad or hole?
- Does the connection need thermal isolation during soldering?
- Does the pad carry high continuous current?
- Can the spokes carry fault or surge current?
- Does the connection need low RF inductance?
- Must the pad transfer operating heat into the PCB?
- Is the feature an exposed thermal pad?
- Is the feature a thermal or stitching via?
- Does the component datasheet require solid copper?
- Does copper weight increase the soldering heat demand?
- Are the spoke width and gap manufacturable?
- Did the CAD tool generate the requested number of spokes?
- Does nearby clearance remove part of the connection?
- Are both pads of a small component thermally balanced?
- Can wave or selective soldering achieve adequate hole fill?
- Has the assembly supplier reviewed high-current exceptions?
- Will first-article testing verify voltage drop and temperature?
Frequently Asked Questions About PCB Thermal Relief
What Is The Purpose Of PCB Thermal Relief?
PCB thermal relief limits heat flow from a soldered pad into a large copper plane. Therefore, the pad reaches soldering temperature more easily.
How Many Thermal Relief Spokes Should A Pad Have?
Four spokes provide a common starting pattern. However, pad geometry, current, copper weight, soldering method, and manufacturing rules may require two, three, more than four, or a custom pattern.
How Wide Should Thermal Relief Spokes Be?
No universal width suits every PCB. The spokes must meet the factory’s minimum finished copper rule and carry the required current without excessive voltage drop or temperature rise.
Are Thermal Reliefs Required For All Ground Pads?
No. Ordinary soldered ground pads often benefit from them. However, exposed thermal pads, thermal vias, stitching vias, RF grounds, and high-current connections may need solid copper.
Do Thermal Vias Need Thermal Relief?
Normally no. Thermal vias should transfer heat into internal and bottom copper layers. Spokes would restrict that path.
Does A QFN Exposed Pad Need Thermal Relief?
Usually no. The exposed pad normally needs direct copper and thermal-via connections. Follow the component manufacturer’s land-pattern and assembly recommendations.
Can Thermal Relief Cause Voltage Drop?
Yes. Narrow or long spokes add electrical resistance. The effect becomes more important for high current, low-voltage rails, precision sensing, and fault current.
Does Reflow Soldering Need Thermal Relief?
It may. Thermal imbalance between SMT pads can affect wetting and tombstoning. However, exposed thermal pads and high-current SMT connections often need solid copper.
Can The PCB Manufacturer Add Thermal Relief?
The manufacturer can recommend or generate plane connections when the customer allows it. However, it should not change critical high-current, thermal, RF, or safety connections without approval.
Is Thermal Relief An IPC Requirement?
IPC standards address PCB design and soldered-assembly requirements, but no single thermal-relief pattern applies to every connection. The product drawing, component requirements, electrical design, and qualified assembly process must define the final geometry.
Final Recommendations For PCB Thermal Relief
PCB thermal relief balances two competing requirements:
The pad must heat efficiently during soldering, but the finished connection must still carry current and heat reliably during operation.
For dependable results:
- Use relief spokes for ordinary pads tied to large planes.
- Use solid connections for thermal vias and most exposed thermal pads.
- Review high-current, RF, press-fit, and protective connections separately.
- Calculate spoke capacity from copper thickness, geometry, and actual current.
- Do not assume four default spokes work for every pad.
- Match the design to reflow, wave, selective, or hand soldering.
- Inspect the final filled-zone geometry before exporting production files.
- Prevent broken spokes, point connections, and copper slivers.
- Obtain approval before the factory changes critical connections.
- Verify solderability, voltage drop, and temperature during first-article production.
The practical rule is:
Use PCB Thermal Relief When Solderability Controls The Connection. Use Solid Copper When Current, Impedance, Or Heat Transfer Controls It.
