PCB material selection and thermal design determine whether a board can be fabricated repeatably, assembled without soldering defects, and operated within component derating limits. The two areas are linked: the substrate and surface finish establish the process window, while component placement and copper geometry establish the heat path. This article defines the process-design requirements for both areas and provides a common basis for PCB design, fabrication review, and board-level process review. It covers substrate and finish selection, thermal placement, clearance for temperature-sensitive parts, thermal relief on copper planes, small-chip symmetry, and mounting of high-heat components.
Highlights:
- Place high-heat components at the air outlet or in a location that promotes convection; taller parts and heat sinks must not block the airflow path.
- For a heat source with a temperature rise above 30°C, keep temperature-sensitive devices such as electrolytic capacitors at least 2.5mm away in forced air and 4.0mm away in natural convection; if the clearance cannot be met, verify derating by temperature test.
- Use thermal relief spokes between pads and large copper areas to support solder penetration, but do not use thermal relief on pads carrying more than 5A; for 0805 and smaller chip components, keep pad heat capacity symmetric and limit the pad-to-trace connection width to 0.3mm on asymmetric pads.
Purpose and Scope
The purpose of this specification is to standardize PCB process design and define the parameters that make a design production-ready. The requirements address manufacturability, testability, safety, EMC, and EMI. Applying them during product development builds process, technology, quality, and cost advantages rather than discovering constraints after the board is released.
The specification applies to PCB process design for all electronic products. It covers PCB design, PCB release process review, and board-level process review. If an earlier related standard or specification conflicts with this document, this document takes precedence.
Terms Used in This Specification
| Term | Definition |
|---|---|
| Via | A metallized hole used for internal layer connection, not for inserting component leads or other reinforcement. |
| Blind via | A via that extends from inside the board to only one outer surface. |
| Buried via | A via that does not extend to either board surface. |
| Through via | A via that extends from one board surface to the other. |
| Component hole | A hole that secures a component terminal to the board and provides electrical connection to the conductive pattern. |
| Stand off | The vertical distance from the bottom of a surface-mount device body to the bottom of its leads. |
Applicable Standards
Terminology follows IEC60194, Printed Board design, manufacture and assembly — terms and definitions. Safety requirements refer to IEC60950. Acceptance criteria for printed boards refer to IPC-A-600F. Internal specifications for PCB safety design, forced-air thermal design, and natural-convection thermal design also apply. These references provide the vocabulary and compliance basis for the requirements below.
PCB Material Requirements
The first material decision is the substrate family: FR-4, aluminum-backed laminate, ceramic, paper-core laminate, and other options each set a different mechanical and thermal envelope. When a high glass-transition temperature (Tg) substrate is selected, the fabrication documentation must state the thickness tolerance. Tg and thickness tolerance affect stack-up control, drilling, and the ability of the board to survive assembly and field temperature excursions.
The copper finish must also be specified: tin plating, nickel-gold, OSP, or another agreed finish. The finish belongs in the fabrication file because it changes the process route, shelf life, and soldering behavior. Leaving it to a default is not acceptable for a controlled process.
Thermal Layout Requirements
Thermal design starts with the airflow path. High-heat components should be placed at the air outlet or in a position that favors convection, where the local air is already moving and the component wake does not heat more sensitive parts upstream. Placing heat sources at the outlet keeps their heated air from flowing across temperature-sensitive devices.
Taller components should also be placed at the air outlet, and they must not obstruct the flow path. A tall part placed upstream can create a wake that starves downstream components of air. Heat sinks require the same treatment: their fins and mounting orientation should promote convection and should not block the flow through adjacent channels.
Temperature-Sensitive Components
A heat source with a temperature rise above 30°C requires clearance from temperature-sensitive devices. Under forced-air cooling, electrolytic capacitors and similar parts should be at least 2.5mm from the heat source. Under natural convection, the clearance should be at least 4.0mm. These distances are minimum layout requirements, not targets to be traded against dense placement without verification.
If space prevents the required distance, temperature testing must confirm that the temperature rise of the sensitive device remains within its derating range. The test is the acceptance condition in that case; a visual check of spacing is not sufficient.
Copper Areas and Thermal Relief
On a large copper area, a component pad connected directly to the plane can draw heat away during soldering and prevent good solder penetration. The pad should therefore be connected through a thermal relief, often in a cross or spoke pattern. The two ends of the PCB thermal pad should have balanced routing or equivalent heat capacity so that the relief works predictably. The pad-to-copper connection may use a cross or spoke form, as shown below.
The exception is a pad that must carry more than 5A. Such a pad should not use a thermal relief; the current-carrying requirement takes priority over the soldering benefit.
Small Chip Components and Thermal Symmetry
For 0805 and smaller chip components that pass through reflow, the two pads must have symmetric heat dissipation. Asymmetric heating causes one joint to melt later than the other and can produce shift or tombstoning. For asymmetric pads, the connection width between the pad and the printed trace should not exceed 0.3mm. This limits heat flow through the trace and reduces the imbalance between the two joints.
High-Heat Components and Bus Bars
The mounting method for a high-heat component must be easy to assemble and solder. As a rule, when the heat density of the component exceeds 0.4 W/cm3, the leads and the body alone cannot dissipate enough heat. Heat-dissipation mesh, bus bars, and similar measures should be used to improve current-carrying capability. Bus-bar legs should use multiple connection points; riveting followed by wave soldering, or direct wave soldering, is preferred to make assembly and soldering reliable.
Long bus bars need special attention. During wave soldering, the CTE mismatch between the bus bar and the PCB can cause board warpage. The support and connection design should account for this effect.
To keep tinning easy to perform, the solder channel width should be no greater than 2.0mm, and the spacing between solder channel edges should be greater than 1.5mm.
Related Reading:
PCB Component Library and Footprint Selection Requirements Guide
PCB Basic Layout and Manufacturability Requirements for PCBA
PCB Routing and Reference Point Design Requirements
PCB Testability Requirements for Reliable ICT and Functional Test
Electrical Clearance, Creepage Distance, and Insulation Levels
