1.1 THT-friendly design

Through-Hole Technology (THT) remains valuable for providing mechanical stability (such as for heavy connectors or relays), accommodating high-power components, and creating joints that benefit from superior mechanical strength compared to surface mount parts. In mass production, THT performs most reliably when the PCB layout is designed with the dynamics of fluid, molten solder in mind. Thoughtfully controlling design elements such as hole clearance, thermal balance, and component orientation can significantly reduce common defects like bridging or non-fills.

DFM Goal: Ensuring Proper Solder Flow and Barrel Fill

For automated THT soldering, molten solder needs to climb the pin and fill the plated hole through capillary action. Capillary action relies on having sufficient physical space for the solder to flow and enough heat to maintain a liquid state. This is why precise hole geometry and effective localized thermal management are critical.

Hole size and pad stack

Hole Clearance: The space between the inside edge of the plated hole and the outside edge of the component lead provides the path for solder. This space allows flux gases to escape and molten solder to pull in. Insufficient hole clearance prevents capillary flow and leads to incomplete barrel fill.

Board and Copper Condition	Finished Hole Diameter (vs. Max Lead Diameter)	Rationale
Standard Board (< 2.0 mm thick, < 2 oz Copper)	+0.20 – 0.30 mm clearance	Provides practical space for capillary rise and allows flux gases to vent.
Thick boards or Heavy Copper (≥ 2.0 mm thick or ≥ 2 oz Copper)	+0.30 – 0.45 mm clearance	Thicker boards have more volume to fill and act as stronger heat sinks, generally requiring a wider channel for flow.

Annular Ring: The ring of copper surrounding the hole on the surface provides structural integrity to withstand mechanical stress and thermal cycles during potential rework. Aiming for a minimum of 0.25 to 0.30 mm of radial copper around the hole is a solid guideline. This translates to a total pad diameter that is roughly 0.5 mm larger than the finished hole edge.

Thermal management

A common cause of incomplete barrel fill or cold joints in THT soldering is a lack of localized heat. When pins connect directly to large internal copper planes or heavy ground pours, these areas act as heat sinks, drawing thermal energy away and cooling the solder before it can flow effectively through the hole.

Thermal Relief Pads: Thermal relief pads must be used when pins connect to internal planes. Small copper “spokes” connect the pad to the plane, limiting the cross-sectional area that draws heat away. This maintains the soldering temperature locally while still providing a reliable electrical connection.
- Standard Practice: Using 4 spokes with a width of 0.25 to 0.40 mm is typical. If a pin connects to heavy copper planes on both the top and bottom layers, thermal relief must be applied symmetrically on both sides.
Copper Balancing: Keep copper distribution symmetrical around dense pin areas (like a large connector). Asymmetric pours create localized cold spots and inconsistent capillary rise.

Layout and orientation for automated equipment

The physical orientation of THT pins relative to the direction of the solder wave or selective nozzle movement influences the likelihood of solder bridges.

Wave Soldering Orientation: Long rows of pins must be placed perpendicular to the direction of wave flow. Rows placed parallel to the wave create narrow channels that trap molten solder, drastically increasing the risk of bridging.
Solder Thieving Pads: For fine-pitch THT parts, non-functional copper pads downstream of the final pin (solder thieving pads) must be added. These pads pull excess solder off the final pin as it exits the wave, preventing icicles and bridging.
SMT Component Keepout: In selective soldering or when using a wave pallet, SMT components on the bottom side of the board must be kept at least 3 to 4 mm away from THT pins. This zone provides a buffer so SMT parts are not impacted by splashed solder or the nozzle. SMT parts near a wave soldering area must be secured with adhesive or moved to the top side of the board.

Lead preparation and fixturing

The preparation of the component lead and the method of holding the board during soldering also influence the final result.

Lead Protrusion: After wave soldering and lead cutting, the component lead must protrude from the top pad by 0.5 to 1.5 mm. A lead cut too short prevents sufficient capillary action, while an excessively long lead wastes solder and increases the risk of bridging.
Avoid Clinching: For automated soldering methods, leads must remain straight without clinching over the pad, unless specifically required for mechanical retention. Clinched leads block solder flow and trap flux residues.
Designing for Pallets: If the board requires a soldering pallet (fixture), designing the PCB with adequate tooling holes and unpopulated panel edges (rails) directly ensures secure mounting. Openings in the pallet must have edges at least 2.5 to 3.0 mm away from the nearest solder pad to avoid interfering with solder flow.

Common design issues and corrections

Design Issue	Symptom	DFM Suggestion
Hole clearance too tight.	Incomplete fills, appearing as starved joints.	Increase finished hole diameter by +0.1 mm, maintaining sufficient annular ring.
Solid copper pours connected directly to THT pins.	Cold, gray joints, requiring manual rework.	Implement a 4-spoke thermal relief (0.25–0.40 mm width).
Pin rows oriented parallel to the solder wave.	Solder bridging between pins.	Rotate the component 90 degrees or add solder thief pads at the trailing end.
Annular ring too small.	Pad lifting or cratering during manual rework.	Design for at least 0.25 mm radial copper. Use teardrop connections for thin traces.

Recap: THT-Friendly Design Parameters

Parameter	Requirement	Value / Condition	Action / Correction
Finished Hole Diameter	Provide clearance for capillary flow and gas venting.	+0.20–0.30 mm clearance over max lead dia. (Standard PCB: <2mm thick, <2oz Cu). +0.30–0.45 mm clearance (Thick PCB/Heavy Cu: ≥2mm thick or ≥2oz Cu).	Increase hole diameter if fill is incomplete.
Annular Ring	Ensure pad structural integrity for rework.	Minimum 0.25–0.30 mm radial copper around hole.	Design pad diameter ~0.5 mm larger than finished hole.
Thermal Relief	Prevent heat sink effect from internal planes.	Mandatory for pins connecting to internal copper planes. Use 4 spokes, 0.25–0.40 mm width each. Apply symmetrically if connected on both top/bottom layers.	Implement thermal relief pads for solid copper connections.
Wave Solder Orientation	Minimize solder bridging risk.	Pin rows must be oriented perpendicular to wave flow direction.	Rotate component 90° if parallel. Add solder thief pads downstream for fine-pitch parts.
SMT Keep-Out Zone	Protect bottom-side SMT components during THT soldering.	Maintain 3–4 mm clearance from THT leads.	Relocate SMT parts or secure with adhesive. Ensure pallet openings are 2.5–3.0 mm from pads.
Lead Protrusion	Ensure sufficient capillary action post-wave soldering.	0.5–1.5 mm protrusion from top pad after lead cutting.	Adjust lead length. Keep leads straight; avoid clinching for automated soldering.