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.

The DFM goal: supporting 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 localized thermal management are so highly recommended.

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. If the hole is too tight, solder may struggle to enter properly.

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: Try to use a thermal relief pad 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 helps keep the soldering location hot 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, applying thermal relief symmetrically on both sides is very helpful.
Copper Balancing: When designing copper pours near dense pin areas (like a large connector), try to keep the copper distribution relatively symmetrical. Large, continuous areas of copper can create localized cold spots, which sometimes lead to inconsistent soldering performance.

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: It is best practice to place long rows of pins perpendicular to the direction of wave flow. Rows placed parallel to the wave create narrow channels that can trap molten solder, increasing the risk of bridging.
Solder Thieves: For fine-pitch THT parts, consider adding small, non-functional copper pads downstream of the final pin in the row. These “solder thieves” or “robber pads” help pull excess solder off the final pin as it exits the wave, preventing icicles and bridges.
SMT Component Keepout: In selective soldering or when using a wave pallet, it is important to keep SMT components on the bottom side of the board 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 should ideally be secured with adhesive or placed on 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, a good target is for the component lead to protrude from the top pad by 0.5 to 1.5 mm. A lead cut too short provides less surface for the solder to climb, while a lead left too long uses excess solder and increases the risk of bending during handling.
Avoid Clinching: For automated soldering methods, it is generally best to leave leads straight without bending or “clinching” them over the pad, unless it is specifically required for mechanical retention. Clinched leads can sometimes 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) helps ensure secure mounting. Openings in the pallet should 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.	Consider increasing 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.	Try implementing a 4-spoke thermal relief (0.25–0.40 mm width).
Pin rows oriented parallel to the solder wave.	Solder bridging between pins.	Consider rotating the component 90 degrees or adding solder thief pads at the trailing end.
Annular ring too small.	Pad lifting or cratering during manual rework.	Try to design for at least 0.25 mm radial copper. Use teardrop connections for thin traces.

Final Checkout: THT-friendly design

Design Category	DFM Guideline	Verification
Hole Geometry	Finished hole diameter ≥ max lead diameter + 0.20 mm.	Check that the annular ring maintains ≥ 0.25 mm radial copper and solder mask is properly relieved.
Thermal Balance	Pins connecting to copper planes use a 4-spoke thermal relief (min 0.25 mm width).	Visually verify thermal spokes on applicable top and bottom connection layers.
Component Layout	Pin rows perpendicular to wave direction; solder thieves on trailing edges of fine-pitch rows.	Verify a 3 to 4 mm keepout zone around THT pins for SMT components.
Lead Preparation	Protruding lead length target is 0.5 to 1.5 mm.	Ensure leads are remaining straight (no clinching) unless mechanically necessary.
Manufacturing Fixturing	Tooling holes and unpopulated edge rails are included for stable palletization.	Verify pallet window edges are ≥ 2.5 mm away from nearest THT solder pad.