2.3 Land Patterns, Spacing and Polarity

A component footprint is not merely a drawing; it is a prediction of how molten solder will behave under surface tension. Relying on component manufacturer datasheets for land patterns often leads to manufacturing defects, as these datasheets rarely account for modern high-speed placement or reflow dynamics. To ensure high First Pass Yield (FPY), the Golden Data Pack must normalize all footprints to a consistent industry standard, eliminating the need for "tribal knowledge" during machine programming.

IPC-7351 & Solder Joint Mechanics

The goal of a land pattern is to form a specific solder joint geometry: the Toe, Heel, and Side fillets. These fillets determine mechanical strength and inspectability.

1. Density Levels

Select the land pattern geometry based on reliability requirements and board density.

• Level A (Maximum Material Condition): Large pads for robust soldering. Use for high-vibration, high-reliability, or wave soldering.
• Level B (Nominal Material Condition): Standard commercial assembly. The default for most consumer electronics.
• Level C (Least Material Condition): Minimal protrusion. Use only for portable/handheld devices where density is the primary constraint.

2. The Toe and Heel Rule

• If the Toe fillet (outward facing) is insufficient, Then the joint lacks mechanical strength against shear forces.
• If the Heel fillet (under the bend) is insufficient, Then the joint will crack under thermal cycling.
• Mandate: Ensure the land extends 0.3 – 0.5 mm beyond the component lead tip (Toe) and 0.35 mm inward (Heel) for standard Gull Wing leads.

Component Spacing & Courtyards

Physical placement machines require space for the vacuum nozzle, not just the component body. "Courtyards" define this keep-out zone.

Spacing Logic:

• If spacing between passive components (0402/0603) is < 0.25 mm, Then risk of solder bridging increases exponentially.
• If a small component is placed immediately adjacent to a tall component (e.g., an 0402 next to a shield can), Then define a Shadowing Distance (typically 1:1 ratio of height to distance). The tall component blocks IR heat and spray flux, causing cold joints.
• If the design uses BGAs, Then require a 3.0 mm clearance around the perimeter for rework station nozzles and inspection mirrors.

Pro-Tip: Always check the "Pick & Place Variance" in your courtyard. Cheap nozzles have a tolerance of ±0.05 mm. If your spacing is 0.1 mm, you will have collisions.

Tombstoning & Thermal Balance

Tombstoning occurs when wetting forces are unbalanced, pulling the component onto one end. This is strictly a function of pad geometry and thermal connection.

Prevention Rules:

• Symmetry: Both pads of a two-terminal device (resistor/capacitor) must have equal thermal mass.
• Ground Planes: Do not connect a pad directly to a large copper plane.
  • Action: Use Thermal Relief spokes (minimum 2, preferably 4) to choke heat dissipation.
• Trace Entry: Traces must enter pads symmetrically.
  • Bad: One pad connected with a thin trace, the other flooded with copper.
  • Good: Both pads connected via equivalent trace widths.

Polarity & Orientation Control

Ambiguous polarity is the leading cause of scrapped PCBA lots. Machine programmers cannot guess orientation based on inconsistent library data.

1. Zero Orientation (IPC-7351 Level A)

Standardize the "Zero Rotation" state in the CAD library.

• Pin 1 Location: Top-Left or Top.
• Consistency: If one IC is defined at 0˚, all similar ICs must follow the same rule. Do not mix 0˚ and 90˚ definitions for the same package type.

2. Silkscreen Indicators

Visual markers must be visible after the component is placed to allow for manual Quality Control (QC).

• Requirement: Place a dot, bar, or chamfered box corner outside the component body outline.
• Constraint: Do not put polarity markers (dots) under the chip body.
• Diode Logic: Use the diode symbol (-->|--) on the silkscreen rather than just "A" or "K", which can be misinterpreted.

Final Checklist