Checkpoint 1: Component Orientation Consistent Major
Consistent component orientation reduces placement errors, simplifies optical inspection, and improves reflow soldering quality. All polarized components should follow a standard orientation convention.
Orientation Standards
IPC-7351 Component Orientation Convention:
Passive components (resistors, capacitors, inductors):
- Long axis aligned in same direction (typically horizontal)
- Pin 1 (cathode for caps) consistently on left or top
ICs and active devices:
- Pin 1 consistently in same corner (upper-left preferred)
- All ICs oriented in the same direction where possible
- Exceptions allowed for routing optimization if clearly marked
Polarized components:
- Diodes: Cathode band consistently pointing same direction
- Electrolytic caps: Positive terminal consistently same side
- LEDs: Cathode consistently same orientation
- Tantalum caps: Anode (band side) consistently same direction
Rule: Maximum 2 orientations (0° and 90°). Avoid 45° or arbitrary angles.
- Establish orientation convention at start of layout (document in design notes).
- Set default rotation for component groups in your EDA library.
- Place all polarized passives with pin 1 (anode/positive) facing left or up.
- Place all ICs with pin 1 in upper-left corner of the component's local orientation.
- Visually verify orientation using silkscreen layer -- polarity marks should be visible and consistent.
- Run orientation check: In Altium, use "Query" to find components with non-standard rotation values.
All 0603 capacitors oriented horizontally (0° rotation). All SOT-23 transistors with pin 1 (gate) facing up. All SOIC-8 ICs with pin 1 in upper-left. Polarity marks clearly visible in silkscreen. Assembly team reports zero orientation-related defects across 1000-board production run.
Components placed in 4 different orientations depending on routing convenience. Some capacitors at 0°, some at 90°, some at 180°. Polarity marks obscured by vias and traces. Pick-and-place programming takes 3× longer. Visual inspection cannot quickly identify wrong-orientation defects. 2% of boards have reversed tantalum caps (causing shorts and potential fires).
- Library inconsistency: Different library sources may define pin 1 differently. Standardize your library so pin 1 is always consistently defined.
- Silkscreen too small: For 0402 and smaller, silkscreen polarity marks may not be readable. Use assembly drawing with clear indicators instead.
- Rotation during panelization: If boards are rotated within a panel for utilization, verify that the assembly program compensates for the rotation.
Checkpoint 2: Reflow Compatible (All SMD One Side) Major
For single-pass reflow assembly, all SMD components should be on one side. If double-sided SMD is required, the heavier/larger components go on the first reflow side (bottom during second pass) and must not fall off during the second reflow.
Component Weight vs. Solder Surface Tension
Maximum component weight for bottom-side reflow survival:
F_hold = γ × L_wetted (surface tension force)
γ = solder surface tension ≈ 0.4 N/m (SAC305 at 240°C)
L_wetted = total pad perimeter
Component stays attached if: m × g < F_hold
Example: SOIC-8 on bottom side during second reflow:
8 pads, each 0.6mm × 2.0mm, pad perimeter = 2×(0.6+2.0) = 5.2mm per pad
L_total = 8 × 5.2mm = 41.6mm = 0.0416m
F_hold = 0.4 × 0.0416 = 0.0166N
m_max = 0.0166 / 9.81 = 1.7g
SOIC-8 mass ≈ 0.1g -- SAFE (16× margin)
Example: Large electrolytic cap (10mm × 10mm × 12mm):
2 pads, each 3mm × 5mm, perimeter = 2×(3+5) = 16mm per pad
L_total = 2 × 16mm = 32mm = 0.032m
F_hold = 0.4 × 0.032 = 0.0128N
m_max = 0.0128 / 9.81 = 1.3g
Large electrolytic mass ≈ 2-5g -- WILL FALL OFF!
Heavy components must go on the final (top) reflow side.
Double-Sided Assembly Strategy
| Side | Reflow Pass | Component Types | Weight Limit |
|---|
| Bottom (first reflow) | 1st pass | Small passives (0402-0805), small ICs (SOT, QFN<5mm) | <1g per component |
| Top (second reflow) | 2nd pass | All large ICs, BGAs, connectors, heavy passives | No limit (right-side up) |
Reflow Profile Compatibility Check:
All components on one side must survive the same reflow profile:
- Peak temperature: 245-260°C (SAC305) for lead-free
- Time above liquidus: 60-90 seconds
- Total profile time: 4-6 minutes
Components that cannot tolerate reflow:
- Electrolytic caps (some types): max 260°C for 10s only
- Certain connectors with plastic bodies: deform above 250°C
- Pre-programmed devices with limited reflow count
- LEDs: check if moisture sensitivity level (MSL) is met
If mixed: SMD-only = reflow, then wave/selective solder for THT
Single-sided SMD assembly: All 200+ SMD components on the top side. One reflow pass. Seven through-hole connectors on bottom side assembled via selective soldering after reflow. No components require special handling. MSL levels checked: all components opened and assembled within floor life. Reflow profile verified compatible with all package types (max MSL-3 component verified for 168hr floor life).
Large aluminum electrolytic capacitors (3g each) placed on the bottom side with small SMD passives. During second reflow (top side), the heavy caps fall off due to gravity exceeding solder surface tension. Assembly house reports 15% fallout. "Fix" requires expensive adhesive application step before reflow, adding $0.50/board and 30 seconds cycle time.
Checkpoint 3: Wave Solder Clearances Met Major
If through-hole components require wave soldering, all bottom-side SMD components must have adequate clearance from the solder wave to prevent bridging, and must be glued down to survive the wave solder process.
Wave Solder Design Rules
Component-to-wave clearance (bottom side SMD):
Minimum 1.5mm from any bottom-side SMD pad to nearest THT pad
Preferred: 2.5mm clearance
THT component orientation for wave solder:
Long axis of component perpendicular to wave direction
Pin 1 (or lead closest to body) enters wave first
Lead spacing ≥ 2.54mm (finer pitch requires selective solder)
Thief pads (solder thieves):
Add sacrificial pads on the trailing edge of large/multi-pin THT components
Size: 1.5-2mm diameter, 0.5mm from last pin
Catches excess solder that would otherwise bridge pins
SMD on wave-solder side (if unavoidable):
- Must be glued (adhesive dot under component center)
- Long axis oriented parallel to wave travel direction
- Minimum 1.27mm pitch (nothing finer survives wave)
- No BGA, QFN, or fine-pitch ICs on wave side
Through-hole connectors wave soldered on bottom side. All SMD components are on top (reflow side). THT leads extend 1.0-1.5mm below board surface. Connectors oriented with rows perpendicular to wave travel. Thief pads added on trailing edge of 20-pin connector. No bottom-side SMD within 5mm of any THT pad.
Fine-pitch SOIC-16 (1.27mm pitch) placed 1mm from through-hole connector pins on the wave solder side. Wave solder bridges between SOIC pins and connector pins. Rework rate: 40%. Requires manual touch-up of every board, negating the speed advantage of wave soldering.
Checkpoint 4: Tombstoning Prevention (Symmetric Pads) Major
Tombstoning occurs when one end of a small passive component lifts off the board during reflow due to unequal solder paste wetting forces. It is the most common assembly defect for 0402 and smaller passives.
Root Causes and Prevention
Tombstoning occurs when:
Force on pad A ≠ Force on pad B during solder melting
Causes of imbalance:
1. Asymmetric thermal mass: One pad connects to large copper pour
→ One pad heats later → Solder melts unevenly
2. Asymmetric pad size: Different pad areas give different wetting forces
3. Asymmetric paste deposit: Stencil aperture differences
4. Trace routing asymmetry: One trace larger than the other
5. Via-in-pad on one side: Via pulls solder away from that pad
Prevention rules:
- Pads MUST be identical size on both ends of passive
- Trace connection must be symmetric (same width, same direction)
- If one pad connects to ground plane, add thermal relief on BOTH pads
or provide identical copper mass on both sides
- No via within 0.5mm of passive pad (for 0402 and smaller)
- Stencil apertures identical for both pads
Thermal Symmetry Rules by Component Size
| Package | Tombstone Risk | Key Rule | Max Copper Asymmetry |
|---|
| 0201 | Very High | Identical pads, equal trace width, no vias within 0.3mm | < 5% area difference |
| 0402 | High | Symmetric pads and routing, thermal relief if plane-connected | < 10% area difference |
| 0603 | Moderate | Reasonably symmetric, avoid via-in-pad | < 20% area difference |
| 0805 | Low | General symmetry sufficient | < 30% area difference |
| 1206+ | Very Low | Component mass prevents tombstoning | Not critical |
Symmetric Trace Routing Example (0402 cap):
BAD: Pad 1 → 0.2mm trace to ground plane (massive copper)
Pad 2 → 0.15mm trace to IC pin (minimal copper)
Result: Pad 1 heats slower, solder melts at pad 2 first → tombstone
GOOD: Pad 1 → 0.15mm trace → thermal relief spoke → ground plane
Pad 2 → 0.15mm trace → IC pin
Both pads have similar thermal mass → symmetric melting
ALTERNATIVE: Route both pads with 0.15mm trace for 0.5mm
before connecting to different nets. The 0.5mm trace acts as
a thermal equalizer between the two pad connections.
All 0402 decoupling caps: Both pads are 0.5mm × 0.5mm. Trace exits both pads with 0.15mm width for at least 0.3mm before widening. Via for ground connection placed 0.5mm from pad edge (not via-in-pad). Thermal relief used on inner layer ground connection. Reflow results: zero tombstones in 5000-board run.
0402 capacitor with one pad directly connected to a via (via-in-pad) and the other pad connected via a 0.1mm trace to a QFN pin. The via acts as a heat sink on one pad AND pulls solder into the via hole. Double asymmetry causes 8% tombstone rate at this specific component location.
Checkpoint 5: BGA Rework Clearance Minor
BGAs occasionally need rework (replacement) after assembly. The layout must provide adequate clearance around BGAs for rework equipment access, including hot air nozzle placement and optical alignment.
BGA Rework Space Requirements
Minimum clearance around BGA for rework:
Hot air nozzle clearance: 2-3mm on all sides (nozzle larger than package)
Component height adjacent: < 5mm within nozzle zone
Bottom-side heater: No tall components on bottom within BGA footprint
Optical alignment: Clear line of sight from two corners minimum
BGA rework process needs:
1. Top nozzle: BGA package size + 2-3mm per side
2. Bottom preheater: Area = 1.5× BGA area minimum
3. Vacuum pickup tool access from top (no overhanging components)
4. Flux application access (syringe dispense around perimeter)
5. Inspection access (X-ray, endoscope, or visual from side)
Clearance Rules
| BGA Size | Min Clearance (all sides) | Max Adjacent Height | Bottom-Side Restriction |
|---|
| ≤ 10×10mm | 2mm | 3mm | No components > 2mm within footprint |
| 10-20mm | 3mm | 4mm | No components > 3mm within footprint+5mm |
| 20-35mm | 4mm | 5mm | No components > 3mm within footprint+8mm |
| > 35mm | 5mm | 6mm | Bottom essentially clear for preheater |
FPGA BGA (23×23mm, 484 balls): 4mm clearance on all sides to nearest component. No component taller than 3mm within 30×30mm zone. Bottom side has only flat passives (< 1mm) in the BGA zone. Two corner fiducials visible for optical alignment during rework. BGA pads are NSMD (non-solder-mask-defined) for easier reball/rework.
BGA processor with 10mm tall electrolytic capacitors placed 1.5mm from the BGA edge. During rework, the hot air nozzle cannot be sized correctly without heating adjacent caps. Caps must be removed first (adding 30 minutes to rework time). Also, a shield can over the BGA prevents nozzle access entirely -- shield must be removed first, further complicating rework.
Checkpoint 6: Fiducial Marks Placed (Global + Local) Critical
Fiducial marks are alignment targets used by pick-and-place machines and AOI (Automated Optical Inspection) systems to precisely locate and orient the PCB. Without proper fiducials, placement accuracy degrades significantly.
Fiducial Types and Requirements
Global Fiducials (Board-Level):
Purpose: Register entire board position and rotation
Quantity: Minimum 2 (diagonal corners), preferred 3 (L-shape)
Location: 5mm minimum from board edge, diagonal corners
Mark: 1.0mm diameter copper circle (exposed, no solder mask)
Clearance: 2mm radius solder mask opening (no copper or silk within)
Surface: Same finish as pads (HASL, ENIG, etc.)
Local Fiducials (Component-Level):
Purpose: Precisely locate fine-pitch ICs and BGAs
Required for: BGA, QFP with pitch ≤ 0.5mm, all CSP packages
Quantity: 2 per component (diagonal corners of the component)
Location: Within 5mm of component corners, outside pad area
Mark: 1.0mm diameter copper circle
Clearance: 2mm radius solder mask opening
Panel Fiducials:
3 fiducials on panel tooling rails (diagonal arrangement)
Used for panel-level registration before individual board correction
Fiducial Placement Rules
- Place 3 global fiducials: two on one edge, one on opposite edge (forms asymmetric triangle for unambiguous orientation).
- For each BGA and fine-pitch QFP (≤ 0.5mm pitch), place 2 local fiducials at diagonal corners of the component.
- Fiducial marks must be copper circles (1.0mm) with NO solder mask for 2mm radius around them.
- Ensure fiducial contrast: copper mark on FR4 background (or solder-mask background if using copper clearance approach).
- No silk screen, copper traces, vias, or other features within the 2mm clearance zone.
- Verify fiducials are on the same layer as the components they serve (top fiducials for top-side placement).
Fiducial Design Variations
| Parameter | Standard | Minimum | Notes |
|---|
| Mark diameter | 1.0mm | 0.5mm | Larger is more reliable for vision systems |
| Clearance radius | 2.0mm | 1.5mm | Clear area around mark for contrast |
| Shape | Circle | Circle | Never use square or diamond (orientation ambiguous) |
| Surface | Exposed copper (ENIG/HASL) | Bare copper | Reflective surface for vision system |
| Solder mask | Removed in clearance zone | Removed over mark | Mark must contrast with background |
| Edge distance | 5mm from board edge | 3mm | Must be within camera field of view |
Three global fiducials: two in top-left and top-right corners (5mm from edge), one in bottom-left corner. Each is a 1.0mm copper circle with 3mm solder mask opening (clear zone). Two local fiducials for each of the 3 BGAs placed at opposite corners, 3mm from BGA pad field edge. All fiducials clearly visible in Gerber review -- verified no overlapping features in clearance zones.
Only 2 fiducials placed on one edge of the board (cannot determine rotation unambiguously). Fiducial clearance zone has a signal trace passing through it (confuses vision system). No local fiducials for 0.4mm-pitch BGA -- placement accuracy relies only on global fiducials, resulting in ±50µm offset. Some BGA balls miss their pads, causing opens after reflow.
