Injection molding is the dominant manufacturing process for high-volume plastic parts — but a plastic part that looks correct in CAD can be completely unsuitable for molding. Draft angles, wall thickness, gate location, and undercut handling must be designed correctly from the start, because mold modifications after tooling is cut are expensive and often produce compromises.
This guide covers the key design rules for injection-molded plastic parts: draft angle requirements, uniform wall thickness and why it matters, sink marks and their causes, weld lines and their effects, gate types and positioning strategy, undercuts and side actions, and shrinkage allowance. These rules apply to thermoplastic injection molding — the most common process for industrial and consumer plastic components.
Draft Angle: The Foundation of Mold Release
Draft angle is the taper applied to vertical walls (relative to the mold opening direction) that allows the part to eject from the mold without sticking or dragging. A perfectly vertical wall has zero draft — the part would need to be pried out of the mold, causing surface damage and potentially permanent mold damage. Draft angles are not a manufacturing compromise; they’re a fundamental requirement for molded parts.
Guideline minimum draft angles: 1° per side for textured or polished surfaces with standard surface finish (Ra 0.8–1.6 μm range); 1.5°–2° for most industrial parts; 3°–5° for deep draws (features with high depth-to-width ratios); additional 0.5°–1° per 0.025mm of texture depth for textured surfaces (a leather grain texture with 0.075mm depth requires approximately 3° additional draft). The higher the cavity depth and the more aggressive the texture, the more draft required.
Zero-draft or negative-draft features create undercuts — covered in detail later. If a vertical wall is absolutely required (typically for precise mating interfaces or press-fit features), it must be located at the parting line or handled with side actions, which significantly increases mold cost. Designing for 1°–2° draft on all walls aligned with the pull direction is the baseline that every plastic part should meet before mold design begins.
Wall Thickness: Uniformity and Its Impact
Non-uniform wall thickness is the single most common cause of cosmetic defects (sink marks, warpage) and structural inconsistency in injection-molded parts. The reason: plastic cools from the outside surfaces inward. Thick sections cool and solidify last; as the molten core cools, it shrinks, pulling the solidified outer surface inward — creating sink marks on the visible surface. The same differential shrinkage that causes sink marks also creates internal stresses that drive warpage in asymmetric parts.
The fundamental guideline: maintain uniform wall thickness throughout the part wherever possible. Where thickness variation is unavoidable, transitions should be gradual — use chamfers or radii rather than abrupt steps, with the ratio of adjacent wall thicknesses not exceeding 2:1. When a thick feature must connect to a thin wall (boss roots, rib connections), core out the thick region from the back to achieve nominal wall thickness rather than leaving a solid thick section.
Recommended wall thickness ranges by material: Polypropylene (PP) — 0.8–3.8mm; ABS — 1.2–3.5mm; Nylon (PA66) — 0.8–3.0mm; Polycarbonate (PC) — 1.0–4.0mm; Acetal (POM) — 0.8–3.0mm. These ranges balance adequate structural performance, achievable fill, and cosmetic quality. Walls thinner than the minimum for a material are difficult to fill reliably; walls thicker than the maximum create excessive shrinkage, cooling time, and sink risk.
Sink Marks: Causes and Prevention
Sink marks appear as depressions on the visible surface of a part, typically opposite thick features (ribs, bosses, gussets) that were molded into the non-visible side. They occur because the thick feature’s core remains molten after the outer surface has solidified, and the shrinking core pulls the surface inward.
Prevention approaches: (1) Limit rib thickness to 60–70% of the adjacent wall thickness — this is the most reliable prevention method. A 2mm wall should have ribs no thicker than 1.2–1.4mm. (2) Core out bosses and thick features from the rear (blind coring) so the section seen from the visible surface has nominal wall thickness. (3) Locate cosmetically sensitive surfaces opposite thin sections rather than thick sections. (4) Apply texture to cosmetically visible surfaces — moderate textures can disguise minor sink marks that would be obvious on a polished surface.
Some sink marks are unavoidable — particularly on structural ribs and bosses on visible surfaces. In these cases, accept the trade-off between structural integrity and cosmetic perfection or add texture to disguise. An entirely sink-free part may not be achievable if structural ribs are required on a Class A surface.
Weld Lines: Where They Form and Why They Matter
Weld lines (also called knit lines or meld lines) form where two flow fronts of molten plastic meet during fill. At this junction, the plastic freezes with a cold-welded interface that has reduced mechanical strength and visible appearance compared to the surrounding material — a weld line in a transparent part is clearly visible as a line; in a pigmented part it may appear as a streak or color variation.
Weld lines always occur downstream of holes, through which the melt flow splits and rejoins. They also occur when the melt front splits around a core pin and meets on the opposite side. The structural penalty depends on material — amorphous materials (ABS, PC) form stronger weld lines than semi-crystalline materials (PP, nylon) because the molecular structure can partially knit across the weld interface in amorphous materials.
Design approaches for managing weld lines: (1) Relocate or reposition gates to move weld line locations away from stress concentration zones or cosmetically critical areas. (2) Increase mold temperature and injection speed (process optimization) to improve weld line strength — better than design changes for existing tooling. (3) Use venting or vacuum-assist to ensure gases don’t trap at weld line locations and degrade the interface. (4) Accept weld lines in low-stress, non-cosmetic locations and design for strength where they occur.
Gate Types and Gate Location Strategy
The gate is where molten plastic enters the mold cavity — gate location and type profoundly affect part quality, because flow from the gate determines where weld lines form, how the part fills, and where shrinkage is compensated or not.
Edge gate: The most common and flexible gate type, located at the parting line on the edge of the part. Easy to adjust for process optimization, leaves a visible gate vestige that typically requires trimming. Good for most general parts.
Submarine (tunnel) gate: A submerged gate that automatically shears during ejection, leaving a minimal vestige below the parting line. Excellent for high-volume production where automated de-gating is required. Cannot be used for extremely thick sections or rigid materials that won’t flex during the de-gating shear.
Hot tip/direct gate (through hot runner): Used with hot runner systems that maintain the runner in a molten state between shots. Eliminates runner waste and is cost-effective for high-volume production. The gate mark is visible on the surface — typically a small circular mark. Used for center-gated disk-like parts (the optimal flow pattern for round parts).
Fan gate: A wide gate that distributes the melt uniformly across a large edge — used for large flat parts (panels, covers) where filling uniformity and warpage control are critical. The wide gate area requires careful vestige management.
Gate location principles: (1) Gate into the thickest section — melt flows from thick to thin, not the reverse, and packing pressure (which compensates shrinkage) must reach through the entire cavity from the gate. (2) Locate gates away from cosmetically critical surfaces. (3) Position gates to create balanced flow — ideally the melt front should reach all extremities of the cavity at approximately the same time. (4) Consider weld line location when selecting gate position — the gate position determines where flow fronts meet.
Undercuts and Side Actions
An undercut is any feature that prevents the part from being ejected in the primary pull direction — holes or protrusions oriented perpendicular to the mold opening, through-holes in walls parallel to pull, external hooks or snaps that engage the mold. Every undercut requires either a side action (a mold component that moves laterally before ejection) or a lifter (an angled internal slide), both of which add mold cost — typically $500–$3,000+ per side action depending on complexity and size.
Minimizing undercuts is one of the highest-leverage DFM activities for injection molded parts. Common redesign approaches: (1) Locate snap features at the parting line rather than in the cavity (parting-line snaps are formed by splitting the mold feature between halves, requiring no side action); (2) Replace through-holes in walls (which create undercuts) with U-shaped slots open to the parting line, which can be formed by core pins perpendicular to the parting line; (3) Redesign external hooks to be formed as simple features on the parting line by adjusting parting line location.
Shrinkage Allowance
All thermoplastics shrink as they cool from melt temperature to room temperature. Mold tooling is designed with dimensions scaled up by the expected shrinkage to produce parts at nominal dimensions. Typical shrinkage rates: PP — 1.5–2.5%; ABS — 0.4–0.7%; PA66 (unfilled) — 1.0–2.0%; PA66 GF30 (30% glass-filled) — 0.3–0.6%; PC — 0.5–0.7%; POM (acetal) — 2.0–2.5%.
Non-uniform shrinkage is the root cause of warpage in asymmetric or variable-wall parts. Glass-filled materials shrink differently in the flow direction versus transverse to flow — the fibers align with flow and reduce shrinkage in that direction, creating anisotropic shrinkage that can cause significant dimensional distortion in large flat parts. For flat panels in glass-filled materials, gate location (which determines fiber orientation) profoundly affects warpage behavior.
Conclusion
Injection molding DFM is not a set of arbitrary manufacturing constraints — each design rule reflects a specific physical phenomenon in the molding process. Draft angles prevent drag and sticking during ejection; uniform wall thickness prevents sink marks and warpage from differential cooling; gate location controls fill balance and weld line positioning; undercut minimization controls tooling cost. Designers who understand why these rules exist can apply them intelligently — recognizing where exceptions are justified and where the rules should be followed strictly. The most effective time to apply these guidelines is during conceptual and early detailed design, before tooling decisions lock in the consequences of any oversights.
コメント