Adding material to make a part stronger often makes it weaker. Thick sections cool slowly, creating internal stresses and voids that compromise both strength and appearance. This counterintuitive reality drives one of injection molding’s most important design principles: wall thickness must be considered from the start, not added later for structural reasons. Understanding how thickness affects filling, cooling, and shrinkage enables designs that are both manufacturable and functional.
The Uniform Wall Principle
Consistent wall thickness throughout a part produces the most predictable, highest-quality results. Variations in thickness create problems at every stage of the molding process.
During filling, material flows preferentially through thicker sections because they offer less resistance. This race-tracking effect can cause thin areas to fill last or incompletely. Air traps form where flow fronts meet unpredictably. Weld lines appear in locations that proper flow balance would avoid.
During cooling, thick sections take longer to solidify than thin sections. The relationship follows a square law: doubling wall thickness quadruples cooling time. A part with both 2mm and 4mm sections has its cycle time dictated by the 4mm section, wasting capacity on the 2mm areas that solidified quickly.
During shrinkage, thick and thin sections contract at different rates and times. Thick sections are still shrinking while thin sections have finished. This differential shrinkage creates internal stresses that cause warpage, bowing parts toward the slower-cooling thick regions.
Sink marks appear where thick sections back up against visible surfaces. The thick region shrinks inward as it cools, pulling the adjacent surface with it. Pack pressure cannot fully compensate because the gate freezes before thick sections finish solidifying.
Achieving perfect uniformity isn’t always possible, but understanding the consequences of variation helps manage tradeoffs. Where variation is unavoidable, gradual transitions and strategic gate placement minimize problems.
Material-Specific Recommendations
Different polymers have different flow characteristics, shrinkage rates, and mechanical requirements that influence optimal wall thickness.
| Material | Recommended Range | Notes |
|---|---|---|
| ABS | 1.2-3.5mm | Forgiving, good flow |
| Polycarbonate | 1.0-4.0mm | Higher viscosity, needs temperature |
| Polypropylene | 0.8-3.0mm | High shrinkage, avoid thick sections |
| HDPE | 1.0-4.0mm | Very high shrinkage |
| Nylon (PA6, PA66) | 0.8-3.0mm | Moisture sensitive, crystalline |
| Acetal (POM) | 0.8-3.0mm | High shrinkage, excellent flow |
| Polystyrene | 0.9-4.0mm | Brittle, good flow |
| PBT | 0.8-3.0mm | Fast crystallization |
Why some materials tolerate thinner walls: Low-viscosity materials (PP, PS, acetal) flow readily, filling thin sections with less pressure. Their flow properties allow thinner designs. High-viscosity materials (PC) require thicker walls or higher processing temperatures and pressures to fill completely.
Minimum practical limits depend on flow length and part geometry. A 50mm square part can fill at thinner walls than a 200mm long narrow section. The length-to-thickness ratio (L/t) matters more than absolute thickness. Conventional molding typically works with L/t ratios under 100:1. Thin-wall applications push toward 200:1 or higher with specialized processes.
Maximum practical limits balance structural needs against cycle time and sink mark risk. Walls thicker than 4mm almost always create problems: long cycles, sink marks, voids, warpage. When structural requirements suggest thicker walls, alternative approaches (ribs, gas assist, foam) usually work better.
Designing for Uniform Cooling
Perfect uniformity isn’t achievable in many functional parts. When thickness must vary, design strategies minimize the consequences.
The 3:1 rule limits maximum thickness transitions. Adjacent wall thicknesses should differ by no more than a 3:1 ratio. A 3mm wall transitioning to a 1mm wall is acceptable; a 4mm wall adjacent to a 1mm wall invites problems.
Gradual transitions distribute shrinkage stress over distance rather than concentrating it at abrupt steps. Thickness changes should occur over a length at least three times the thickness difference. A transition from 3mm to 2mm should span at least 3mm of length, not step abruptly.
Coring out thick sections removes material that serves no structural purpose. A boss that would be solid at 8mm diameter should be cored to create a wall thickness matching surrounding features. Ribs add stiffness more efficiently than solid sections.
Rib design follows specific rules to avoid sink marks:
Rib thickness should be 40 to 60 percent of the adjacent wall thickness (40 percent for high-gloss surfaces where sink visibility is critical, up to 60 percent for textured or hidden surfaces).
Rib height can extend to three times the adjacent wall thickness without causing problems.
Draft on rib sides (typically 0.5-1 degree minimum) aids ejection.
Base radius (approximately 0.25 times wall thickness) reduces stress concentration without creating thick intersections.
Gate location affects how uniformly the part fills and packs. Gates positioned near thick sections allow pack pressure to compensate for shrinkage longest. Gates in thin sections may freeze before thick areas are adequately packed.
When Thick Walls Are Unavoidable
Some applications require thickness beyond guidelines for structural, assembly, or cosmetic reasons. Strategies exist to manage the consequences.
Gas assist molding injects nitrogen into thick sections after the mold fills. The gas displaces molten core material against the walls, creating hollow channels. Thick sections that would take minutes to cool become thin-wall tubes that cool quickly. The technique eliminates sink marks and reduces cycle times dramatically for appropriate parts.
Structural foam incorporates blowing agent into the melt. The foaming action creates cellular structure in thick sections, reducing density while maintaining exterior surfaces. Foam parts have lower sink mark risk and faster cooling than solid parts of similar dimensions.
Sequential valve gating uses multiple hot runner gates that open in sequence, controlling flow patterns and pack pressure delivery. Independent gate control allows packing thick sections while thin sections are sealed.
Extended cooling accepts longer cycle times when other options aren’t feasible. Sometimes the economics work: a part that must be thick for functional reasons may justify the cycle time penalty if alternatives (redesign, gas assist, multiple components) cost more.
Assembly approaches split thick features into multiple parts that join together. A thick handle that would be problematic as a single molding might work as two thinner shells that snap or weld together.
Thin Wall Molding
At the opposite extreme, thin-wall molding pushes boundaries of what injection molding can fill.
Definition varies, but walls under 1mm or length-to-thickness ratios above 100:1 generally qualify as thin-wall. Food packaging, medical components, and electronics housings often require thin-wall approaches.
Different challenges arise: freezing before fill completion, high injection pressure requirements, shear sensitivity that can degrade material, and mold filling imbalance from tiny geometry variations.
Process requirements include high injection speeds (often 500+ mm/second), elevated melt temperatures, elevated mold temperatures, machines with high injection rate capability, and molds designed for the extreme pressures involved.
Material requirements favor high-flow grades specifically designed for thin-wall applications. Standard grades may not fill thin geometries regardless of process adjustments.
Moldflow analysis becomes essential rather than optional. Simulation predicts filling problems, pressure requirements, and weld line locations that cannot be anticipated from experience alone.
Thin-wall applications require more engineering investment than conventional molding but enable parts that would otherwise be impossible or require different manufacturing technologies.
Analyzing Wall Thickness Impact
Before committing to tooling, evaluating how wall thickness affects manufacturability prevents expensive problems.
Simple analysis involves reviewing part geometry for thickness variations, calculating maximum L/t ratios, checking rib proportions, and identifying potential sink mark locations. Experienced designers catch many problems through visual review.
Warning signs that suggest analysis is needed:
Wall thickness varies by more than 2:1 anywhere in the part.
Maximum thickness exceeds 4mm.
L/t ratio exceeds 100:1 in any flow path.
Ribs, bosses, or other features intersect at thick junctions.
Part function requires tight flatness or dimensional tolerances.
When moldflow simulation is necessary:
Complex geometry where intuition doesn’t predict flow patterns.
Tight tolerances where warpage prediction matters.
Multiple gate options requiring comparison.
Thin-wall applications pushing process limits.
High-value tooling where upfront analysis costs less than trial-and-error.
Simulation predicts fill patterns, pressure requirements, cooling time, warpage magnitude and direction, and optimal gate locations. The investment in analysis often pays back through avoiding mold modifications that result from unanticipated problems.
Wall thickness is the single most important factor in part design for injection molding. Getting it right simplifies everything else; getting it wrong creates cascading problems that no amount of process adjustment can fully resolve. Starting with thickness considerations, rather than adding them as constraints late in design, produces parts that are both functional and manufacturable.
Sources
- Bralla, James G. “Design for Manufacturability Handbook.” McGraw-Hill.
- Kazmer, David O. “Injection Mold Design Engineering.” Hanser, 2007.
- Malloy, Robert A. “Plastic Part Design for Injection Molding.” Hanser, 2010.
- Proto Labs Design Guidelines. “Wall Thickness Recommendations.”
- Autodesk Moldflow. “Design Optimization Guidelines.”