Injection molding product design standards are a set of guiding principles designed to ensure that products can be produced efficiently, economically, and with high quality through injection molding process. Following these standards can significantly reduce production issues (such as sink marks, warpage, mold sticking, and short shots), lower mold costs, shorten development cycles, improve product yield and performance.

 

Following are some key points for injection molded product design:

1. Uniformity: This is the most important principle! Wall thickness should be as uniform as possible. Uneven wall thickness can lead to:
Uneven cooling rates: This can cause internal stress and warpage.
Uneven shrinkage: This can cause sink marks and craters (especially in thick-walled areas).
Uneven flow resistance: This can cause short shots or air entrapment.
2. Reasonable range: Wall thickness depends on material, product size, and functional requirements. Common range is 1.5mm - 3.0mm.
Too thin: High flow resistance, difficulty filling cavity (short shot), low strength, easy deformation.
Too thick: Long cooling time, prone to sink marks, pits, bubbles, internal porosity, and high cost.
3. Thickness transition: When wall thickness changes are necessary, transition should be smooth and gradual (tapered transition) to avoid abrupt changes. Transition zone should be at least three times thickness difference.
4. Refer to material supplier's data: Different materials have recommended minimum/typical wall thickness ranges (e.g., PC may require thicker than PP).

1. Necessity: Almost all surfaces perpendicular to parting plane require a draft angle to ensure smooth demolding. Lack of draft angle can result in demolding difficulties, surface scratches, and even damage to mold or part.
2. Angle Size:
This depends on the surface depth, texture, material shrinkage, and mold finish.
External surfaces: 0.5° - 1° is generally sufficient.
Internal Surfaces/Deep Cavities/Roughly Textured Surfaces: A larger slope is required, typically 1°-3° or greater (at least 1° per 25mm of depth).
Fine Etching: Slope of 2°-5° or greater may be required.
3. Direction: Slope should be in a direction that facilitates demolding, typically increasing toward parting surface.

1. Purpose: To increase strength and rigidity, avoid use of thick walls.
2. Thickness: Root thickness of rib should not exceed 50%-60% of thickness of main wall to which it connects (50% is common). Excessive thickness will cause sink marks on the back of rib.
3. Height: Height should generally not exceed three times main wall thickness. Excessive height may cause demolding difficulties or cause rib to buckle.
4. Root Radius: Rib must have a radiused transition (R-angle) at junction with main wall to reduce stress concentration and improve flow. R-angle is typically 25%-50% of rib root thickness.
5. Top: Top of rib can be designed as a small platform (flat top) rather than a sharp corner to facilitate mold processing and demolding.
6. Draft: Sides of rib also require a draft angle (usually at least 0.5°-1°).
7. Layout: Avoid thick wall areas at the ends of rib. Rib direction should align with primary load direction. Avoid sharp intersections between ribs or between ribs and wall.

 

1. Necessity: Avoid sharp 90-degree angles at all internal and external corners. Using radiused corners can:
Greatly reduce stress concentration: Improve product strength and impact resistance.
Improve melt flow: Ensure smoother plastic flow, reducing turbulence, stagnation, and air entrapment.
Improve mold filling: Reduce flow resistance.
Extend mold life: Avoid cracking caused by stress concentration at sharp corners and facilitate demolding.
 2. Dimensions:
Inner Fillet: Recommended minimum radius is 0.5 times wall thickness. Ideal value is 0.6-1 times wall thickness.
Outer Fillet: Recommended minimum radius is 1.0 times wall thickness. Ideal value is 1.5 times wall thickness.
General principle: Inner Fillet Radius + Outer Fillet Radius ≈ Wall Thickness.

1. Type:
Through Holes: Through holes are preferred, as they are easier to form than blind holes (supported by cores at both ends, providing better strength).
Blind Holes: Depth should be as shallow as possible (depth ≤ 2-3 times diameter), and bottom should be spherical or conical. Wall thickness at the bottom of hole should be at least 1/6 of hole diameter.
2. Edge Distance: Distance from hole edge to product edge or other holes should be at least 1.5-2 times hole diameter. Too close a distance can lead to uneven wall thickness, air trapping, weak strength, and die problems.
3. Shape: Design for round holes whenever possible. Irregular-shaped holes (square holes, slotted holes) increase mold complexity and cost (may require sliders or electrodes).
4. Side holes/undercuts: These require sliders or a tilting mechanism, significantly increasing mold cost and complexity. Avoid them unless absolutely necessary. If necessary, allow sufficient space for slider movement and consider location of slider parting line.
5. Hole edge reinforcement: Bosses or localized thickening can be designed around load-bearing holes to strengthen them.
6. Countersunk holes: Design them in two parts (pilot hole + tapered hole) to avoid sharp steps in mold.

1. Ejector Pin Position: Consider location and number of ejector pins (ejector pins, ejector plates, and air ejectors). Ejector pins should be placed in areas with good strength, high load bearing capacity, and low risk of ejection whitening or deformation (such as rib bases, bosses, and thick walls).
2. Ejector Pin Marks: Ejector pins leave marks on product, so their impact on both appearance and function should be considered during design.
3. Estimating demolding force: Areas with high product clamping forces (such as deep cavities, rough textures, and areas without slopes) require stronger ejection forces or more ejector pins.

1. Fixing: Inserts must be reliably positioned and secured in mold (e.g., using pins, slots, or vacuum suction).
2. Anti-rotation/pullout: Insert surfaces must be designed with anti-rotation and anti-pullout features (e.g., knurling, grooves, holes, or flattening).
3. Wall Thickness: Plastic layer covering the insert should be sufficiently thick (typically ≥ 0.8 times insert diameter or maximum dimension) to ensure bonding strength and prevent cracking.
4. Thermal Expansion Difference: Consider difference in thermal expansion coefficients between metal insert and plastic to avoid excessive stress after cooling that could cause cracking. Preheating insert may be necessary.
5. Avoiding Sharp Corners: Edges where insert contacts plastic should be chamfered or rounded.

1. Reasonableness: Injection molded parts have inherent dimensional fluctuations. Tolerances should be set reasonably and sufficiently loose to avoid unnecessary mold adjustments and increased costs.
2. Influencing Factors: Tolerances are affected by factors such as material shrinkage (which has its own range), mold precision, injection molding process (pressure, temperature, time), wall thickness, and geometry.
3. Reference Standards: Reference industry standards (such as ISO 20457:2018, "Plastic Molded Parts — Dimensional Tolerances") or set based on experience. Typical tolerance grades for injection molded parts range from MT2 to MT5 (medium precision). ±0.1mm to ±0.3mm are common linear dimension tolerance requirements; more precise tolerances may require specialized processing and higher costs.
4. Cumulative Tolerances: Avoid excessively long dimensional chains, as cumulative tolerances can increase.

1. Mold Surface: Product appearance depends on mold surface condition (polishing, graining/etching, sandblasting, etc.). Design considerations:
Draft angle: The deeper texture, the greater required draft angle.
Parting line: Location and detail of parting line directly impact appearance. Try to place parting line in an inconspicuous location or where functionality allows.
Polishing direction: If a high gloss finish is required, consider direction of polishing pattern.
2. Gate marks: Type and location of gate will affect size and visibility of residual marks (such as point gate marks and latent gate marks). Consider placing them on concealed surfaces during design.
3. Weld lines/meld lines: These are formed where multiple material streams converge. They affect appearance and strength. Designs should minimize formation of weld lines on surfaces with high appearance requirements or in high-stress areas. These can be improved by adjusting gate location, wall thickness, adding overflow wells, or optimizing flow paths.
4. Air entrapment: Air can easily become trapped at the end of cavity or at flow confluences, leading to burning and material shortages. Design should ensure smooth venting, or incorporate venting grooves/overflow wells.

Material properties (flowability, shrinkage, strength, toughness, temperature resistance, chemical resistance, flame retardancy, cost, etc.) must be considered at outset of design, as material directly impacts design parameters such as wall thickness, corner radius, ribs, and draft angle.
Shrinkage: Shrinkage varies significantly among different materials (e.g., PP ~1.5-2.5%, ABS ~0.4-0.7%, POM ~1.8-2.5%, PC ~0.6-0.8%). Mold dimensions should be scaled accordingly.

Product designers need to understand basic mold structure (parting surface, core/cavity, slider, lifter, ejector system, gating system, and cooling system). Consider following during design:
Parting surface selection: How can mold parting be achieved most simply and efficiently? Is parting line positioned appropriately?
Mold processability: Is structure amenable to CNC machining, EDM processing, and polishing?
Mold strength and life: Avoid design-induced weaknesses such as thin steel sections and sharp corners. Simplify mold structure: Avoid or minimize use of side core pulls (sliders/elevators) to reduce costs. Where possible, utilize elastic deformation of part to achieve mold release (forced demolding).

 

1. Design for Manufacturing (DFM): Core of injection molded product design is design for manufacturing. Always consider, "Can this design be molded efficiently, cost-effectively, and with high quality?"
2. Communication: Thorough communication with mold designers and injection molding process engineers during product design phase is crucial. They can provide valuable experience and timely feedback.
Simulation Analysis: Using mold flow analysis software (such as Moldflow) to perform simulations during design phase can predict issues such as filling, cooling, warpage, weld lines, and air entrapment, optimize design and process parameters, significantly reducing mold trial risks and costs.
3. Iterative Optimization: Designs are rarely perfect the first time. Iterative optimization based on mold trial results and feedback is norm.
Adhering to these design standards and leveraging tools and teamwork are key to successfully developing injection molded products.