Plastic Injection Molded Part Design Guide

Injection molding can be used to manufacture a wide range of parts, from small components like AAA battery cases to large components like truck body panels. After part design is complete, a mold is created and precision-machined to create desired part's features. Injection molding process involves feeding a thermoplastic or thermoset plastic feedstock into a heated barrel, mixing it, and pressing it into a metal mold cavity. Plastic cools and solidifies within cavity before being removed, completing injection molding process.

Terms "mold" and "die" are used interchangeably to describe tooling used in plastic part production. Molds are typically made of pre-hardened steel, hardened steel, aluminum alloy, and/or beryllium copper. Of these materials, hardened steel molds are the most expensive to manufacture, but they offer a long service life—and by spreading cost over larger production batches, cost per part can be reduced. For small batches or large parts, pre-hardened steel molds are a more economical option, but they offer lower wear resistance.
Aluminum alloy molds are the lowest-cost option. When designed and manufactured using computer numerical control (CNC) or electrical discharge machining (EDM), these molds can economically produce tens to hundreds of thousands of parts. Note: Beryllium copper alloy is often used in areas of mold where rapid heat dissipation is required or where shear heat generation is most concentrated.

Injection molding process uses granular plastic feedstock, which is gravity-fed through a hopper. A screw-type plunger forces feedstock into a heated chamber called barrel, where it melts. Plunger continues to advance, forcing polymer melt through a nozzle at the end of barrel (which fits snugly into mold). Molten plastic enters mold cavity through gate and runner system.
Once cavity is filled, a holding pressure must be maintained to compensate for shrinkage as plastic cools. At the same time, screw rotates, delivering material needed for next injection ("shot") to injection position. Barrel retracts as material for next shot heats up. Because mold remains cool, plastic quickly solidifies once cavity is filled. Once part inside mold has completely cooled, mold opens and part is ejected. Mold closes and polymer melt is injected into cavity again, marking beginning of next injection cycle.

A variety of thermoplastics are available commercially, and specific choice depends on specific application of part. Following table lists some of the most commonly used materials:
Common Engineering Thermoplastics for Injection Molding: Nylons, Polyphenylene Sulfide (PPS); Polycarbonates; Polyether Sulfone; Acetals; Polyetheretherketone (PEEK); Acrylics; Fluoropolymers; Polypropylenes; Polyetherimide (PEI); Polyethylenes; Polyphenylene Oxide (PPO); Acrylonitrile-Butadiene-Styrene (ABS); Polyurethanes (PUR); Thermoplastic Elastomers; Polyphthalamide (PPA).

Cost savings are greatest when wall thickness is minimized while ensuring proper part functionality and mold filling requirements. Obviously, thin-walled parts cool faster, shortening injection molding cycle and increasing number of parts produced per unit time. Furthermore, thin-walled parts are lighter and require less plastic per part.
Typically, wall thickness of injection molded parts ranges from 2mm to 4mm (0.080 in. to 0.160 in.); thin-wall injection molding can produce parts with walls as thin as 0.05mm (0.020 in.).

Parts with uniform wall thickness make it easier to fill mold cavity because molten plastic does not have to overcome resistance caused by varying wall thickness during filling.
If wall thickness is uneven, thin-walled areas cool and solidify first. As thicker walled areas cool and contract, stresses are generated at interface between thin and thick walls. Since thin-walled areas are already solidified, they cannot deform. Deformation in thicker walled areas can cause part to warp or twist. Excessive stress can even cause part to crack.

 

Figure 1: Uniform wall thickness can reduce or eliminate warpage (labeled: Warping)

If uniform wall thickness is unattainable due to design constraints, wall thickness transition should be as smooth as possible.

 

Figure 2: Wall thickness transition design (H is baseline wall thickness; a good transition requires a transition length ≥ 3H)
Coring: By removing some plastic from thick wall areas, wall thickness is maintained uniform, fundamentally addressing problem of uneven wall thickness.

 

Figure 3: Coring eliminates sink marks (labeled: Cored for Uniform Wall Thickness - no sink marks; Not Cored - sink marks; T is thickness of thick wall area, t is target uniform wall thickness, T>>t)
Gussets: Incorporating gussets into part design as support structures can reduce risk of part warpage.

 

Figure 4: Gussets Reduce Warpage (Note: Warping without gussets—warping; Gussets Minimize Warping with gussets—reduced warping)

Severe shrinkage can occur when areas of uneven wall thickness (such as ribs, screw posts, or other protrusions that extend beyond base wall thickness) intersect. Because thicker areas cure more slowly, connection between them and base wall shrinks along with protrusions, resulting in sink marks on base wall surface.
Maintaining rib thickness between 50% and 60% of wall thickness to which it connects can minimize this shrinkage. Furthermore, screw posts designed at part corners can create thicker areas, which can lead to sink marks. Isolating screw posts from the corners is crucial to avoid sink marks (see figure below).

 

Figure 5: Boss design eliminates sink marks (Note: Boss at Corner - Sink mark; Boss isolated from Corner - No sink mark)

Differential cooling rates between thin-walled and thick-walled areas can also cause part warpage. As thick-walled areas cool and shrink, they "drain" material from unsolidified areas, ultimately causing part warpage.
Other factors that may contribute to warpage include injection molding process parameters (such as injection pressure and cooling rate), packing issues, and mold temperature. For optimal molding results, follow process guidelines provided by resin manufacturer.

 

Figure 6: Warpage caused by uneven wall thickness

Bosses serve several functions: positioning mating parts, securing fasteners (such as screws), and accommodating threaded inserts.

 

Figure 7: Screw stud design guidelines (Note: D is screw stud diameter, R is root radius, H is screw stud height, and T is base wall thickness; Key parameters: H ≤ 5T, R ≥ 0.25T, screw stud wall thickness ≤ 0.6T (Xs = 60% of T), screw stud top wall thickness ≤ 0.7T (Ys = 70% of T); "D - Radius Prevents Core Pin Burning" - Boss root radius prevents core pin burning.
Screw stud wall thickness should be less than 60% of part wall thickness to reduce sink marks. If screw stud is located in a non-appearance area, wall thickness can be increased appropriately to withstand greater stress of self-tapping screw.
Screw stud root radius should be at least 0.25 times part wall thickness.
Screw stud strength can be enhanced by adding a gusset at the root or connecting stud to adjacent wall with a connecting rib.

 

Figure 8: Screw column reinforcement methods (labeled: Connecting Rib; Gussets)

Purpose of rib design is to increase bending stiffness of a part without increasing wall thickness. Ribs increase part's moment of inertia, thereby increasing bending stiffness.
Flexural stiffness calculation formula: Flexural stiffness = E (Young's modulus) * Moment of Inertia

Rib thickness should be less than part wall thickness to minimize sink marks. It is recommended that rib thickness not exceed 60% of part wall thickness. Furthermore, corners connecting rib to wall should be as rounded as possible.

 

Figure 9: Proper Rib Design Minimizes Sink Marks (Note: W is rib thickness, T is part wall thickness; W = 40%-60% of T means no sink mark; W is too large and a sink mark appears; R ≥ 0.25T is recommended fillet, and R2 25% of T is preferred.)

Material thickness at rib intersection increases, requiring hollowing or other material removal methods to avoid excessive sink marks on the back of part.

 

Figure 10: Rib Intersection Hollowing Design (Note: Core at Rib Intersection Hollowing — Minimizes Sink)

Rib height should be within three times its thickness (H ≤ 3T). To increase bending stiffness, multiple ribs are recommended rather than a single, high rib.

 

Figure 11: Rib Design Parameters (Note: H is rib height, T is part wall thickness, and W is rib thickness; Key parameters: H ≤ 3T, W = 40%-60% of T, rib spacing Sz ≥ 2T)

Rib orientation must provide maximum bending stiffness for part. During design, part geometry must be considered to ensure that rib orientation matches bending load direction; otherwise, ribs will not increase part stiffness.

 

Figure 12: Effect of Ribs and Load Direction on Part Stiffness (Note: Load is load direction, Reaction Force is reaction force; correctly oriented ribs transmit reaction force, while incorrectly oriented ribs do not increase stiffness.)
Supplement: Draft angle of rib should be at least 0.25° to 0.5° per side.

Draft angle is used to facilitate part removal from mold. It should be parallel to mold opening and closing direction. Ideal draft angle for a part depends on its depth in mold and its end-use function.

 

Figure 12: Draft Angle (labeled: Draft Angle)
Maximizing draft angle allows for easier part release. Typically, a basic draft angle of 1° to 2° is sufficient. If part surface has texture, an additional 1.5° of draft angle should be added for every 0.25 mm of texture depth.
Mold parting line should be strategically positioned to minimize draft angle. If design constraints prevent use of draft angle, a side action mold should be used.

Mold surface can be textured or engraved to add identification information (such as part model number) or enhance appearance (for aesthetic purposes). It can also be used for factory traceability. Texture can also mask surface defects such as weld lines.
Texture or lettering depth is limited, and additional draft angle may be required to prevent scratching or damage during part demolding.
Draft angle should be determined based on part design and desired texture. As a general guideline, a minimum draft angle of 1.5° should be added for every 0.025 mm (0.001 in) of texture depth, in addition to base draft angle.
Office equipment (such as laptops) typically uses a texture depth of 0.025 mm (0.001 in), with a minimum recommended draft angle of 1.5°.
Coarser textures (such as leather, with a depth of 0.125 mm/0.005 in) require a larger draft angle, with a minimum recommended value of 7.5°.

Sharp corners can significantly increase stress concentrations, which can lead to part failure if stresses are too high. Sharp corners often appear in subtle locations, such as at junction of screw posts and walls or at the ends of ribs. Pay close attention to fillet radius of sharp corners—for a given wall thickness, stress concentration factor (SCF) varies with fillet radius.

 

Figure 13: Stress Concentration Factor (K) vs. Corner Radius/Wall Thickness Ratio (R/T) (X-axis: Corner Radius/Wall Thickness = R/T/Wall Thickness; Y-axis: Stress Concentration Factor (K); Curve shows that when R/T < 0.5, the SCF is higher; when R/T > 0.5, SCF is significantly lower.)
SCF is a multiple of amplified stress, so it is recommended that inside corner radius of a part be at least 1 times wall thickness.
In addition, fillets (rounded corners) provide a smooth flow path for molten plastic, making mold cavity easier to fill.
Recommended corner radius values for part corners:
Inside corner radius = 0.5 × wall thickness;
Outside corner radius = 1.5 × wall thickness;
If design allows, a larger corner radius should be used.

 

Figure 14: Recommended Corner Radius Design (Note: Sharp Corner - Raises Stress Concentration; Corner Radius - Minimizes Stress Concentration; Inner Corner Radius R = 1/2 × T, Outer Corner Radius R = 3/2 × T)

Inserts in plastic parts are used to secure fasteners (such as machine screws). Typically made of brass, inserts are strong, can withstand multiple assembly and disassembly cycles. There are three main methods for installing inserts in injection-molded parts:

 

Figure 15: Threaded Inserts (Note: Thread; Insert; Groove; Plastic; Knurl)

Insert is "vibrated" into part using "horn" (driven by an ultrasonic transducer) in an ultrasonic device. To ensure optimal results, a horn must be specifically designed for specific application.
Ultrasonic energy is converted into heat through vibration, melting insert into pre-opened hole in part. This process is fast, has a short cycle time, and produces low residual stress in part; however, it requires plastic to have good melt flow properties to ensure effective insertion.

Insert is heated using a heating tool (such as a soldering iron). Once insert melts plastic, it is pressed into pre-opened hole. As plastic cools and shrinks, it envelops and secures insert.
This process offers advantages of low tooling costs and simple operation. However, care must be taken to avoid overheating insert or plastic—overheating can lead to a loose fit and potentially plastic degradation.

Insert is directly embedded into part during injection molding cycle, secured by core pins. Molten plastic completely envelops insert, providing excellent retention.
This process may increase injection molding cycle (manual insert placement is required), but it eliminates secondary operations such as ultrasonic or thermal compression molding. For high-volume production, automated loading equipment can be used to place inserts, but this increases mold complexity and cost.

Living hinges are thin-walled plastic structures that connect two parts of a part, allowing them to remain connected, open and close. These hinges are commonly used in mass-produced containers, such as tool boxes and CD cases.

 

Figure 16: Box with a living hinge (labeled: Living Hinge)

Living hinges require highly flexible plastics, such as polypropylene (PP) or polyethylene (PE). A properly designed living hinge can typically withstand over one million opening and closing cycles without failure.

 

Figure 17: Design parameters for polypropylene and polyethylene living hinges (units: inches/mm).

When hollowing out thick-walled areas of a part is impractical and sink marks are unacceptable, gas-assist molding can be used to hollow out thick-walled areas. This process is suitable for nearly all thermoplastics, most conventional injection molding machines can be converted to gas-assist molding equipment.

 

Figure 18: Gas-Assist Molding Principle (Labels: Gas Channel; Thin Section; Gas Entrance; Gas Penetration; Well is Full; Overflow; Control Valve—closed for resin injection, open for gas injection)

Overmolding is a process in which a flexible material is injected onto a rigid substrate. If material is selected appropriately, flexible overmolding layer forms a strong bond with rigid substrate, achieving optimal bonding without use of adhesives.

Insert molding is the most widely used overmolding process: a preformed rigid substrate is placed in a mold, and a flexible material is injected directly onto substrate. This process has advantage of being able to use conventional single-shot injection molding machines.

Two-shot molding is a multi-material overmolding process that requires a specialized injection molding machine equipped with two or more barrels. This equipment can inject two or more materials into same mold during same injection cycle. Two-shot molding is typically used for high-volume production, exceeding 250,000 pieces per year.