This article provides practical design tips for injection molding to help mitigate common mistakes, improve product quality, and reduce costs by avoiding expensive mold changes and rework.
Overview of Injection Molding
Injection molding is one of the most cost-effective manufacturing process for producing high volumes of identical plastic parts. In this process, polymer pellets are first melted and then injected under pressure into a mold. Once the plastic cools and solidifies, the mold is opened, and the part is ejected. The cycle then repeats, often in as little as 15 to 60 seconds, depending on part size and mold complexity. In comparison, CNC machining or 3D printing might require minutes to hours to produce the same geometry.
This process offers high repeatability, tight tolerances, and excellent design flexibility. It is widely used in mass production projects all around you, including car dashboards, plastic containers, mobile phone housings, bottle caps, and even everyday toys. The main limitations are the high initial costs of mold design and manufacturing, as well as longer lead times—from initial design to production—which typically take at least four weeks.
Material Selection
Almost all thermoplastic materials can be injection molded, and some thermosets and liquid silicones are also compatible with the process. Additionally, their properties can be tailored by adding fillers and additives (e.g., glass and carbon fibers) or by blending different pellets (e.g., PC/ABS blends) to achieve the desired appearance and functionality. Below is an overview of commonly used injection molding materials:
Material
Characteristics
Polypropylene (PP)
Ultra‑low density and cost, excellent flow and chemical resistance; low stiffness and poor UV/oxidative durability.
Polyethylene (PE)
Chemical resistance, available in HDPE/LDPE for strength or flexibility; low rigidity and poor adhesion.
Polystyrene (PS)
Very rigid and dimensionally stable; easy to mold; brittle with low impact strength.
Acrylonitrile Butadiene Styrene (ABS)
Tough and impact resistant, good surface finish and moldability; moderate heat resistance, poor long term weatherability.
Acetal (POM)
High stiffness, low friction and water uptake, excellent dimensional stability; limited high temperature performance.
Acrylic (PMMA)
Optically crystal clear, UV/weather resistant, high rigidity; brittle and prone to stress cracking.
Nylon (PA)
Excellent toughness, wear and fatigue resistance, high strength; hygroscopic (moisture uptake) requiring drying and design compensation.
Polybutylene Terephthalate (PBT)
Strong, stiff with low moisture absorption and good electrical insulation; moderate shrinkage—needs proper gating.
Polycarbonate (PC)
High impact strength, natural transparency, wide temperature range; sensitive to stress cracking, needs uniform wall thickness.
Polyether Ether Ketone (PEEK)
Exceptional chemical/thermal resistance and mechanical strength; very expensive, requires specialized molding.
Thermoplastic Elastomer (TPE)
Rubber like flexibility and soft touch feel, good chemical/weather resistance; lower load bearing capacity.
Thermoplastic Polyurethane (TPU)
Outstanding abrasion resistance and elasticity, good load‑bearing; can stick in mold—needs optimized draft and release.
PC/ABS
Balanced toughness and heat resistance with easier moldability than PC and better stability than ABS; moderate chemical resistance.
Part Design Considerations
To ensure that parts are produced consistently, with minimal defects, and at the lowest possible cost, designers should follow some established guidelines. The following sections outline the key considerations when designing parts for injection molding:
Wall Thickness
Wall thickness affects the mechanical performance, overall cost, and appearance of your injection molded part. There are two wall thickness terms that designers need to understand:
Uniform Wall Thickness
Whenever possible, maintain a uniform wall thickness in your part. This promotes even cooling, resulting in more consistent shrinkage, and helps reduce stress concentrations, deformation, and other injection molding defects .
Uniform wall thickness does not necessarily mean that every wall must have exactly the same thickness. Rather, it emphasizes minimizing large variations between neighboring wall sections. Generally, the thickness of a wall should be no less than 40% to 60% of adjacent walls. When thickness variation is necessary for functional or structural reasons, transitions should be gradual—using chamfers or fillets with a length at least 3 times the difference in thickness—to avoid abrupt changes in flow or cooling that could lead to part failure.
Nominal Wall Thickness
Nominal wall thickness refers to the target or average thickness of a part, and it serves as the starting point for design. A proper wall thickness helps ensure sufficient part strength and reducing material waste. It also lays the foundation for mold design, processing parameters, equipment setup, and material selection.
Walls that are too thick increase the risk of shrinkage and deformation. They also require more material and longer cycle times，driving up production costs. On the other hand, walls that are too thin may can solidify too quickly or trap air, leading to short shots—defects caused by incomplete mold filling.
To avoid these issues, always keep wall thickness within the recommended range for your chosen material. Below is a list of the recommended wall thicknesses for common plastic resins:
Material
Recommend Wall Thickness（in）
Recommend Wall Thickness（mm）
Acetal (POM)
0.030–0.120
0.76–3.05
Acrylic (PMMA)
0.025–0.500
0.64–12.70
Acrylonitrile butadienestyrene (ABS)
0.045–0.140
1.14–3.56
Nylon (PA)
0.030–0.115
0.76–2.92
Polybutylene Terephthalate(PBT)
0.080-0.250
2.032-6.350
Polycarbonate (PC)
0.040–0.150
1.02–3.81
Polyether Ether Ketone (PEEK)
0.020-0.200
0.508-5.080
Polyetherimide (PEI)
0.080-0.120
2.032-3.048
Polyethylene (PE)
0.030–0.200
0.76–5.08
Polyphenylsulphone (PPSU)
0.030-0.250
0.762-6.350
Polypropylene (PP)
0.035–0.150
0.89–3.81
Polystyrene (PS)
0.035–0.150
0.89–3.81
Thermoplastic Elastomer(TPE)
0.025–0.125
0.64–3.18
Thermoplastic Polyurethane (TPU)
0.025–0.125
0.64–3.18
Corners
Sharp corners tend to concentrate stress, make demolding more difficult, and accelerate wear on the mold surface. Material can accumulate or cool unevenly at these sharp transitions, resulting in flow lines or other defects. In addition, sharp corners often require the use of EDM (electrical discharge machining) to form the mold, which raises tooling costs.
The best practice is to use rounded corners. General design guidelines are as follows:
▪ Use an internal radius of at least 50% of the wall thickness (minimum 25% if space is limited). ▪ Make the external radius equal to the internal radius plus the wall thickness. ▪ The internal and external corner radii share the same center point.
Parting Line
The parting line is the seam formed where the two halves of the mold meet. It typically appears on the surface of the molded part and is an unavoidable feature in injection molding. The placement of the parting line affects mold complexity, production efficiency, and the final appearance or functionality of the part.
An intuitive idea might be to place the parting line straight down the middle of the part. But this is not always possible—or even practical. In reality, the parting line should be positioned strategically to balance visual appeal, function, and mold complexity. For example:
Hide the parting line in less visible areas. A good example is the LEGO brick, where the parting line is subtly concealed along the underside rather than the top face, ensuring the most visible surfaces remain flawless.
Avoid placing the parting line on critical functional areas, such as sealing surfaces, mating holes, or threaded inserts. The presence of a parting line in these regions can cause slight dimensional variations, flash, or poor fit.
Avoid positioning the parting line on fillets or curved surfaces. These features require higher mold precision, which increases manufacturing costs and may lead to incomplete mold closure, resulting in flash or other defects. Instead, You should place the parting line along natural split lines (e.g., sharp edges, steps, or break lines) to simplify mold construction, improve demolding efficiency, and reduce tooling and maintenance costs.
For more complex geometries, designers may need to introduce irregular parting lines or even incorporate side actions to accommodate undercuts or hidden features.
Draft
Draft is the angle applied to vertical surfaces of an injection-molded part to allow for smooth ejection from the mold. Without adequate draft, the part would tightly contact the mold surface, risking excessive force during ejection. This can lower part quality, lead to scrap parts, and may even result in damage to the tooling.
Many CAD software programs make it easy to add draft angles, but it’s best to apply them in the final stages of the design to prevent unnecessary complexity. When determining the appropriate draft angle, following factors must be considered:
Material
Different plastics have different flow characteristics, which affect the required draft angle. Materials like polypropylene (PP), polyethylene (PE), and polystyrene (PS) generally have good flow properties and low viscosity. For these materials, a draft angle of 1°to 3°is typically sufficient. In contrast, thermosetting plastics like epoxy and phenolic resins often require larger draft angles (3°or more) to ensure smooth ejection.
Surface Finish
Draft is related to the surface texture and smoothness of your injection molded parts. Smoother finishes require less draft, while heavier textures require more. For example:
▪ For smooth finish, a draft angle of about 1–2°is generally sufficient. ▪ For parts with light or moderate textures, a draft angle of 3–5°is usually required. ▪ For heavy textures, a draft angle of at least 5°is needed. ▪ A general rule of thumb is to add 1.5°of draft for every 0.001" (0.025 mm) of texture depth.
During injection molding, the texture from the mold is transferred to the part’s surface. The type of product you are designing will influence your choice of mold finish. Industry organizations such as the Society of the Plastics Industry (SPI) and the Society of German Engineers (VDI), as well as companies like Mold-Tech (MT) and Yick Sang (YS), have established standardized classifications for polished and textured mold finishes. These standards help guide the selection of proper draft angles based on surface finish requirements.
The surface finish chart below lists the recommended draft angles for the most common finishes.
SPI Standard
Draft (°)
Mold Tech Texture
Draft (°)
A-1
0.5
MT-11000
1.0
A-2
0.5
MT-11010
1.5
A-3
0.5
MT-11020
2.5
B-1
1.0
MT-11030
3.0
B-2
1.0
VDI Texture-PC
B-3
1.0
VDI-18
1.0
C-1
1.5
VDI-24
1.5
C-2
1.5
VDI-33
3.0
C-3
1.5
YS Texture
D-1
2.0
YS 1xx
1.0
D-2
2.5
YS 3xx
4.0 – 5.5
D-3
3.0
YS 5xx
6.0– 12.0
Mold Construction
Set your draft angles with the way the mold opens—the mold’s “draw” direction. Otherwise, the part can stick to the half that holds the ejector pins and won’t release properly. In addition, be sure to apply draft not only to all vertical walls but also to any features like holes or bosses.
For example, imagine a rectangular part with four through holes. If the holes are drafted toward the cavity, the part may remain stuck there after molding. Instead, drafting them toward the core side—where the ejector system lives—so the pins can push the part out cleanly.
Ribs and Gussets
Ribs and gussets are both used to reinforce localized structures and improve part stiffness without increasing the overall wall thickness.
Ribs
Ribs are slender, wall like protrusions that extend from a part’s surface—often across broad, thin walled areas or inside box shaped features—to distribute loads evenly and improve overall stiffness. To ensure effective rib design, follow these best practices:
▪ Rib thickness should be 40–60% of the main wall thickness. ▪ Rib height should not exceed three times the wall thickness. ▪ Apply a draft angle of 0.5°–1° to aid mold release. ▪ Add a fillet at the rib base with a radius of 0.25–0.5× the wall thickness. ▪ Space each rib at least four times its own thickness from nearby vertical features (other ribs, bosses, or hole edges) to provide extra cooling room and prevent hot spots.
Gussets
Gussets are small triangular or trapezoidal plates placed at the junction of walls, bosses, or ribs to strengthen local high stress points. Best practices for gusset design include:
▪ The gusset should usually be about one-third to one-half as thick as the wall it’s supporting. ▪ A gusset should never be taller than the boss or rib it’s reinforcing. In fact, you often only need the gusset to be about 30–50% of the height of that boss, which is enough to provide support in most cases. ▪ Apply a draft of 0.5°to 1°to ensure smooth ejection. ▪ Use generous fillets at the gusset base to reduce stress concentration and improve plastic flow; a radius of 0.25 to 0.5 times wall thickness is generally appropriate. ▪ Place gussets symmetrically when used in pairs and avoid overcrowding. ▪ Maintain a gap of at least 2 to 3 times the gusset thickness from adjacent features to ensure uniform cooling and prevent molding defects.
Bosses
Bosses are cylindrical features designed to receive inserts, self-tapping screws, or pins for assembly or mounting. It can be also viewed as circular ribs that contribute to the overall structural strength. Freestanding bosses should be avoided. Always connect them to adjacent walls or surfaces using ribs or gussets rather than being fully integrated into the wall itself.
When designing bosses, remember the following:
▪ Place bosses where structural integrity or fastening strength is needed ,such as at screw locations. ▪ For self tapping screws, size the boss OD to about 2–2.5× the screw’s major diameter. ▪ Limit boss wall thickness to ≤ 60% of the adjoining wall to avoid sink marks or voids. ▪ Add a fillet at the boss base to improve melt flow and reduce stress concentration. ▪ Oversize the hole diameter slightly to compensate for plastic shrinkage and ensure a proper fit after molding.
Undercuts
Undercuts are recessed or overhanging features that create an interlock between the part and one or both mold halves, preventing clean ejection along the mold opening direction. Common examples include hooks, snap-fits, holes, grooves, and side slots that are perpendicular or transverse to the mold’s parting direction.
While undercuts are sometimes necessary for mechanical function or assembly fit, they typically require additional tooling—such as sliding cores, lifters, or cams—which increase mold complexity, cycle time, and manufacturing cost. Improperly designed undercuts can cause ejection difficulties, part distortion, excessive wear, or tool failure.
Some design guidelines for undercuts are as follows:
▪ Avoid undercuts whenever possible by modifying the geometry, reorienting the part, or shifting the parting line so that features align with the mold’s pull direction and eliminate recesses. ▪Use bump offs or flexible zones for shallow undercuts in soft, non reinforced materials—ideally high elasticity thermoplastics (e.g. TPE/TPU grades or specialty nylon elastomers). Avoid PP/PE unless the undercut height is ≤ 0.3 mm with very thin walls. Provide a 30°–45° lead in chamfer and add 0.5°–1° draft on the bump off face to ensure smooth ejection. ▪ If undercuts are necessary, keep them minimal, localized, and placed on a single side to reduce the need for multiple side actions. ▪ Incorporate proper draft angles (typically ≥1°) and generous radii around undercut features to ease ejection and reduce stress on both the part and the mold.
Text & Symbols
Text and symbols (e.g., part numbers, logos, recycling marks) are commonly embossed or debossed on molded parts for traceability, branding, or regulatory compliance. Here are some helpful tips:
▪ Use raised (embossed) text rather than recessed (engraved) when possible, as engraved text requires more complex mold tooling, accelerates tool wear, and increases cost—especially for high volumes or intricate designs. ▪ Consider embossed text with a height of 0.5 mm. ▪ Choose simple sans-serif fonts (e.g., Arial, Helvetica) to improve readability, ensure consistent plastic flow, and reduce tool wear. ▪ Use a uniform stroke thickness and a minimum font size of 20 points (approximately 7 mm in height). ▪ Avoid placing text near thin walls, sharp corners, ribs, or high-cosmetic surfaces, as these areas are more prone to defects, sink marks, or ejection issues. ▪ Orient text perpendicularly to the parting line or in the mold’s draw direction to simplify machining and prevent distortion during ejection.
Tolerances
Injection molding tolerance defines the allowable deviation of a part’s dimensions from its nominal design. In design, tighter tolerances should be applied to critical features, such as assembly interfaces, sealing grooves, and locating holes, as these directly impact fit and functionality. For non-critical dimensions, such as the width of non-load-bearing surfaces, looser tolerances can be used to reduce manufacturing costs.
There are two common tolerance levels:
Commercial tolerances: Relatively loose (typically ±0.1 mm or ±0.004"), and work well for most non critical features at a lower cost.
Fine tolerances: Tighter (typically ±0.05 mm or ±0.002"), required for high-accuracy parts, with higher tooling and manufacturing cost.
During design, dimensional tolerances must be adjusted according to material shrinkage. Different plastics have different shrinkage rates—semi crystalline materials (e.g., PA, PP, PE, POM) shrink more than amorphous materials (e.g., ABS, PC, PMMA). Although shrinkage is generally predictable, slight variations in resin formulation or processing conditions (like melt temperature) can influence the final part size. As part size increases, shrinkage variation becomes more pronounced. Depending on the material, you should expect a shrinkage‐related tolerance of roughly ±0.002 in/in (0.05 mm/mm).
Tolerance stack up analysis must also be considered in multi part assemblies, because even if each individual feature (e.g., a hole) is within its specified tolerance, cumulative variation can lead to misalignment—especially when multiple holes across different parts need to align for fasteners to pass through.
Note that mold tolerances also influence final part quality. Standard mold machining tolerances are around ±0.005" (0.13 mm), but tighter tolerances may be required for high precision parts. Additionally, molds experience wear over time, which can lead to dimensional drift. It’s important to plan for tool maintenance and refurbishment to maintain consistent part quality during long term production runs.
Mold Design Basics
Part design and mold design are closely linked in determining the success of an injection molded product. As part design focuses on geometry and functionality, mold design translates those requirements into a manufacturable tool. The following section outlines the fundamental aspects of mold design:
Mold Base and Cavity Layout
The mold tooling consists of a standard mold base, cavity and core inserts, and any moving components (slides, lifters, ejector plates, etc.). The mold base provides the rigid framework—holding guide pillars, support plates, and the ejection system—while the cavity and core inserts define the part’s shape. Together, they control how precisely and consistently each part is molded.
A good mold design should:
▪ Use a standard base (e.g., DME or HASCO) for cost effective sourcing and easy replacement of worn components. ▪ Maintain proper plate thickness and guide pillar size to withstand injection pressure and ensure alignment. ▪ Lay out cavities and cores for easy access—inserts should be removable for cleaning, maintenance, or replacement without dismantling the entire mold. ▪ Balance cooling channels around each cavity to keep temperature uniform and minimize warping or shrinkage variation. ▪ Include adequate draft and ejection space so parts release cleanly and cycle times stay short. ▪ For new products, a single cavity mold is often the fastest and most cost effective way to validate the design. Once the design is finalized, you can move to multi cavity or family molds to scale up production.
Gates
Gates are the entry points through which molten plastic flows into the mold cavity. Their size, shape, and placement have a great impact on part appearance, structural strength, and the presence of molding defects such as flow marks and weld lines.
▪ Larger parts need larger gates to maintain pressure and flow rate for complete filling. ▪ Position gates at the part’s thickest section to promote uniform fill, control shrinkage, and minimize defects. ▪ Place gates in low stress, low visibility areas whenever possible, since they leave small vestiges and can weaken the part. ▪ Use multiple gates on large or complex parts to balance flow and prevent short shots. ▪ Since gates leave a small vestige, locate them on the parting line for easy trimming and minimal visibility.
Gates can be categorized by trimming method—manual or automatic—and certain types are better suited to specific part geometries. Below picture shows the common examples of the gates.
Manual Gate Types
▪ Edge Gate (Standard Gate): Rectangular cross section along the parting line; ideal for flat or rectangular parts; can be tapered for better flow. ▪ Fan Gate: Wide, flared opening for large or thin walled parts; minimizes shear and improves filling balance. ▪ Tab Gate: Edge gate variant with a small tab to absorb shear and heat; suited for shear sensitive materials. ▪ Diaphragm Gate: Circular gate around the core for concentric flow; excellent balance but difficult and costly to trim. ▪ Ring Gate: Continuous ring around the core for even radial filling; used in tube shaped parts. ▪ Spoke Gate: Ring gate variant with radial ribs; good for symmetrical tubular parts but maintaining concentricity is challenging. ▪ Film (Flash) Gate: Very thin, wide gate for large/thin parts; ensures uniform fill but leaves a long vestige that needs manual trimming.
Automatically Gates Types
▪ Submarine (Tunnel) Gate: Angled entry below the parting line; auto breaks during ejection for minimal blemish. ▪ Pinpoint Gate: Small, direct gate inside the parting line; ideal for high flow materials and cosmetic parts; common in multi cavity or precision molds.
Runner System
The runner system guides molten plastic from the sprue to the gates and into the mold cavities. The runner design impacts material flow, cycle time, and part quality—especially in multi-cavity or family molds. An efficient runner system ensures that molten plastic flows evenly to all cavities. Balanced flow prevents defects such as dimensional variation, short shots, and weld lines. Uneven distribution can also cause localized overheating or underfilling, which affects both strength and surface finish.
The shape and size of the runner channel directly impact flow behavior and processing efficiency. Full-round runners reduce pressure loss but increase tooling complexity, while trapezoidal or semi-circular runners are easier to machine but less efficient. Oversized runners waste material and slow cooling; undersized ones restrict flow and may cause incomplete fill. In multi-cavity molds, runners should be symmetrical and evenly distributed to ensure each cavity fills simultaneously.
There are two main types of runner systems:
Cold runners are simpler and cost-effective, but they generate excess material (runner scrap) that must be removed or recycled.
Hot runners eliminate this waste and offer better control over flow and temperature, but they require higher tooling cost and maintenance effort.
The runner system must be designed in coordination with the gate and cooling systems. A well-optimized layout reduces cycle time, improves consistency, and supports efficient, high-quality molding.
Ejector Pins
Ejector pins are used to push the molded part out of the cavity once it has solidified. Their placement and design significantly affect part quality, ejection efficiency, and mold life. Design recommendations are:
▪ Position ejector pins on non-cosmetic surfaces, such as near the parting line. ▪ Avoid placing pins on thin-walled or angled areas that may deform under ejection force. ▪ Locate pins in mechanically strong areas of the part to ensure it remains intact during ejection. ▪ Material choice matters—sticky resins may require more ejection force, while softer plastics benefit from larger or more numerous ejector pins to spread the load and prevent deformation. ▪ The number and type of pins depend on factors such as part geometry, draft angles, and wall thickness. For instance, parts with edge or fan gates may need additional pins for balanced ejection. ▪ Ejector pins must be made of high-strength, wear-resistant materials to ensure long-term durability.
Cooling System
The cooling system maintains mold temperature to control shrinkage, cycle time, and final part quality. Channels should be routed for uniform cooling, with tighter spacing (3–5 mm from the cavity) around thick sections. Ensure cooling lines do not conflict with gates, runners, or ejection hardware. Proper channel diameter (typically 6–10 mm) and balanced manifolds further improve thermal consistency and shorten cycle times.
Work with Chiggo for Expert and Prototype DFM Feedback
Now that you have a clearer understanding of how injection molding design impacts manufacturability, performance, and cost, it's time to move forward. Once your design is ready, Chiggo offers a free DFM (Design for Manufacturability) analysis along with your request for quote. This analysis helps identify potential issues or risks related to mold making and injection molding.
What’s next? Creating a prototype can help validate your design decisions before tooling begins. Chiggo is here to guide you through each step of the injection molding journey, ensuring a smooth transition from design to production.
