Injection molding is a manufacturing method that creates parts by injecting material into a mold. It is a type of plastics processing technology.
In this process, plastic is placed into a hopper, which then injects heated plastic. Plastic is pushed through a long chamber and a reciprocating screw. It softens into a fluid state. A nozzle at the end of chamber forces fluid plastic through nozzle to cool, closing mold. When plastic cools and solidifies, semi-finished product is ejected from press.

 

This section begins to introduce design guidelines for injection molded parts. Following figure is a simple mind map created by author. Save as to see a clearer image.

 

Understand principles of injection molding and design parts suitable for injection molding.
After much consideration, author believes this point may be the first one to be explained to beginners or those outside industry. Those with limited experience in metalworking need to specifically understand what injection molding is, as shown in diagrams in Section 2 above. Don't use machining methods to make plastic parts, and don't deliberately challenge limits of injection molding to create parts that are impossible to manufacture.
As shown in diagram below:

 

Mechanical Design Handbook - Metal Cutting: Enlarge or rough-turn the center portion to reduce machining or finish turning length. However, if part is an injection molded part, a central depression will hinder demolding and may be less effective than a straight through hole.
Design requirements for metal cutting and injection molding are different!
Some may consider this innovation and force suppliers to manufacture it. However, if you can afford this process, others can too, and competitors could easily copy it, which is more costly than good.
From author's perspective: Designing an injection molded part is like designing a shell that can be demolded.
First, part must be demoldable, so it must conform to demolding motion and have a draft angle.

When plastic material transitions from a molten state to a solid state, it undergoes a certain amount of dimensional shrinkage. This causes part to shrink and tighten around punch and core. To facilitate smooth demolding of plastic part from mold and prevent scratches on part surface during demolding, part surface parallel to demolding direction should generally have a reasonable draft angle, as shown in Figure 3-27.

 

Figure 3-27 Draft Angle
Factors that determine draft angle are as follows:
1) Unless part has special requirements, draft angle is generally 1° to 2°.
//This is just a general guideline; see figure below for details and then consider specific design.
Table 2-7-26. Recommended Demolding Angles for Different Surfaces

Table 2-7-27 Recommended Demolding Angles for Different Plastics

2) For plastic parts with high shrinkage, a larger draft angle should be used.
3) For part features requiring high dimensional accuracy, a smaller draft angle should be used.
4) Draft angle on punch side is generally smaller than draft angle on die side to facilitate part demolding.
5) Thicker plastic parts experience increased molding shrinkage, so draft angle should be larger.
6) Draft angle for textured and complex surfaces should be large, with size of texture determining draft angle.
7) For glass fiber reinforced plastics, draft angle should be large.
8) Size and direction of draft angle should not affect product's functionality.
For example, when two parts have a kinematic relationship, draft angle at mating point must be considered, as this will affect product's functionality.
Example: Cross-sectional diagram of button and panel on an electrical appliance is shown in Figure 3-28. Button's function is to activate appliance. Optimal design direction for this diagram is to have same draft angle for panel and button.

 

Figure 3-28 Design of demoulding slope considering motion relationship of parts
9) Some surface areas of a part may not require a draft angle due to functional requirements, but this will require a side core pull design, which will complicate mold structure and increase costs.
10) Draft angle should be as large as possible, provided part's function and appearance allow.
A smaller draft angle increases likelihood of surface scratches and damage during ejection. Furthermore, a smaller draft angle requires mold surface polishing or a complex ejection mechanism, increasing mold costs.
//Part draft angles are typically 0.5° for internal surfaces, 1° for external surfaces, and 3° for surface textures. This is not recommended, but it can be used as a reference.
//Regarding draft angles, it is best for structural engineers to draw draft angles for all part surfaces themselves. For uncertain surfaces, a draft angle of 0.5° should be used, then negotiated with mold manufacturer. Less desirable is drawing draft angles for surface textures and critical structures themselves, then negotiating with mold manufacturer. Therefore, structural design often becomes a matter of verbal negotiation.

Snap-fit structures are a common assembly method for plastic parts, formed by a side-pull mechanism using inclined pins (or sliders) in mold. Inclined pin (or slider) has a travel distance to withdraw from the latch during part demolding. Part design must provide sufficient space for inclined pin (or slider) to withdraw. Otherwise, inclined pin (or slider) may not withdraw or may interfere with other features on part (such as pillars) during withdrawal, as shown in Figure 3-71.

 

Figure 3-71 Inclined pin should have enough space to exit

In plastic parts, if two features are very close together, corresponding area on mold will be a thin piece of iron, as shown in Figure 3-72. This can easily lead to low mold strength and a short lifespan. Therefore, thin iron and low-strength mold designs should be avoided.

 

Figure 3-72 Avoiding thin iron and low mold strength

In plastic part design, part wall thickness is primary parameter to consider. Part wall thickness determines part's mechanical properties, appearance, injectability, and cost. It can be said that selection and design of part wall thickness can determine success or failure of a part design.

Due to properties of plastic materials and specificities of injection molding process, wall thickness of plastic parts must be within an appropriate range, neither too thin nor too thick.
If wall thickness is too thin, flow resistance during injection is high, making it difficult for molten plastic to fill the entire mold cavity. This necessitates the use of higher-performance injection molding equipment to achieve higher filling speeds and injection pressures.
If wall thickness is too thick, part cooling time increases (statistically, a doubling of part wall thickness increases cooling time by four times), part molding cycle increases, and part production efficiency decreases. Furthermore, excessive wall thickness can easily lead to quality issues such as shrinkage, porosity, and warpage.
Different plastic materials have different requirements for appropriate wall thickness of plastic parts, and even same plastic material produced by different plastic material manufacturers may have different requirements for appropriate wall thickness. Appropriate wall thickness ranges for parts made of commonly used plastic materials are shown in Table 3-7. If wall thickness of a plastic part approaches upper and lower limits of appropriate wall thickness values in table, product design engineer should seek advice from plastic material manufacturer.
Table 3-7 Suitable Wall Thickness Ranges for Common Plastic Parts (Unit: mm)

Table 6-3 Wall Thickness Selection for Plastic Parts

Table 1-9-2 Wall thickness of thermoplastic parts (recommended value) mm

Note: Minimum wall thickness value may vary with forming conditions.
//Since I've been working in furniture industry, this wall thickness information is truly only a reference. Average thickness of many chair plastic armrests (made of PP) is over 5mm. Therefore, wall thickness is a crucial know-how for injection molded parts and a comprehensive reflection of a company's manufacturing capabilities. This includes factors such as structure, material, mold, and injection molding parameters. This requires regular observation and statistical analysis. Because a company's manufacturing capabilities don't improve in leaps and bounds, wall thickness can be used as a reference for parts with same structure and material.

Key factors determining plastic part wall thickness include:
1) Whether part's structural strength is sufficient. Generally speaking, thicker walls increase part strength. However, if part wall thickness exceeds a certain range, increasing wall thickness can actually reduce part strength due to quality issues such as shrinkage and porosity.
2) Whether part can withstand ejection force during molding. Parts that are too thin are prone to deformation due to ejection.
3) Whether it can withstand tightening force during assembly.
4) If there are metal inserts, whether surrounding area of insert is strong enough. Generally, metal inserts and surrounding plastic material shrink unevenly, which can easily lead to stress concentration and reduced strength.
5) Can part evenly distribute impact force it is subjected to?
6) Is hole strong enough? Hole strength can be easily reduced by weld marks.
7) Assuming above requirements are met and injection molding does not cause quality issues, wall thickness of plastic part should be minimized. Thicker wall thickness not only increases material cost and part weight, but also prolongs molding cycle, thereby increasing production costs.
Figure 3-19 shows relationship between wall thickness and cooling time for a certain ABS plastic part.

 

Figure 3-19 Relationship between part wall thickness and cooling time
To ensure and improve part strength, product design engineers often tend to choose thicker wall thicknesses.
In fact, choosing thicker wall thicknesses to ensure and improve part strength is not the best approach. Increasing part strength can be achieved by adding reinforcing ribs, designing curved or wavy cross-sections, etc. This not only reduces material waste but also shortens injection molding cycle.

Ideal part wall thickness distribution is uniform thickness across all cross-sections. Uneven wall thickness can cause uneven cooling and shrinkage, leading to defects such as surface shrinkage, internal pores, warping, and difficulty maintaining dimensional accuracy.

 

Figure 3-20 Parts with uniform wall thickness
Figure 3-20 shows an example of a common plastic part with uniform wall thickness.
If uniform wall thickness is not possible, at least ensure a smooth transition between thick and thin areas to avoid abrupt changes in wall thickness. Sharp changes in wall thickness can affect flow of plastic melt and easily create stress marks on the back of plastic, affecting product's appearance. They can also lead to stress concentration, reducing strength of plastic part and making it difficult for part to withstand loads or external impacts.
Figure 3-21 shows four examples of wall thickness design for uneven wall thickness.
The worst wall thickness design, shown in Figure 3-21a, exhibits a sharp change in wall thickness.
The best wall thickness designs, shown in Figures 3-21b and 3-21c, show a smooth transition between thick and thin parts. Generally, length of transition zone is three times thickness.
The best wall thickness design, shown in Figure 3-21d, not only achieves a smooth transition but also incorporates a hollowing design where wall thickness is thick, preventing shrinkage while maintaining part strength.

 

Figure 3-21 Smooth transition of uneven wall thickness of parts

Software's wall thickness analysis function can be used to more clearly visualize wall thickness of plastic parts.

 

Sharp corners should be avoided on both inside and outside of plastic parts. Sharp corners can hinder flow of molten plastic and easily cause cosmetic defects. They also easily cause stress concentration, reducing part strength and potentially leading to failure under load. Therefore, sharp corners should be rounded to achieve a smooth transition.
Therefore, structural engineers should try to add rounded corners to 3D models. 3D drawings are used when opening molds for plastic parts.

Figure 3-22 shows design of rounded corners on the outside of plastic parts.

 

Figure 3-22 Avoiding external sharp corners
Of course, avoiding sharp corners on the outside of parts is not a one-size-fits-all approach. Rounded corners at parting surface complicate mold structure, increasing mold cost, and can easily cause part discontinuity, affecting appearance. A right-angle design at parting surface is preferred, as shown in Figure 3-22.

 

Figure 3-23 Avoiding rounded corners on parting surface
If a flat surface approximately 1.5 meters long is added at joint, flash and gate can be easily removed during removal process, as shown in Figure 5-18. (This precaution is generally not required for injection molded parts.)

 

Figure 5-18 Avoid sharp angles between part walls and parting surfaces

Avoid sharp corners in direction of plastic melt flow, as shown in Figure 3-24. Arrow in figure indicates direction of plastic melt flow. In original design, sharp corners can easily trap air during injection process, leading to localized high temperatures that can cause plastic decomposition and cosmetic defects on part surface. Sharp corners can also easily generate internal stress. In improved design, design optimization avoids sharp corners to ensure smooth flow of molten plastic.

 

Figure 3-24 Avoiding sharp corners in direction of plastic melt

Stress concentration is one of main causes of plastic part failure. Stress concentration reduces part strength, making it more susceptible to failure under impact and fatigue loads.
Stress concentration often occurs at sharp corners. Sharp corners should be avoided in plastic part designs. Fillets should be added to reduce and prevent stress concentration. Sharp corners are most common at junctions between main wall and side walls, between wall and ribs, between wall and support.
Relationship between internal fillet and stress concentration factor is shown in Figure 3-25. Where T is part wall thickness, R is internal fillet, and p is load applied to part.

 

Figure 3-25 Stress concentration factor of parts
As shown in Figure 3-25, when R < 0.3T, stress increases dramatically; when R > 0.8T, stress concentration virtually disappears.
Generally speaking, R of internal fillet at joints of part sections is 0.5T, and external fillet is 1.5T. This ensures uniform wall thickness and reduces stress concentration at joints, as shown in Figure 3-26. Of course, fillet should not be too large, otherwise it can easily lead to excessive wall thickness in some areas of part, causing shrinkage.

 

Figure 3-26 Rounded corner design

In mold processing, electrical discharge machining is a commonly used machining method, especially for complex curved surfaces. This machining method requires use of electrodes.
Sharp corners, edges, and other raised areas of electrode wear faster during EDM than flat areas.
For this reason, some responsible mold engineers will require part designs with filleted corners, or else they will add a minimum fillet of 0.2 to their plastic molds.

This is just my summary and suggestions.
Filling plastic corners isn't always a one-shot process. It's recommended to adhere to following guidelines.
2.3.5.1 Filleting Plastic Parts at Last Step
According to national standard GB26099, filleting is performed as shown below:

 

2.3.5.2 Fillet all edges of plastic part model. Generally, a fillet value of R0.5 is recommended for the first fillet.
As mentioned above, since external sharp corners, flow direction areas, and joints all require fillets, the entire plastic model needs fillets. Therefore, I recommend filleting all edges of plastic model. Fillets at parting lines can be removed later by mold engineer.
Filletizing Procedure: Generally, important edges are rounded first, followed by less important edges, and finally, remaining edges are rounded with face fillets. Use face fillets sparingly, as they are difficult to control and modify.
Fillet fillets can be applied multiple times using edge fillets. Avoid applying fillets all at once, as this also makes them difficult to control and modify.
2.3.5.3 Following the principle of (avoiding sharp corners), modify corner radius to achieve optimal results. Of course, some unique, immediately visible corners can be directly radiused to values such as R1.

Strength of plastic parts is always a concern for product design engineers. Compared to metal parts, plastic parts are generally weaker in strength. However, through proper part design, their strength can be significantly improved, thereby expanding their application range.

Increasing wall thickness can be a method of increasing part strength during part design, but this is often unreasonable. Increasing part wall thickness not only increases part weight but also makes it more susceptible to defects such as shrinkage and bubbles. It also increases injection molding time and reduces production efficiency. To improve part strength, correct approach is to add reinforcing ribs rather than increasing wall thickness. Adding ribs not only increases part strength but also prevents defects such as shrinkage and bubbles, as well as lowering production efficiency. Of course, when designing ribs, relevant dimensions must adhere to rib design principles. Excessively thick ribs can also cause defects such as part shrinkage and bubbles.
Figure 3-45 shows two methods for doubling part strength. One is to increase wall thickness, and the other is to maintain wall thickness and add ribs. To achieve a doubling of part strength, increasing wall thickness requires a 25% increase in part volume, while adding ribs only requires a 7% increase. Therefore, adding ribs is the best method for increasing part strength.

 

Figure 3-45 Comparison of methods for doubling part strength
Figure 3-46 shows how to increase strength of a seat by adding ribs.

 

Figure 3-46 Improving strength of seat by adding reinforcement ribs
//Note: Ribs can reduce overall part deformation, but their addition will cause surface shrinkage, affecting appearance. Therefore, when appearance of a part is of utmost importance, consider thickening part rather than adding ribs.

It is important to note that ribs only enhance strength of a plastic part in one direction. Direction of ribs must be considered when designing load; otherwise, ribs will not increase part's ability to resist load, as shown in Figure 3-47.

 

Figure 3-47 Direction of reinforcement needs to take load direction into consideration
If part is subjected to multi-directional loads or torsional loads, consider adding X-shaped or divergent ribs to improve part strength, as shown in Figure 3-48. In everyday life, backs of plastic stools often feature X-shaped or divergent ribs to enhance part strength.

 

Figure 3-48 X-shaped reinforcement and divergent reinforcement

Multiple ribs are more effective in improving part strength than a single thicker or taller rib. They also avoid quality issues such as surface shrinkage or incomplete injection at rib tip. Therefore, if a single rib is too tall or too thick, two smaller ribs of equal height and thickness can be used as a replacement, as shown in Figure 3-49.

 

Figure 3-49 Using multiple ribs instead of a single thicker or taller rib

Strength of plastic parts can be improved by designing shape of part reinforcement profile. Common reinforcement profiles include rounded, zigzag, and arc-shaped, as shown in Figure 3-50. Disadvantage of this method is that part does not provide a flat surface, making it unusable in some cases.

 

Figure 3-50 Common parts reinforcement section

Avoid designing flat plastic parts, as flat plastic parts have very low strength. This can be improved by adding sidewalls around perimeter, as shown in Figure 3-51.

 

Figure 3-51 Adding side walls to improve part strength
Sidewalls can be simple straight walls. When conditions permit, curved sidewalls or those with reinforced cross-sections can further improve part strength, as shown in Figure 3-52.

 

Figure 3-52 Common parts side wall reinforcement shapes
Figure 3-53 shows an example of a box design with curved sidewalls.

 

Figure 3-53 Curved side wall box design
Figure 3-54 shows an example of improving box strength through use of corrugated structures.

 

Figure 3-54 Corrugated box design

Part stress concentration often occurs at sharp corners, locations with sharp changes in wall thickness, in holes, slots, and metal inserts. Stress concentration can significantly reduce part strength and can lead to failure under impact loads. Part design should avoid stress concentration. To prevent stress concentration in parts, part design should strictly adhere to design guidelines in preceding sections.

During injection molding process, molten plastic flows in two or more directions when passing through holes, slots, pillars, and large areas of part, or when multiple gates are used. When plastic flows from these two directions meet, a weld mark forms in this area.
Weld mark area is one of areas with the lowest strength and is most susceptible to failure. Therefore, location and number of gates must be appropriately positioned to prevent part from bearing load in weld mark area. As shown in Figure 3-55, in original design, gate position places weld mark exactly where part is subjected to load, making part susceptible to failure under load. In improved design, gate position is adjusted to avoid weld mark in this area, significantly enhancing reliability of part.

 

Figure 3-55 Reasonable gate placement to prevent parts from bearing loads in weld mark area
Location of weld lines can be predicted using mold flow analysis software such as Mold Flow. Product design engineers can request mold suppliers provide mold flow analysis reports when creating a part, allowing them to optimally select gate locations and quantity.
//Presence of weld lines can easily cause a product to fail strength testing. During actual injection molding, molder can be asked to partially fill mold to observe weld line's location in production and determine whether structural modifications are necessary.

1) Glass fiber reinforced plastics are often used to replace ordinary plastics to improve strength of plastic parts. It's important to note that glass fiber reinforced plastics only improve part strength in direction of glass fibers.
//This is difficult to say. For example, a high GF content in PP increases material strength, but also makes it more brittle and prone to fracture. Strength materials are prone to deformation but not fracture. Deformation alone is often considered a passing test.
2) Plastic parts are more capable of withstanding compressive loads than tensile loads.
//Please refer to material physical property inspection and property table.
3) When subjected to tensile loads, design consistent part cross-sections to evenly distribute load.
4) Avoid circumferential loads on parts. Parts (such as metal inserts) subjected to circumferential loads are prone to cracking and failure.
5) When subjected to impact loads, maintain integrity of part cross-section to avoid notches and stress concentrations in direction of impact load.

In today's increasingly competitive market, product appearance has become a key factor in attracting consumers. Due to characteristics of plastic materials and injection molding process, plastic parts are prone to appearance defects such as shrinkage, bubbles, weld marks, air entrapment, and jet flow, which seriously affect part's appearance quality. Appearance quality issues in plastic parts primarily stem from problems with part design, mold design, and incorrect injection molding parameters during injection molding process. For product design engineers, addressing appearance quality issues should first be addressed through part design, especially when part is a cosmetic component. Appearance requirements for internal parts can be relaxed. From a part design perspective, in addition to meeting design guidelines outlined in previous section, following aspects can also be used to improve appearance quality of plastic parts.

Selection of plastic materials plays a significant role in product's appearance, and different plastic materials exhibit varying appearance quality. For example, compared to non-glass fiber reinforced materials, glass fiber reinforced materials generally exhibit lower appearance quality after injection molding and are more prone to warping.

Surface shrinkage is one of the most common appearance defects in plastic parts. Shrinkage typically occurs on exterior surface of parts where wall is thicker, such as at junctions between ribs and struts, as shown in Figure 3-56.

 

Figure 3-56 Thicker ribs cause shrinkage of corresponding surface of part
2.5.2.1 Concealing Shrinkage through Design
Where permitted, surface shrinkage can be concealed through use of U-shaped grooves, surface discontinuities, and surface texturing, as shown in Figure 3-57.

 

Figure 3-57 Covering up part surface shrinkage through design
// Surface shrinkage is typically addressed by reducing rib thickness or increasing wall thickness. 2.5.2.2 "Crater" Design
Locally removing material from thick wall of a pillar or rib (referred to as a "crater" in Taiwan) can significantly reduce possibility of surface shrinkage in a part, as shown in Figure 3-58. Of course, this "crater" design will reduce strength of pillar or rib to a certain extent.

 

Figure 3-58: Pillar and reinforcement "crater" design
2.5.2.3 Properly Positioning Gate
The farther part is from gate, the more susceptible it is to surface shrinkage. For critical areas of part where surface shrinkage is critical, gate can be positioned close to these areas to minimize possibility of surface shrinkage. Furthermore, gate should be positioned so that molten plastic flows from thicker to thinner areas, as shown in Figure 3-59. If molten plastic flows from thinner to thicker areas, thinner areas will cool and solidify first, making thicker areas more susceptible to surface shrinkage and internal bubbles more likely to form.

 

Figure 3-59 Reasonable setting of gate position

Part deformation not only results in poor dimensional accuracy, easily leading to assembly problems and compromising part functionality, but also affects part's appearance. There are many reasons for part deformation, primarily four of which include: different shrinkage ratios in plastic melt flow direction and cross-sectional direction, uneven cooling, uneven wall thickness, and asymmetric part geometry.
1) Different shrinkage ratios in plastic melt flow direction and cross-sectional direction
Different shrinkage ratios in plastic melt flow direction and cross-sectional direction cause part deformation, as shown in Figure 3-60.
Non-glass fiber reinforced materials shrink more in plastic melt flow direction than in cross-sectional direction, resulting in greater shrinkage in plastic melt flow direction and less shrinkage in cross-sectional direction, causing part deformation.
Glass fiber reinforced materials, on the other hand, experience opposite effect: smaller shrinkage in plastic melt flow direction than in cross-sectional direction, resulting in less shrinkage in plastic melt flow direction and greater shrinkage in cross-sectional direction, causing part deformation.

 

Figure 3-60 Part deformation caused by different shrinkage ratios
2) Uneven cooling of part
Uneven cooling of part wall thickness can cause part deformation. Uneven cooling can be caused by imbalanced injection mold water channel design. Alternatively, it can be caused by part's outer heat dissipation area being larger than inner heat dissipation area. Heat dissipation and cooling occur more slowly on outer side, while heat dissipation and cooling occur more quickly on inner side (see Figure 3-61). Consequently, part deformation is always directed toward hotter side of part.

 

Figure 3-61 Uneven cooling of parts causes deformation of parts
3) Uneven wall thickness causes deformation. Plastic part shrinkage increases with increasing wall thickness. Differential shrinkage due to uneven wall thickness is one of main causes of deformation in thermoplastic parts. Specifically, variations in cross-sectional wall thickness often lead to differential cooling rates and crystallinity, resulting in differential shrinkage and deformation, as shown in Figure 3-62.

 

Figure 3-62 Uneven wall thickness of parts causes deformation of parts
4) Asymmetrical part geometry causes deformation.
Asymmetrical part geometry can lead to uneven cooling and differential shrinkage, causing deformation, as shown in Figure 3-62.

 

Figure 3-63 Asymmetric geometry of part causes deformation of part
5) Predicting part deformation trends and minimizing them through design. Causes and methods of part deformation have been discussed previously, but this is not main point. The key to product design is to predict part deformation trends and reduce or even prevent deformation through part design optimization, as shown in Figures 3-64 and 3-65.

 

When two exterior plastic parts are mated, gaps and offsets (where one part's surface is higher than the other's) will always exist due to manufacturing and assembly errors. This can affect product's appearance, as shown in Figure 3-66a.
Artistic grooves can be designed to conceal gap between two exterior plastic parts, thereby improving product's appearance. There are two common artistic groove designs, as shown in Figures 3-66b and 3-66c.

 

Figure 3-66 Design of art groove
Size of artistic groove depends on product's dimensions. For example, artistic groove on a computer mainframe panel is 0.5 mm x 0.5 mm. Of two artistic groove designs, second method is superior to the first. Gap in the first artistic groove design allows consumers to see product's internal components and does not provide dust protection. When relationship between two plastic parts is front-to-back or top-to-bottom, such as upper and lower covers of a mobile phone, step becomes a factor affecting part's appearance. If rear/lower part is higher than front/upper part, product will look very unsightly. Therefore, when designing art groove, rear/lower part should be lower than front/upper part.

 

Weld marks are a common surface appearance defect in plastic parts and should be avoided. Specific methods are as follows:
1) Textured surfaces can partially conceal weld marks, but not completely.
2) Painting can also conceal weld marks.
3) Appropriately position and number gates to avoid weld marks on key surface areas of part.
4) Ensure good mold ventilation.

Steps or flash are common at intersection of die and core, at intersection of core and die, at intersection of core and die. Therefore, product design engineers should carefully examine location of parting surfaces within mold structure to avoid gaps or flash on critical surface areas, which can affect part's appearance quality.

Also, avoid placing ejector structures on critical surface areas, as this can also cause flash. This is especially important for transparent plastic parts.

Injection molds are typically expensive. Designing multifunctional plastic parts can help offset mold costs, thereby reducing part development costs. Furthermore, because plastic parts can have complex shapes and internal structures, a single part can often replace two or even multiple parts manufactured using traditional processes. Multiple parts can sometimes be combined into a single part to save costs.
For example, in electronic and electrical products, proper cable routing and securing are crucial for heat dissipation and electromagnetic interference reduction. Cables are typically secured with dedicated cable ties or clamps. However, adding simple features to plastic parts can achieve this, as shown in Figure 3-67, thus reducing need for cable ties or clamps.

 

Figure 3-67 Design of a multifunctional plastic part to replace cable ties or clips

 

Design multifunctional plastic parts to replace cable ties or clips

Plastic materials are a product of petroleum industry. As oil reserves continue to dwindle, price of plastic materials is also rising. When oil prices soared a few years ago, surge in plastic material prices even forced Chinese home appliance manufacturers to raise prices of their appliances.
Therefore, while ensuring product functionality and other requirements, part design should use as little material as possible. Less material reduces part cost while also avoiding increased injection time and thus higher costs. When reducing part material usage, it's important to consider following:
1) Improving part strength by adding ribs rather than increasing wall thickness.
2) Removing material from thicker areas of the part.

KISS principle, discussed in Design for Assembly (DFA) chapter, also applies to individual part design. The simpler design of a plastic part, the better. Complex plastic part shapes and structures not only increase mold complexity and cost, but also compromise part quality and performance.
Plastic parts should be designed to be as multifunctional as possible, but multifunctionality does not necessarily mean complexity. If multifunctional design of a plastic part actually increases the overall cost of product, this defeats purpose of multifunctionality of plastic parts, as one of purposes of multifunctional plastic parts is to reduce product cost.

Table 3-9 Factors Affecting Dimensional Tolerances of Plastic Parts

Table 3-10 Three Levels of Plastic Part Dimensional Tolerance

It can be seen that the tighter dimensional tolerances of a plastic part, the higher requirements for mold accuracy, mold cavity count, injection molding process, and inspection, and the higher cost of plastic part. Product design engineers should be aware of significant impact that tight dimensional tolerances have on both part and mold costs. Therefore, when designing a product, while ensuring part functionality, optimize product design and avoid tight dimensional tolerances as much as possible.
In addition to common measures mentioned in tolerance analysis section, other measures for plastic parts include:
① In applications requiring high dimensional accuracy, choose plastics with low shrinkage.
② Avoid strict tolerances in areas where mold cavities, inserts, bevel pins, and sliders may have additional alignment errors.
③ Predict warping area of plastic part and avoid strict tolerance requirements in this area; usually, warping can be reduced by adding reinforcing ribs.

An undercut refers to a feature that prevents part from being demolded normally, such as an opening on upper side of mold opening direction and a boss on the side. In mold, undercuts are achieved through lateral parting and core pulling mechanisms, which are one of more complex structures in mold and are also an important factor in increasing mold costs. Commonly used lateral parting and core pulling mechanisms include inclined pins and sliders.
In order to reduce mold costs, avoiding undercuts in part design is an important means.
(1) Some external undercuts can be avoided by redesigning parting surface
As shown in Figure 3-68, redesigning parting surface can avoid undercuts on the outside of part and prevent smooth demolding.

 

Figure 3-68 Redesigning parting surface to avoid undercutting of parts
(2) Redesign part features to avoid undercuts
Many undercut features can be removed through feature optimization, thus avoiding use of lateral core pulling mechanisms and reducing part mold costs, as shown in Figure 3-69

 

Figure 3-69 Redesigning part features to avoid undercuts
As shown in Figure 3-70, in original design, part has undercuts and requires demolding using lateral core pulling mechanisms such as inclined pins or sliders. By redesigning part features, use of lateral core pulling mechanisms can be avoided. Four methods are provided in improved design, as shown in Figures 3-70b, c, d, and e.

 

Figure 3-70 Redesigning part features to avoid undercuts

Once a plastic part injection mold is manufactured, cost of mold modification is very high. Incorrect plastic part design often increases number of mold modifications, increases mold costs, and thus increases cost of parts and products. Therefore, design of plastic parts needs to minimize or even avoid mold modifications.
2.6.6.1 Design of part injectability
When designing plastic parts, injectability of part should be fully considered. Good part injectability leads to high quality after injection molding, fewer mold modifications, and lower mold modification costs. If plastic part design fails to consider part injectability, poor part injectability and low quality after injection molding will result in frequent mold modifications, resulting in higher mold modification costs. Therefore, plastic part design must adhere to plastic part design guidelines discussed in this chapter.
2.6.6.2 Reducing Product Design Revisions
Of course, mold modifications may also occur because plastic part cannot fulfill its intended function within the entire product. Therefore, before mold development, product design engineers should refine and optimize part design through CAE analysis, motion simulation, and prototype production. Only after ensuring part design is flawless can mold design and development proceed, thereby reducing product design modifications after mold manufacturing is complete.
2.6.6.3 Avoiding Mold Modifications that Involve Material Additions
Molds that involve material removal are relatively easy and require lower modification costs, while molds that involve material addition are more complex and require higher modification costs. Therefore, plastic part design modifications should ideally involve material removal rather than material addition. Therefore, plastic part design modifications should involve material addition, not material removal. When designing a part, if you're unsure of design, you can leave a certain margin for part dimensions and then verify design by removing material.

Plastic part fixing methods include clips, screws, heat staking, and ultrasonic welding. Clips allow for quick assembly and disassembly and offer the lowest cost. While ensuring product assembly and functionality, using clips can reduce part costs.

Number of mold cavities affects plastic part processing efficiency. The greater number of mold cavities, the more complex mold, but the higher processing efficiency and lower processing cost. Furthermore, amount of runner material allocated to each part is reduced. Based on expected production capacity requirements for plastic parts, number of mold cavities can be appropriately selected by calculating plastic part cost (material cost, mold cost allocation, and processing cost).
In addition, properly selecting runner system can also help reduce plastic part costs. Traditional cold runner systems have disadvantage of runner material loss, especially for expensive plastic materials. Hot runner systems, on the other hand, experience virtually no runner material loss. Furthermore, lack of a runner system shortens part's cooling time and mold opening stroke, thereby reducing molding cycle. Furthermore, there's no need for gate trimming or runner reprocessing, facilitating automated production. However, their disadvantage is that they're more expensive than traditional cold runner molds.

1) Design part and mold so that gate can be automatically removed, or hide gate inside part to avoid secondary processing.
2) Hide parting surface inside part to avoid secondary removal.

Some features are unique to injection molded parts, such as ribs, struts, and injection holes.
These typical feature designs are well-suited for designers to learn from, and numerous design guidelines exist, which author intends to describe in separate chapters.

There are many ways to assemble injection molded parts. Common methods can be roughly divided into four categories: snap-fit, mechanical fastening, heat staking, and welding. Each method has its own advantages and disadvantages, as shown in Table 3-11.
Product design engineers should select appropriate assembly method from initial design stage based on product's assembly requirements and factory's available assembly equipment and technology.
Table 3-11 Comparison of Advantages and Disadvantages of Plastic Assembly Methods

Of course, plastic part assembly methods can be combined, leveraging strengths and weaknesses of various methods to achieve unexpected results. For example, a combination of snap-fit and screws not only ensures a stable fixation but also simplifies and speeds assembly.
From an assembly perspective, welding, snap-fit, and heat staking take significantly less time than mechanical fastening, resulting in lower overall costs and a current design trend.
However, given company's current processing capabilities and reliability requirements, comprehensive consideration is required.
Plastic part assembly structure is also a major challenge and a source of errors that can easily occur later.

 

Practice DFMA by following it upfront and filling in gaps afterward. An example form is as follows: