Mold injection, the most popular manufacturing process for mass producing products, requires consideration of many variables. Here are some basic rules of mold design that can affect the production process, lead time, maintenance costs, and quality for mass production.

Basic Design Rules

Consistent Wall Thickness

A consistent wall thickness can reduce warping warping or sink marks. If sections with varying thicknesses are necessary, use chamfers or fillets to eliminate as many sharp corners as possible and ensure smooth resin flow, even distribution within the cavity and complete filling of the entire mold.

화면 캡처 2021-10-25 180756.jpg

Ribs

Thick walls can cause various serious defects in injection-molded parts, such as warping and shrinkage. Thick walls also require longer cooling times, reducing productivity. In such cases, a structural solution can be found. Designing with interconnected supporting structures, as shown above, allows you to create parts with the same performance but less volume. These supporting structures are called ribs.

화면 캡처 2021-10-25 183748.jpg

Recommendations

It is more effective to install several thin ribs than one thick rib.

The direction of the ribs should align with the flow direction of the resin in the mold.

Ribs thicker than the recommended thickness can cause surface defects.

Rib thickness: Part wall thickness x 0.5

Rib height: ≥ Rib thickness x 3

Rib fillet: ≥ 1/4 of rib thickness

Rib spacing: ≥ Rib thickness x 4

Draft angle: Nylon = 0.5°, ABS & PC = 0.5 to 1.5°, reinforced ABS & PC = 1 – 3°

Shell

To increase the strength of a hollow part with a shelled shape, it is essential to design it with ribs to compensate for the strength and rigidity that is lost when reducing the wall thickness.

화면 캡처 2021-10-25 181207.jpg

Between 1.2 mm and 3 mm is a safe wall thickness range for most materials.
The table below summarizes the recommended wall thicknesses according to the injection molding materials.

Material	ecommended Wall Thickness [mm]
Polypropylene (PP)	0.8 - 3.8mm
ABS	1.2 - 3.5mm
Polyethylene (PE)	0.8 - 3.0mm
Polystyrene (PS)	1.0 - 4.0mm
Polyurethane (PUR)	2.0 - 20.0mm
Nylon (PA 6)	0.8 - 3.0mm
Polycarbonate (PC)	1.0 - 4.0mm
PC/ABS	1.2 - 3.5mm
POM	0.8 - 3.0mm
Silicone	1.0 - 10.0mm

Boss

보스_인서트_너트 제거.png

Bosses are pillars that are mainly used to connect parts. Common joining methods using bosses include interference fitting and screw fastening. To join with screws, the inner diameter needs to have a threaded structure, which is an undercut and therefore not formed during the injection stage.

In such cases, insert nuts are used to solve the problem. For more information on insert nuts, please refer to the functional element design below.

Recommendations

Boss outer diameter: Insert outer diameter x 2

Boss inner diameter: Design it the same as the outer diameter of the screw core.

Generally, bosses are designed together with ribs.

The wall thickness of the boss should be uniform.

Chamfer the entrance so that the screw head does not protrude.

Draft Angle

Once the injected material solidifies and molding is complete, the mold opens and a part called the ejector pin pops out and pushes the hardened molded part out of the mold. Even in this simple process, serious defects can occur, so caution is needed. Defects caused by plastic products scratching against metal molds may seem minor. However, surface defects are major defects that can significantly reduce marketability. To prevent this, 제an additional angle is designed into the mold to allow the product to easily slide out. This is the draft angle.

화면 캡처 2021-10-20 120742.jpg

Recommendations

The minimum recommended draft angle is 0.5° or more.

The recommended draft angle is 2° or more.

When the part height is 50 mm or more, increase the draft angle by 1° for every 25 mm.

For surface treatment post-processing, increase the draft angle by 1°–2°.

Ribs also need draft angles. However, it is necessary to check whether the minimum recommended wall thickness is observed.

Fillet

It is best to design the product with a uniform thicknesses for all walls, but variations may be necessary depending on intentions. Sharp corners formed by steps can become notches and concentrate stress, increasing the probability of breakage or relatively weak strength. To prevent such problems, avoid creating steps in the outer shape.

화면 캡처 2021-10-20 122455.jpg

Recommendations

Smooth shapes considering the flow of material are essential.

The recommended length of a fillet is as follows. (fillet length > wall thickness difference x 3)

The recommended fillet value for inner corners is as follows. (fillet value < wall thickness x 0.5)

The recommended fillet value for outer corners is as follows. (fillet value = inner fillet value + wall thickness)

Undercut

Undercuts are shapes that cannot be removed from the mold by simply opening and closing it. Protruding or recessed parts are the main factors. Undercuts require additional parts and design. Parts such as slide cores need to be added, which can reduce the durability of the mold or cause defects to appear. In addition, undercuts complicate the mold structure, significantly increasing costs. They also slow down the production speed, so it is good to design in a way that avoids undercuts as much as possible.

화면 캡처 2021-10-26 114413.jpg

Workaround Design

There may be situations where shapes that cause undercuts are absolutely necessary. In such cases, a different approach can be considered. Consider a structure that allows the product to be released from the mold by simply opening and closing it. Designing around undercuts can dramatically reduce project costs.

Moving the Parting Line

화면 캡처 2021-10-26 121615.jpg

The parting line is where the top and bottom halves of the mold meet. The parting line must be determined very carefully when designing the mold. If done well, situations where undercuts occur can be prevented. The position of the parting line can be used to offset undercuts on external surfaces.

Forced Ejection

화면 캡처 2021-10-20 164203.jpg

Parts with small undercuts or that are molded from elastic materials can use the forced ejection technique. This is a clever workaround that makes full use of the material's properties. However, it has the disadvantage of having many limitations. It is recommended that you use forced ejection if the product you want to manufacture meets the following four conditions.

Recommendations

The material should be soft and have good elasticity (HDPE, PA, etc.).

It should have a shape that can be elastic (cap shape, etc.).

There should be no structures that reduce elasticity, such as ribs or corners.

The angle of the undercut lead should be 30 – 40°.

Functional Element Design

Functional Element Design

화면 캡처 2021-10-21 120449.jpg

Inserts are parts that securely fasten screws. They are precisely machined parts, so they have the advantage of being able to use standard screws. In addition, they are made of durable metal materials, so they can be repeatedly disassembled and assembled. Inserts are inserted into molded parts using heat or ultrasound, or placed in an appropriate position in the mold and then fixed by injecting material.

Recommendations

It is recommended that a dish-shaped hole be made for the boss.

The threads should be cut with a standard tap.

Snap Fit

화면 캡처 2021-10-21 135748.jpg

The simplest part fastening method, easy to assemble and disassemble. It also has the advantage of reducing the assembly cost of the product. However, since it utilizes the elasticity of the material, it is essential to consider the material's physical properties and structural rigidity. To design a durable snap fit, the appropriate flexural modulus, elasticity, and yield strength must be accurately calculated. Therefore, numerous prototypes are required, and collaboration with experts is essential.

Structural design is needed to prevent undercuts.

Snap fit thickness: Part wall thickness x 0.5

Draft angles should be considered for the vertical walls of snap fits.

Hinge

A hinge is a structure that connects two parts of a component so that it can bend. Hinges designed using the elasticity of the material are generally used in containers such as plastic bottles. Flexible materials are used as the structure needs to make full use of elasticity. Similar to snap fits, numerous prototype tests are required to accurately calculate elasticity and yield strength.

화면 캡처 2021-10-21 140904.jpg

It is recommended that the R value of the hinge be as large as possible to minimize stress.

It is recommended that the R value of the hinge be as large as possible to minimize stress.

It is recommended that the hinge be designed with the same thickness as the main wall of the part.

For household goods - Polypropylene (PP)/polyethylene (PE) is mainly used.

For engineering purposes - Nylon (PA) is mainly used.

Embossing/Debossing (Lettering)

화면 캡처 2021-10-26 110541.jpg

Adding logos, text, or symbols to products is an effective branding element. Such detailed depictions require additional CNC machining on the mold. Therefore, for such embossed expressions, design suitable for the CNC machining process is necessary.

Embossing (debossing from the mold perspective) with a height of 0.5 mm or more is recommended.

Text with uniform thickness is recommended.

It is recommended that round fonts of 20 Pt or more be used for text.