Structural Design Principles for Plastic Product Development

Time：2024-09-02 08:39:04 / Popularity： / Source：

Structural Design Principles for Plastic Product Development

Structural design should be reasonable: assembly gap is reasonable, and all plug-in structures should reserve gaps: ensure sufficient strength and rigidity (safety test), and appropriately design a reasonable safety factor.
Structural design of plastic parts should comprehensively consider manufacturability of mold and simplify mold manufacturing as much as possible.
Structure of plastic parts should consider its plasticity, that is, injection molding production efficiency of parts should be high, and scrap rate of injection molding should be reduced as much as possible.
·Consider convenience of assembly production (especially it should not conflict with assembly)
Structure of plastic parts should adopt standard and mature structures as much as possible, so-called modular design
For universal/public use, try to use existing parts and do not open new molds
·Consider cost

Injection mold product design

1. Material shrinkage rate, whether product thickness is evenly distributed.
2. Improve rigidity design and rib position design
3. Demolding slope, BOSS column, fillet, hole, hinge design, insert, logo, etc.
4. Specific position of parting line
5. Whether glue inlet and resulting joint line are acceptable
6. Specific position of lifter and slider
7. Whether there are design bugs in mechanical drawings
8. Are there other mold material requirements, surface leather texture, product material requirements

Product shrinkage rate

Material	Shrinkage	Material	Shrinkage	Material	Shrinkage
ABS	3-5/1000	PS		PA/6	10/1000
ABS+GF	1-2/1000	HI-PS	5/1000	PA/6+GF	5/1000
PC	3-6/1000	PS+GF	2/1000	PA+66	11/1000
PC+10%GF	4/1000	PP	15/1000	PA/66+GF	5/1000
PC+>10%GF	2/1000	PP+40%GF	5/1000	PC+ABS	3-4.5/1000

Wall thickness

Design of wall thickness mainly considers three aspects: one is thickness; the second is uniformity; third is smooth transition.
Thickness: Wall thickness of injection molded parts is mainly determined by its use, plastic type, structure, etc. For thermoplastic materials, it is generally not suitable to be less than 0.6mm, and 2-4mm is often used. For thermosetting plastics, due to their poor fluidity, thickness should be larger, 1.2~2.5mm for small parts, 2.5~4mm for large parts, and no more than 6mm at most.
Uniformity: Uniformity of wall thickness has a great influence on quality of injection molded parts. If thickness difference of an injection molded part is too large, it will cause uneven shrinkage, resulting in defects such as deformation and cracks. Therefore, equal thickness structure should be used as much as possible in structural design.
Smooth transition: In some injection molded parts, some parts must have different thicknesses due to structural requirements, such as turning points. At this time, a smooth transition should be used to avoid sudden changes in cross-section.

Wall thickness design

Minimum wall thickness and common wall thickness recommendations for plastic products (unit: mm)
Engineering plastics	Minimum wall thickness	Wall thickness of small products	Wall thickness of medium-sized products	Wall thickness of large products
Nylon(PA)	0.45	0.76	1.50	2.40~3.20
Polyethylene (PE)	0.60	1.25	1.60	2.40~3.20
Polystyrene (PS)	0.75	1.25	1.60	3.20~5.40
Modified polyethylene	0.75	1.25	1.60	3.20~5.40
Plexiglass (PMA)(372)	0.80	1.50	2.20	4.00-6. 50
Polypropylene (PP)	0.85	1.45	1.75	2.40~3.20
Polycarbonate(PC)	0.95	1.80	2.30	3.00~4.50
Polyoxymethylene (POM)	0.8	1.40	1.60	2.40-3.20
Polysulfone (PSU)	0.95	1.80	2.30	3.00~4.50
ABS	0.80	1.50	2.20	2.40~3.20
PC+ABS	0.75	1.50	2.20	2.40~3.20
Polyvinyl chloride (hard)	1.15	1.60	1.80	3.2~5. 8
Polyvinyl chloride (soft)	0.85	1.25	1.50	2.4~3.2
Polyamide	0.45	0.75	1.50	2.4~3.2
Polyphenylene ether	1.20	1.75	2.50	3.5-6.4
Polysulfone	0.95	1.80	2.30	3.0~4. 5
Chlorinated polyether	0.90	1.35	1.80	2.5~3.4
Cellulose acetate	0.70	1.25	1.90	3.2-4.8
Ethylcellulose	0.90	1.25	1.60	2.4~3.2
Acrylic	0.70	0.90	1.40	3.0~4.5

Uneven wall thickness is the biggest troublemaker in injection molding, which is particularly obvious for thin-walled parts. These problems include following:
·1. Concave or void
·2. Bending deformation or cracking
·3. Short shot
·4. Redness
·5. Jet
·6. Runway
·7. Long cooling time

Hollowout design

Improve rigidity design

Plastics are relatively flexible, and rigidity of containers made of them is poor. However, injection molded shell sometimes has a large load capacity, so various measures to improve rigidity of structure should be taken.
Adding reinforcing ribs: reinforcing ribs can enhance strength and rigidity of container. Basic requirements for reinforcing ribs are: number should be large, wall thickness should be thin, height should be short, there should be enough slope, bottom of ribs should be in a circular arc transition, and direction of reinforcing ribs should be consistent with direction of material flow to improve toughness of plastic.
Improve shape: box-shaped containers are mostly rectangular thin-walled parts, which are easy to deform. Various reinforcement measures should be taken to make four side walls of container slightly convex outward to improve rigidity; side walls are reinforced in a strip shape to prevent distortion; edge of container is reinforced to prevent mouth from deforming; bottom of container is designed to be corrugated or arched.

Rib design

When rib is thick, junction between rib and bottom plate is also thick. Injection molding is concentrated here. When cooling, surrounding ribs and bottom solidify first. Middle of junction between rib and bottom plate remains liquid. Plastic that solidifies later shrinks on plastic that solidifies first, and has an attraction to plastic around it. If coagulation force is weak at any point, it may collapse and form a depression. If coagulation force is strong enough, a cavity will form in the center of junction between rib and bottom plate.
Thickness of rib should be 50% of thickness of bottom plate, or thinner.

Design example

Formation of cavities and depressions

Bottom thickness of rib

Thickness of rib is generally half or less than half of wall thickness of product

Ribs: more ribs, thinner wall thickness, shorter height

Processing of BOSS columns

·External dimensions of BOSS column should be small when drafting, and internal dimensions should be large. Draft angle value is usually between 0.5-2 degrees. For sleeve ejector pin used in mold design, 3D should design BOSS column outer diameter as an integer or a decimal, and change it every 0.5mm, design its inner diameter as an integer or a decimal, and change it every 0.1mm.

BOSS shrinkage

Prevent BOSS column from shrinking and increasing "crater"

Demolding slope

Proper demolding slope can prevent product roughness. Demolding slope of smooth surface should be greater than 0.5 degrees, that of fine leather grain surface should be greater than 1 degree, and that of coarse leather grain surface should be greater than 1.5 degrees.
·Proper demolding slope can prevent product damage.
When designing deep cavity structure products, outer surface slope is required to be smaller than inner surface slope to ensure that mold core is not offset during injection molding, obtain uniform product wall thickness, and ensure material density strength of product opening.
Direction of slope is generally based on small end of inner hole, which conforms to drawing, and slope is obtained from expansion direction. Outer shape is based on large end, which conforms to drawing, and slope is obtained from reduction direction. As shown in Figure 1-1 below
For plastic parts with high precision requirements, a smaller demoulding slope should be used
For higher and larger sizes, a smaller demoulding slope should be used
For plastic parts with large shrinkage rates, a larger slope value should be used
When wall thickness of plastic part is thicker, molding shrinkage will increase, and demoulding slope should use a larger value
Under normal circumstances, demoulding slope is not included in tolerance range of plastic part
Demoulding slope of transparent parts should be increased to avoid scratches. Under normal circumstances, demoulding slope of PS materials should be greater than 3°, demoulding slope of ABS and PC materials should be greater than 2.

Fillet design

If fillet is too small, it may cause stress concentration in product and crack product.
If fillet is too small, it may cause stress concentration in mold cavity and crack cavity.
Setting a reasonable rounded corner can also improve processing technology of mold. For example, cavity can be directly processed by R cutter milling to avoid inefficient electrical processing.
Different rounded corners may cause movement of parting line. Different rounded corners or corner clearances should be selected according to actual conditions.

Finished product is deeper here and has a sharp corner, which leads to a high and sharp boss on mold. At this time, it is necessary to add R angle or enlarge sharp corner to avoid sharp corners
Rounded corner design

Hole design

·Shape of hole should be as simple as possible, generally circular.
· Axial direction of hole is consistent with mold opening direction to avoid core pulling.
When aspect ratio of hole is greater than 2, demoulding slope should be set. At this time, diameter of hole should be calculated according to minor diameter (maximum physical size).
Aspect ratio of blind hole is generally not more than 4.
· Distance between hole and edge of product is generally greater than hole diameter.

Hole design diagram

Integrated hinge

Taking advantage of toughness of PP material, hinge can be designed to be integrated with product
· Size of film used as a hinge should be less than 0.5mm and remain uniform.
· When injection molding an integrated hinge, gate can only be designed on one side of hinge.

Inserts

·Inserting inserts into injection molded products can increase local strength, hardness, dimensional accuracy and set small threaded holes (axles) to meet various special needs. At the same time, it will increase product costs.
·Inserts are generally copper, but can also be other metals or plastic parts.
Part of insert embedded in plastic should be designed with anti-rotation and anti-pullout structures. Such as: knurling, holes, bends, flattening, shoulders, etc.
Plastic around insert should be appropriately thickened to prevent stress cracking of plastic part
When designing inserts, positioning method in mold (holes, pins, magnets) should be fully considered

Identification

·Product identification is generally set on flatter inner surface of product, and is in the form of a convex. Select surface where normal direction may be consistent with mold opening direction to set identification to avoid strain.

Parting surface

Parting surface is interface between movable mold and fixed mold, and is surface for removing plastic parts or condensate from pouring system. Its reasonable selection is condition for plastic parts to be well formed, which is not only related to demolding of plastic parts, but also involves mold structure and manufacturing cost. A reasonable parting surface can not only meet performance requirements of various aspects of product, but also make mold structure simple and cost will be satisfactory. There are some principles to follow when selecting parting surface:
Parting surface should be selected at the largest cross-section of plastic part (Figure 2), otherwise it will bring difficulties to demolding and processing (Figure 1), which can be said to be the first principle of selection
Keep plastic part on male mold side as much as possible, because it is simple and easy to set up a demolding mechanism on male mold side

·When arranging orientation of part in cavity, try to avoid lateral parting or core pulling to simplify mold structure.
Parting surface form: plane, inclined surface, stepped surface, curved surface, flap
Selection principles of parting surface: 1 It is conducive to demolding. 2 It is conducive to ensuring quality of plastic parts. 3 It is conducive to simplifying mold structure. 4 It is conducive to processing of molded parts. 5 It should be selected at maximum contour of plastic part. 6 It should be conducive to exhaust. 7 It is conducive to lateral parting and core pulling. 8 Difference between large and small ends of plastic parts caused by demolding slope should be minimized. 9 Technical parameters of injection machine should be considered

Core pulling mechanism of injection mold and avoidance

When plastic part cannot be demolded smoothly according to mold opening direction, a core pulling mechanism should be designed. Core pulling mechanism can form a complex product structure, but it is easy to cause defects such as product stitching lines and shrinkage, increase mold cost and shorten mold life
When designing injection molding products, if there is no special requirement, try to avoid core pulling structure. For example, direction of hole axis and rib is changed to mold opening direction, and cavity core is used to hit method.

Gud Mould Industry Co., Ltd