1.1 Function of Boss Column: Boss columns in plastic parts are typically used to support PCBAs, fix PCBA or plastic part itself, fix electronic components, or connect front and rear shells of product. One of its biggest advantages is that height is easily adjustable. Therefore, under normal circumstances, we should try to use plane formed by end face of column as support surface. The plane formed by several ribs can be used as support surface.
1.2 Draft Angle and Height of Boss Column: When column height is greater than 10mm, it is usually ejected using an ejector sleeve, so its draft angle can be very small or 0 degrees. Inner hole can be set to 0 degrees, and outer surface to 0.25 degrees. When column height is less than 10mm, inserts may be used on mold, draft angle can be set to 0.5 degrees for inner hole and 1 degree for outer surface. If height adjustment is desired, please indicate it on drawing and require mold to consider height adjustment during processing. Generally, height of an M3 self-tapping screw post should not exceed 30mm. If it's too high, ejector pin is easily bent and deformed by adhesive flow.
1.3 Post Size: Since posts with a height greater than 10mm are usually ejected using an ejector sleeve, outer and inner diameters of post are limited.
Common ejector sleeve outer diameter series: φ4.0, 4.5, 5, 6, 6.5, 7, 8, 10, 12
Common ejector pin series: 1.5, 2.0, 3.0, 3.5, 4.0, 4.5, 5.0
Corresponding relationships are shown in the table below.

 

Inner diameter of post is obtained by grinding down ejector pin. As shown in the table above, we should avoid designing posts with a wall thickness less than 1.0mm, it's best to avoid designing posts with outer diameters that are not standard values.
1.4 Treatment of column base: Two common issues are shrinkage or shadows (or watermarks). To prevent shrinkage, glue at column base needs to be reduced, and ejector pin lengthened. If shadows (or watermarks) have already appeared, glue needs to be added to column base or ejector pin shortened. Therefore, for columns with a wall thickness of 3mm and a diameter greater than or equal to 6mm (using M3 self-tapping screws), to prevent shrinkage, glue at column base should be reduced during mold processing. If shadows appear during trial molding, glue should be added. (Note requirements for column base: ejector pin surface and crater surface should not be at same height to reduce stress.)
1.5 Selection and use of embedded studs: For areas requiring frequent disassembly or maintenance, embedded (hot-pressed) studs should be used, replacing self-tapping screws with ordinary screws. After hot pressing or embedding nuts, glued column must not crack or have glue overflow.
1.6 Cracking Issues at Connection Between Embedded Studs and Plastic Parts:
Due to significant difference between dimensional changes of embedded studs during cooling and shrinkage of plastic part, large internal stresses are generated around embedded studs, leading to cracking of plastic part. This is particularly severe for high-rigidity engineering plastics. Given high internal stress, embedded studs are generally prohibited in PC, and PC+ABS is also not recommended, especially when there are more than four embedded studs, or studs of varying heights, resulting in too many stud types and increasing risk of errors. Furthermore, prolonged storage can cause material in injection molding machine barrel to deteriorate due to prolonged high temperatures. Following lists M2, M2.5, M3, and M4 self-tapping screw posts.

 

Function of reinforcing ribs is to increase strength of plastic parts and prevent deformation. Simply increasing wall thickness to improve strength of plastic parts is often unreasonable. Firstly, it easily leads to shrinkage; secondly, it increases injection molding costs. Reinforcing ribs should not be designed too thick, otherwise shrinkage will easily occur at their root. They should also not be too thin, as uneven glue flow is likely. Recommended thicknesses are: When mold is machined with a large gate, thickness at the root of reinforcing rib should be less than 1/2 of wall thickness, and thickness at the top of rib should not be less than 1mm. When mold is machined with a small gate, thickness at the root of reinforcing rib should be less than 2/5 of wall thickness, thickness at the top of rib should not be less than 0.8mm. Regarding draft angle of reinforcing rib: For ordinary reinforcing ribs, draft angle on both sides can be taken according to above thickness requirements. For reinforcing ribs with special height requirements, a draft angle of 0.1-0.25 degrees can be taken on both sides. In this case, reinforcing rib will need to be made into an insert. If possible, adding pillars to reinforcing ribs can aid in demolding. (See diagram below)

 

Reinforcing Ribs on Pillars: Reinforcing ribs must be designed for plastic pillars where structurally permissible. Since these ribs are ejected together with pillar, they can be much higher than ordinary reinforcing ribs, only 1-3mm lower than pillar's end face in height direction. Simultaneously, reinforcing ribs should be machined as symmetrically as possible to minimize pillar deformation. Their shape is shown in Figure 1, with an indicated slope of D=3-5 degrees.

For industrial products, especially fixed lighting fixtures, if environmental conditions permit (for some products, especially those in dusty or particulate environments, decorative seams are not allowed), it is best to design them. Decorative seams are designed to compensate for appearance defects caused by plastic part deformation. To ensure good fit between plastic parts and easy assembly and disassembly, stops and forks need to be designed at mating points. Design of stop and fork ribs varies. Recommended shapes for stop and fork ribs are shown in Figures 2 and 3. Pay special attention to ensuring reduction of excess material is uniform and gradual, avoiding abrupt changes, otherwise, shadows may appear on the surface.

 

3.1 Stop Design Experience
3.1.1 Stop Type 1: From an aesthetic perspective, it is recommended that part 1 be front shell and part 2 rear shell. Furthermore, if front and rear shells are not flush after mold processing and require mold repair, it is recommended to add more material to front shell, making it larger than the rear shell (D1>D2). This is aesthetically superior than having rear shell larger than front shell (D2>D1). It is recommended to specify a positive tolerance for front shell D1 and a negative tolerance for rear shell D2 during design. This type of stop has following characteristics: beautiful appearance, large decorative seam, suitable for larger parts, but thinner outer shell may cause shadows on the surface, and sealing performance is slightly poor.

 

3.1.2 Stop Type 2: Good sealing, small decorative seam, aesthetically pleasing, suitable for small structures, but seam may be more noticeable on large parts.

 

3.1.3 Stop Form 3: Slightly inferior feel, suitable for larger parts, beneficial for concealing dimensional errors between front and rear shells.

 

3.1.4 Stop Form 4: Aesthetically pleasing, decorative seam size can be adjusted, excellent sealing (sealing strips can be added), requires greater wall thickness, complex mold structure.

 

3.1.5 Interlocking Design Between Front and Rear Shells: In plastic part design, to simplify assembly and reduce screws, elasticity of plastic can be utilized to design interlocking connections. There are many types of interlocking connections; here we need to pay special attention to connection between front and rear shells. Recommended interlocking forms are as follows:

 

Structure shown in the left is generally made on rear shell, and structure shown in the right is generally made on the front shell. Special attention should be paid to ensuring uniform and gradual reduction of material, avoiding abrupt changes. Otherwise, shadows or shrinkage may appear at reduction points.

Except for sharp corners required for practical use, all other corners of plastic parts should be rounded as much as possible. Sharp corners in plastic parts are prone to stress concentration, which can lead to cracking under stress or impact. Cracking can even occur during demolding. Following principles are generally recommended for rounded corners:
Top ends of ribs: R>1mm. Square holes in the center of plastic parts: Rounded corners, with rounded corners greater than 1/4 of part's wall thickness. Rounded corners of square parts that mate with holes on the top of plastic parts. Rounded corners at the base of pillars subjected to special stress: approximately R0.5.

Transparent Materials: Many types of transparent materials are commonly used. We frequently use transparent ABS, PC, PMMA in our designs. Due to poor flowability of transparent materials, appearance problems are easily caused during injection molding. For example, transparent button caps are prone to watermarks on the top. Lenses are prone to nail-like or snake-like patterns near sprue. To address above issues, please note following during design: For parts such as transparent button caps: top thickness should be designed to be thicker than surrounding area. If cavity is too deep, reduce amount of glue near sprue so that glue flows to top of part first, and then to surrounding area. For parts such as decorative pieces and lenses: when designing, please reserve a wider (greater than 6-8mm) and thicker sprue area (greater than 1-1.5mm). When machining mold, use a wide fan-shaped sprue as much as possible, make sure runner is short and thick.