Inserts, also called "fitters," play a crucial role in injection molds. They facilitate mold modifications. Molds frequently require design changes, and inserts can be pre-installed in areas needing modification. Future mold changes only require replacing inserts, and even spare inserts can be made during mold opening for replacement, simplifying mold maintenance. Inserts can also be added where venting is needed, utilizing fit clearance for air release. Benefits of inserts also include simplified mold machining. Machining, polishing, filling, demolding deep ribs and holes in molds are very difficult; inserts reduce these difficulties. Inserts also increase mold lifespan. Generally, areas requiring inserts are prone to damage; damaged inserts can be replaced, extending mold's lifespan.
For medium and large molds, purpose of inserts is not limited to points mentioned above. Partial insert designs are unlikely to truly improve manufacturability in medium and large molds. A fully insert structure is a mold design method that focuses on mold core manufacturing process, aiming to shorten mold manufacturing cycle, improve manufacturing precision, enhance injection molding processability. For medium to large, large, or extra-large injection molds, a fully insert structure design, commonly known as a modular insert design, is adopted to shorten processing cycle and facilitate processing. Idea is to divide the entire mold core (usually referring to rear mold core) into multiple inserts, which are processed simultaneously. This simplifies insert processing time and saves a significant amount of mold steel. Therefore, fully insert structure is widely used in Japanese mold design.
When plastic product size is 150mm x 150mm or larger, and there are many deep ribs on moving mold side, a fully insert structure for moving mold is the most common practice. Principle of a fully inlaid structure is that segmentation positions of inserts should facilitate reducing CNC machining, avoid or reduce EDM corner clearing processes, and allow mold parts to be machined by wire EDM or grinding as much as possible. Wire EDM or grinding offers high dimensional accuracy and shorter processing time.
Figure 4-71 shows fully inlaid design of a telephone bottom shell mold. Telephone bottom shell product dimensions are (239.7 ± 0.1) mm x (181.4 ± 0.1) mm x 52.1 mm, with an average plastic thickness of 2.0 mm, and material is ABS. Due to large size of plastic part, a fully inlaid mold structure was designed for moving mold to facilitate injection molding and reduce EDM corner clearing work. In Figure 4-71, Figure (a) is product drawing of plastic part, and Figure (b) is 3D drawing of fully inlaid design of moving mold, where S01 is side core-pulling slider, EO1 is direct ejector, and CO1~C28 are core inserts. Figure (c) shows 3D model of fixed mold cavity and its small inserts. Appearance of molded plastic part is not suitable for a fully inlaid design. VO1~V15 are cavity and small inserts, respectively. Figure (d) is an exploded view of moving mold (core). Separating central large insert CO1 from edge inserts C02~C05 reduces amount of corner clearing work at junction between C01 and C02~C05. Thickness direction of C02~C05 can be ground to required dimensions. This is a typical fully inlaid structure design. Core is divided into central part CO1 and four edge inserts CO2~C05. Ordering C02~C05 material can reduce height and also reduce machining.

 

Figure 4-71 Full-set design of telephone bottom shell mold
Figure 4-72 shows a fully inlaid design for a printer paper guide bracket mold. Printer paper guide bracket product dimensions are 235mm x 65.05mm x 52.5mm, average glue thickness of plastic part is 2.0mm, and material is HIPS. Plastic part is relatively long. To facilitate venting and mold processing, both moving and fixed molds are designed with a fully interlocking mold structure, with one mold cavity and two outlet cavities. Figure 4-72(a) shows product image of plastic part. Shape of plastic part is approximately a triangular support. Upper surface of one side has 16 arc-shaped ribs, which are paper passage surface for A4 paper. This surface needs to be flat, and ribs need to be highly polished. At the same time, no gate or ejection system should be designed on this surface, and there should be no interlocking marks to avoid affecting passage of paper. Figure 4-72(b) shows 3D drawing of fully interlocking design of moving mold. Mold core parts C01~CO8 are all core inserts, and C02A is a small insert, which is inserted into large insert C04. Figure 4-72(c) shows 3D drawing of fully interlocking design of fixed mold.

 

Figure 4-72 Full-set design of printer paper guide bracket mold

Starting point of fully interlocking structure is based on mold processing feasibility, dividing mold core into multiple inserts. In large and complex molds, such as automotive molds, and molds for printers, air conditioners, and large household appliances, numerous inserts exist within mold core. Complexity of curved surfaces and draft angles of plastic parts cause irregularities in inserts. Inserts can be regular or irregular in shape, large or small, and sometimes large inserts contain smaller inserts. Segmentation of inserts in a fully inlaid structure must fully consider manufacturability; key points of segmentation are as follows:
1. Before segmenting inserts in a fully inlaid structure, it is necessary to determine machining datum for inserts and datum for assembling all inserts. Datum for mold core and datum for precision frame on mold blank coincide. There are two types of datums for opening precision frame on mold blank: one is machining with center as datum for dividing four sides, other is machining with datum corner as datum. For mold designs with fully inlaid structures, the latter method has advantage of higher precision. When segmenting inserts and determining datums, care must be taken to avoid weak points and to avoid compromising strength of mold core.
2. Insert segmentation should prioritize ease of CNC machining, minimizing need for EDM (Electronic Discharge Machining) corner clearing. Grooves and irregular holes in inserts should be decomposed into parts that can be machined using wire EDM, while flat and stepped surfaces should be machined to dimensions using grinding.
3. Circular structural elements should be decomposed into circular inserts for easier CNC lathe machining or subsequent internal and external cylindrical grinding.
4. For small, deep ribs or other small areas that cannot be machined using wire EDM or cutting, split inserts to reduce EDM machining.
5. For areas with large areas and significant height differences, splitting inserts can greatly reduce machining volume, solve problems of insufficient tool length or rigidity, and save a significant amount of steel.
6. For areas where heat dissipation is poor, resulting in insufficient cooling, beryllium copper inserts should be added for heat dissipation.
7. When segmenting inserts in a fully inlaid structure, factors such as ease of assembly, convenient mold disassembly, high precision, and ability to maintain accuracy even after repeated disassembly must be considered.
8. Selected insert location should be in a position that does not damage appearance and function of plastic part. Inserts should be placed within mold cavity. If insert clamping lines are created within cavity, customer confirmation is required.
9. Determine location of lifting and assembly process holes.
Determining number and location of inserts is a crucial task. It requires close consideration of company's mold manufacturing process, stroke, parameters, machining range of existing machine tools, tool parameter selection, factors such as venting in injection molding and mold polishing. Improper insert splitting may prevent inserts from fulfilling their function and advantages, waste machining time, weaken mold cooling, may also affect strength and rigidity of mold, causing irreparable damage. Poor insert splitting will make mold assembly difficult, lacking assembly benchmarks.
Figure 4-73 shows a product image of top cover plate for a color duplex printer. Product dimensions are 282.0mm x 211.50mm x 84.50mm, with an average plastic thickness of 2.20mm. Material is PC+ABS, and part is relatively large, weighing 235g. Mold design is shown in Figure 4-74. Fixed mold cavity is a single-piece design, with inserts V02 and V03. To facilitate injection molding and reduce EDM corner clearing, moving mold features a fully inlaid mold structure. Considering manufacturing process, moving mold inserts C01~C10 are separated, effectively simplifying mold processing.

 

Figure 4-73 Top cover plate of a color duplex printer

Figure 4-74 3D drawing of mold for top cover plate of a color duplex printer
Product shown in Figure 4-73 has multiple perpendicular ribs on the back. Without inserts, these ribs are prone to air entrapment during injection molding, and mold processing is inconvenient. Therefore, it is necessary to separate inserts, breaking down ribs into simple geometric elements that can be machined by wire cutting or grinding. After disassembling inserts, insert Co1 has relatively small height variations and can be machined using CNC. Ejector pin holes are wire-cut, requiring only local EDM machining. Since plastic part's shape resembles a step, it's foreseeable that height direction of moving mold inserts C02 and C03 will also resemble a step shape, a shape perfectly suited for wire EDM machining.
Part drawing for moving mold insert C02 is shown in Figure 4-75. After preparing steel material for this part, first determine reference angle position according to drawing and mark "base" on steel. Next, machine cooling water channels, threaded holes, and through holes for ejector pin holes, followed by wire EDM and CNC machining. Whether to perform wire EDM or CNC machining first requires specific analysis. For CO2 insert, wire EDM followed by CNC machining will save CNC machining time. Finally, EDM machining is performed.

 

Figure 4-75 Part drawing of moving mold insert C02
Wire EDM process for CO2 insert consists of two steps. First, wire EDM ejector pin holes, as shown in the top view of Figure 4-75. Then, steps on parting surface of part are wire-cut according to Figure 4-76. Width dimensions 74.04 and 73.11 indicate presence of a step on part, with a radius of 0.8 at the root. This step can be machined using a hand-operated grinder. Coordinate dimensions 117.56 and 108.28 indicate a groove, which can be machined using a hand-operated grinder or wire-cut.
Machining process for moving mold insert CO3 is similar to that of CO2 and will not be repeated here. Moving mold inserts C06, C09, and C10 differ significantly in height from moving mold insert CO5; to reduce machining workload, they are processed as multiple inserts.
From above analysis, it can be seen that so-called full-insert machining is a machining method that improves mold processing efficiency by starting from mold manufacturing process. When plastic part is large and has many ribs, it can effectively improve mold processing accuracy, simplify mold processing process, and enhance injection molding processability.

① Carefully study mold design specifications and perform 3D demolding according to required parting surfaces to separate cavity and core.
② Compare plastic part drawing and technical requirements to understand and analyze areas requiring key cooling, ejection points, and venting points. Water-cooling rings should not be located at junction of two inserts. Inserts with water-cooling rings at the bottom must be fixed with screws; mounting platforms should not be used.
③ When designing inserts, follow principle of starting with the largest and then moving to the smallest. Generally, determine position of larger inserts first, consider cooling water circuit design, and arrange positions of fixing screws. Using mold base reference angle as a reference, length direction sides of two inserts adjacent to reference angle should be perpendicular to frame bottom, and length direction sides of two inserts far from reference angle should be at an angle of 3~5° to frame bottom. Preliminarily divide inserts, ensuring that each insert has two mutually perpendicular edges as processing references.
④ For irregularly shaped inserts, pre-determine processing process references.
⑤ Organize experienced technicians to review the feasibility of insert segmentation.
Figure 4-78 shows a product drawing of a telephone faceplate. Product dimensions are 238.4mm x 185.0mm x 31.50mm, average thickness of plastic part is 2.52mm, material is HIPS, plastic part is relatively large, and its weight is 135.84g. 3D mold design drawings are shown in Figures 4-79 and 4-80, and exploded 3D view is shown in Figure 4-81. Fixed mold cavity is a partial inlay design, while moving mold is a fully inlay design. One of the most prominent features of Japanese plastic molds is use of inserts. When plastic product size is greater than 150mm x 150mm, and there are many deep ribs on moving mold side, it is common practice to break down moving mold into inserts. Principle of breaking down mold into inserts is that insert segmentation position should facilitate reducing EDM (Electrical Discharge Machining), allowing parts to be machined by wire EDM or grinding as much as possible. Wire EDM or grinding offers high dimensional accuracy and shorter processing time.

 

Figure 4-78 Telephone casing product image

 

Figure 4-79 3D model of moving mold of telephone casing

 

Figure 4-80 3D drawing of fixed mold for telephone casing

 

Figure 4-81 Exploded 3D view of moving mold of telephone casing
When designing a modular insert, position of larger inserts is generally determined first, cooling water circuit design is considered, and positions of fixing screws are arranged. Using mold blank reference angle as a reference, sides of two inserts adjacent to reference angle are perpendicular to each other, and included angle of sides of two inserts far from reference angle is 3~5, as shown in sides A and B of Figure 4-82. Mold assembly method is similar to a children's toy puzzle. Figure 4-82 is a plan view of moving mold of a telephone face shell. Drawing number of each insert is marked on figure, and reference symbol "base" is marked in lower right corner. During assembly, this plan view is used as a reference, starting from reference angle, and finally assembling two inserts with angled sides.

 

Figure 4-82 Plan view of moving mold of telephone casing
From above analysis, we can see advantages of modular insert design: simplified processing technology, saving mold steel.Mold has good injection molding processability and good venting. Future mold modification or maintenance is very convenient.

① Select machining datum for workpiece and mark it with a colored pen. Machining lifting and assembly process holes. Workpiece's external dimensions should be within ±0.01mm; grinding adjustments will be made during assembly to eliminate accumulated errors.
② Arrange order of operations. For large inserts, water channels need to be drilled in advance to avoid difficulties drilling later due to irregular shapes. Machining of deep holes in large molds must consider distance from hole to workpiece surface. Because deep hole drilling drills are very long, they can become eccentric during machining, and this eccentricity is more severe as hole depth increases. Improper design can easily lead to drilling through cavity.
③ Machine each hole according to datum positioning. For workpieces with allowance in previous stage, method of pre-reservation must be confirmed.
④ Based on unit's machining process and equipment, all inserts should be machined simultaneously, manufactured according to drawings, and fitted together as much as possible.
⑤ After each process is completed, conduct thorough inspection. Use a three-dimensional coordinate measuring machine (CMM) to inspect curved surfaces until they conform to drawings and tolerances.
⑥ Before fitting mold, check that all parts meet drawing requirements. For any areas that are not properly machined, rework them on machine; manual correction is not allowed. For parts that are loose due to machining errors or being too small, replacement or additional inserts are required; do not use steel sheets, paper, or other materials as padding.

Method of dividing cavity and core in an inlaid structure directly affects quality of mold and ease of machining. When considering an inlaid structure, first consider shape, size, tolerances, and function of plastic part, then consider strength and rigidity of cavity and core, simultaneously consider machining method and assembly measures.
① Inlay according to shape and function of assembly. Joint of inlay will leave marks on the surface of product, so inlay position should be set where it does not affect appearance of plastic product. In addition, the surfaces of inlaid parts will have differences of a few micrometers and are prone to burrs, so inlay position should avoid surface of plastic part with special functional requirements.
② Inlay according to processing technology. Complex cavities and cores, if subdivided, can basically be transformed into circular and straight line structures. If these shapes are easy to grind and polish, then parts with uniform dimensions can be easily obtained. Inserts should be broken down to their basic shape or process step; identical shapes should not be further broken down to avoid increasing number of parts and reducing processing efficiency.
③ In terms of processing technology, while considering processing technology, it is also necessary to consider mechanical equipment available in unit.
④ Divide into insulated parts that are difficult to deform. To improve performance of insulated parts, heat treatment is sometimes required. Since heat treatment can easily cause deformation of parts, it is best to divide them into shapes with minimal or no deformation.
⑤ Consider venting effect of insulated parts. Precision insulated parts often have narrow and deep grooves, where flow of plastic is subject to significant resistance. If a monolithic structure is used, venting is difficult, affecting molding quality of product. If an insulated structure is used, dividing these parts into insulated sections makes it easier to solve venting problem.
⑥ Fully consider decomposition and assembly of insulated parts. Since number of parts increases after adopting an insulated structure, if decomposition and assembly process is not considered in advance, it will cause difficulties in decomposition and assembly, and may even result in inability to restore dimensional accuracy. Therefore, it is often used to set inlay parts on insulated parts, and through mutual cooperation, the whole part can be correctly reset.