Complex Designs with MIM
The metal injection molding (MIM) process excels in the production of complex geometries; however, the simplest MIM shape is produced in a mold made of two sections with plane surfaces that meet to seal off the cavity. One section consists of a core which fits into an impression in the other section with uniform clearances that produce shapes with uniform wall thicknesses. The core produces the internal features while the impression produces the external features. All features are designed to permit the cavity to release the solidified form, which is pushed off the core with ejector pins.
The mold cavity has a large influence on the dimensional capability of the part. Once the component is ejected from the tool there remains little capability to adjust dimensions except with extra cost. So, the mold cavity inherently sets a limit on the dimensional control of the sintered product.
Increased complexity in MIM components can be achieved with the addition of slides, cores, and other tools commonly used in plastic injection molding. While added features, along with their increased complexity, can have economic benefits by eliminating secondary processes or assembly operations, they typically entail additional costs associated with tooling and start-up engineering.
There are many critical aspects that must be considered when designing a MIM component in order to take full advantage of all the benefits of the process. A clear understanding of these considerations as you work closely with your MIM parts fabricator will ensure the best possible manufacturing results for your component. Additionally, your MIMA-member parts fabricator can assist with assessing the benefits versus the cost as you go through the stages of designing the tooling.
Cored holes can be used to reduce cross sections to within guideline limits, achieve uniform wall thickness, reduce material consumption, and reduce or eliminate machining operations. As shown in Figure 1, the preferred direction is parallel to the direction of the mold opening, in other words, perpendicular to the parting plane. Through holes are preferred to blind holes when the length/diameter ratio is greater than 4:1 because the core pin is supported on both ends, whereas blind holes use a cantilevered pin.
Features such as logos, knurls, part numbers, and cavity identification marks can be easily molded in place, without added cost to the piece price. These features can be either raised or sub-surface. MIM can provide high levels of feature detail, including relatively sharp diamond knurling.
Draft is the small angle on surfaces that would otherwise be parallel to the direction of movement of mold members. This is particularly true for core pins. Draft is provided to facilitate the release and ejection of the molded form. The normal range is 0.5° to 2.0°. As the length of the component element becomes longer of if the surface is textured, a greater draft should be used. As shown in Figure 2 shows some of the circumstances that require draft.
Fillets and radii are generally advantageous to product function as they reduce stresses at the intersection of features. They are also advantageous to the molding process, by eliminating sharp corners that can cause cracking or erosion of mold features, by facilitating the flow of feedstock into the mold, and by assisting in the ejection of the part from the cavity. They may also provide a softening of sharp corners for esthetics and handling. Fillets and radii of 0.4–0.8 mm (0.015–0.030 in.) are generally preferred.
Feedstock enters the mold cavity through an opening called a “gate”; due to the high metals loading of MIM feedstock, these openings are generally much larger for MIM than for plastic injection molding. Because gates usually leave a mark on the finished part where they are separated from the molded form, locating them involves balancing the demands of manufacturability, function, dimensional control, and esthetics.
As shown in Figure 3, gates are generally best located on the parting line of the mold, positioned so the flow path impinges on a cavity wall or a core pin. There are other considerations for gate locations, such as subgates, tunnel gates, or pin point gates. for a component with different wall thicknesses, it is usually placed at the thickest cross section so the material flows from thick to thin section. Such a placement reduces voids, sink marks, stress concentrations, and flow lines on the part surface. If the part will be produced in multiple cavities, added consideration must be given to gate size and placement to assure that an identical amount is delivered to each cavity at a balanced fill rate.
Besides being used to reduce part mass and provide uniform wall thicknesses, holes and slots can provide useful functional features in MIM components, and can generally be produced without adding to the piece price. However, adding these features does increase the complexity of the mold, as shown in Figure 4a, which potentially adds to its cost. Holes that are perpendicular to the parting line are the easiest (and least costly) to mold in. Holes that are located parallel to the parting line, while readily achievable, require mechanical slides or hydraulic cylinders, which increases the up-front tooling costs.
Internally connected holes are possible, as shown in Figure 4b. To prevent potential sealing-off problems and issues with flashing, careful consideration must be given to the design. If possible, one hole should be D-shaped in order to provide a flat on the core pin for a robust tool seal-off, as well as to eliminate inordinate wear of the feathered edges that would otherwise be required on the contoured face of the mating member.
The parting line is the plane in which the two halves of the mold meet. To the extent possible, all features should be oriented perpendicular to the parting line to facilitate removal from the mold. Normally, the parting line is transferred to the surface of the part as a witness line, an unavoidable result of two mating mold members. In some cases, as in the example shown in Figure 5, the full part geometry can be maintained in the ejector side or “B” side of the mold, in which case the parting line would be along the bottom edge of the component and no witness line would be created. At other times, the mold may be designed to separate along an inconspicuous edge, thus “hiding” the parting line.
A parting line that can be contained in a single plane is preferred. However, it is sometimes necessary to modify the simple shape in order to mold desirable features. The added complexity, although it increases the cost of fabricating and maintaining the tools, may be cost effective when the features it molds would otherwise require machining or assembly operations.
Ribs and webs are useful for reinforcing relatively thin walls and avoiding thick sections. In addition to increasing the strength and rigidity of a thin wall, they improve material flow and limit distortion. Rib thickness should not exceed that of the adjoining wall. Where structural requirements indicate thicker ribs, multiple ribs should be used instead. Figure 6a shows recommended proportions for ribs. Figure 6b shows how ribs may be used as a means to provide coring for mass reduction while maintaining the functional strength of the component.
During the debinding and high-temperature sintering processes, green parts shrink about 20% (binder volume dependent). At this time, the parts must be adequately supported to minimize the possibility for distortion. As metal injection molded parts are typically placed on flat ceramic plates or trays, as shown in Figure 7, it is ideal that they be designed with a large flat surface, or several component features that have a common plane, so that standard fixtures can be used. Parts that have long spans, cantilevers, or delicate points may need to be supported with part-specific fixtures or setters, which can be expensive to produce.
Although it is highly desirable for wall thickness to be uniform throughout a MIM part, there may be times when coring to achieve thickness uniformity is not an option and variations cannot be avoided. In those instances, the design should provide for a gradual transition between differing thicknesses. Figure 8 shows a recommended wall thickness transition ratio for such cases.
Both internal and external threads can be formed by MIM; however, tapping internal threads is usually more precise and cost effective than using unscrewing cores. The optimum location for external threads is on a parting line of mold members to eliminate the need for unscrewing the mold members that form them. To hold a thread tolerance on a thread diameter, narrow flats—typically .005”—at the parting line are generally specified, as shown in Figure 9. This insures proper mold seal-off, reduces the likelihood of a parting-line vestige, and eliminates problems with flash in the root of the threads, thus reducing mold maintenance.
External undercuts as shown in Figure 10 can be readily formed on a parting line using a split mold; where additional mold members are required to produce them. Some internal undercuts can be produced using slides while some others may be molded through the use of collapsible cores. The added costs and potential flashing problems that may ensue in these cases dictate avoidance of internal undercuts in most MIM designs.
Where feasible, walls should be of uniform thickness throughout. Variations in thickness lead to distortion, internal stresses, voids, cracking, and sink marks. In addition, they cause non-uniform shrinkage, interfering with dimensional and tolerance control. Thicknesses in the range 1.3–6.3 mm (0.05–0.25 in.) are preferred, but exceptions in both directions are possible.
Figure 11 shows several common ways to modify a form to achieve more uniform wall thicknesses. Removing material to create uniformity in wall thickness offers the added advantage of saving material; given the high cost of the very fine metal powders used in MIM, this can be a significant economic benefit.