Sequentially Coupled Injection Molding to Stress Analysis

Injection molding is a manufacturing process for producing parts by injecting molten material into a mold. Injection molding can be performed with many types of materials, most commonly thermoplastic polymers. The material, sometimes mixed with chopped fiber, is injected into a mold cavity at high pressure, where it cools and hardens to a desired shape.

There are many design considerations and possibilities for the injection molding process. For fiber-reinforced plastics (FRPs), the gate location where the material is injected into the mold determines how fibers are aligned in the molded part. In a subsequent stress analysis with appropriate load and boundary conditions, you can study how the fiber orientation affects the strength of the material. The design of the molding machine can also result in different residual temperature and stress in the molded part when taken out of the mold cavity. Special considerations are required to minimize the warpage of the part due to the residual stress from the manufacturing process. The warpage analysis can also be performed in a subsequent stress analysis.

Injection molding results saved in the output database (.sim) file can be read into the subsequent stress analyses as predefined fields. Fiber dispersion results are stored as a second-order orientation tensor. If homogenized composite material properties are used in the subsequent analysis and if the properties are not isotropic, material orientations (usually principal directions of the orientation tensor) must be stored and read into the second analysis as distributions.

Stress and temperature also need to be stored in the output database (.sim) if they are to be read as predefined conditions.

Fiber orientation, temperature, and stress can be stored either at nodes, material points, or element centroids. When read as predefined fields, mapping is performed automatically if they are read at different locations or from a dissimilar mesh.

The orientation of the fiber mixed into the molded parts can significantly affect the mechanical response of the parts. If the composite material is modeled at the macrolevel with homogenized properties, the fiber orientations are read into the subsequent stress analysis as material orientations. If the composite material is modeled with multiscale material (see Multiscale Material Modeling), the fiber orientation tensor results are read into the stress analysis as part of the material definition. Homogenization is then performed during the stress analysis using the orientation tensor results.

The temperatures are read into the stress analysis as a predefined field. The temperature field is usually defined as initial conditions. Such predefined fields are always read intoAbaqus/Standard at the nodes. If temperatures are stored on a dissimilar mesh or at different locations such as material points or element centroids, mapping is performed automatically. Material properties such as elastic moduli and thermal expansion coefficients can be defined to depend on the temperature.

The stresses are read into the stress analysis as a predefined field. The stress field is usually defined as initial conditions. Such predefined fields are always read into Abaqus/Standard at the material points. If stresses are stored on a dissimilar mesh or at different locations such as nodes or element centroids, mapping is performed automatically. Residual stresses can result in different responses of the molded part under service load compared to the case when residual stresses are ignored.