Here, we introduce two analysis tools that are effective in solving problems with composite materials.
Multiscale.Sim: Prediction of material behavior based on a model of the material structure
Multiscale.Sim is an add-in tool for Ansys Software that was jointly developed by Nitto Boseki Co., Ltd., Quint Corporation, and Cybernet Systems Co.,Ltd. under the guidance of Professor Kenjiro Terada of Tohoku University. Its main purpose is to solve problems related to material modeling. By using the two functions of this analysis tool – homogenization analysis and localization analysis – it is possible to realize multiscale analysis in a way that considers the non-uniform material structure of composite materials.
Homogenization analysis - CAE as a material test device
Homogenization analysis can be used to acquire information to predict the physical properties of composite materials. Fig. 3 shows the flow of homogenization analysis. Here, an inhomogeneous microstructure of a composite material is prepared as an analysis model (hereinafter referred to as a micro model). In the case of a plain weave material, it supports the woven shape of the fiber bundle, and in the case of a particle-reinforced material, it supports the particle shape and the dispersion form. Fig. 4 shows a typical example of a micro model. Templates are provided for automatically creating models of some typical microstructures. By performing a virtual material test (called a numerical material test) using FEM on the created microstructure, it is possible to obtain the apparent material response (such as the stress-strain characteristics) of the micro model. At this time, it is assumed that the micro models are periodically arranged in an infinite direction, and an ideal single stress field can be easily applied to the single unit cell model. The big advantage is that difficult pure shear tests can also easily be applied to simulations during real material tests. The material constants can be obtained by fitting the apparent material response thus acquired to the Ansys Mechanical anisotropic material model. While the fitting function for anisotropic material models is not provided as a standard function in Ansys Software, it is implemented as a function in Multiscale.Sim. Material constants can be easily identified if material test data for each direction is available.
The information obtained by numerical material testing does not include only the apparent material response and the material constants. Since the microstructural inhomogeneities are actually modeled, the stress and strain distributions in the material can also be evaluated. Identification of the fracture mechanism is extremely important information for material design, but it can be said that it was obtained for the first time only by introducing this analysis method.
Fig. 5 shows the results of a numerical material test performed by applying a material model of a fracture in the resin.
You can see that the cracks (transverse cracks) that occurred inside the resin are proceeding while bypassing the fibers.
Fig. 4 - Example of micro-model shapes
Fig. 5 - Example of a numerical material test of a fracture
Localization analysis - CAE as a microscope
If the material constants for fractures in the composite material can be obtained using the homogenization method above, it is possible to estimate the occurrence of fractures in the actual structure, as well as various general fracture areas using different general-purpose CAE tools such as Ansys Software. However, it is not possible to estimate the specific factors of the fracture when analyzing a model in which an originally inhomogeneous material is replaced by a homogeneous material. This problem can be resolved using Multiscale.Sim’s localization analysis feature.
The localization analysis function is introduced using a simple analysis example. Fig. 6 shows an example of a three-point bending test on a composite material. The sample is a unidirectional reinforced material in which the fibers are oriented in the longitudinal direction, and for which the fracture strength was acquired by homogenization analysis. It can be confirmed that the fractured regions shown in red are present on the bottom and top surfaces, as well as on the midsurface of the sample. Localization analysis can be used to zoom in on parts of a homogenized analysis model to evaluate the material structure scale results.
Localization point 1 in Fig. 6 shows the localization result on the bottom surface of the sample, and localization point 2 shows the localization result on the mid-surface. Since the bottom surface of the sample exhibits a deformation mode in which it is pulled in the direction of the fiber, the fibers with a lesser rupture strain than the resin will break first, which results in a fracture of the composite material. On the other hand, since the shear deformation mode is dominant on the mid-surface, the fibers are hardly affected by the stress, and it can be confirmed that the fracture occurs due to the debonding of the fibers and the resin, and due to the expansion of the crack inside the resin. Identifying the cause of fractures using conventional CAE is difficult, therefore, and is one of the reasons why using CAE for the material design of composite materials is considered difficult.
The localization analysis function may, at first glance, seem similar to a sub modeling approach, but the major difference is that the two models being integrated have different size ratios. In the submodeling approach, the two models to be integrated must be of equal size, whereas in localization analysis, the size ratio is expected to be extremely large (see Fig. 7).
Fig. 6 - Example of fracture mode observation based on localization analysis
Fig. 7 - Differences between sub-modeling and localization analysis
Ansys Composite PrepPost: FE modeling of laminated structures
Ansys Composite PrepPost (hereinafter referred to as ACP) is a tool developed to efficiently implement the pre- and post-processing that is unique to composite materials. In this section, we introduce the pre-processing functions for the definition of laminated structures and the definition of the fiber orientation.
Fig. 8 - Differences between the conventional method for defining laminated structures and the ACP method
Definition of the laminated structure: From the definition method of the element unit to the definition method of the layer unit
The FEM analysis tool in Ansys Mechanical has always provided functions for defining laminated structures. However, it has certainly not been the most suitable modeling technique for defining the complex and large-scale laminated structures of actual structures in recent years. Fig. 8 shows the differences between these conventional tools and the ACP laminated structure modeling approach.
In conventional modeling methods, laminated structures are defined on an element (or segmented surface) basis. When the laminated structure of each region is different, as shown in Fig. 8, it is necessary to define the number of layers in each region, the material constants for each layer, and the principal axis of each layer. On the other hand, the definition method in ACP involves specifying the layer units, and it is possible to stack arbitrary materials by specifying the region sequentially from the bottom surface. This procedure is similar to the creation process of the actual material, so the modeling can be performed intuitively, and the more complex the model becomes, the more efficiently the process can be applied with fewer menu operations compared to conventional approaches.
These differences in specifications have a significant impact not only when defining the laminate structure, but also when making modifications. The composite material design process often involves trial and error tasks such as deleting certain layers, changing the material of layers, and interchanging the order of laminates. Even when such modifications are performed, operational efficiency is greatly improved by the ACP definition specifications. These sophisticated approaches to laminated structures improve work efficiency and play an important role in reducing the probability of human error.
Fig. 9 - Differences between the conventional method and the ACP method for defining a material’s principal axis
Definition of the oriented direction: Departure from the definition method based on the local coordinate system
In an anisotropic composite material, the orientation of the material’s major axis must be defined. The conventional Ansys Mechanical definition method for a material’s principal axis is to create a coordinate system that specifies its orientation and which references the coordinate system in any family of elements. In the case of a model in which the material’s principal axis is curved, a technique of arranging a cylindrical coordinate system at the center of the curvature and aligning the material’s principal axis in the angular direction was used. While this can be very effective for simple, cylindrical models, it is necessary to create a large number of cylindrical coordinates when applying it to structures with complex curved surfaces, which is work intensive.
On the other hand, the methods of defining the material’s principal axis by ACP are extremely diverse, and were devised to handle the various complex geometric shapes found in composite materials.
Fig. 9 is an example of a partial definition. It is also possible to define the material’s principal axis along the lines that configure the model. This is an extremely useful tool for models with complex shapes. The drape simulation function in ACP enables engineers to predict changes in fiber orientation once a flat composite material is shaped on a curved surface; these results can also be used as the material’s principal axis for structural analysis.