# Mesh-objective two-scale finite element analysis of damage and failure in ceramic matrix composites

- Pascal Meyer
^{1}and - Anthony M Waas
^{1}Email author

**4**:5

**DOI: **10.1186/s40192-015-0034-z

© Meyer and Waas. 2015

**Received: **14 December 2014

**Accepted: **3 March 2015

**Published: **26 March 2015

## Abstract

A mesh-objective two-scale finite element approach for analyzing damage and failure of fiber-reinforced ceramic matrix composites is presented here. The commercial finite element software suite Abaqus is used to generate macroscopic models, e.g., structural-level components or parts of ceramic matrix composites (CMCs), coupled with a second finite element code which pertains to the sub-scale at the fiber-matrix interface level, which is integrated seamlessly using user-generated subroutines and referred to as the integrated finite element method (IFEM). IFEM calculates the reaction of a microstructural sub-scale model that consists of a representative volume element (RVE) which includes all constituents of the actual material, e.g., fiber, matrix, and fiber/matrix interfaces, details of packing, and nonuniformities in properties. The energy-based crack band theory (CBT) is implemented within IFEM’s sub-scale constitutive laws to predict micro-cracking in all constituents included in the model. The communication between the micro- and macro-scale is achieved through the exchange of strain, stress, and stiffness tensors. Important failure parameters, e.g., crack path and proportional limit, are part of the solution and predicted with a high level of accuracy. Numerical predictions are validated against experimental results.

### Keywords

Multi-scale analysis Crack band Ceramic matrix composites Finite elements## Background

Polymer matrix composites (PMCs) and ceramic matrix composites (CMCs) are increasingly used in a wide range of applications. With the demand for lighter and more versatile structural components, the need to understand interactive and complex failure mechanisms in these materials has grown and has become the focus of many research projects. The deformation response, subsequent damage development, and failure of these multi-constituent materials are dependent on microstructural details such as variations in fiber packing arrangement, properties at fiber-matrix interfaces, and interactions between neighboring fibers. This dependency of failure modes on the microstructure is well known for composite materials which led to the development of numerous homogenized theories. Kanoute et al. [1] reviewed various multi-scale methods for mechanical and thermomechanical responses of composites. Heinrich and Waas [2] utilized the smeared crack approach to describe the post-peak softening in laminated materials. They predicted the cracking behavior of an open-hole tensile specimen and recorded crack directions for various fiber angles. Accurate numerical predictions for layered, fibrous materials are inherently difficult due to the intricate mechanisms that tie global component failure to microstructural degradation. Modeling strategies based on homogenized material properties neglect the importance of the physical behavior at the microstructural level, and thus, homogenized models fail to predict experimentally observed critical parameters accurately. Those include, e.g., maximum load, strain to failure, crack spacing, and other salient features. Oftentimes, the material orientation is used as a guide for directing failure. This might lead to erroneous crack paths for materials with similar fiber and matrix properties such as CMCs. Hence, multi-scale methods have become the focus of many research papers in recent years. These models dehomogenize the strain and stress state for each constituent. Typically, a representative volume element (RVE) that preserves the microstructural dimensions is identified. Yuan and Fish [3] developed a computational homogenization approach for linear and nonlinear solid mechanics problems. In this work, two commercial solvers were bridged by a python code. The authors showed that linear problems could be accurately modeled. Ghosh et al. [4] introduced a multi-scale methodology based on the Voronoi cell finite element method (VCFEM). Material coefficients are generated by VCFEM and used in a global finite element model. Nonlinearities can be included in the finite element formulation of the Voronoi cells. Key et al. [5] used multi-continuum technology in a multi-scale simulation to analyze the separation of rib to skin interfaces. Multi-continuum theory decomposes the stress and strain field for each constituent using volume averages. This method is numerically fast with the cost of inaccuracy particularly for components that experience high shear. Bacarreza et al. [6] developed a semi-analytical homogenization method to model damage in woven composite materials. Effective material properties are derived and used in a progressive damage analysis. Nonlocal or gradient failure theories assume that the post-peak stress-strain behavior of an element is influenced by the field gradients within a characteristic radius around the element. Jirásek [7] analyzed analytical and numerical solutions of simple one-dimensional localization problems. Aboudi et al. [8] introduced the generalized method of cells (GMC), a semi-analytical method, which discretized the microstructure with rectangular subcells. Pineda et al. [9] achieved mesh objectivity with a thermodynamics-based approach within GMC as well as high-fidelity generalized method of cells (HFGM). Multi-scaling methods often suffer from lower computational efficiency compared to homogenized models. This disadvantage can usually be overcome by using the multi-scale method in areas where microstructural failure is to be expected, e.g., at stress concentrators (notches, etc.). Homogenized element stress-strain relation can be utilized in regions of low failure probability. In recent years, significant improvements have been made in terms of fidelity and computational efficiency [10-13].

In the present paper, the commercial finite element software suite Abaqus is used to generate lamina-level structural model of a ceramic matrix composite (CMC). A second sub-scale microstructural model has been developed and fully integrated with the main Abaqus solver through a user material subroutine (UMAT). Integrated finite element method (IFEM) calculates the reaction of a microstructural model to an imposed displacement field. The microstructural model consists of a RVE which includes all constituents of the real material, e.g., fiber, matrix, and fiber/matrix interfaces, details of packing, and nonuniformities in properties. The energy-based crack band theory (CBT), first introduced by Baz̆ant [14], is implemented within IFEM constitutive laws to predict micro-cracking in all constituents that are included in the micromechanics model. The communication between the micro- and macro-scale is achieved through the exchange of strain, stress, and stiffness tensors. Important failure parameters, e.g., crack path and proportional limit, are part of the solution and predicted with a high level of accuracy. Numerical predictions are validated against experimental results.

## Methods

### Representative volume element modeling in a multi-scale framework

*Abaqus User Manual*[15]), are readily accessible through the computer language Fortran. The UMAT subroutine is called at each integration point of the Abaqus model for each element within an element set that has been defined with a user material. In a multi-scale scheme, information is exchanged between multiple length and/or time scales. Here, the focus lies on a concurrent technique that exchanges essential stiffness, current stress, and strain information between two scales: the lamina-level simulation and a microstructure-level simulation. This technique employs the finite element method (FEM) at both the fiber/matrix scale and the macroscopic, e.g., lamina-level scale. The constitutive response at the macro-scale is purely dictated by the fiber/matrix-level model. Localization techniques, as discussed below and referenced in Equation 10, are employed for transforming displacement fields from a global state to a local state. Back-transformation is achieved through a homogenization step according to Equation 1. The concurrent information exchange between the scales is shown in Figure 1. A strain field is passed to the user-defined material definition. Stress and stiffness tensors are calculated and passed back to Abaqus.

*X*

_{ i },

*Y*

_{ i },

*Z*

_{ i }) of the nodes. Each node

*i*has three degrees of freedom (

*u*

_{ i },

*v*

_{ i },

*w*

_{ i }), and the nodal degree of freedom vector

**q**can be written as:

*X*,

*Y*,

*Z*) can be interpolated by the nodal displacements:

*X*,

*Y*,

*Z*) to isoparametric coordinates can be written as:

Implementing IFEM in Fortran was essential for a highly efficient multi-scale framework. It allows the macroscopic model to be run in a cluster environment and hence solving multiple material integration points simultaneously.

### Dehomogenization of displacement field with periodic boundary conditions

*ε*

_{ ij }are the macroscopic strains passed down from Abaqus at each integration point.

*L*

_{1},

*L*

_{2}, and

*L*

_{3}are the corresponding side lengths of the RVE in

*x*-,

*y*-, and

*z*-directions as shown in Figure 3a. A sketch of the periodically deformed RVE is shown in Figure 3b.

where *Q*
_{1} and *Q*
_{2} are the degrees of freedom (dofs) to be coupled and *β*
_{0} the applied displacement between *Q*
_{1} and *Q*
_{2}. *β*
_{1} and *β*
_{2} are integer parameters with a value of 1 and −1, respectively.

### Numerical calculation of Jacobian matrix for implicit simulations

*δ*

*Δ*

*σ*∖

*δ*

*Δ*

*ε*has to be passed back at the end of the user-defined material law [15]. In case of the undamaged subcell, the Jacobian matrix is constant and calculated only once for each RVE prior to the multi-scale simulation. It is stored in a Fortran-compiled file and can be called at any time during the IFEM simulation. In case of damage in the subcell model, a new Jacobian matrix should be calculated to guarantee fast convergence of the macroscopic model. It should be noted that a constant Jacobian matrix might lead to convergence but at the cost of loosing a quadratic convergence rate during the Newton-Raphson method used in the Abaqus FEM solution process. Since the sub-scale includes details of the microstructure, failure mechanisms, and interactions among these, the sub-scale generated material law to be used at the macro-scale is embedded in details of the Jacobian matrix, denoted in Abaqus UMATs as DDSDDE, and this is determined numerically:

*S*

_{1212}:

This scheme requires additional numerical effort on the micro-scale model but ultimately leads to a reduction of time required to solve the macroscopic finite element problem due to faster convergence of the Abaqus model.

### RVE characteristics

The choice of the three-phase RVEs, including fiber, interface, and matrix, created to represent the microstructure of ceramic matrix composites (CMCs) is based on observations from experiment; however, the approach developed here is not limited to these types of materials. Two-phase (polymer matrix composites) or one-phase material (pure matrix) RVEs for example are possible and can be used. The objective here is to demonstrate that RVE features are an integral part of developing physics-based multi-scale strategies that fall within the realm of predictive science.

## Crack band failure model

*ε*

^{′}is the maximum principle strain and

*ε*

_{cr}is the strain to failure of the material and assumed to be a material parameter. The crack band failure method falls into the category of approaches that smear the effect of a sharp crack over a finite volume, leading to a practically useful, yet robust approach to preserve mesh objectivity. This is because the characteristic material length is embedded within the formulation of the crack band model. Thus, cracks are not explicitly modeled within an element but rather incorporated in the element constitutive law. In this work, it is assumed that after crack growth has been initiated the stiffness of the element is reduced according to a traction separation law that dissipates energy while preserving the energy release rate. In most numerical applications, the current secant stiffness is chosen such that the tractions will follow the details of the traction-separation law shown in Figure 5, where

*σ*is the normal traction and

*δ*is the crack opening. In this study, a triangular traction-separation law is employed. The area under the mode I traction-separation law corresponds to the mode I fracture toughness (

*G*

_{ IC }) of the material, while the energy release rate

*G*

_{ I }is defined as:

*ε*

_{cont}represents the continuum strain of the element and

*ε*

_{cr}represents the additional smeared strain which results due to cracking. One can rewrite Equation 16 for a linear elastic isotropic material in the principal frame as:

*σ*

_{11}and

*ε*

_{11}are written in the local crack coordinate system.

*E*denotes the undamaged Young’s modulus in the principle frame. A fracture scalar variable

*D*(0≤

*D*≤1) is introduced which corresponds to zero if damage has not initiated.

*D*is set to one if

*ε*

_{11}exceeds

*ε*

_{ f }, when the element has failed catastrophically and no load can be transferred normal to the crack direction.

*D*can be determined from the stress-strain relation in Figure 6:

*D*can be calculated as:

*x*-,

*y*-,

*z*-coordinate system:

*T*is given as

where *n*
_{1},*n*
_{2},*n*
_{3} are the principal strain directions and *e*
_{1},*e*
_{2},*e*
_{3} are the unit basis vectors.

### Characteristic length scale

*h*, which is the length over which the crack opening is ‘smeared’ in order to define the effective strain due to cracking, as shown in Figure 6. Independent of the element size, the critical energy release rate, G

_{ IC }, which is assumed to be a material constant associated with damage in a particular finite element needs to be preserved. Satisfying the restriction of the mesh size guaranties a mesh-objective simulation. As can be seen in Figure 6, the strain softening modulus

*E*

_{ t }must be negative. Therefore, the following equation holds true:

*C*

_{ f }can be replaced by \(\sigma _{\text {cr}}^{0} / \epsilon {f,}\) and thus, Equation 28 can be rewritten as:

As Baz̆ant [14] noted, *h* should be smaller but at least half of that value in practical FEM problems. The limiting case is given by \(E_{t}^{-1}=0\) which corresponds to a sudden drop in the stress-strain response. Since *h* is the distance within the element that is perpendicular to the cracking due to damage, the effective post-peak response of different element sizes will be different, yet *G*
_{
IC
} is held fixed, leading to a mesh-objective formulation.

## Results and discussion

### Notched CMC tension simulation

_{2S }and model details are given in Figure 7. The gauge section width is 10.16 mm, the grip section width is 12.7 mm, and the overall length is 152.4 mm.

It further shows the boundary conditions and loading on the model. The edges *X*
_{0} and *X*
_{1} are subjected to a displacement in negative and positive *x*-direction, respectively. The corner *A* at *X*
_{0} is prevented from moving in the *y*- and *z*-directions to avoid rigid body movements. All models were meshed with three-dimensional elements (C3D8 Abaqus v6.11 [15]) with one element per layer through the thickness. Important to note here is that like any real specimen no strict symmetry in geometry with respect to the center line of the notch exists which leads to unsymmetric failure as described below. In order to break symmetry in the model, six geometrically different RVEs were randomly distributed throughout the model. The RVEs include one, two, or three fibers each. One RVE was modeled with touching fibers. Although the RVEs are comparable in elastic properties, e.g., pre-peak behavior, differences exist for the post-peak regime. RVEs with clustering fibers exhibit higher stress concentrations and tend to initiate damage at a lower load stage compared to other RVEs.

*%*from 0.98 predicted with the coarse mesh (Figure 9a) to 0.95 as predicted by the discretization size used in mesh III (Figure 9c). The normalized strain at ultimate stress changes by 3.1

*%*from 1.046 predicted with mesh I to 1.079 as predicted by the fine structured mesh.

*X*

_{0}and

*X*

_{1}are subjected to a displacement in negative and positive

*x*-direction, respectively. Similar to the results from a cross-ply laminate, two cracks initiate at the notch. However, the angle spanned between the cracks is larger. These predictions are very consistent with experimental observations shown in Figure 12. Comparable to the cross-ply laminate, the cracks turn perpendicular to the loading direction further away from the notch. Eventually, one crack propagates faster which defines the final crack path.

For both laminates, crack initiation and propagation were predicted accurately. No change to the input of the IFEM model was required. This demonstrates the strength of the IFEM two-scale approach. The fact that the experimentally observed physical behavior is accurately captured with sufficient detail at the sub-scale model lends confidence to its use for predictive studies.

### Smooth bar CMC tension simulation

_{2S }) cross-ply smooth bar ceramic matrix composite specimen. The specimen was 152.4 mm long, 10.16 mm wide at the gauge section, and 12.7 mm wide at the grip section. Figure 13 depicts the boundary conditions. The left vertical edge was simply supported with a displacement restriction in the

*x*-direction. The right edge was displaced in the

*x*-direction by 0.1 mm. As before, nine randomly distributed RVEs containing five fibers each were used in order to more accurately represent the real microstructure. Three of these RVEs contained touching fibers which is often observed in this type of CMCs.

## Conclusions

In this work, a two-scale finite element approach has been developed and fully integrated within Abaqus’ user material subroutine. This enables a computationally efficient tie between a component-level model to a fiber/matrix-level model. It is shown that information exchange between these two scales through stiffness and stress transfers can capture damage on the structural-level model with effects of failure, damage, and mechanism interaction, implemented on the fiber/matrix-level model. A crack band model for the 3D-IFEM method has been developed. Numerical predictions were verified against experimental results. Good agreement was achieved for notched tensile specimens and smooth bar fibrous ceramic matrix composites. The predicted failure modes obtained with 3D-IFEM matched well with physical failure modes observed from experiments.

It was shown that the proposed failure scheme is well suited in a multi-scale framework to model progressive failure. Mesh objectivity on the RVE scale was achieved through introduction of a characteristic element length. Effects of anomalies of the fiber packing were captured by resolving stress and strain fields for each constituent and using randomly distributed RVEs throughout the lamina-level model. Nonsymmetric failure modes as shown for the notched specimen were predicted accurately with this technique. However, future work should more rigorously study the effect of property-based ‘randomness’, e.g., varying matrix strength and fracture toughness within a RVE. This effect could be most important for CMC specimens which lack a geometric stress concentration. Future work should also include a study on the effects of the amount of detail included in a RVE. Multi-scale methods need to find a healthy mean between details included in a RVE, time required to execute a simulation and accuracy of the predicted failure modes.

## Declarations

### Acknowledgements

The authors are grateful to the Aerospace Engineering Department at the University of Michigan for the continued support of the research studies presented here.

## Authors’ Affiliations

## References

- Kanoute P, Boso DP, Chaboche JL, Schrefler BA (2009) Multiscale methods for composites: a review. Arch Comput Methods Eng 16: 31–75.View ArticleGoogle Scholar
- Heinrich C, Waas AM (2013) Investigation of progressive damage and fracture in laminated composites using the smeared crack approach. CMC-Computers Mater Continua 35: 155–181.Google Scholar
- Yuan Z, Fish J (2008) Towards realization of computational homogenization in practice. IJNME 73: 361–380.View ArticleGoogle Scholar
- Ghosh S, Kyunghoon L, Moorthy S (1995) Multiple scale analysis of heterogeneous elastic structures using homogenization theory and voronoi cell finite element method. Int J Solids Struct 32: 27–62.View ArticleGoogle Scholar
- Key CT, Garnich MR, Hansen AC (2004) Progressive failure predictions for rib-stiffened panels based on multicontinuum technology. Composite Struct 65: 357–366.View ArticleGoogle Scholar
- Bacarreza O, Aliabadi MH, Apicella A (2012) Multi-scale failure analysis of plain-woven composites. J Strain Anal 47: 379–388.View ArticleGoogle Scholar
- Jirásek M (1998) Nonlocal models for damage and fracture: comparison of approaches. Int J Solids Struct 35: 4133–4145.View ArticleGoogle Scholar
- Aboudi J, Pindera MJ, Arnold SM (2001) Linear thermoelastic higher-order theory for periodic multiphase materials. J Appl Mech 68: 697–707.View ArticleGoogle Scholar
- Pineda EJ, Bednarcyk BA, Waas AM, Arnold SM (2013) Progressive failure of a unidirectional fiber-reinforced composite using the method of cells: discretization objective computational results. IJSS 50: 1203–1216.Google Scholar
- Feyel F, Chaboche JL (2000) Fe
^{2}multiscale approach for modelling the elastoviscoplastic behaviour of long fibre SiC/Ti composite materials. Comput Methods Appl Mech Eng 183: 309–330.View ArticleGoogle Scholar - Ladevèze P, Nouy A (2003) On a multiscale computational strategy with time and space homogenization for structural mechanics. Comput Methods Appl Mech Eng 192: 3061–3087.View ArticleGoogle Scholar
- Michel JC, Moulinec H, Suquet P (1999) Effective properties of composite materials with periodic microstructure: a computational approach. Comput Methods Appl Mech Eng 172: 109–143.View ArticleGoogle Scholar
- Smit RJM, Brekelmans WAM, Meijer JEH (1998) Prediction of the mechanical behavior of nonlinear heterogeneous systems by multi-level finite element modeling. Comput Methods Appl Mech Eng 155: 181–192.View ArticleGoogle Scholar
- Baz̆ant ZP (1983) Crack band theory for fracture of concrete. Mater Struct 16: 155–177.Google Scholar
- Abaqus (2008) Abaqus User’s Manual. Dassault Systèmes Simulia Corp, Providence, RI. version 6.11 edition.Google Scholar
- Chandrupatla TR, Belegundu AD (2002) Introduction to finite elements in engineering. Pearson Education Inc., Upper Saddle River, NJ.Google Scholar
- Heinrich C, Aldridge M, Kieffer J, Waas AM, Shahwan K (2012) The influence of the representative volume element (RVE) size on the homogenized response of cured fiber composites. Model Simul Mater Sci Eng 20. doi:10.1088/0965-0393/20/7/075007.
- Xia Z, Zhang Y, Ellyin F (2003) A unified periodical boundary conditions for representative volume elements of composites and applications. Int J Solids Struct 40: 1907–1921.View ArticleGoogle Scholar
- Corman GS, Luthra KL (2005) Silicon melt infiltrated ceramic composites (HiPerComp) In: Handbook of ceramic composites, 99–115.. Kluwer Academic Publisher, Boston, MA.View ArticleGoogle Scholar
- Pineda EJ, Waas AM (2012) Modelling progressive failure of fibre reinforced laminated composites: mesh objective calculations. Aeronaut J 116: 1221–1246.View ArticleGoogle Scholar
- Baz̆ant ZP, Cedolin L (1991) Stability of structures: elastic, inelastic, fracture and damage theories. Oxford University Press, New York.Google Scholar
- Pineda EJ, Bednarcyk BA, Waas AM, Arnold SM (2013) On multiscale modeling using the generalized method of cells: preserving energy dissipation across disparate length scales. Comput Mater Continua 35: 119–154.Google Scholar

## Copyright

This is an Open Access article distributed under the terms of the Creative Commons Attribution License (http://creativecommons.org/licenses/by/4.0), which permits unrestricted use, distribution, and reproduction in any medium, provided the original work is properly credited.