In this chapter, two fiber arrangements, i.e. square edge packing (SEP) array and square diagonal packing (SDP) array, were adopted to investigate the fiber arrangement effects on nonlinear behavior of off-axis fiber composites by using the commercial finite element program ANSYS. The procedure for finite element analysis will be addressed in this section, and the associated results will be demonstrated in chapter 6 together with the numerical results obtained from the square fiber model and the generalized method of cells to investigate the fiber shape and fiber arrangement effects.
5.1 Finite Element Approach
The methodology about how to establish a finite element model for unidirectional composites subjected to off-axis loadings was basically coming from the paper published by Zhu and Sun [24]. Fig. 5.1 shows a 3-D RVE for the square diagonal packing (SDP) array employed in the finite element analysis, and it is noted that because of symmetry, only one quarter of the RVE was considered. The associated meshes generated automatically from ANSYS mesh generator for the RVE are shown in Figs. 5.2(a)-(b). The element type used in this study is solid 185.
Since the quantities, such as stress, strain and displacement, are independent of the x1-axis, there is only one single layer of elements established in the fiber direction [24]. It was noted that in Fig 5.1, all stresses were shown in the positive direction, and the relation between the applied stresses in the loading coordinate system and those in the material principle coordinate system is converted through the following translation law
θ θ σ
−
= σ
θ σ
= σ
θ σ
= σ
cos sin sin cos
x 12
2 x 22
x 2 11
(5.1.1)
where σ are the stresses in the material principle coordinate system, θ is the ij off-axis angle with respect to the loading direction and σ is the applied uniaxial x stress. In the FEM analysis, the fiber was assumed to be an orthotropic elastic material with the material properties as shown in Table 2. While, the matrix is assuming to be elastic-plastic obeying the J2 flow rule. The assumed stress – strain curve of the matrix shown in Fig. 5.3 was selected for FEM analysis. This constitutive curve was imported into ANSYS through the commanding process,
“Main Menu” > “Preprocessor” > “Material Props” > “Material Models” >
“Structural” > “Nonlinear” > “Inelastic” > “Rate Independent” > “Isotropic Hardening Plasticity” > “Mises Plasticity” > “Nonlinear”. Then, four coefficients of a nonlinear potential function have to be determined to characterize the stress and plastic strain curve. This function is
) e 1 ( R R
k+ 0εp+ ∞ − −bεp
=
σ (5.1.2)
where k is the yield stress, R0 and R∞ are parameters and their physical meanings are shown in the ANSYS user manual [28]. Basically, only the variable b needs to be evaluated by try-and-error manner and the others can be determined directly from the given stress – plastic strain curve. The matrix properties were also listed in Table 2.
After material properties had been given, the boundary conditions were applied on the RVE shown in Fig. 5.1 to satisfy the periodicity condition when the material subjected to off-axis loading.
On 0x1= and x1= faces a
( ) ( )
periodic boundary conditions. Note that the first relation in eqn (5.1.3) makes it possible for the RVE to undergo an extension in the x1 direction but not to affects the periodicity.where a1 and a2 represent any two different points with other two identical coordinates, and the first and the second relations of eqn (5.1.4) describe geometric symmetry and periodicity, respectively. Moreover, the third and the fourth relations of eqn (5.1.4) were employed to keep all nodes on faces x2 = or 0 x2 = with the same height xa 3
without relative motion. It was noted that the third and the forth relations in eqn (5.1.4) were not applied in the current analysis since there was only single layer of element existing in the RVE and these two relations can also be covered by the third relation in eqn (5.1.3).
On 0x3 = and x3 = faces a
which implies similar meanings as eqn (5.1.4) and the third and the forth relations in eqn (5.1.5) are involved by the second relation in eqn (5.1.3). To avoid the rigid body translation, an additional displacement constraint was imposed in the x1
direction, i.e.
(
0,0,0)
0u = (5.1.6) In order to implement the boundary conditions, three ANSYS options “CP”,
“CE” and “D” were applied. “CP” option lets a set of nodes possess the same degree of freedom. Therefore, the second and the third relations in eqn (5.1.3) and the second relation in eqns (5.1.4) and (5.1.5) are established by using this command.
“CE” option lets the degree of freedoms of a set of nodes obey desired constraint equations. The first relation in eqn (5.1.3) can be expanded as
a
where the subscript 1 to N denotes N sets of corresponding nodes with the same x2
and x3 coordinates respectively on x1= and 0 x1= faces and eqn (5.1.7) can be a further decomposed as
a
Obviously, there are N-1 independent constraint equations existing in the RVE and can be built up using “CE” command. The latest option “D” can assign a fixed displacement value on desired nodes, so the displacements equal to zero in the boundary conditions can be carried out. After the boundary conditions were appropriately defined, the stresses evaluated from eqn (5.1.1) at material principle coordinate system were multiplied by the loading surface area to obtain external forces. Shear forces on x1 = and 0 x2 = faces and all normal forces were a placed at single node on associated loading surface since the boundary conditions had been appropriately defined. But the shear forces at x2 = and 0 x2 = must be a
distributed to every node through the element shape function provided by user manual [29] to ensure the nodal force being consistent with the distributed loading. All forces were divided into several tiny steps and implemented gradually by using the following commands
“Main Menu” > “Solution” > “Analysis Type” > “Sol’n Controls”
By collecting element strains at each load step, the average strain of the RVE can be evaluated by taking an average from all element strains, i.e.
∑
=ε
=
ε M
1 i
i iV V
1 (5.1.9)
where M is the total number of elements, ε and ε are respectively to average i strain and element strain, and V and V represent the volume of RVE and the i element volume, respectively.