4. Numerical models for the study of mechanical properties of long fiberreinforced composites

Measurement and analytical models of long fiber-reinforced composite structures designed to study mechanical properties are generally able to provide only limited information. This is due to the fact that the measurements are limited by the possibilities of positioning of the sensors and also by the fact that some properties cannot be measured well (e.g., the distribution of the main stress and deformation in the composite structure). The knowledge of the distribution of the main stresses and deformations in the structure is important for assessing how the structure is changed and under which stress. In this case, the corresponding model simulation using numeric methods represents a significant support for the development. Very suitable is to build model simulation in finite element method (FEM), but other numerical methods, such as discrete element (DEM), boundary element (BEM) or finite volume method (FVM) method, are also available. The mechanical loading of composite causes many different processes in the inner structure that varies with the actual deformation. Therefore, it is necessary to simplify or neglect some characteristic features in modeling of such structures. A major problem of mechanical properties modeling of composite structures is in particular the description of the principal stresses in short time Δt ¼ tiþ<sup>1</sup> � ti. The solution of problem of composite with boundary conditions under tensile loading lies not only in the specification of the correct boundary conditions and material properties but also in the design of the proposed finite element mesh. The FEM programs are currently very sophisticated and allow the solution of a continuous problem transform into a final solution where the corresponding geometric simple subareas (finite elements) can be designed in the preprocessor. Let Ω ⊂ ℜ<sup>3</sup> is the continuous area of the three-dimensional space in which the problem is solved. Its borders will be denoted Γ, where Γis Lipschitz border and let the approximation of the selected base functions is derived above each finite element of length lelement, because any continuous function can be represented by a linear combination of algebraic polynomials converging to a continuous solution, that is, limlelement!<sup>0</sup> ! 1: Thus, the FEM method can be understood as a special type of variation method by using the mathematical description of the problem solution. The current commercial software and FEM programs (e.g., Ansys, Abaqus, Permas, LS-Dyna, Marc, PAM CRASH) allow to assemble and subsequently solve a series of problems with nonlinear materials not only with elastic but also plastic behavior corresponding to the properties of the long fiber-reinforced composite.

deformations, and so on. Both ways can be also combined. It is mixed boundary conditions, as shown by Li [25]. Boundary and initial conditions for the model were made by the boundary conditions of the second type. One side of the sample was fixed against the displacement and rotation of nodes Ui ¼ Ri ¼ 0 in all directions (layout), and the opposite side of the edge of the sample was fixed identically; only in X direction, the movement was allowed, whereas Ux <sup>¼</sup> 1 mm that corresponds to the deformation <sup>ε</sup><sup>x</sup> <sup>¼</sup> <sup>1</sup> %. The strain rate was 2 mm.min�<sup>1</sup>

FEM Analysis of Mechanical and Structural Properties of Long Fiber-Reinforced Composites

http://dx.doi.org/10.5772/intechopen.71881

4.1.2. Assembling of extended continuous composite model of long fiber-reinforced composite

The second numerical FEM model, which was created in the concept of structure unit, is formed from three components: fiber matrix—the interfacial interface, where the microscopic dimensions of such a model are closer to the more real composite. Such a model can be created from a structural unit with the 1, 2,…, n fibers, wherein the volume geometric configuration (e.g., structural unit is a cube, cuboid, sphere) can affect the volumetric quantity of fibers and a

example of the structural unit of the cuboid, which is shown in the section in Figure 6. The structural unit consists of six fibers represented by circles with the same spacing mi, which are

Figure 5. Continuum FEM model of the composite reinforced with long fibers with defined boundary and initial

Figure 6. The influence of fiber spacing in the structural unit on V<sup>f</sup> fiber volume ratio.

, Vm, as shown by Neckář [12]. The change in volume ratio V<sup>f</sup> can be given on the

The boundary conditions are shown in Figure 5.

matrix V<sup>f</sup>

conditions.

.

13

### 4.1. FEM simulation of mechanical properties of long fiber-reinforced composite

Model simulations in FEM were performed for different combinations of reinforcement arrangements of long fiber-reinforced composites, which are important for comparison with experiments and analytical relationships. This gives the material properties for numerical simulation of the strength characteristics of whole frames.

This chapter describes the creation of two numerical models and their comparison:


The simulations were performed for a complete assessment of the mechanical properties σ11, σ22, ε11, ε22, γ12, γ<sup>23</sup> and elastic constants E11, E22, G12, G23, ν12, ν23, whereas also information explaining the shape changes of the samples observed especially during tensile stress. Model simulations were performed in the following steps:


### 4.1.1. Assembling of continuum of the long fiber-reinforced composite model

The FEM model was created in the concept of coherent continuum consisting of a surface geometry corresponding to the test sample with length L = 100 mm, width b = 20 mm, and thickness h = 1.7 mm. The finite element mesh of the numerical model was created from SHELL elements (2D elements) with a constant element size of 2 mm. The boundary conditions affecting the magnitude of the displacements and stress can be defined in two ways, that is, the boundary conditions of the first and second types. The first way is to determine the displacement and stress distributions if force conditions are known, that is, volume forces, surface forces, and nodal loads. The other way is to determine the displacement and tension distribution if the geometric conditions are known, that is, the size of node displacement, the deformations, and so on. Both ways can be also combined. It is mixed boundary conditions, as shown by Li [25]. Boundary and initial conditions for the model were made by the boundary conditions of the second type. One side of the sample was fixed against the displacement and rotation of nodes Ui ¼ Ri ¼ 0 in all directions (layout), and the opposite side of the edge of the sample was fixed identically; only in X direction, the movement was allowed, whereas Ux <sup>¼</sup> 1 mm that corresponds to the deformation <sup>ε</sup><sup>x</sup> <sup>¼</sup> <sup>1</sup> %. The strain rate was 2 mm.min�<sup>1</sup> . The boundary conditions are shown in Figure 5.

### 4.1.2. Assembling of extended continuous composite model of long fiber-reinforced composite

will be denoted Γ, where Γis Lipschitz border and let the approximation of the selected base functions is derived above each finite element of length lelement, because any continuous function can be represented by a linear combination of algebraic polynomials converging to a continuous solution, that is, limlelement!<sup>0</sup> ! 1: Thus, the FEM method can be understood as a special type of variation method by using the mathematical description of the problem solution. The current commercial software and FEM programs (e.g., Ansys, Abaqus, Permas, LS-Dyna, Marc, PAM CRASH) allow to assemble and subsequently solve a series of problems with nonlinear materials not only with elastic but also plastic behavior corresponding to the

4.1. FEM simulation of mechanical properties of long fiber-reinforced composite

This chapter describes the creation of two numerical models and their comparison:

Model simulations in FEM were performed for different combinations of reinforcement arrangements of long fiber-reinforced composites, which are important for comparison with experiments and analytical relationships. This gives the material properties for numerical

The simulations were performed for a complete assessment of the mechanical properties σ11, σ22, ε11, ε22, γ12, γ<sup>23</sup> and elastic constants E11, E22, G12, G23, ν12, ν23, whereas also information explaining the shape changes of the samples observed especially during tensile stress.

• creating the corresponding mesh of finite elements of the computational model in the

The FEM model was created in the concept of coherent continuum consisting of a surface geometry corresponding to the test sample with length L = 100 mm, width b = 20 mm, and thickness h = 1.7 mm. The finite element mesh of the numerical model was created from SHELL elements (2D elements) with a constant element size of 2 mm. The boundary conditions affecting the magnitude of the displacements and stress can be defined in two ways, that is, the boundary conditions of the first and second types. The first way is to determine the displacement and stress distributions if force conditions are known, that is, volume forces, surface forces, and nodal loads. The other way is to determine the displacement and tension distribution if the geometric conditions are known, that is, the size of node displacement, the

properties of the long fiber-reinforced composite.

(I) continuum model

preprocessor,

simulation of the strength characteristics of whole frames.

12 Finite Element Method - Simulation, Numerical Analysis and Solution Techniques

(II) extended continuous model with structural unit

Model simulations were performed in the following steps:

• defining the corresponding initial and boundary conditions,

• assembling a material model of the long fiber-reinforced composite,

4.1.1. Assembling of continuum of the long fiber-reinforced composite model

• the evaluation and comparison of model simulation results in postprocessor.

• creating two model simulations of the long fiber-reinforced composite,

The second numerical FEM model, which was created in the concept of structure unit, is formed from three components: fiber matrix—the interfacial interface, where the microscopic dimensions of such a model are closer to the more real composite. Such a model can be created from a structural unit with the 1, 2,…, n fibers, wherein the volume geometric configuration (e.g., structural unit is a cube, cuboid, sphere) can affect the volumetric quantity of fibers and a matrix V<sup>f</sup> , Vm, as shown by Neckář [12]. The change in volume ratio V<sup>f</sup> can be given on the example of the structural unit of the cuboid, which is shown in the section in Figure 6. The structural unit consists of six fibers represented by circles with the same spacing mi, which are

Figure 5. Continuum FEM model of the composite reinforced with long fibers with defined boundary and initial conditions.

Figure 6. The influence of fiber spacing in the structural unit on V<sup>f</sup> fiber volume ratio.

bounded by a matrix (rectangle). By changing of the spacing can then be increased or decreased volume ratio of fibers V<sup>f</sup> : The finite element mesh of the numerical model was created from a combination of following elements: BRICK elements (3D elements) with a designed element size of 0.0002 mm defined for fibers and matrix (Figure 7).

It will be assumed that <sup>E</sup><sup>11</sup> <sup>¼</sup> <sup>σ</sup><sup>11</sup> <sup>ε</sup><sup>11</sup> , <sup>E</sup><sup>22</sup> <sup>¼</sup> <sup>σ</sup><sup>22</sup> <sup>ε</sup><sup>22</sup> , <sup>G</sup><sup>12</sup> <sup>¼</sup> <sup>τ</sup><sup>12</sup> γ<sup>12</sup> , <sup>G</sup><sup>23</sup> <sup>¼</sup> <sup>τ</sup><sup>23</sup> γ<sup>23</sup> .

The problem lies in joining of fibers with the matrix because the interconnections form an interphase. The structural FEM model assembling presents a problem of the determination of appropriate boundary conditions, which is important in terms of accuracy and model verification. Incorrect design may result in concentrators and singularities of stress. The boundary conditions are created by the second type (geometric boundary conditions) as follows: the perimeter surfaces of the model perpendicular to the plane of the stretching direction have defined symmetry conditions on one side (symmetry in axis y and z) and on the opposite side, the boundary conditions are not prescribed. On surfaces in the plane of the stretch direction, that is, in the direction of the X axis, the displacements and rotations were not allowed Ui ¼ Ri ¼ 0 in all directions. On the opposite surface of the specimen, the condition was the same, only displacement in the stretching direction was allowed. The displacement was defined constantly to the maximum strain 1%, that is, Ux ¼ k:j <sup>ε</sup>x¼1%, <sup>k</sup>: <sup>¼</sup> const:, with strain rate 2 mm min�<sup>1</sup> . Boundary conditions are shown in Figure 8 and Table 2. The material properties applied in both FEM models (I. Continuum Model and the II. Continuum Model with the Structure Unit) are based on the generally known values reported by fiber and matrix manufacturers. The fiber and epoxy matrix parameters are listed in Table 3. The results of both numerical simulations have exhibited approximately the same stress at the defined strain ε<sup>i</sup> ¼ 1% under tensile load in applied direction for a given fiber reinforcement (carbon or glass). The resulting dependence of force on the displacement of the samples obtained from the models showed an approximately linear course, both for carbon and glass fiber-reinforced composite. Figure 9 shows the tensile test for volume ratio <sup>V</sup><sup>f</sup> <sup>¼</sup> <sup>0</sup>:3, where carbon fiber-reinforced composite with the epoxy matrix

exhibits approximately 2.2 times higher force response than the glass fiber-reinforced composite

Figure 8. The boundary conditions of the structural FE model of the composite structure reinforced with long fibers.

Planes in axis x Planes in axis y Planes in axis z

þx �x þy �y þz �z

Uz ¼ 0

Uz ¼ 0

Shear module [GPa]

<sup>12</sup> <sup>G</sup><sup>f</sup>,<sup>m</sup>

Carbon fibers 1750 � 150 230 15 24 5.4 0.279 0.49 2.3 � 1.2 1.9 � 0.6 Glass fibers 2370 � 230 72.4 72.4 28.7 28.7 0.22 0.22 1.06 � 0.65 4.8 � 0.7 Epoxy matrix 1150 � 370 3.573 3.573 1.31 1.31 0.345 0.345 0.067 � 0.033 3.6

<sup>23</sup> <sup>ν</sup><sup>f</sup>,<sup>m</sup>

<sup>22</sup> <sup>G</sup><sup>f</sup>,<sup>m</sup>

<sup>ε</sup>x¼1% Ui, Ri <sup>¼</sup> <sup>0</sup> Uy, Rz, Rx <sup>¼</sup> <sup>0</sup> — Uz, Rx, Ry <sup>¼</sup> <sup>0</sup> —

FEM Analysis of Mechanical and Structural Properties of Long Fiber-Reinforced Composites

<sup>ε</sup>y¼1% Ui, Ri <sup>¼</sup> <sup>0</sup> Uz, Rx, Ry <sup>¼</sup> <sup>0</sup> —

Poisson's ratio [�] Tensile strength

Uy ¼ k: εy¼1%

http://dx.doi.org/10.5772/intechopen.71881

Ux ¼ 0

[GPa]

Uz ¼ 0 Uz ¼ 0

Ux ¼ 0 Uy ¼ 0 15

Elongation [%]

Ux ¼ 0 Uz ¼ 0

Ux ¼ 0 Uz ¼ 0

<sup>12</sup> <sup>ν</sup><sup>f</sup>,<sup>m</sup> 23

 

The obtained results shown in Figures 10 and 11 can be stated that the continuous model (FE model I) has an approximately steady monotonic course manifested not only in continuous

with epoxy matrix.

E11, μ<sup>12</sup> Ux ¼ k:j

<sup>G</sup><sup>12</sup> Uy <sup>¼</sup> <sup>k</sup>:

Material Density

 

[kg m�<sup>3</sup> ]

<sup>E</sup>22, <sup>μ</sup><sup>23</sup> Ux, Ry, Rz <sup>¼</sup> <sup>0</sup> — Uy <sup>¼</sup> <sup>k</sup>:

G<sup>23</sup> Ux ¼ 0 Ux ¼ 0 Ux ¼ 0

Ef,<sup>m</sup>

Table 2. FEM model boundary conditions for obtaining elastic constants.

Modulus of elasticity [GPa]

<sup>11</sup> Ef,<sup>m</sup>

Table 3. Material and mechanical properties of individual constituent of composite.

<sup>ε</sup>y¼1% Uz <sup>¼</sup> <sup>0</sup> Uy <sup>¼</sup> <sup>0</sup> Uz <sup>¼</sup> <sup>0</sup> Ux <sup>¼</sup> <sup>0</sup>

Figure 7. Structural FEM model of a composite reinforced with long fibers.

FEM Analysis of Mechanical and Structural Properties of Long Fiber-Reinforced Composites http://dx.doi.org/10.5772/intechopen.71881 15

Figure 8. The boundary conditions of the structural FE model of the composite structure reinforced with long fibers.


Table 2. FEM model boundary conditions for obtaining elastic constants.

bounded by a matrix (rectangle). By changing of the spacing can then be increased or

created from a combination of following elements: BRICK elements (3D elements) with a

The problem lies in joining of fibers with the matrix because the interconnections form an interphase. The structural FEM model assembling presents a problem of the determination of appropriate boundary conditions, which is important in terms of accuracy and model verification. Incorrect design may result in concentrators and singularities of stress. The boundary conditions are created by the second type (geometric boundary conditions) as follows: the perimeter surfaces of the model perpendicular to the plane of the stretching direction have defined symmetry conditions on one side (symmetry in axis y and z) and on the opposite side, the boundary conditions are not prescribed. On surfaces in the plane of the stretch direction, that is, in the direction of the X axis, the displacements and rotations were not allowed Ui ¼ Ri ¼ 0 in all directions. On the opposite surface of the specimen, the condition was the same, only displacement in the stretching direction was allowed. The displacement was defined constantly

Boundary conditions are shown in Figure 8 and Table 2. The material properties applied in both FEM models (I. Continuum Model and the II. Continuum Model with the Structure Unit) are based on the generally known values reported by fiber and matrix manufacturers. The fiber and epoxy matrix parameters are listed in Table 3. The results of both numerical simulations have exhibited approximately the same stress at the defined strain ε<sup>i</sup> ¼ 1% under tensile load in applied direction for a given fiber reinforcement (carbon or glass). The resulting dependence of force on the displacement of the samples obtained from the models showed an approximately linear course, both for carbon and glass fiber-reinforced composite. Figure 9 shows the tensile test for volume ratio <sup>V</sup><sup>f</sup> <sup>¼</sup> <sup>0</sup>:3, where carbon fiber-reinforced composite with the epoxy matrix

γ<sup>12</sup>

, <sup>G</sup><sup>23</sup> <sup>¼</sup> <sup>τ</sup><sup>23</sup> γ<sup>23</sup> .

<sup>ε</sup><sup>22</sup> , <sup>G</sup><sup>12</sup> <sup>¼</sup> <sup>τ</sup><sup>12</sup>

designed element size of 0.0002 mm defined for fibers and matrix (Figure 7).

<sup>ε</sup><sup>11</sup> , <sup>E</sup><sup>22</sup> <sup>¼</sup> <sup>σ</sup><sup>22</sup>

14 Finite Element Method - Simulation, Numerical Analysis and Solution Techniques

: The finite element mesh of the numerical model was

<sup>ε</sup>x¼1%, <sup>k</sup>: <sup>¼</sup> const:, with strain rate 2 mm min�<sup>1</sup>

.

decreased volume ratio of fibers V<sup>f</sup>

to the maximum strain 1%, that is, Ux ¼ k:j

Figure 7. Structural FEM model of a composite reinforced with long fibers.

It will be assumed that <sup>E</sup><sup>11</sup> <sup>¼</sup> <sup>σ</sup><sup>11</sup>


Table 3. Material and mechanical properties of individual constituent of composite.

exhibits approximately 2.2 times higher force response than the glass fiber-reinforced composite with epoxy matrix.

The obtained results shown in Figures 10 and 11 can be stated that the continuous model (FE model I) has an approximately steady monotonic course manifested not only in continuous

Figure 9. Comparison of experiments and FEM models: Dependence of applied force on sample strain.

distribution of deformation (Figure 12 above) but also in uniform distribution of the principal stress <sup>σ</sup><sup>I</sup> <sup>¼</sup> <sup>σ</sup><sup>11</sup> acting in the load direction (Figure 12 center).

Due to the simplicity of the FEM model I, it appears to be very suitable for determining the mechanical properties of composite structures and their optimization. However, such a model does not provide information about strain and stress between the fibers and the matrix, let alone the interphase. The continuous model with the structural unit (FEM model II) is significantly more complex, and for some elastic constants, its resultant course is not monotone (G23, ν23); in other words, the resulting dependency is not stable and may not be accurate enough but more complex in terms of results. FEM model II allows to approximate the layout distribution of the structure unit in the loading direction (Z axis) as shown in Figure 12 (left) and also the principal stress distribution. The principal stress can be determined in isosurfaces or in sequential sections (Figure 12 right), which allow to analyze the stress distribution between the fibers and the matrix including the interphase. By comparing the maximum values of the stress of 189.1 and 190.9 MPa at same strain ε<sup>11</sup> ¼ 1% and with the volume ratio <sup>V</sup><sup>f</sup> <sup>¼</sup> <sup>0</sup>:5 can be stated that the models have significant agreement. This is affected not only by the same material parameters and boundary conditions but also appropriately selected types of elements of the finite element mesh as discussed earlier. FEM model II of the composite structure reinforced with longitudinal fibers with the epoxy matrix is more complex, and the time of the calculation is larger than the FEM model I.

However, it must be added that the FEM model II shows valuable scientific knowledge of the approximate distribution of the maximum stress between the fibers and the matrix, which is the largest in the interphase (Figure 13 left). This confirms the theoretical assumption of the system mechanism (fiber-matrix interphase), where the highest stress transmits newly created component, that is, the interphase, which causes the synergic effect of the resultant construction of the composite structure. Figure 13 also shows the information that FEM model II shows a nonuniform maximum stress in the composite structure (unlike the FEM model I) and also shows that maximum stress is concentrated only on two fibers (instead of six in the structural unit) of the structural unit. It will reduce the maximum synergic effect that theoretically in the composite structure can occur. The distribution of the interphase in the numerical model and in the real measurement is shown in Figure 13. It is necessary to add that from the analyses carried out by measurements on real samples was in all cases evident that the identification of the interphase is very complicated. Due to the

FEM Analysis of Mechanical and Structural Properties of Long Fiber-Reinforced Composites

http://dx.doi.org/10.5772/intechopen.71881

17

of transversally isotropic composites

Figure 10. Dependence of modulus G23 (left above), ν<sup>12</sup> (left below), ν23(right) on V<sup>f</sup>

with epoxy matrix and carbon fibers and glass fibers.

FEM Analysis of Mechanical and Structural Properties of Long Fiber-Reinforced Composites http://dx.doi.org/10.5772/intechopen.71881 17

Figure 10. Dependence of modulus G23 (left above), ν<sup>12</sup> (left below), ν23(right) on V<sup>f</sup> of transversally isotropic composites with epoxy matrix and carbon fibers and glass fibers.

distribution of deformation (Figure 12 above) but also in uniform distribution of the principal

Figure 9. Comparison of experiments and FEM models: Dependence of applied force on sample strain.

Due to the simplicity of the FEM model I, it appears to be very suitable for determining the mechanical properties of composite structures and their optimization. However, such a model does not provide information about strain and stress between the fibers and the matrix, let alone the interphase. The continuous model with the structural unit (FEM model II) is significantly more complex, and for some elastic constants, its resultant course is not monotone (G23, ν23); in other words, the resulting dependency is not stable and may not be accurate enough but more complex in terms of results. FEM model II allows to approximate the layout distribution of the structure unit in the loading direction (Z axis) as shown in Figure 12 (left) and also the principal stress distribution. The principal stress can be determined in isosurfaces or in sequential sections (Figure 12 right), which allow to analyze the stress distribution between the fibers and the matrix including the interphase. By comparing the maximum values of the stress of 189.1 and 190.9 MPa at same strain ε<sup>11</sup> ¼ 1% and with the volume ratio <sup>V</sup><sup>f</sup> <sup>¼</sup> <sup>0</sup>:5 can be stated that the models have significant agreement. This is affected not only by the same material parameters and boundary conditions but also appropriately selected types of elements of the finite element mesh as discussed earlier. FEM model II of the composite structure reinforced with longitudinal fibers with the epoxy matrix is more complex, and the time of the calculation is larger than the FEM model I.

stress <sup>σ</sup><sup>I</sup> <sup>¼</sup> <sup>σ</sup><sup>11</sup> acting in the load direction (Figure 12 center).

16 Finite Element Method - Simulation, Numerical Analysis and Solution Techniques

However, it must be added that the FEM model II shows valuable scientific knowledge of the approximate distribution of the maximum stress between the fibers and the matrix, which is the largest in the interphase (Figure 13 left). This confirms the theoretical assumption of the system mechanism (fiber-matrix interphase), where the highest stress transmits newly created component, that is, the interphase, which causes the synergic effect of the resultant construction of the composite structure. Figure 13 also shows the information that FEM model II shows a nonuniform maximum stress in the composite structure (unlike the FEM model I) and also shows that maximum stress is concentrated only on two fibers (instead of six in the structural unit) of the structural unit. It will reduce the maximum synergic effect that theoretically in the composite structure can occur. The distribution of the interphase in the numerical model and in the real measurement is shown in Figure 13. It is necessary to add that from the analyses carried out by measurements on real samples was in all cases evident that the identification of the interphase is very complicated. Due to the

Figure 12. Distribution of deformation (above) and principal stress in the loading direction (center) of the FEM model I of long fiber-reinforced composite with epoxy matrix. The resulting distribution of axial strain (below left) and the principal stress acting in the loading direction (below right) and the FEM model II of composite reinforced with long carbon fiber

FEM Analysis of Mechanical and Structural Properties of Long Fiber-Reinforced Composites

http://dx.doi.org/10.5772/intechopen.71881

19

Figure 13. Distribution of principal stress in direction of loading with maximal stress in interphase (left), real sample with

with epoxy matrix.

visible interphase (right).

Figure 11. Dependence of modulus E11, E22, G12 on V<sup>f</sup> of transversally isotropic composites with epoxy matrix and carbon fibers (left) and glass fibers (right).

unidentifiable technological process, interphase (third component) could not be created. Also, it is problem to identify and measure the interphase that is important both for verifying of numerical models and for a statistical evaluation how many fibers are involved in synergistic effect.

FEM Analysis of Mechanical and Structural Properties of Long Fiber-Reinforced Composites http://dx.doi.org/10.5772/intechopen.71881 19

Figure 12. Distribution of deformation (above) and principal stress in the loading direction (center) of the FEM model I of long fiber-reinforced composite with epoxy matrix. The resulting distribution of axial strain (below left) and the principal stress acting in the loading direction (below right) and the FEM model II of composite reinforced with long carbon fiber with epoxy matrix.

Figure 13. Distribution of principal stress in direction of loading with maximal stress in interphase (left), real sample with visible interphase (right).

unidentifiable technological process, interphase (third component) could not be created. Also, it is problem to identify and measure the interphase that is important both for verifying of numerical models and for a statistical evaluation how many fibers are involved in syner-

Figure 11. Dependence of modulus E11, E22, G12 on V<sup>f</sup> of transversally isotropic composites with epoxy matrix and

gistic effect.

carbon fibers (left) and glass fibers (right).

18 Finite Element Method - Simulation, Numerical Analysis and Solution Techniques
