Bilinear approach to tensile properties of flax composites in finite element analyses

Abstract

Flax fibers show potential in bio-efficiency compared to conventional composite fibers with good mechanical properties. The tensile behavior of flax fibers shows a nonlinear stress–strain relation. Within this work, a bilinear elastic–plastic approach is described, which is based on the generalized Hill potential theory and easily applicable in ANSYS. The method was used to model the nonlinear stress–strain behavior under quasi-static tensile loading of flax fiber-reinforced laminates. Hashin failure mechanisms using the stress–strain data of the bilinear model are applied as well. The results were compared to experimental data, carried out using pre-impregnated flax fibers in three types of tensile test specimens. The layups of investigation were $[0]_6$, $[90]_6$ and $[\pm \, 45]_8$. The strain was evaluated using the non-contact, digital image correlation measurement ARAMIS. Good agreement with the test results was achieved, and the method of bilinear elastic–plastic modeling of flax fiber-reinforced structures was evaluated as simple but effective for quasi-static elongation under uniaxial tensile loading.

Appendix: Implementation in ANSYS

The described model is available in commercial ANSYS releases. In this work, the ANSYS 17.2 Workbench version with the Academic Research Mechanical and CFD license was used.

The tensile tests were modeled as surface geometry, where layers were modeled using the ANSYS Composite PrePost (ACP) environment. On the surface geometry of $150 \times 15$ mm, a mesh of 0.75 mm side length with Hex8 elements was created. In the ACP environment, a rosette was aligned in x to the longitudinal fiber direction, y transversal to the fibers and z pointing in the stack-up thickness direction. For each fiber direction, a different orientation rosette should be used, no matter whether the material properties are the same or not. The ACP environment creates a solid element model from the surface geometry by extruding the layers in thickness direction, the model is then exported to a transient structural analysis. The imported model consists of one element per layer in thickness direction, with side dimensions of the surface mesh. Such layered composites have a side-length proportion which is prone to locking; this should be considered when applied to bending problems.

With command snippets, the imported materials, layers and coordinate systems can be reviewed in the imported geometry part (PREP7). The element type was here set to SOLID45.

In the analysis part (SOLUTION), the material characteristics are defined, overwriting the initial elastic moduli, Poisson’s ratios and shear moduli for each material. For the xy- and xz-directions, it should be distinguished between the major and minor Poisson’s ratio (PRXY and NUXY in ANSYS). Then, the bilinear anisotropic plasticity approach needs the TB, ANISO command to define the nine yield stresses and tangential moduli. The set initial and tangential moduli are equal for tensile $()_{\mathrm{t}}$ and compressive loads $()_{\mathrm{c}}$. Qualitatively, the curves (Fig. 4) show similar shape of respective experimental results [26, 29, 30].

The load was applied by a linear displacement in x-direction at the one end. Therefore, the strain in load direction should be linear as well. The displacement was done in the transient analysis over 20 s with equally distributed time steps of 0.5 s.

For the analysis, the elements in the middle part of the specimen with x-coordinates between 65 and 85 mm and y-coordinates between 5 and 10 mm were evaluated in order to neglect the influence of boundary conditions. The user-defined results were used to show the tensile response, SX as stress in the load direction, versus EPTOX and EPTOY to show strains in longitudinal and transversal directions (see Figs. 7, 8, 9). For the failure criteria, the top layer was selected and the fiber-coordinate system was used.

The EPTO command as user-defined result gives the sum of the elastic, plastic and creep strains. For more detailed analysis, the EPPL and EPEL commands can be used, referring to either plastic or elastic strains.