Issue 39

M. Romano et alii, Frattura ed Integrità Strutturale, 39 (2016) 226-247; DOI: 10.3221/IGF-ESIS.39.22 235 convergence behavior is considered in sensitivity analyses. The numerical investigations are carried out with the FE- software ANSYS Workbench Version 14.0.1 [34]. FE-model of plain representative sequences The kinematic is investigated parametrically by varying the characteristic geometric dimensions as well as the boundary conditions. In order to enable a proper meshing, avoid too small or acute triangle elements, reduce computing time and improve convergence two slight but essential modifications of the geometry are necessary. First, the lens-shaped fill yarns are cut by 2 % regarding the length L R in the region of each intersection. The resulting length of the cross-section of the fill yarn is L L R,mod R 0.96   . The length of the complete plain representative sequence L PL according to Eq. (5) is thereby not affected. Second, the upper and lower horizontal boundary of the surrounding matrix region is increased by 10 % of the amplitude A . The resulting thickness of the modified plain representative sequences is then t A mod 4.2   . Fig. 3 illustrates the modified parametric model for the numerical investigations by the FE-analyses confronting the extremes of its geometric dimensions. Figure 3 : Modified parametric model for investigations by the FEA based on analytic dimensions confronting its extremes. Upper left: Biggest length L =15 with lowest amplitude A =0.05 yielding O ~ =0.00333; Upper right: Shortest length L =5 with lowest amplitude A =0.05 yielding O ~ =0.01000; Lower left: Shortest length L =5 with highest amplitude A =0.25 yielding O ~ =0.05000, Lower right: Biggest length L =15 with highest amplitude A =0.25 yielding O ~ =0.01667. FE-settings: Meshing, element types and contact definition As a first approximation a two dimensional FE-analyses is carried out. The representative sequence is discretized by elements with an average edge length of 3 10 1   . As the FE-model represents a cross-section of a structure, a plain strain condition in the x - y -plane is presumed. Plain four-node solid elements with linear shape functions are assigned to each region of the model. An orthotropic material model is chosen for properly applying the material properties to warp and fill yarn. In case of the region of the warp yarn elements of the formulation PLANE42 are assigned to by APDL (ANSYS Parametric Design Language). In this case the enabled first keyoption by the command KEYOPT(1) for the element formulation PLANE42, makes the local x - y -element coordinate system follow the element I - J sides. As a mapped meshing has been applied to this region, the element coordinate systems follow the sine-shaped ondulation. As the material properties of orthotropic materials in ANSYS [34] are orientated along the element coordinate system, the modification is essential for a reality based FE-simulation. To the two other regions (fill yarns and matrix) the default elements of the formulation PLANE182 are retained. It does not provide the afore mentioned keyoption. It neither is necessary because the fill yarns are modeled in their plane of isotropy and the matrix is modeled isotropic. After sensitivity analyses and as a reasonable approach for the real conditions the contact between the single regions is defined by coincident nodes. Fig. 4 illustrates the effect of the different element formulations on the orientation of the element coordinate systems in the region of the zero-crossing.