Benchmark Problems for Large Strain Analyses of Shell Structures
There are many practical problems in which shell structures undergo large strains, such as in metal forming and in the crashing or crushing of motorcars. In the development of procedures for the analysis of shell structures in large strains, it is very important to validate the solution procedures with benchmark solutions. Unfortunately there are not many such solutions in the literature.
Here we present two benchmark solutions for shell structures in large strains. We have constructed these benchmark problems to study the capabilities of elements in situations that typically can occur in practical large strain analyses.
The benchmark problems are solved using the 3D-shell element of ADINA, and also the 27/4 3D solid element for comparison. The 3D-shell element is available in ADINA specifically for large strain analysis of shells, and this element was already presented in the April 2010 Tech Brief.
It is important to note that this element is based on a formulation without spurious zero energy modes (that would have to be suppressed by artificial numerical factors, hence there is no hour-glass control), and can directly be used for static and dynamic (implicit and explicit) solutions.
Benchmark problem 1: Plane strain folding of a thin shell
Typically folds form when a thin shell is crushed. In this problem we form a single fold under controlled conditions.
Figure 1 shows the problem considered. The shell is thin (thickness / length = 1/500) and an elastic-perfectly plastic material model is used. As the moving contact surface displaces downwards, the shell is squeezed and a fold forms where the shell is fixed.
For the solution, we use meshes of 4-node 3D-shell elements and also meshes of 27/4 3D solid elements. The meshes are graded so that the elements are smallest at the built-in end. In all of the analyses, 3-point Gauss integration is used through the thickness.
For the 100 element mesh of 3D-shell elements, Figure 2 shows a detail of the undeformed model near the built-in end, and Figures 3 and 4 show the deformed model as the imposed displacement due to contact is increased.
Figure 5 shows the calculated force-deflection curves. On both axes, a log scale is used so that the entire solution response over the whole range of displacements can be shown in one figure. The calculated responses are quite close to each other, however, as expected, the 50 element 3D solid element model is stiffer than the other models.
For displacements above 49.5 mm, the force-deflection curves exhibit a "stair-step" behavior. This behavior arises due to the contact algorithm; the force-deflection curve stiffens each time an additional node comes into contact.
Although this is a thin shell structure, as typically encountered in the motor car industries, the plastic strain at the built-in end is almost 70%.
Benchmark problem 2: Buckling of a thin geometrically perturbed cylindrical shell
Another way to form a fold is to create a plastic hinge by buckling. Figures 6 to 9 show the problem considered. The shell segment is thin (thickness / length = 1/100) and an elastic-perfectly plastic material model is used. The geometry of the midsurface of the perturbed cylindrical shell segment is given in terms of parametric coordinates as follows:
and . Here and are the radius and the length of the shell segment, and is the perturbation. With , the above formulas reduce to the geometry of a cylindrical segment with length and radius , and with boundaries . The above formulas are explained in the figures below.
The shell geometric perturbation at a constant coordinate is shown in Figure 8. It is seen that the cross-section (thick line) is constructed using two circles, one circle with radius and the other circle with radius . The slope of the cross-section line is zero at .
The shell cross-section for is shown in Figure 9. We note that the slope is zero at .
For the finite element solution, we use 3D-shell element meshes and also 3D solid element meshes (with the 27/4 solid element) for comparison. In all cases, 3-point Gauss integration is used through the thickness.
The movies at the top of this web page show the deformations and the accumulated effective plastic strain as a compressive prescribed displacement is applied to a 50 x 75 3D-shell element mesh. A fold forms near the line of symmetry and very large strains are generated at the fold.
Figure 10 shows the force-deflection curves obtained using 3D-shell and 3D solid element meshes of various mesh refinements. The calculated force-displacement responses are very close to each other.
Clearly, these benchmark problems demonstrate that the 3D-shell element capability in ADINA can be used to analyze shell structures undergoing very large strains. The elements can be used reliably and efficiently in many industrial applications.