Membrane patch test

• ${\sigma }_x={\sigma }_y=$ 1333 for plane stress, shell, and membrane elements.

• ${\sigma }_x={\sigma }_y=$ 1600 for plane strain elements.

• ${\sigma }_z=$ 800 for plane strain elements.

• ${\sigma }_{xy}=$ 400 for all elements.

• ${\epsilon }_x={\epsilon }_y={\gamma }_{xy}=$ 10⁻³.

The hand-calculated solutions will differ because of the various assumptions made for each category of element. The assumptions made correspond to those that are implemented in Abaqus. The two that cause significant differences in the results of this step are the strain measure used and the elemental cross-sectional area used to calculate the edge load and output stresses.

The strain measure used for shells, for example, is Green's strain. This strain measure is intended for large displacements and rotations but small strains. The remainder of the elements, including finite-strain shells, use logarithmic strain, which is intended for large-strain analyses.

The use of nonlinear geometric effects implies that the nodal coordinates will change for each element. This, in turn, implies that the cross-sectional area of the elements will change. The change of length and width is taken into account for all elements. This is not the case for the thickness, however. The thickness of the plane strain elements, of course, is assumed to remain constant. The thickness is also assumed to remain constant for the shell elements, excluding finite-strain shells. The remainder of the elements take into account a change in thickness determined by assuming constant elemental volume. This change in thickness, combined with a change in length and width, results in a cross-sectional area that differs from the initial area. This result affects the output stress calculations, as well as the applied edge load.

Since the edge load is calculated as the pressure divided by the area, the edge load will vary because of the variation in the cross-sectional area. Edge loads are presently not available for shells and membranes. Equivalent concentrated nodal forces are applied to these elements in this step, and as a result the load remains constant.

In the Abaqus/Explicit simulations this is the third step. (The second step in the Abaqus/Explicit simulations returns the model to its unloaded state.)

• ${\sigma }_x={\sigma }_y=$ 1323 for plane stress, shell, and membrane elements.

• ${\sigma }_x={\sigma }_y=$ 1590 for plane strain elements.

• ${\sigma }_z=$ 795 for plane strain elements.

• ${\sigma }_{xy}=$ 397.0 for plane stress, shell, and membrane elements.

• ${\sigma }_{xy}=$ 397.5 for plane strain elements.

• ${\epsilon }_x={\epsilon }_y={\gamma }_{xy}=$ 9.92 × 10⁻³ for plane stress, shell, and membrane elements.

• ${\epsilon }_x={\epsilon }_y={\gamma }_{xy}=$ 9.94 × 10⁻³ for plane strain elements.

  In the Abaqus/Explicit simulations this is the fourth step. The results from the third step in the Abaqus/Explicit simulations must be subtracted from the results of the fourth step to obtain the perturbation about the loaded state.