The incompressible nature of plastic deformation in metals places limitations on the types of elements that can be used for an elastic-plastic simulation. The limitations arise because modeling incompressible material behavior adds kinematic constraints to an element; in this case the limitations constrain the volume at the element's integration points to remain constant. In certain classes of elements the addition of these incompressibility constraints makes the element overconstrained. When these elements cannot resolve all of these constraints, they suffer from volumetric locking, which causes their response to be too stiff. Volumetric locking is indicated by a rapid variation of hydrostatic pressure stress from element to element or integration point to integration point.

Fully integrated, second-order, solid elements are very susceptible to volumetric locking when modeling incompressible material behavior and, therefore, should not be used in elastic-plastic simulations. The ABAQUS fully integrated, first-order, solid elements do not suffer from volumetric locking because ABAQUS actually uses a constant volume strain in these elements. Thus, they can be used safely in plasticity problems.

Reduced-integration, solid elements have fewer integration points at which the incompressibility constraints must be satisfied. Therefore, they are not overconstrained and can be used for most elastic-plastic simulations. Second-order, reduced-integration elements should be used with caution if the strains exceed 20–40% because at this magnitude they can suffer from volumetric locking. This effect can be reduced with mesh refinement.

If you have to use fully-integrated, second-order elements, use the hybrid versions, which are designed to model incompressible behavior; however, remember that the additional degrees of freedom in these elements will make the analysis more computationally expensive.