Selecting continuum elements

The correct choice of element for a particular simulation is vital if accurate results are to be obtained at a reasonable cost. You will undoubtedly develop your own guidelines for selecting elements for your own particular applications as you become more experienced in using Abaqus. However, as you begin to use Abaqus, the guidelines given here may be helpful.

The following recommendations apply to both Abaqus/Standard and Abaqus/Explicit:

  • Minimize the mesh distortion as much as possible. Coarse meshes with distorted linear elements can give very poor results.

  • Use a fine mesh of linear, reduced-integration elements (CAX4R, CPE4R, CPS4R, C3D8R, etc.) for simulations involving very large mesh distortions (large-strain analysis).

  • In three dimensions use hexahedral (brick-shaped) elements wherever possible. They give the best results for the minimum cost. Complex geometries can be difficult to mesh completely with hexahedrons; therefore, wedge and tetrahedral elements may be necessary. The linear versions of these elements, C3D4 and C3D6, are poor elements (fine meshes are needed to obtain accurate results); as a result, these elements should generally be used only when necessary to complete a mesh, and, even then, they should be far from any areas where accurate results are needed.

  • Some preprocessors contain free-meshing algorithms that mesh arbitrary geometries with tetrahedral elements. The quadratic tetrahedral elements in Abaqus/Standard (C3D10 or C3D10HS) are suitable for general usage; but when used with contact, they should be used only with the surface-to-surface contact discretization. An alternative to these elements is the modified quadratic tetrahedral element (C3D10M) available in both analysis products. This element is robust for large-deformation problems and contact problems using either the traditional node-to-surface or the surface-to-surface contact discretization and exhibits minimal shear and volumetric locking. With either type of element, however, the analysis will take longer to run than an equivalent mesh of hexahedral elements. You should not use a mesh containing only linear tetrahedral elements (C3D4): the results will be inaccurate unless you use an extremely large number of elements.

Abaqus/Standard users should also consider the following recommendations:

  • Use quadratic, reduced-integration elements (CAX8R, CPE8R, CPS8R, C3D20R, etc.) for general analysis work, unless you need to model very large strains or have a simulation with complex, changing contact conditions.

  • Use quadratic, fully integrated elements (CAX8, CPE8, CPS8, C3D20, etc.) locally where stress concentrations may exist. They provide the best resolution of the stress gradients at the lowest cost.

  • For contact problems use a fine mesh of linear, reduced-integration elements or incompatible mode elements (CAX4I, CPE4I, CPS4I, C3D8I, etc.). See Contact.