Linear Static Analysis

The basic finite element equation to be solved for structures experiencing static loads can be expressed as:

K u = f

Where, K is the stiffness matrix of the structure (an assembly of individual element stiffness matrices). The vector u is the displacement vector, and f is the vector of loads applied to the structure. The above equation is the equilibrium of external and internal forces.

The stiffness matrix is singular, unless displacement boundary conditions are applied to fix the rigid body degrees-of-freedom of the model.

The equilibrium equation is solved either by a direct or an iterative solver. By default, the direct solver is invoked, whereby the unknown displacements are simultaneously solved using a Gauss elimination method that exploits the sparseness and symmetry of the stiffness matrix, K , for computational efficiency. Alternatively, an iterative solver using the preconditioning conjugate gradient method may be used. While the direct solver is very robust, accurate and efficient, the iterative solver is sometimes superior, in terms of speed, for thick-walled solid structures. The iterative solver is selected through the SOLVTYP Subcase Information Entry, which in turn references a SOLVTYP Bulk Data Entry.

Once the unknown displacements at the nodal points of the elements are calculated, the stresses can be calculated by using the constitutive relations for the material. For linear static analysis where the deformations are in the elastic range, that is, the stresses, σ , are assumed to be linear functions of the strains, ε , Hooke's law can be used to calculate the stresses. Hooke's law can be stated as: σ = C ε with the elasticity matrix C of the material. The strains ε are a function of the displacements.

The Static Loads and Boundary Conditions are defined in the Bulk Data section of the input deck. They need to be referenced in the Subcase Information section using an SPC and LOAD statement in a SUBCASE. Each SUBCASE defines a load vector. Thermal loading is defined by referencing Bulk Data Entries with the TEMPERATURE statement in a SUBCASE.

Unconstrained models can be solved using Inertia Relief. SUPORT1 Subcase Information Entry can then reference the boundary conditions that restrain the rigid body motions. Up to six degrees-of-freedom can be restrained. These restraints can also be defined without subcase reference using the SUPORT Bulk Data Entry or automated using PARAM,INREL,-2.