Solvers Overview: Nonlinear Static

Description

Although the majority of engineering structures operate within an acceptable linear regime, and the assumptions made in the linear analysis are valid, there exists a wide class of problems which do exhibit nonlinear behaviour, and for which a linear analysis is not valid. The Nonlinear Static solver predicts the behaviour of such structures, taking into account three main types of nonlinearity:

• Nonlinear geometry (GNL) which accounts for the fact that the structural stiffness and the equilibrium can change as the structure deforms, and therefore the displacement will not be proportional to the applied load;
• Nonlinear material (MNL) which accounts for materials that do not obey Hooke's law; also included here are materials that vary with temperature; and
• Boundary nonlinearity which accounts for the fact that contact between components depends on the load between the components, which in turn affects the stiffness of the contacting parts, and therefore produces a displacement response that is not proportional to the applied load.

This solver does not consider time-dependent effects such as inertia or viscous effects.

Procedure

The Nonlinear Static solver executes the following steps:

1. Initialises the nodal displacement vector, , element stress, , element strain, , etc.
2. Sets the current load step.

3. Calculates and assembles the element stiffness matrices, equivalent element force vectors and external nodal force vectors. In the stiffness calculation, material temperature dependency is considered (see Special Topics: Temperature Dependence). Depending on whether material and/or geometric nonlinearity are considered, the material modulus and geometry will be updated as required. The element geometric stiffness matrix is also included if the corresponding option is set. Either consistent or lumped element equivalent load vectors can be calculated according to the option setting (see Entities: Consistent vs Lumped Load) and also depending on the elements and the loading. Constraints and links are also assembled in this process and the constant terms in enforced displacements, shrink links, and multi-point links are combined and applied according to the specified factors for the load step.

   At the end of this assembly procedure, the following equation system of equilibrium is formed:

   

   where

   = current global stiffness matrix,

   = iterative displacement vector,

   = global residual force vector or unbalanced force vector.

   

   where

   = current external force (based on the factors for the current load step),

   = current element nodal force vectors.

4. Solves the above equation for .
5. Updates the total nodal displacement vector, .

6. Checks convergence:

   Displacement norm , and

   Residual force norm ,

   where and are convergence tolerances on displacement and residual force, respectively, and are norms of iterative and total displacement vectors, respectively, is the norm of the currently applied force vector, and is the norm of the residual force vector in the current iteration.

7. If either of the criteria is not satisfied, continues the iteration by returning to Step 3. If both of the convergence criteria are satisfied, returns to Step 2 to start the next load step, or stops if at the last load step.

Notes

• The Nonlinear Static solver uses an algorithm based on the modified Newton-Raphson method.
• The load steps are defined in the load table. In this table, each column contains load combination factors for the corresponding load step or increment. For example, if the full load is applied in ten steps, there will be ten columns in this table. In each column, combination factors are entered for each load case to define the total combined load to be applied in the load step. Each column represents to total currently applied load, not the difference between the current load and the previous load. (See SOLVERS: Load (Nonlinear Static))
• Multiple freedom cases may be used, with the constant enforced displacement terms combined using the factors in the load table.
• The stiffness matrix need not be updated at every iteration. Different strategies for global stiffness matrix updating are available (see SOLVERS Parameters: ITERATION (Structural)).
• Automatic load step adjustment can be enabled to control the load increment to achieve a better convergence rate and more importantly to avoid divergence. Before the solution is available, it is sometimes difficult to know exactly how the load increments should be set. By using the automatic load stepping, the solver will adjust the load based on a number of factors, including convergence or lack thereof. (See SOLVERS Parameters: SUB-STEPPING (Static))
• Realistic model data is essential for the validity and convergence of the nonlinear solution.
• Contact elements require a nonlinear analysis. These are always considered in the Nonlinear Static solver, irrespective of the type of nonlinearity selected in SOLVERS Home: Nonlinearity (i.e., MNL, GNL).
• Restart can be used to continue a previously completed or terminated solution. The restart can proceed from any of the previously saved solution steps, provided the restart file has been saved (see SOLVERS: Files and Special Topics: Solution Restart).

See Also

• SOLVERS: Nonlinear Static Settings
• Solvers Overview