Concentrated Loads

Concentrated loads:

  • apply concentrated forces and moments to nodal degrees of freedom; and

  • can be fixed in direction; or

  • can rotate as the node rotates (referred to as follower forces), resulting in an additional, and possibly unsymmetric, contribution to the load stiffness

In steady-state dynamic analysis both real and imaginary concentrated loads can be applied (see Direct-Solution Steady-State Dynamic Analysis and Mode-Based Steady-State Dynamic Analysis for details).

Multiple concentrated load cases can be defined in random response analysis (see Random Response Analysis for details).

Concentrated loads are also used to apply the pressure-conjugate at nodes with pressure degree of freedom in acoustic analysis (see Acoustic and Shock Loads).

Actuation loads in connector elements can be defined as connector loads, applied similarly to concentrated loads. See Connector Actuation for more detailed information.

The procedures in which these loads can be used are outlined in About Prescribed Conditions. See About Loads for general information that applies to all types of loading.

This page discusses:

 

See Also
About Loads
*CLOAD

Concentrated Loads

In Abaqus/Standard and Abaqus/Explicit analyses concentrated forces or moments can be applied at any nodal degree of freedom.

You should not apply a moment load at the origin of a cylindrical coordinate system; doing so would make the radial and tangential loads indeterminate.

Specifying Concentrated Follower Forces

You can specify that the direction of a concentrated force should rotate with the node to which it is applied. This specification should be used only in large-displacement analysis and can be used only at nodes with active rotational degrees of freedom (such as the nodes of beam and shell elements or, in Abaqus/Explicit, tie nodes on a rigid body), excluding the reference node of generalized plane strain elements. If you specify follower forces, the components of the concentrated force must be specified with respect to the reference configuration.

Follower loads lead to an unsymmetric contribution to the stiffness matrix that is generally referred to as the load stiffness. Some issues associated with the load stiffness contribution are discussed in Improving the Rate of Convergence in Large-Displacement Implicit Analysis.

Defining the Values of Concentrated Nodal Force from a User-Specified File

You can define nodal force using nodal force output from a particular step and increment in the output database (.odb) file of a previous Abaqus analysis. The part (.prt) file from the original analysis is also required when reading data from the output database file. In this case both the previous model and the current model must be defined consistently, including node numbering, which must be the same in both models. If the models are defined in terms of an assembly of part instances, part instance naming must be the same.

Defining Time-Dependent Concentrated Loads

The prescribed magnitude of a concentrated load can vary with time during a step according to an amplitude definition, as described in About Prescribed Conditions. If different variations are needed for different loads, each load can refer to its own amplitude.

Modifying Concentrated Loads

Concentrated loads can be added, modified, or removed as described in About Loads.

Improving the Rate of Convergence in Large-Displacement Implicit Analysis

When concentrated follower forces are specified in a geometrically nonlinear static and dynamic analysis, the unsymmetric matrix storage and solution scheme should normally be used. See Defining an Analysis for more information on the unsymmetric matrix storage and solution scheme.