Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
“Defining a concentrated force,” Section 16.9.1 of the Abaqus/CAE User's Manual
“Defining a moment,” Section 16.9.2 of the Abaqus/CAE User's Manual
“Defining a generalized plane strain load,” Section 16.9.10 of the Abaqus/CAE User's Manual
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
Multiple concentrated load cases can be defined in random response analysis (see “Random response analysis,” Section 6.3.11, 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,” Section 30.4.5.
Actuation loads in connector elements can be defined as connector loads, applied similarly to concentrated loads. See “Connector actuation,” Section 28.1.3, for more detailed information.
The procedures in which these loads can be used are outlined in “Prescribed conditions: overview,” Section 30.1.1. See “Applying loads: overview,” Section 30.4.1, for general information that applies to all types of loading.
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.
| Input File Usage: | *CLOAD |
| Abaqus/CAE Usage: | Load module: Create Load: choose Mechanical for the Category and Concentrated force, Moment, or Generalized plane strain for the Types for Selected Step |
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.”
| Input File Usage: | *CLOAD, FOLLOWER |
| Abaqus/CAE Usage: | Load module: Create Load: choose Mechanical for the Category and Concentrated force, Moment, or Generalized plane strain for the Types for Selected Step: Follow nodal rotation |
The prescribed magnitude of a concentrated load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 30.1.1. If different variations are needed for different loads, each load can refer to its own amplitude.
Concentrated loads can be added, modified, or removed as described in “Applying loads: overview,” Section 30.4.1.
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 “Procedures: overview,” Section 6.1.1, for more information on the unsymmetric matrix storage and solution scheme.