Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
“Defining a concentrated force,” Section 16.9.1 of the Abaqus/CAE User's Guide
“Defining a moment,” Section 16.9.2 of the Abaqus/CAE User's Guide
“Defining a generalized plane strain load,” Section 16.9.10 of the Abaqus/CAE User's Guide
“Defining a fluid reference pressure,” Section 16.9.23 of the Abaqus/CAE User's Guide
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 34.4.6) and to specify a fluid reference pressure for incompressible flow (see “Incompressible fluid dynamic analysis,” Section 6.6.2).
Actuation loads in connector elements can be defined as connector loads, applied similarly to concentrated loads. See “Connector actuation,” Section 31.1.3, for more detailed information.
The procedures in which these loads can be used are outlined in “Prescribed conditions: overview,” Section 34.1.1. See “Applying loads: overview,” Section 34.4.1, for general information that applies to all types of loading.
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.
| Input File Usage: | *CLOAD node number or node set, degree of freedom, magnitude |
| 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 or Moment for the Types for Selected Step: Follow nodal rotation |
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.
| Input File Usage: | *CLOAD, FILE=file, STEP=step, INC=inc |
| Abaqus/CAE Usage: | Defining the values of concentrated nodal force from a user-specified file is not supported in Abaqus/CAE. |
For incompressible fluid dynamic analyses in Abaqus/CFD, when no other pressure condition is prescribed, you must specify a fluid reference pressure at one node to set the hydrostatic pressure level. Multiple reference pressures can be specified, but only the last specified hydrostatic pressure load is applied. For more information, see “Incompressible fluid dynamic analysis,” Section 6.6.2, and “Boundary conditions in Abaqus/CFD,” Section 34.3.2.
| Input File Usage: | *CLOAD node number or node set, HP, magnitude |
| Abaqus/CAE Usage: | Load module: Create Load: choose Fluid for the Category and Fluid reference pressure for the Types for Selected Step |
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 34.1.1. 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 34.4.1.
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 “Defining an analysis,” Section 6.1.2, for more information on the unsymmetric matrix storage and solution scheme.