Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
External loading can be applied in the following forms:
Concentrated or distributed tractions.
Concentrated or distributed fluxes.
Incident wave loads.
Concentrated and distributed tractions are discussed in “Concentrated loads,” Section 19.4.2, and “Distributed loads,” Section 19.4.3, respectively. Thermal loading (heat flux) is discussed in “Thermal loads,” Section 19.4.4. Loads due to incident wave fields such as due to an underwater explosion are discussed in “Acoustic loads,” Section 19.4.5. Pore fluid flow is discussed in “Pore fluid flow,” Section 19.4.6. All other load types, which are applicable to only a single type of analysis, are discussed in the appropriate sections in Part III, “Analysis.”
There are two ways of specifying distributed loads in ABAQUS: element-based distributed loads and surface-based distributed loads. Element-based distributed loads can be prescribed on element bodies, element surfaces, or element edges. Surface-based distributed loads can be prescribed on geometric surfaces or geometric edges. In ABAQUS/CAE distributed surface and edge loads are always surface-based, while distributed body loads are prescribed on geometric bodies or element bodies.
Use element-based loads to define distributed loads on element surfaces, element edges, and element bodies. With element-based loads you must provide the element number (or an element set name) and the distributed load type label. The load type label identifies the type of load and the element face or edge on which the load is prescribed (see Part V, “Elements,” for definitions of the distributed load types available for particular elements). This method of specifying distributed loads is very general and can be used for all distributed load types and elements. In ABAQUS/CAE, however, distributed loads are always defined on geometric regions of the model rather than elements; i.e., they are essentially surface-based loads.
Use surface-based loads to prescribe a distributed load on a geometric surface or geometric edge. With surface-based loads you must specify the surface or edge name and the distributed load type. The surface or edge, which contains the element and face information, is defined as described in “Defining element-based surfaces,” Section 2.3.2. In ABAQUS/CAE surfaces can be defined as collections of geometric faces and edges or collections of element faces and edges. This method of prescribing a distributed load facilitates user input for complex models. It can be used with most element types for which a valid surface can be defined. You can specify in the surface definition how the distributed load is applied to the boundary of an adaptive mesh domain in ABAQUS/Explicit (see “Defining adaptive mesh domains in ABAQUS/Explicit,” Section 7.17.2).
The magnitude of a load is usually defined by the input data. The variation of the load magnitude during a step can be defined by the default amplitude variation for the step; by a user-defined amplitude curve; or, in some cases, by a user subroutine (see “Prescribed conditions: overview,” Section 19.1.1; “Amplitude curves,” Section 19.1.2; “DLOAD,” Section 25.2.5; and “VDLOAD,” Section 25.3.1).
If the analysis consists of one step only, the loads are defined in that step. If there are several analysis steps, the definition of loading in each analysis step depends on whether that step and the previous steps are general analysis steps or linear perturbation steps. Loading during linear perturbation steps is discussed below.
In general analysis steps, load magnitudes must always be given as total values, not as changes in magnitude. Multiple definitions of the same load condition in the same step are applied additively. Element-based and surface-based distributed loads are considered independently. For example, element-based and surface-based pressures applied to an element face in the same step are added. A single redefinition of that same load condition in a subsequent step, however, replaces all the like definitions (same load option, same load type) given in previous steps according to the rules described in “Removing loads” below.
Any combination of loads can be applied together during a step. For a linear step it is possible to analyze several load cases based on the same stiffness.
At each new step the loading can be either modified or completely redefined. To redefine a load, the node, element, node set, element set, or surface name must be specified in exactly the same way and the load type must be identical. For example, if a node is part of a loaded node set in one step and is loaded as an individual node (by listing its node number) in another step, the loads will be added.
All loads defined in previous steps remain unchanged unless they are redefined. When a load is left unchanged, the following rules apply:
If the associated amplitude was specified in terms of total time, the load continues to follow the amplitude definition.
If no amplitude was associated with the load or if the amplitude was given in terms of step time, the load remains constant at the magnitude associated with the end of the previous step.
| Input File Usage: | Use either of the following options to modify an existing load or to specify an additional load (*LOADING OPTION represents any load type): |
*LOADING OPTION *LOADING OPTION, OP=MOD |
| ABAQUS/CAE Usage: | Load module: Create Load or Load Manager: Edit |
If you choose to remove any load of a particular type (concentrated load, element-based distributed load, surface-based distributed load, etc.) in a step, no loads of that type will be propagated from the previous general step. All loads of that type that are in effect during this step must be respecified. Refer to “Prescribed conditions: overview,” Section 19.1.1, for a discussion of amplitude variations when removing loads.
| Input File Usage: | Use the following option to release all previously applied loads of a given type and to specify new loads (*LOADING OPTION represents any load type): |
*LOADING OPTION, OP=NEW For example, *CLOAD, OP=NEW with no data lines will remove all concentrated forces and moments from the model. If the OP=NEW parameter is used on any loading option in a step, it must be used on all loading options of the same type within the step. |
| ABAQUS/CAE Usage: | Use the following option to remove a load within a step: |
Load module: Load Manager: Deactivate ABAQUS/CAE automatically respecifies any loads that should remain in effect during this step. |
In the history definition input file section shown below, the distributed load (type BX) applied to element set A2 has a magnitude of 20.0 in the first step, which is changed to 50.0 in the second step. Both the set identifier (or element or node number) and the load type must be identical in both steps for ABAQUS to identify a load for redefinition.
In Step 1 a concentrated load of magnitude 10.0 is applied to degree of freedom 3 of all nodes in node set NLEFT. In Step 2 a concentrated load of magnitude 5.0 is applied to degree of freedom 3 of node 1. If node 1 is in node set NLEFT, the total load applied in Step 2 at this node is 15.0: the loads add.
The two distributed loads of type P1 acting on element set E1 in Step 1 will be added to give a total distributed load of 43.0.
The pressure loads on element sets B3 and E1 are active during both steps.
*STEP Step 1 *STATIC *CLOAD NLEFT, 3, 10. *DLOAD A2, BX, 20. B3, P1, 5. E1, P1, 21. *DLOAD E1, P1, 22. *END STEP ** *STEP Step 2 *STATIC *CLOAD 1, 3, 5. *DLOAD, OP=MOD A2, BX, 50. *END STEP
In large-displacement analysis distributed loads will be treated as follower forces when appropriate. For beam and shell elements point loads may be fixed in direction or they may rotate with the structure depending on whether you specify follower forces for the load (see “Concentrated loads,” Section 19.4.2). Follower loads defined at a rigid body tie node rotate with the rigid body in ABAQUS/Explicit.
In a linear perturbation step (available only in ABAQUS/Standard) the state at the end of the previous general analysis step is considered as the “base state.” If the linear perturbation step is the first step of the analysis, the initial conditions of the model form the base state. Loading during a linear perturbation step must be defined as the change in load from the base state (the perturbation of load), not the total of the base state load plus the perturbation load.
In consecutive linear perturbation steps, the perturbation of load that applies to each step must be defined completely within that step—the analysis within each such step always starts from the base state (except when you specify that a modal dynamic step should use the initial conditions from the immediately preceding step—see “Transient modal dynamic analysis,” Section 6.3.7).
In nonlinear steps that follow linear perturbation analysis steps, the analysis is continued from the base state as if the intermediate linear perturbation steps did not exist.
If a user subroutine is used to define loading in a mode-based linear dynamics analysis, the subroutine will be called only at the beginning of the step to obtain the magnitude of the load. The load magnitude then remains constant in the step unless it is modified by an amplitude curve.