About Loads

External loading can be applied in the following forms: concentrated or distributed tractions, concentrated or distributed fluxes, and incident wave loads.

This page discusses:

See Also
About Prescribed Conditions
Concentrated Loads
Distributed Loads
Thermal Loads
Electromagnetic Loads
Acoustic and Shock Loads
Pore Fluid Flow
In Other Guides
General and Perturbation Procedures
Creating and modifying prescribed conditions
Using the load editors

ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE

Many types of distributed loads are provided; they depend on the element type and are described in About the Element Library. This section discusses general concepts that apply to all types of loading; see About Prescribed Conditions for general information that applies to all types of prescribed conditions.

Concentrated and distributed tractions are discussed in Concentrated Loads and Distributed Loads, respectively. Thermal loading (heat flux) is discussed in Thermal Loads. Electromagnetic loads are discussed in Electromagnetic Loads. Loads due to incident wave fields such as due to sound sources or an underwater explosion are discussed in Acoustic and Shock Loads. Pore fluid flow is discussed in Pore Fluid Flow. All other load types, which are applicable to only a single type of analysis, are discussed in the appropriate sections in Analysis Procedures and Analysis Solution and Control.

In some situations, concentrated loads and some commonly used distributed loads (such as pressure applied on a surface) may rotate during a geometrically nonlinear analysis. Such loads are known as follower loads; further details on follower loads can be found in Follower Loads in Large-Displacement Analysis, Specifying Concentrated Follower Forces, Follower Surface Loads, and Follower Edge and Line Loads. Follower loads may also lead to an unsymmetric contribution to the stiffness matrix, which is generally referred to as the load stiffness; some issues related to the load stiffness contribution are discussed in Improving the Rate of Convergence in Large-Displacement Implicit Analysis and Improving the Rate of Convergence in Large-Displacement Implicit Analysis.

Element-Based Versus Surface-Based Distributed Loads

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 can be element-based or surface-based, while distributed body loads are prescribed on geometric bodies or element bodies.

Element-Based Loads

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 About the Element Library 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.

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 Element-Based Surface Definition. 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 ALE Adaptive Mesh Domains in Abaqus/Explicit).

Loading during General Analysis Steps

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.

Modifying Loads

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 (and for gravity and surface-based general surface traction loading, the load direction) 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, except for submodel distributed surface loads (see Surface-Based Submodeling for details). When a load is left unchanged, the following rules apply:

  • If no amplitude is associated with the load, the load remains constant at the magnitude associated with the end of the previous step.

  • If an associated amplitude is specified in terms of total time, the load continues to follow the amplitude definition.

  • If an associated amplitude is specified in terms of step time, the load remains constant at the magnitude associated with the end of the previous step unless the amplitude is specified in user subroutine UAMP (Abaqus/Standard) or VUAMP (Abaqus/Explicit), in which case the load is removed immediately.

If you apply multiple loads of the same type at the same node (and the same degree of freedom if the degree of freedom is part of the loading definition), element, node set, element set, or surface, you cannot modify these loads in the following steps; you need to remove the loads and respecify them.

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

Removing Loads

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. 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. Refer to About Prescribed Conditions 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.

Example

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

Follower Loads in Large-Displacement Analysis

In large-displacement analysis distributed loads will be treated as follower forces when appropriate. For beam and shell elements point (concentrated) 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). Follower loads defined at a rigid body tie node rotate with the rigid body in Abaqus/Explicit.

Loading during Linear Perturbation Steps

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).

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.

Loading during Linear (Mode-Based) Dynamics Procedures

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.