External loading can be applied in the following forms: concentrated or distributed
tractions, concentrated or distributed fluxes, and incident wave loads.
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.
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).
Varying the Magnitude of a Load
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 (see
About Prescribed Conditions); by a user-defined amplitude curve (see Amplitude Curves); or, in some cases, by user subroutine DLOAD, UDECURRENT, UDSECURRENT, UTRACLOAD, or VDLOAD.
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.
External work calculations when removing loads in a static analysis
External work calculations are approximate if a load is removed in a static step that is
defined with a (nondefault) step amplitude. This is because a static analysis does not
account for transient effects associated with the sudden removal of loads. Therefore, the
total energy might be nonzero following load removal.
In this situation, you can obtain a better approximation to the external work by
redefining such loads, but with a zero magnitude. In the latter case, you must ensure that
you redefine the load in exactly the same way (that is, using the same node, element, node
set, element set, or surface, as well as the load label) as it was defined in prior
steps.
In the following example, a load of magnitude 100.0 is applied in the 3-direction to all
the nodes in node set NSET_LOAD during Step 1. The load is removed
in Step 2. The redefinition of the load with a zero magnitude is optional; however, it
ensures accurate external work calculations. If accuracy of the external work calculations
is not a concern, you do not need to redefine the load.
STEPSTATICCLOAD
NSET_LOAD, 3, 100.
…
END STEPSTEP, AMP=STEPSTATICCLOAD, OP=NEW
** The redefinition of the load with a zero magnitude is optional, and added here
** to ensure more accurate external work calculations.
NSET_LOAD, 3, 0.
…
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.