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 the Abaqus Analysis Guide.
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.
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.
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.
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.
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.
|