External loading can be applied in the following forms:

Concentrated or distributed tractions.

Concentrated or distributed fluxes.

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
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.

If you apply multiple loads of the same type at the same node, 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.

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.