is used to study the linear responses of a structure subjected to distinct sets of loads,
predefined temperature fields, and boundary conditions defined within a step (each set is
referred to as a load case);
can be much more efficient than an equivalent multiple perturbation step analysis;
allows you to change mechanical loads, temperatures, and boundary conditions from linear
load case to linear load case;
includes the effects of the base state; and
can be performed with static perturbation, direct-solution steady-state dynamic, and
SIM-based steady-state dynamic analyses.
A linear load case refers to a set of loads, temperatures, boundary conditions, and base
motions comprising a particular loading condition. For example, in a simplified model the
operational environment of an airplane might be broken into five linear load cases: (1)
take-off, (2) climb, (3) cruise, (4) descent, and (5) landing. Often a linear load case is
defined in terms of unit loads or prescribed boundary conditions, and a multiple linear load
case analysis refers to the simultaneous solution for the responses of each linear load case
in a set of such linear load cases. These responses can then be scaled and linearly combined
during postprocessing to represent the actual loading environment. Other postprocessing
manipulations on linear load cases are also common, such as finding the maximum von Mises
stress among all linear load cases. These types of linear load case
manipulations can be requested in the Visualization module of Abaqus/CAE (see the Introduction).
Using Multiple Linear Load Cases
A multiple linear load case analysis is conceptually equivalent to a multiple step analysis
in which the linear load case definitions are mapped to consecutive perturbation steps.
However, a multiple linear load case analysis is generally much more efficient than the
equivalent multiple step analysis. The exception occurs when a large number of boundary
conditions exist that are not common to all linear load cases (that is, degrees of freedom
are constrained in one linear load case but not others). It is difficult to define what
“large” is since it is model dependent. The relative performance of the two analysis methods
can be assessed by performing a data check analysis for both the multiple linear load case
analysis and the equivalent multiple step analysis. The data check analysis writes resource
information for each step to the data file, including the maximum wavefront, number of
floating point operations, and minimum memory required. If these numbers are noticeably
larger for the multiple linear load case step compared to those across all steps of the
equivalent multiple step analysis (the number of floating point operations can be summed
over all steps before comparing), the multiple step analysis is more efficient.
Although generally more efficient, the multiple linear load case analysis might consume
more memory and disk space than an equivalent multiple step analysis. Thus, for large
problems or problems with many load cases it is again advisable, as described above, to
compare resource usage between the multiple linear load case analysis and the equivalent
multiple step analysis. If resource requirements for the multiple linear load case analysis
are deemed too large, consider dividing the linear load cases among a few steps. The
resulting analysis (a hybrid of multiple linear load cases and multiple steps) requires
fewer resources while retaining an efficiency advantage over an equivalent pure multiple
step analysis.
Defining Linear Load Cases
You define a linear load case within a static perturbation, direct-solution steady-state
dynamic, and SIM-based steady-state dynamic analyses.
Linear load case definitions do not propagate to subsequent steps. Only the following types
of prescribed conditions can be specified within a linear load case definition:
Boundary conditions
Concentrated loads
Distributed loads
Distributed surface loads
Predefined temperature fields
Inertia-based loads
Base motions
Output requests to the output database
Additional rules governing these prescribed conditions are described in the sections that
follow. No other types of prescribed conditions can appear in a step that contains linear
load case definitions. All other valid analysis components, such as output requests to the
data file, must be specified outside the linear load case definitions.
Each linear load case definition is assigned a name for postprocessing purposes.
Input File Usage
Use the first option to begin a linear load case and the second option to end a linear
load case:
Prescribed conditions specified within a linear load case definition apply only to
that linear load case. In static perturbation and direct-solution steady-state dynamic
analyses, prescribed conditions can be specified outside the linear load case definitions
(in this case they apply to all linear load cases in the step).
Abaqus/CAE Usage
Load module: Create Load Case: Name: name
In Abaqus/CAE if a step contains linear load cases, all prescribed conditions in the step must be
included in one or more linear load cases.
Procedures
Linear load cases can be defined only in perturbation steps with the following procedures:
Static
Direct-solution, steady-state dynamic
SIM-based, steady-state dynamic
As with other perturbation steps, a multiple linear load case analysis includes the
nonlinear effects of the previous general step (base state). The following analysis
techniques are not supported in the context of a linear load case step:
Restart from a particular linear load case
Submodeling using results from other than the first linear load case in the global
analysis
Importing and transferring results
Cyclic symmetry analysis
Contour integrals
Design sensitivity analysis
Boundary Conditions
Boundary conditions can be specified both outside and inside linear load case definitions
in the same step. Specifying a boundary condition outside the linear load case definitions
in a step is equivalent to including it in all linear load case definitions in the step
(that is, the boundary condition is applied to all linear load cases). Unless any boundary
conditions are removed in the perturbation step, the boundary conditions that are active in
the base state will propagate to all linear load cases in the perturbation step. If any
boundary condition is removed in a step with linear load cases (either outside or inside the
linear load case definitions), the base state boundary conditions will not be propagated to
any linear load case in the step. See Boundary Conditions for more information.
You should redefine identical boundary conditions between linear load cases as described in
Boundary Conditions. You must apply constraints consistently using either the
“type” (name) format or the degree of freedom “direct” format without changing the format
between linear load cases. Otherwise, Abaqus treats the redefined boundary conditions as changing between linear load cases, which
increases the computational cost of the analysis.
Note:
In Abaqus/CAE if a step contains linear load cases, all boundary conditions in the step must be
included in one or more linear load cases. Boundary conditions can only be used with
linear load cases in static perturbation and direct-solution steady-state dynamic
analyses.
Loads
In static perturbation and direct-solution steady-state dynamic analyses, you can specify
concentrated, distributed, and distributed surface loads both outside and inside linear load
case definitions in the same step. The only exceptions are Coriolis and rotor dynamic loads,
which cannot be specified inside linear load case definitions in a direct-solution
steady-state dynamic step. These loads contribute to the left hand side of the system of
element equations. Any changes to these loads within the linear load case definitions
results in changes to the left hand side of the overall system of equations from linear load
case to linear load case.
You can specify inertia relief loads either outside linear load case definitions or inside
linear load case definitions in the same step but not both simultaneously. Specifying one of
these load types outside the linear load case definitions in a step is equivalent to
including it in all linear load case definitions in the step (that is, the loading is
applied to all linear load cases).
Connector loads and connector motion are not supported for a linear load case analysis.
In SIM-based steady-state dynamic analyses concentrated,
distributed, distributed surface loads, and base motion can be specified only inside linear
load case definitions in the same step. Inertia relief loads are not supported.
Linear load cases cannot be used in models that include aqua loads (see Abaqus/Aqua Analysis).
As with any perturbation step, perturbation loads must be defined completely within the
perturbation step (see About Loads).
Note:
In Abaqus/CAE if a step contains linear load cases, all loads in the step must be included in one or
more linear load cases.
Predefined Fields
In static perturbation analyses you can specify predefined temperature fields both outside
and inside linear load case definitions within the same step. Specifying temperature outside
the linear load case definitions in a step is equivalent to including it in all linear load
case definitions in the step. If a temperature field is specified at the same node both
outside and inside a linear load case, the temperature definition inside the linear load
case takes precedence, and the temperature definition outside the linear load case is
discarded at this node.
You cannot specify field variables in a step with linear load cases.
Elements
Linear load cases cannot be used in models that include piezoelectric elements (see Piezoelectric Analysis).
Output
In a step containing one or more linear load cases, only selected field and history output
requests to the output database and output requests to the data file are supported. Output
requests to the results file are not supported. Output requests specified outside linear
load case definitions apply to all linear load cases in a step. Output requests to the
output database specified inside a specific linear load case definition apply only to that
linear load case. Output requests to the data file are not supported inside a linear load
case. Output requests inside a linear load case do not propagate to subsequent steps. For
all other output requests, the step propagation rules are the same as for other perturbation
steps (see About Output).
The available field output corresponding to each linear load case is stored in a separate
frame on the output database with the linear load case name included as a frame attribute.
To distinguish between linear load cases for history output variables, the name of the
linear load case is appended to the history variable name. The
Visualization module of Abaqus/CAE and the Abaqus Scripting Interface (see Using the Abaqus Scripting Interface to access an output database) can be used
to access and manipulate linear load case output.Abaqus/Standard does not perform consistency checks on the physical validity of the linear load case
manipulations. For example, the linear superposition of two linear load cases, each with
different boundary conditions, is allowed even though the combined results might not be
physically meaningful.
Limitations
For frame elements, the temperature specified inside a linear load case definition is
ignored.
Input File Template
HEADING
…
STEP, PERTURBATIONSTATICorSTEADY STATE DYNAMICS, DIRECT
…
OUTPUT, FIELD
…
BOUNDARYData lines to specify boundary conditions for all linear load cases.DLOADData lines to specify distributed loads for all linear load cases.CLOADData lines to specify point loads for all linear load cases.DSLOADData lines to specify distributed surface loads for all linear load cases.INERTIA RELIEFData lines to specify inertia relief loading directions.
(This option cannot be used inside linear load cases if it is used here.)
…
LOAD CASE, NAME=name1BOUNDARYData lines to specify boundary conditions for first linear load case.DLOADData lines to specify distributed loads for first linear load case.CLOADData lines to specify point loads for first linear load case.DSLOADData lines to specify distributed surface loads for first linear load case.INERTIA RELIEFData lines to specify inertia relief loading directions.
(This option cannot be used outside linear load cases if it is used here.)END LOAD CASELOAD CASE, NAME=name2Load and boundary condition options for second linear load caseEND LOAD CASE
…
Subsequent linear load case definitions
…
END STEPSTEP, PERTURBATIONFREQUENCY, SIMorFREQUENCY, EIGENSOLVER=AMSEND STEP
…
STEP, PERTURBATIONSTEADY STATE DYNAMICSLOAD CASE, NAME=name3BASE MOTIONData lines to specify base motion for first linear load case.DLOADData lines to specify distributed loads for first linear load case.CLOADData lines to specify point loads for first linear load case.DSLOADData lines to specify distributed surface loads for first linear load case.END LOAD CASELOAD CASE, NAME=name4Load and base motion options for second linear load case.END LOAD CASE
…
Subsequent linear load case definitions
…
OUTPUT, HISTORY
…
END STEPSTEP, PERTURBATIONSTATIC
…
OUTPUT, FIELD
…
BOUNDARYData lines to specify boundary conditions for all linear load cases.LOAD CASE, NAME=name5, GENERATEDSLOADData lines to specify distributed nodal pressure linear load cases on surfaces.END LOAD CASE
…
Subsequent linear load case definitions
…
END STEPSTEP, PERTURBATIONSTATICTEMPERATUREData lines to specify temperature for all linear load cases.LOAD CASE, NAME=name6TEMPERATUREData lines to specify temperature for first linear load case.END LOAD CASE
…
Subsequent linear load case definitions
…
END STEP