|
Load Cases
A 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 load cases: (1) take-off,
(2) climb, (3) cruise, (4) descent, and (5) landing. Often a load case is defined in terms
of unit loads or prescribed boundary conditions, and a multiple load case analysis refers to
the simultaneous solution for the responses of each load case in a set of such load cases.
These responses can then be scaled and linearly combined during postprocessing to represent
the actual loading environment. Other postprocessing manipulations on load cases are also
common, such as finding the maximum von Mises stress among all load cases.
Using Multiple Load Cases
A multiple load case analysis is conceptually equivalent to a multiple step analysis in which the
load case definitions are mapped to consecutive perturbation steps. However, a multiple 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 load cases (that is, degrees of freedom are constrained in one 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 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 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 load case analysis may 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 load case analysis and the equivalent multiple step analysis. If
resource requirements for the multiple load case analysis are deemed too large, consider
dividing the load cases among a few steps. The resulting analysis (a hybrid of multiple load
cases and multiple steps) requires fewer resources while retaining an efficiency advantage
over an equivalent pure multiple step analysis.
Defining Load Cases
You define a load case within a static perturbation, direct-solution
steady-state dynamic, and SIM-based
steady-state dynamic analyses. Load case definitions do not propagate to
subsequent steps. Only the following types of prescribed conditions can be
specified within a 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 load case definitions. All other valid analysis components,
such as output requests to the data file, must be specified outside load case
definitions.
Each load case definition is assigned a name for postprocessing purposes.
Procedures
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 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 load case step:
-
Restart from a particular load case
-
Submodeling using results from other than the first 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 load case definitions in the same
step. Specifying a boundary condition outside the load case definitions in a step is
equivalent to including it in all load case definitions in the step (that is, the boundary
condition is applied to all 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 load cases in the perturbation step. If any boundary condition is removed in a step
with load cases (either outside or inside load case definitions), the base state boundary
conditions will not be propagated to any load case in the step. See Boundary Conditions for more information.
You should redefine identical boundary conditions between 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 load cases. Otherwise, Abaqus treats the redefined boundary conditions as changing between load cases, which increases
the computational cost of the analysis.
Loads
In static perturbation and direct-solution steady-state dynamic analyses, you can specify
concentrated, distributed, and distributed surface loads both outside and inside load case
definitions in the same step. The only exceptions are Coriolis and rotor dynamic loads,
which cannot be specified inside 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 load case definitions results in changes to
the left hand side of the overall system of equations from load case to load case.
You can specify inertia relief loads either outside load case definitions or inside load
case definitions in the same step but not both simultaneously. Specifying one of these load
types outside the load case definitions in a step is equivalent to including it in all load
case definitions in the step (that is, the loading is applied to all load cases).
Connector loads and connector motion are not supported for a load case analysis.
In SIM-based steady-state dynamic analyses
concentrated, distributed, distributed surface loads, and base motion can be
specified only inside load case definitions in the same step. Inertia relief
loads are not supported.
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).
Predefined Fields
In static perturbation analyses you can specify predefined temperature fields both outside
and inside load case definitions within the same step. Specifying temperature outside the
load case definitions in a step is equivalent to including it in all load case definitions
in the step. If a temperature field is specified at the same node both outside and inside a
load case, the temperature definition inside the load case takes precedence, and the
temperature definition outside the load case is discarded at this node.
You cannot specify field variables in a step with load cases.
Elements
Load cases cannot be used in models that include piezoelectric elements (see
Piezoelectric Analysis).
Output
In a step containing one or more 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 load case definitions apply to all load cases in a
step. Output requests to the output database specified inside a specific load
case definition apply only to that load case. Output requests to the data file
are not supported inside a load case. Output requests inside a 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).
Element and energy history output variables are not available during a
multiple load case analysis (see
Abaqus/Standard Output Variable Identifiers).
Additional restrictions apply for a SIM-based
steady-state dynamic analysis; see
Using the SIM Architecture for Modal Superposition Dynamic Analyses
for more information.
The available field output corresponding to each load case is stored in a
separate frame on the output database with the load case name included as a
frame attribute. To distinguish between load cases for history output
variables, the name of the load case is appended to the history variable name.
Abaqus/Standard
does not perform consistency checks on the physical validity of the load case
manipulations. For example, the linear superposition of two load cases, each
with different boundary conditions, is allowed even though the combined results
may not be physically meaningful.
Limitations
For frame elements, the temperature specified inside a load case definition is ignored.
Input File Template
HEADING
…
STEP, PERTURBATION
STATIC or STEADY STATE DYNAMICS, DIRECT
…
OUTPUT, FIELD
…
BOUNDARY
Data lines to specify boundary conditions for all load cases.
DLOAD
Data lines to specify distributed loads for all load cases.
CLOAD
Data lines to specify point loads for all load cases.
DSLOAD
Data lines to specify distributed surface loads for all load cases.
INERTIA RELIEF
Data lines to specify inertia relief loading directions.
(This option cannot be used inside load cases if it is used here.)
…
LOAD CASE, NAME=name1
BOUNDARY
Data lines to specify boundary conditions for first load case.
DLOAD
Data lines to specify distributed loads for first load case.
CLOAD
Data lines to specify point loads for first load case.
DSLOAD
Data lines to specify distributed surface loads for first load case.
INERTIA RELIEF
Data lines to specify inertia relief loading directions.
(This option cannot be used outside load cases if it is used here.)
END LOAD CASE
LOAD CASE, NAME=name2
Load and boundary condition options for second load case
END LOAD CASE
…
Subsequent load case definitions
…
END STEP
STEP, PERTURBATION
FREQUENCY, SIM or FREQUENCY, EIGENSOLVER=AMS
END STEP
…
STEP, PERTURBATION
STEADY STATE DYNAMICS
LOAD CASE, NAME=name3
BASE MOTION
Data lines to specify base motion for first load case.
DLOAD
Data lines to specify distributed loads for first load case.
CLOAD
Data lines to specify point loads for first load case.
DSLOAD
Data lines to specify distributed surface loads for first load case.
END LOAD CASE
LOAD CASE, NAME=name4
Load and base motion options for second load case.
END LOAD CASE
…
Subsequent load case definitions
…
OUTPUT, HISTORY
…
END STEP
STEP, PERTURBATION
STATIC
…
OUTPUT, FIELD
…
BOUNDARY
Data lines to specify boundary conditions for all load cases.
LOAD CASE, NAME=name5, GENERATE
DSLOAD
Data lines to specify distributed nodal pressure load cases on surfaces.
END LOAD CASE
…
Subsequent load case definitions
…
END STEP
STEP, PERTURBATION
STATIC
TEMPERATURE
Data lines to specify temperature for all load cases.
LOAD CASE, NAME=name6
TEMPERATURE
Data lines to specify temperature for first load case.
END LOAD CASE
…
Subsequent load case definitions
…
END STEP |