6.1.4 Multiple load case analysis
Products: Abaqus/Standard Abaqus/CAE
Overview
A multiple load case analysis:
is used to study the linear responses of a structure subjected to distinct sets of loads 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 for the changing of mechanical loads and boundary conditions from load case to 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.
Load cases
A load case refers to a set of loads, 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 Mises stress among all load cases. These types of load case manipulations can be requested in the Visualization module of Abaqus/CAE (see the Abaqus/CAE User's Guide).
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 (i.e., 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 should be summed over all steps before comparing), the multiple step analysis will be 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) will require 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
Inertia-based loads
Base motions
Each load case definition is assigned a name for postprocessing purposes.
| Input File Usage: | Use the first option to begin a load case and the second option to end a load case: |
*LOAD CASE, NAME=name *END LOAD CASE Prescribed conditions specified within a load case definition apply only to that load case. In static perturbation and direct-solution steady-state dynamic analyses, prescribed conditions can be specified outside the load case definitions (in this case they apply to all load cases in the step). |
| Abaqus/CAE Usage: | Load module: Create Load Case: Name: name |
In Abaqus/CAE if a step contains load cases, all prescribed conditions in the step must be included in one or more load cases. |
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
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 (i.e., the boundary condition will be 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 in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1, for more information.
Note: In Abaqus/CAE if a step contains load cases, all boundary conditions in the step must be included in one or more load cases. Boundary conditions can only be used with load cases in static perturbation and direct-solution steady-state dynamic analyses.
Loads
In static perturbation and direct-solution steady-state dynamic analyses concentrated, distributed, and distributed surface loads can be specified both outside and inside load case definitions in the same step. Inertia relief loads can be specified 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 (i.e., the loading will be applied to all load cases).
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,” Section 6.11.1).
As with any perturbation step, perturbation loads must be defined completely within the perturbation step (see “Applying loads: overview,” Section 34.4.1).
Note: In Abaqus/CAE if a step contains load cases, all loads in the step must be included in one or more load cases.
Elements
Load cases cannot be used in models that include piezoelectric elements (see “Piezoelectric analysis,” Section 6.7.2).
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 can be specified only outside load case definitions, and they apply to all load cases in a step. The step propagation rules for output requests are the same as for other perturbation steps (see “Output,” Section 4.1.1).
Element and energy history output variables are not available during a multiple load case analysis (see “Abaqus/Standard output variable identifiers,” Section 4.2.1). Additional restrictions apply for a SIM-based steady-state dynamic analysis; see “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1, 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. The Visualization module of Abaqus/CAE and the Abaqus Scripting Interface (see Chapter 9, “Using the Abaqus Scripting Interface to access an output database,” of the Abaqus Scripting User's Guide) can be used to access and manipulate load case output. 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.
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