김경종
250 lines
16 KiB
Markdown
250 lines
16 KiB
Markdown
<!-- source-page: 61 -->
|
||
|
||
during a linear perturbation analysis step. For hyperelasticity (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) or hypoelasticity (“Hypoelastic behavior,” Section 22.4.1), the tangent elastic moduli in the base state are used. If cracking has occurred—for example, in the concrete model (“Concrete smeared cracking,” Section 23.6.1)—the damaged elastic (secant) moduli are used.
|
||
|
||
• Contact conditions cannot change during a linear perturbation analysis. The open/closed status of each contact constraint remains as it is in the base state. All points in contact (i.e., with a “closed” status) are assumed to be sticking if friction is present, except the contact nodes for which a velocity differential is imposed by the motion of the reference frame or the transport velocity. At those nodes, slipping conditions are assumed regardless of the friction coefficient.
|
||
• The effects of temperature and field variable perturbations are ignored for materials that are dependent on temperature and field variables. However, temperature perturbations will produce perturbations of thermal strain.
|
||
|
||
<!-- source-page: 62 -->
|
||
|
||
<!-- source-page: 63 -->
|
||
|
||
# 6.1.4 MULTIPLE LOAD CASE ANALYSIS
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• \*LOAD CASE
|
||
• \*END LOAD CASE
|
||
• Chapter 34, “Load cases,” of the Abaqus/CAE User’s Guide
|
||
|
||
# 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
|
||
|
||
<!-- source-page: 64 -->
|
||
|
||
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
|
||
|
||
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, must be specified outside load case definitions.
|
||
|
||
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.
|
||
|
||
<!-- source-page: 65 -->
|
||
|
||
# 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 will include 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 (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).
|
||
|
||
<!-- source-page: 66 -->
|
||
|
||
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.
|
||
|
||
# Predefined fields
|
||
|
||
Field variables cannot be specified in a step with 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
|
||
|
||
```txt
|
||
*HEADING
|
||
...
|
||
*STEP, PERTURBATION
|
||
```
|
||
|
||
<!-- source-page: 67 -->
|
||
|
||
```txt
|
||
*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
|
||
```
|
||
|
||
<!-- source-page: 68 -->
|
||
|
||
```txt
|
||
*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
|
||
```
|
||
|
||
<!-- source-page: 69 -->
|
||
|
||
# 6.1.5 DIRECT LINEAR EQUATION SOLVER
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2
|
||
• “Using the Abaqus environment settings,” Section 3.3.1
|
||
• “Iterative linear equation solver,” Section 6.1.6
|
||
• “Parallel execution in Abaqus/Standard,” Section 3.5.2
|
||
• “Configuring analysis procedure settings,” Section 14.11 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
Linear equation solution is used in linear and nonlinear analysis. In nonlinear analysis Abaqus/Standard uses the Newton method or a variant of it, such as the Riks method, within which it is necessary to solve a set of linear equations at each iteration. The direct linear equation solver finds the exact solution to this system of linear equations (up to machine precision). The direct linear equation solver in Abaqus/Standard:
|
||
|
||
• uses a sparse, direct, Gauss elimination method; and
|
||
• often represents the most time consuming part of the analysis (especially for large models)—the storage of the equations occupies the largest part of the disk space during the calculations.
|
||
|
||
# The sparse solver
|
||
|
||
The direct sparse solver uses a “multifront” technique that can reduce the computational time to solve the equations dramatically if the equation system has a sparse structure. Such a matrix structure typically arises when the physical model is made from several parts or branches that are connected together; a spoked wheel is a good example of a structure that has a sparse stiffness matrix. Space frames and other structures modeled with beams, trusses, and shells often have sparse stiffness matrices. In contrast, a blocky structure—such as a single, solid, three-dimensional block (see “Elastic-plastic line spring modeling of a finite length cylinder with a part-through axial flaw,” Section 1.4.3 of the Abaqus Example Problems Guide)—provides little opportunity for the sparse solver to reduce the computer time. For large blocky structures, the iterative linear equation solver may be more efficient (see “Iterative linear equation solver,” Section 6.1.6).
|
||
|
||
Input File Usage: Use the following option to use the default direct sparse solver: \*STEP
|
||
|
||
Abaqus/CAE Usage: Step module: step editor: Other: Method: Direct
|
||
|
||
<!-- source-page: 70 -->
|
||
|
||
# Setting controls for the direct linear solver
|
||
|
||
The linear equation solver can optimize elimination of constraint equations associated with hard contact and hybrid elements. There are two potential undesirable side-effects associated with this option:
|
||
|
||
• Possible small degradation of solution accuracy may adversely impact the nonlinear convergence behavior.
|
||
• Possible minor performance degradation for models without hard contact constraints and/or hybrid elements.
|
||
|
||
Input File Usage: Use the following option to turn on constraint optimization:
|
||
|
||
\*SOLVER CONTROLS, CONSTRAINT OPTIMIZATION
|
||
|
||
Abaqus/CAE Usage: You cannot specify constraint optimization in Abaqus/CAE.
|