김경종
178 lines
14 KiB
Markdown
178 lines
14 KiB
Markdown
<!-- source-page: 1201 -->
|
||
|
||
# Initial conditions
|
||
|
||
The solution mapped from the initial analysis forms the initial conditions for the remeshed analysis. Initial conditions such as temperature for a pure stress/displacement analysis can be specified. Any other specified initial conditions will be ignored.
|
||
|
||
# Boundary conditions
|
||
|
||
Boundary conditions are not carried over from the old mesh to the new mesh. The boundary conditions applied at the beginning of the remeshed analysis should normally be the same as those in effect at the step and increment selected from the initial analysis. Although boundary conditions can be changed, the problem may fail to converge if the structure is far from an equilibrium state.
|
||
|
||
There are no restrictions on applying boundary conditions in a mapped solution analysis. Boundary conditions can be applied to all available degrees of freedom in the same way as they are applied in an analysis without a mapped solution (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1).
|
||
|
||
# Loads
|
||
|
||
There are no restrictions on applying loads in a mapped solution analysis. Loads can be applied in the same way as they are applied in an analysis without a mapped solution.
|
||
|
||
The loads applied at the beginning of the remeshed analysis should normally be the same as those in effect at the end of the initial analysis. Although the loads can be changed, the problem may fail to converge if the structure is far from an equilibrium state.
|
||
|
||
# Predefined fields
|
||
|
||
Temperature and field variables are mapped from the old mesh to the new mesh. If the number of field variables is changed in the remeshed analysis, the number common to both analyses will be transferred. Predefined fields can be modified in the same way as they are modified in an analysis without solution mapping (see “Predefined fields,” Section 34.6.1).
|
||
|
||
# Material options
|
||
|
||
Any of the mechanical constitutive models available in Abaqus can be used in a mapped solution analysis (see Part V, “Materials”). There is no restriction on agreement between material models in the old and new analyses. The solution mapping algorithm will transfer those variables common to both models. You must ensure that the material models are compatible.
|
||
|
||
# Elements
|
||
|
||
The solution mapping capability can be used only with continuum elements (see “Solid (continuum) elements,” Section 28.1.1).
|
||
|
||
<!-- source-page: 1202 -->
|
||
|
||
# Output
|
||
|
||
There is no output specific to a mapped solution analysis. Output can be requested in the same way as in an analysis without a mapped solution. The output variables available in Abaqus are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
|
||
|
||
Input file template
|
||
```txt
|
||
*HEADING
|
||
*NODE
|
||
Data lines to define the new-model nodes occupying the space of the old model in its deformed configuration
|
||
*ELEMENT
|
||
Data lines to define the new-model elements occupying the space of the old model in its deformed configuration
|
||
...
|
||
*MAP SOLUTION, STEP=step, INC=inc
|
||
translation and rotation data
|
||
*STEP
|
||
*STATIC (or *COUPLED TEMPERATURE-DISPLACEMENT or *GEOSTATIC or *SOILS or *VISCO)
|
||
...
|
||
*END STEP
|
||
```
|
||
|
||
<!-- source-page: 1203 -->
|
||
|
||
# 13. Optimization Techniques
|
||
|
||
Structural optimization: overview 13.1
|
||
|
||
Optimization models 13.2
|
||
|
||
<!-- source-page: 1204 -->
|
||
|
||
<!-- source-page: 1205 -->
|
||
|
||
# 13.1 Structural optimization: overview
|
||
|
||
• “Structural optimization: overview,” Section 13.1.1
|
||
|
||
<!-- source-page: 1206 -->
|
||
|
||
<!-- source-page: 1207 -->
|
||
|
||
# 13.1.1 STRUCTURAL OPTIMIZATION: OVERVIEW
|
||
|
||
Structural optimization using Abaqus is an iterative process that helps you refine your designs. The result of a well-designed structural optimization is a component that is lightweight, rigid, and durable. Abaqus provides the following approaches to structural optimization: topology optimization, shape optimization, sizing optimization, and bead optimization. Topology optimization starts with an initial model and determines an optimum design by modifying the properties of the material in selected elements, effectively removing elements from the analysis. Shape and sizing optimization further refine the model. Shape optimization modifies the surface of the component by moving the surface nodes to reduce local stress concentrations. Sizing optimization modifies the sheet thickness of sheet metal components; typically, to increase the stiffness or reduce vibration. Bead optimization creates stiffening beads in a shell model. Topology, shape, sizing, and bead optimization are governed by a set of objectives and constraints.
|
||
|
||
Optimization is a tool for shortening the development process by adding value to a designer’s experience and intuition with an automated procedure. To optimize your model, you need to know what to optimize. It is not sufficient to say that you want to minimize stresses or maximize eigenvalues, your statements must be more specific. For example, you might want to minimize the maximal nodal stresses experienced during two load cases. Similarly, you might want to maximize the sum of the first five eigenvalues. The goal of an optimization is called the objective function. In addition, you can enforce certain values during the optimization. For example, you can specify that the displacement of a given node must not exceed a certain value. An enforced value is called a constraint.
|
||
|
||
You use Abaqus/CAE to create the model to be optimized and to define, configure, and execute the structural optimization. For more information, see Chapter 18, “The Optimization module,” of the Abaqus/CAE User’s Guide.
|
||
|
||
# Terminology
|
||
|
||
Structural optimization introduces its own terminology. The following terms are used throughout the Abaqus documentation and the Abaqus/CAE user interface:
|
||
|
||
• Design area: The design area is the region of your model that the structural optimization modifies. The design area can be the whole model, or it can be a subset of the model containing only selected regions. Given the prescribed conditions (such as boundary conditions, loads, and manufacturing constraints),
|
||
|
||
• a topology optimization process removes and adds material from elements in the design area while it attempts to reach an optimal design,
|
||
• a shape optimization modifies the surface of the design area by moving surface nodes,
|
||
• a sizing optimization modifies the thickness of the design area by changing the thickness of shell elements, and
|
||
• a bead optimization moves nodes of shell elements in the design area in the direction of the shell normal.
|
||
|
||
<!-- source-page: 1208 -->
|
||
|
||
• Design variables: For an optimization problem, the design variables represent the parameters to be changed during the optimization.
|
||
|
||
For a topology optimization, the densities of the elements in the design area are the design variables. The Optimization module changes the density during each iteration of the optimization and couples the stiffness of each element with the density. In effect, the optimization removes elements from your model by giving them a mass and stiffness that is small enough to ensure they no longer participate in the overall response of the structure. The model with the revised material properties is then analyzed by Abaqus.
|
||
|
||
For a shape optimization, the displacements of the surface nodes in the design area are the design variables. During the optimization, the Optimization module either moves a node outward (growth) or inward (shrinkage) or leaves the position unchanged (neutral). Restrictions influence the amount a surface node can move and the direction in which it can move. The optimization directly modifies only the position of the corner nodes of elements; the Optimization module interpolates the displacement of midside nodes from the movement of the corner nodes.
|
||
|
||
For a sizing optimization, the thicknesses of the shell elements in the design area are the design variables. The Optimization module can adjust the thickness of individual shell elements, or you can require clustering—the simultaneous modification of shell thicknesses in specific areas.
|
||
|
||
For a bead optimization, the displacements of the nodes of the shell elements that form the stiffening beads in the design area are the design variables. Restrictions limit the amount a node can move and the direction in which it can move.
|
||
|
||
• Design cycle: Optimization is an iterative design process that updates the design variables, executes an Abaqus analysis of the modified model, and reviews the results to determine if an optimized solution has been reached. Each optimization iteration is called a design cycle.
|
||
|
||
• Optimization task: An optimization task contains the definition of your optimization, such as the design responses, objectives, constraints, and geometric restrictions. To run an optimization, you execute an optimization process. An optimization process refers to an optimization task.
|
||
|
||
• Design responses: The inputs to the optimization are called the design responses. Design responses can be read directly from the Abaqus output database (.odb) file; for example, stiffness, stress, eigenfrequencies, and displacements. Alternatively, the Optimization module can read data from the output database file and calculate the design responses from your model; for example, its weight, center of mass, or relative displacements.
|
||
|
||
A design response is associated with a region of your model; however, it consists of a single scalar value, such as the maximum stress within a region or the total volume of the model. In addition, a design response can be associated with a particular step or load case.
|
||
|
||
• Objective functions: Objective functions define the objective of the optimization. An objective function is a single scalar value extracted from a design response, such as the maximum displacement or the maximum stress. An objective function can be formulated from multiple design responses. If you specify that the objective functions minimize or maximize the design responses, the Optimization module calculates the objective function by adding each of the values determined from the design responses. In addition, if you have multiple objective functions, you can use a weighting factor to scale their influence on the optimization.
|
||
|
||
<!-- source-page: 1209 -->
|
||
|
||
• Constraints: Constraints are also a single scalar value extracted from a design response; however, a constraint cannot be derived from a combination of design responses. Constraints restrict the value of a design response; for example, you can specify that the volume must be reduced by 45% or the absolute displacement in a region must not exceed 1 mm. You can also apply manufacturing and geometric constraints that are independent of the optimization; for example, a structure must be able to be cast or stamped or the diameter of a bearing surface cannot be changed.
|
||
• Stop conditions: A global stop condition defines the maximum number of iterations an optimization can perform. A local stop condition specifies that the optimization should end when a local minimum (or maximum) has been reached.
|
||
|
||
# Structural optimization with Abaqus/CAE
|
||
|
||
The following steps are required to incorporate structural optimization into your Abaqus/CAE model:
|
||
|
||
• You create an Abaqus model that can be optimized. For example, the design area must include only supported elements and materials. See “Creating Abaqus optimization models,” Section 13.2.3.
|
||
• You create an optimization task. See “Creating and configuring an optimization task,” Section 18.6 of the Abaqus/CAE User’s Guide.
|
||
• You create design responses. See “Design responses,” Section 13.2.1.
|
||
• You use the design responses to create objective functions and constraints. See “Objectives and constraints,” Section 13.2.2.
|
||
• You create an optimization process and submit it for analysis. See “What is an optimization process?,” Section 19.5.1 of the Abaqus/CAE User’s Guide.
|
||
|
||
Based on the definition of the optimization task and the optimization process, the Optimization module iteratively:
|
||
|
||
• prepares the design variables (element densities or surface node positions) and updates the Abaqus finite element model, and
|
||
• executes an Abaqus/Standard analysis.
|
||
|
||
These iterations or design cycles continue until either:
|
||
|
||
• the maximum number of design cycles is reached, or
|
||
• the specified stop conditions are reached.
|
||
|
||
Figure 13.1.1–1 shows the interaction of Abaqus and the optimization process.
|
||
|
||
# Topology optimization
|
||
|
||
Topology optimization starts with an initial design (the original design area), which also contains any prescribed conditions (such as boundary conditions and loads). The optimization process determines a new material distribution by changing the density and the stiffness of the elements in the initial design while continuing to satisfy the optimization constraints, such as the minimum volume or the maximum displacement of a region. In addition, you can apply a number of manufacturing constraints that ensure
|
||
|
||
<!-- source-page: 1210 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>flowchart</summary>
|
||
|
||
```mermaid
|
||
graph TD
|
||
A["Create model"] --> B["Create optimization task"]
|
||
B --> C["Create design responses"]
|
||
C --> D["Create objective functions"]
|
||
D --> E["Create constraints"]
|
||
E --> F["Create optimization process"]
|
||
F --> G["Submit optimization process"]
|
||
G --> H["Prepare design variables and update finite element model"]
|
||
H --> I["Abaqus analysis"]
|
||
I --> J{Optimization complete?}
|
||
J -->|No| I
|
||
J -->|Yes| K["Optimization process is finished"]
|
||
K --> L["Review results"]
|
||
M["User actions"] --> A
|
||
N["Automated optimization actions"] --> A
|
||
O["Perform optimization"] --> I
|
||
P["Design cycle iteration"] --> I
|
||
Q["Monitor optimization progress"] --> I
|
||
R["Monitor job progress"] --> I
|
||
```
|
||
</details>
|
||
|
||
Figure 13.1.1–1 User actions and automated Abaqus/CAE actions in the optimization process.
|
||
|
||
the proposed design can be created using standard production processes, such as casting and stamping. You can also freeze selected regions and apply member size, symmetry, and coupling constraints.
|