The option of the Optimization Type property enables shape optimization using mesh node relocations. As with the other optimization methods, this is a physics driven optimization based on a set of loads and boundary conditions provided by either a single preceding analysis or multiple preceding analyses.
Compared to Shape Optimization, Topography Optimization is used for shell-based models only.
Using this method, the application computes an optimal shape in the design domain that you can apply to a selected region of your model and that also includes specific design Objectives and Constraints.
Upstream System Recommendations
Review the following to properly prepare your upstream systems. Topography Optimization has the same capability as the Shape Optimization method. Any differences are mentioned when necessary.
- Geometric Analysis
Review the Geometric Analysis topic in the Prerequisites and Requirements content in the Topology Optimization - Level-Set Based section for the supported Response Type and Response properties when performing a geometric analysis.
Only Mass and Volume are available.
- Static Structural Analysis
Review the Configuring Static Structural Analysis topic in the Prerequisites and Requirements content in the Topology Optimization - Level-Set Based section for the supported Response Type/Response for the Objective Worksheet or a Response Constraint object.
In addition, when specifying your upstream Static Structural analysis, note that any surface of the optimizable body that is scoped to boundary conditions (fixed displacements, loads, bonded contacts, etc.) must be defined in the Exclusion Region.
- Modal Analysis
This method only supports User Defined Criterion that you define in the upstream Modal analysis. This result data can then be used in the Structural Optimization analysis by the Objective object or as a Response Constraint .
In addition, when specifying your upstream Modal analysis, note that you can control an eigenmode whose frequency always has the same ranking during the optimization process. If its ranking changes, the algorithm will face some difficulty.
- Manufacturing Constraint
For this analysis method, no manufacturing constraint are yet available
Application Differences
Note the following when using the Topography Optimization method.
- Specifying the Mesh
This analysis method supports triangle and quadrangles.
Important: When specifying the mesh on your model, it is strongly recommended that you:
Always use a uniform mesh (homogeneous element size). This enables you to capture the design with the same precision everywhere on the model.
Make sure that you have a sufficiently fine mesh.
- Specifying Optimization Type
You use the Optimization Region object to select a region of your geometry on which to perform optimization as well as the optimization method to be used.
In order to scope the optimization regions using the Topography Optimization method, you need to first generate the mesh.
Specify the Design Region. The properties of the Design Region category enable you to define the geometry as a Geometry Selection or a Named Selection. This is the region that you wish to optimize.
Specify the Exclusion Region. The properties of the Exclusion Region category enable you to specify a region (geometric entities or elements) to be excluded from optimization. You specify excluded regions using defined Boundary Conditions, Geometry Selection, or a Named Selection.
The surfaces scoped to boundary conditions (such as Fixed Support, Force, Bonded Contact, etc.) must be included in the scoping of the Exclusion Region.
Set the Optimization Type property to . Specify the following additional properties as needed:
Move Limit Per Iteration: This property enables you to define how far each node can move at each iteration. It must be defined in length units, such as one element size. By default, this property is set to . Select the option to change the value.
Total Move Limit: This property enables you to define how far each node can move in total. It must be defined in length units, such as three element sizes. By default, this property is set to (equal to the size of one element or slightly larger depending the fineness of the mesh). Select the option to change the value.
Mesh Deformation Control: This property enables you to define how much the mesh can be stretched. It is an additional control to avoid element distortion. This unit-less value is a sort of penalty factor that ranges from 0 (no control) to 1.0. By default, this property is set to . Select the option to change the value.
- Specifying Results
This method supports Topology Density results. The Topology Density object is added automatically to the analysis system. You can add additional objects by selecting Topology Density from the Results group on the Solution Context tab or by right-clicking the Solution folder (or in the Geometry window) and selecting > .