Geometric variations can be created using a free-form variation model. In contrast to a synthetic random field model, the variation patterns are tent-like shapes with a single maximum (> 0) going asymptotically to zero with growing distance to its support point. Creating the option for generating geometric free-from variations creates two nodes:
Free-form variation (oSP3D)
- Boundary to be parameterized
The part of the boundary for which to find a random field parametrization. It can be a named selection of type face, element face, or node.
- Fixed boundary
The part of the boundary that is not to be modified (fixed). It can be a named selection of type face, element face, or node. All boundary parts that are not fixed or parametrized are "free" in the sense that oSP3D can modify them to interpolate between directly changed boundaries and fixed boundaries. It is recommended that the fixed boundary does not touch the directly parametrized boundary.
- Mesh part to be exported to oSP3D
The substructure that is to be exported to oSP3D. The boundary to be parametrized or fixed should belong to this substructure. The smaller the exported substructure, the smaller are the computational resources required by oSP3D. The scoping can be a named selection of type body or element.
- Definition
Support points
The mode for choosing the support points for each shape.
When set to Auto, the support node identifiers are automatically generated. Each shape is associated with a single FEM node. The location of the nodes are chosen to distribute them homogeneously on the boundary with respect to the distance between the individual supports.
When set to Manual + Auto, manually defined support points can be added to the automatically generated support points.
Scoping
This option is visible only when Support points is set to Manual + Auto. It defines the (named) selection of the manual supports. FEM nodes, vertices, and edges are allowed. Neighbouring FEM nodes are collected into a single support region, which allows you to influence the shape of the associated variation pattern.
Number of auto-parameters
The number of automatically generated support points.
Magnitude of free variation
The number for the index of the shape.
- Visualization
Enable visualization
After creating the model, you can visualize the individual scatter shapes associated with the random field parameters as a colored contour plot. Use this parameter to turn visualization off (default) or on. For a larger model, you should turn visualization off because visualizing a large model can be slow.
Visible variation shape index
The number for the index of the shape.
- Advanced options
Constant variation
The default setting is Do not use. If you set this to Use extra parameter, an additional parameter is created that is associated with a constant variation for all FEM nodes.
Magnitude of constant variation
This option is visible only when Constant variation is set to Use extra parameter. It defines the magnitude of variation being associated with a parameter of
1.Use mesh stabilization
When set to False, the computed geometric deviation is applied directly to the nodes. However, there is no check if the result is feasible. Thus, the result is fast, but it is very likely not solvable by Ansys Mechanical.
When set to True, an iterative algorithm tries to relax element distortions that are too strong. This avoids situations with negative volumes or negative Jacobians. The larger the applied deformations and the greater the number of nodes or elements, the more computation time that is needed.
Linearize Morphing for quadratic elements
This option affects only quadratic elements.
When set to True, for quadratic elements, oSP3D places the mid-edge nodes using a linear interpolation of the finite element geometry between the corner vertices. During morphing, some elements can be greatly distorted, leading to negative volumes or negative Jacobians. This option can help to avoid these problems and tends to produce more stable results.
When set to False, quadratic elements are morphed with quadratic curvature.
Erase degenerated shapes
When set to True, shapes with short wavelengths or short correlation lengths (that is with a very localized effect) are deleted. Wehn set to False, all shapes are retained.
Test on mesh distortion
When set to True, oSP3D throws an error before the mesh is transferred to the Ansys Mechanical kernel. Because oSP3D uses a different FEM formulation, however, the test in oSP3D may be stricter than in Mechanical. You should use this option if the preparation in the Mechanical kernel takes a lot of time and if you do not want to start it when creating non-meaningful geometric variations.
Move nodes along
When set to Boundary normal, the variations are applied along the direction of the normal vector assigned with each FEM node on the boundary.
When set to Three coordinate axis, each variation pattern can be applied along the x,y, and z axis. This results in three times as many parameters, one parameter for each direction.
The variation along the normal direction is the default. The other option is more stable in the context of complex geometries.
- Solver options
Number of CPUs used by oSP3D
The number of CPU cores that oSP3D can use during the creation of the random field model. The default of
0means that oSP3D is to use all cores.Internal directory
This path is a local directory in the SYS/MECH path of the Workbench project directory. It contains all data that oSP3D requires to generate the random field model. You may also find the log files in there (in the sos_log subdirectory), which is a good starting point in case of errors. Also, you can open the sos_data.sdb file in that directory in the standalone oSP3D GUI for detailed analysis of the random field model.
Generate variations (oSP3D)
You must update the Synthetic random field model node before options are visible for defining or changing the second node.
See the previous option descriptions for Generate variations (oSP3D).
Caution: Never clear or reset the mesh. You may clear the generated data of the Generate variations node, but a reset of the Synthetic random field node also clears the random field model. Further, Ansys Mechanical cannot proceed with the Generate variations node automatically if the Synthetic random field mode is updated.