Extracting a smoothed mesh

When the optimization process has completed, you can choose to extract a smooth isosurface meshed representation of the optimized model surface in the form of a file that can be transferred to a CAD system or back into Abaqus/CAE.

You can extract a smoothed surface mesh from either a topology, shape, or bead optimization. You can extract a single file from the entire assembly, or you can extract individual files from selected part instances.

See Also
Understanding optimization processes
Creating, editing, and manipulating optimization processes

Context:

The optimized model is usually a combination of tetrahedral and hexahedral elements and can include a significant number of interior elements that are not included in the isosurface representation that will be generated. In addition, the surface of the model might be rough and irregular, depending on the element density. The smoothing operation is an iterative process that displaces the nodes at the surface and generates a smooth triangular mesh on the surface of the model.

The smoothing operation can be followed by a data reduction operation that combines adjacent triangles with nearly coincident planes and reduces the number of surface triangles. Data reduction continues iteratively until the decrease in the number of triangles reaches a specified percentage of the original number of triangles. You can specify the angle that determines if adjacent planes are coincident.

Finally, you can choose to apply an optional filtering operation to remove local irregularities. The filtering is applied before the smoothing operation.

  1. From the main menu bar, select OptimizationExtractoptimization process name. You can also smooth the results by selecting the optimization process name in the Optimization Process Manager and clicking Extract.

    The Extract Surface Mesh dialog box appears.

  2. Enter the name of the output file that will be extracted.
  3. Select the content of the output files that will be extracted. You can choose either of the following:

    • Create a single file from the entire assembly.

    • Create individual files from selected part instances. Abaqus/CAE names the files by appending the name of the part instance to the name of the output file.

  4. Select the format of the file that will be generated. You can choose from the following:

    • Abaqus input file (.inp): file that can be imported into Abaqus/CAE.

    • STL (.stl): file that can be read by 3D CAD systems, such as CATIA V5 and SOLIDWORKS.

    • IGES1 (.igs): IGES file using block 114.

    • IGES2 (*_2.igs): IGES file with explicit point information.

    • IGES3 (*_3.igs): IGES file using block 128.

  5. In the Design Cycle field, enter the design cycle from which the isosurface should be extracted. By default, the Extract Surface Mesh dialog box displays the last design cycle. The default value will not be displayed for sensitivity-based topology optimization since the solver is called once at the beginning of the optimization procedure.
  6. Enter a value between zero and one specifying the Iso value.

    The smoothing process determines which elements are on the surface of the model and uses the isovalue to calculate where on the interior edges of the elements new nodes are created. Increasing the isovalue leads to shifting the isosurface toward the inside of the model, which results in a decrease in the model volume. For structures with thin components, you should not enter an isovalue greater than 0.7 to prevent the structure from becoming disconnected.

  7. Enter the Reduction percentage, which defines the percent of faces that should be removed during the data reduction operation. A value of 0 indicates that no faces should be removed. A value of 100 indicates the data reduction stops when no more faces can be removed, given the value of the reduction angle.
  8. Enter a value between 0 and 90 specifying the Reduction angle. The reduction angle defines the maximum angle between adjacent faces at a node such that the node might be removed during the data reduction.
  9. Select the number of iterative smoothing cycles. Larger values lead to smoother models but can result in an increase of the computation time. In practice, 5 to 10 smoothing cycles are usually sufficient. Further smoothing can result in the narrowing or contracting of thin components. You can turn off smoothing by selecting a value of 0.
  10. Enter a value between zero and one specifying the Target volume.

    The target, or relative, volume of a solid model is the ratio of the volume defined by the isosurface and the original volume (calculated from the volume of the solid elements generated by the optimization). Likewise, the target area of a shell model is the ratio of the volume defined by the isosurface and the original area (calculated from the area of the shell elements generated by the optimization). If the model contains both solid and shell elements, only the solid elements are considered. The calculated volume does not account for voids inside a solid model.

    If you specify the target volume, the data reduction process calculates the isovalue that will result in the specified volume (the value of the isovalue that you enter is ignored). The data reduction process generates an error if you enter an excessively large value for the target volume that is larger than the volume calculated with an isovalue of zero or if you enter an excessively small value for the target volume that is smaller than the volume calculated with an isovalue of one. The data reduction process also generates an error if it fails to converge before 20 iterations.

  11. In some cases, the optimized model will contain small irregularities that you can choose to remove with an optional filtering operation. Filtering is applied before the smoothing operation and results in a more homogeneous material distribution. Select Moderate to apply a single filtering cycle, select Full to apply five filtering cycles.
  12. Click OK to extract the smoothed mesh.

    The specified output file is created in the TOSCA_POST directory. For subsequent runs, a unique number is appended to the file name; for example, name_002.inp.

    Note:

    If you extracted the smoothed mesh in the form of an Abaqus input file, you can select FileImportModel from the main menu bar to import the mesh into Abaqus/CAE. For more information, see Importing a model.