Topology optimization can be applied to conceptual and lightweight design of structures, providing designers with more design possibilities. In this example, a bracket model, as shown in Figure 1, is subjected to structural topology optimization.
The analysis process is as follows:
(1) Launch ANSYS Workbench and load the Static Structural module for structural mechanics.
(2) Right-click on cell A3 and select Import Geometry → Browse… from the pop-up menu. In the file selection dialog box, choose the geometry model file ex5-1\ex5-1.scdoc.
(3) Double-click on cell A4 to enter the structural mechanics module, using the default material.
(4) Click on the Mesh in the model tree and set the overall element length of the model to 4mm in the Details of Mesh.
(5) Right-click on the Mesh in the model tree, select Insert → Method, and add a mesh control method. Select all parts of the model and set the meshing method to MultiZone.
(6) Right-click on the Mesh in the model tree and click Generate Mesh to generate the model mesh, as shown below.
(7) Right-click on the Static Structural in the model tree and select Insert → Fixed Support to insert a fixed constraint. Select the circular face of the bracket hole, as shown below.
(8) Right-click on the Static Structuralin the model tree and select Insert → Force to insert a distributed load. Load a vertical downward force of 2000N on the support plane, as shown.
(9) Right-click on the Solutionin the model tree and select Solve to perform the calculation.
(10) After the calculation is completed, use Solution → Insert → Equivalent Stress to insert an equivalent stress result and use Solution → Insert → Total Deformation to insert a model displacement result. Obtain the equivalent stress and displacement cloud maps as shown.
(11) After the calculation is completed, exit the structural analysis module. In the Workbench platform, load a topology optimization module, drag it into cell A6, and right-click on cells A5, A6, and A7 to update them. The results are shown below after completion.
(12) Double-click on cell B5 to enter the topology optimization module. Here, default optimization region, objective, and response constraint settings can be used.
(13) Right-click on the Solution in the model tree and perform the calculation. After the calculation is completed, obtain the topology optimization result as shown below, which shows the preserved region of the model.
(14) After the calculation is completed, exit the topology optimization module. In the Workbench platform, right-click on cell B7 and select Transfer to Design Validation System (Geometry). Then, update the topology optimization result by right-clicking on cell B7, followed by updating the geometry model in cell C2, as shown below.
(15) Right-click on cell C2 and select Edit Geometry in SpaceClaim to enter SpaceClaim. After entering, the original bracket model and the topology-optimized model can be seen.
(16) Suppress the original model in the model tree, and only display the optimized model.
(17) In the model tree, it can be seen that the current model is not yet a solid model, but is composed of multiple Facets faces. Select all Facets and use the Convert to solid → Merge faces function to convert the surface model to a solid model.
(18)As a model comes to life, it may show some minor imperfections on its surface. To fix these issues, you can use tools like “Merge Faces” in the Repair feature of SpaceClaim. Once you’ve completed the necessary modifications, exit SpaceClaim.
(19)Within the Workbench platform, double-click on the C4 cell to enter the structural mechanics module, where you can perform validation calculations on the optimized model. The resulting equivalent stress cloud map and overall deformation cloud map are shown below.