Introduction to ANSYS Mechanical

Transcription

1 Workshop 4.2 Meshing Control 15.0 Release Introduction to ANSYS Mechanical ANSYS, Inc. February 12, 2014

2 Goals Use the various ANSYS Mechanical mesh controls to enhance the mesh for the model below. Problem statement: The model consists of a CAD file representing a solenoid. Our goal is to mesh the model using all defaults and inspect the result. Next we will add mesh controls to modify the mesh in various regions of the model ANSYS, Inc. February 12, 2014

3 Assumptions Since this is a meshing exercise we will not be applying loads or solving the model. Instead we will assume a linear static structural analysis is to follow the meshing operation. Note, due to a certain randomness in the nature of meshing, the actual number of elements generated during the workshop may vary from machine to machine. This is normal ANSYS, Inc. February 12, 2014

4 Project Schematic 1. In the Toolbox, double click Static Structural to create a new analysis system RMB on the Geometry cell and Import Geometry. Browse to Solenoid_Body.stp. 3. Double click the Model cell to start the Mechanical application ANSYS, Inc. February 12, 2014

5 Basic Meshing In Mechanical, specify US customary (in, lbm, lbf, F, s, A, V) Start by meshing the model using all defaults. This will establish a base line from which we can compare changes. 4. Highlight the mesh branch, RMB > Generate Mesh. 4. When mesh generation completes we can view the mesh and inspect the statistics in the details for the mesh branch. Note: node/element count may vary slightly across machines/platforms ANSYS, Inc. February 12, 2014

6 Basic Meshing 5. View the mesh metrics: a. Highlight the mesh branch. b. In the details under Statistics > Mesh Metric specify Element Quality. 5a. 5b ANSYS, Inc. February 12, 2014

7 Mesh Size Control Based on our inspection we may decide a more refined mesh is necessary for our analysis. 6. In the mesh branch details expand the sizing section and set the Relevance Center to Medium. 7. RMB the mesh branch and Generate Mesh. 6. The finer mesh is visually obvious. The details show an increase in the number of elements as expected ANSYS, Inc. February 12, 2014

8 Mesh Shape Control A closer look at the mesh shows some anomalies where certain faces meet. By zooming to the area in question we can see several small sliver surfaces are forcing a fine mesh locally. We ll attempt to clean this up using virtual topology ANSYS, Inc. February 12, 2014

9 Virtual Topology 8. Highlight the Model branch > RMB > Insert > Virtual Topology. Since it appears that the sliver area is closer to being tangent to the sides, we will combine these into virtual cells. 8. Sliver Side In order to preserve the basic topology we will join pairs of surfaces into virtual cells rather than trying to combine all surfaces together. The result will be 3 cells per side, 6 in total ANSYS, Inc. February 12, 2014

10 ... Virtual Topology 9. Create Virtual Cells: a. Select one of the sliver surfaces. b. Hold the CTRL key and select the adjacent surface (as shown at right). c. RMB > Insert > Virtual Cell. 9b. 9a. 9c. The resulting virtual cell is displayed in red. Although underlying surfaces still exist, this is the surface the mesher will use ANSYS, Inc. February 12, 2014

11 ... Virtual Topology Continue by creating the remaining 5 virtual cells (select in pairs as before). When complete you will have a total of 6 virtual faces and 4 virtual edges. Remesh the model: 10.Highlight the Mesh branch, RMB > Generate Mesh. 10. The resulting mesh shows a much more uniform mesh with a significant reduction in element count ANSYS, Inc. February 12, 2014

12 Mapped Face Meshing 11. Map mesh several faces (highlight Mesh branch): a. Select the 3 planar faces shown here. b. RMB > Insert > Mapped Face Meshing. c. RMB > Generate Mesh. 11a. As shown map meshing results is elements on the selected faces which share very regular shapes. 11b. 11c ANSYS, Inc. February 12, 2014

13 Face Size Control 12. Specify face sizing on selected face: a. Select the face of the gusset section shown here. b. RMB > Insert > Sizing. c. Set Element Size = d. Set Behavior = Hard. 13. Remesh the model (highlight the mesh branch): RMB > Generate Mesh. 12a. 12b c. 12d ANSYS, Inc. February 12, 2014

14 Edge Size Control 14. Specify edge sizing on selected edges: a. Select the 4 edges of the gusset shown here. b. RMB > Insert > Sizing. c. Change Type to Number of Divisions. d. Set Number of Divisions = 25. e. Set Behavior = Hard. 15. Remesh the model (highlight the mesh branch): RMB > Generate Mesh. 14a. 14b c. 14d. 14e ANSYS, Inc. February 12, 2014

15 Edge Size Control Review the mesh metric as compared to the original mesh. With just a few refinements overall mesh quality has improved. Original Mesh Metric Final Mesh Metric ANSYS, Inc. February 12, 2014

16 To go further To go further, suppress previous meshing options and define : a) an inflation on the center hole b) a sphere of influence on the 4 faces shown on the picture c) a pinch to repare CAD default on the edges shown below a) c) b) ANSYS, Inc. February 12, 2014

17 Appendix After creating mesh, in case of mesh setting changes, a color code is applied on the existing mesh in order to know the meshing state. As shown in this WorkShop, orange color indicates an obsolete mesh. It is necessary to re-run mesh ANSYS, Inc. February 12, 2014