1. Mesh Control Winter Semester 2009-2010

2. 2 PART 1 Meshing

3. 3 Goals  Use the various mesh controls to enhance the mesh for the crankshaft model.  Problem statement: The model consists of a parasolid file representing a crankshaft for a small engine shown below. Our goal is to mesh the model using all defaults meshing tools and inspect the result. Next we will add mesh controls to modify the mesh in various regions of the model.

4. 4 Assumptions  Since this is a meshing exercise we will not be applying loads or solving the model.  Instead, we will assume that a linear static structural analysis is to follow the meshing operation (in order for the static structural analysis to be accurate, the model shall be well meshed).

5. 5 Start Page  From the launcher start Simulation.  Choose “Geometry” > “From File “ and browse to the file “Crankshaft.x_t”.

6. 6 1. Basic Meshing Highlight the mesh branch to view the mesh and access the meshing controls.

7. 7 1. Basic Meshing Inspect the mesh detail window. Notice the default parameters are: 1.Physics preference: mechanical 2.Relevance: 0 RMB on the mesh branch and choose to “Generate Mesh”.

8. 8 1. Basic Meshing  The completed mesh (shown here) is made up of a relatively coarse tetrahedral mesh. Expand the “Statistics” section of the details window to check the number of nodes and elements. Note: The number of nodes and elements will vary slightly across different machines and platforms.

9. 9 2. Mesh Relevance In the detail window for the mesh change the “Relevance” to 50 (note: relevance may be set by dragging the slider bar or typing the desired value into the field).  Again RMB the mesh branch and choose the “Generate Mesh” to preview the new mesh.  A visual inspection of the mesh along with the statistics section in the detail window can be used to compare the effects of the meshing changes.  Please note the difference in the number of elements.

10. 10 3. Sizing Control  We will assume the pin section (shown boxed at right) is an area of interest for us. We will apply a local mesh control in this region.  We’ll take advantage of several shortcuts in order to help us evaluate the appropriate size for the control.

11. 11 3. Sizing Control  First orient the model so we are viewing down the X axis as shown here.  A handy shortcut to do this is to use the triad to re- orient the model. Clicking on any of the axes (or the “iso” ball) the triad will rotate the model accordingly.

12. 12 3. Sizing Control  Zoom into the area of interest. Notice the region is made up of 3 surfaces. To gauge the size of the region we can use the ruler tool (If the ruler is not displayed, use the ruler toggle under “view” menu)  Inspection of the model shows the pin section is roughly 10 mm across.

13. 13 3. Sizing Control Select the 3 surfaces in the pin region.  Note: by holding the CTRL key we can select each of the desired surfaces individually using left mouse clicks.  An alternative shortcut called “paint selecting”, is to hold the left mouse button while dragging the cursor over the desired areas (no CTRL key necessary). 3 surfaces

14. 14 With the 3 surfaces selected choose “Sizing” from of the following options: 1. The mesh control menu. 2.RMB on the “Mesh” branch: ”Insert”  “Sizing”. 3. Sizing Control In the detail for the size control change “Type” to “Element size”. Change the element size to be 1mm

15. 15 4. Mesh Refinement  Again “Generate Mesh” and inspect the new mesh as before.  We will also assume the chamfer section on the side of the flywheel is also an area of interest.

16. 16 4. Mesh Refinement To apply the refinement control first select the chamfer surface. Highlight the mesh branch and RMB. Choose “Insert > Refinement”.

17. 17 4. Mesh Refinement  Mesh refinement is an iterative meshing tool that can be set to integer values from 1 to 3. A value of 1 provides the least refinement (coarsest mesh) while a value of 3 provides the most refinement (finest mesh). Leave the refinement level set to 1 and again “Generate Mesh”.

18. 18 5. Mapped Faces  Apply a “Mapped Face Meshing” control to a surface in the model. Mapped face meshing is typically used in contact analyses to insure a “regular” mesh on the contact surface. High quality elements are often required when detailed contact results are desired. Select the cylindrical surface shown here (either side of the part is OK). 11

19. 19 5. Mapped Faces Highlight the mesh branch and RMB. Choose “Insert > Mapped Face Meshing”.  Again “Generate Mesh”. Mapped Face MeshDefault Mesh

20. 20 6. Changing element type  The element type can also be selected.  The available element types are: Tetrahedron Hex dominant Sweep CFX Mesh (Using in flow analysis) Switch to body selection by clicking on “Body” and select the crankshaft. Highlight the mesh branch and RMB. Choose “Insert > Method”.

21. 21 6. Changing element type  Change the element type and note the difference in the element’s shape.  Choose the method in the “Details” window to be “Tetrahedron”  RMB on the Mesh  “Generate”  Repeat and notice the differences between the Hex dominate and sweep.

22. 22 Static structural & Meshing PART 2

23. 23 Goals  To examine the influence of the different meshing upon the results.  In this section you will be required to: Create a simple geometry, using the design modeler tool. Solve static structural analysis several times, each time with a different meshing.

24. 24 Creating rectangular beam, using ANSYS Design Modeler  Open ANSYS and choose “Geometry”  Select the length unit to be mm

25. 25 Creating the geometry  Under “Create” menu choose “Primitive”  “Box”

26. 26 Creating the geometry  In the details window, create the geometry using the following parameters:

27. 27 Creating the geometry  The box now is shaded, highlight the “Box” in the tree outline, RMB on the ‘Box’ and choose “Generate”.

28. 28 Stating simulation  Switch to “Project” tab and choose “New simulation”

29. 29 Static structural  Solve the problem under these initial conditions: - Fixed support (A) - Vertical force of 300N along the free edge (B) - Solve for equivalent stress

30. 30 Meshing – part 1  Solve the problem with no mesh control (i.e. with the default meshing).  Document the results for a specific point, write down the stress value.  Solve the analysis again with the following mesh control (Document the results after each run at the same point): ‘Hex dominant’ element with element midside node ‘kept’ ‘Sweep’ with element midside node with ‘Use global setting’ Relevance of -50 Relevance of 50 Refinement of 1 Element size of 1 mm Element size of 2 mm

31. 31  Solve the analysis with different element sizes (for example – 5mm 2mm 1.5mm 1mm etc).  Plot the stress results for specific point versus the element size.  At which point does the element size cease to influence the results?  What are your conclusions? Meshing – part 2

32. 32 Part 3 Virtual topology

33. 33 Goal  Exploring the virtual topology tool in order to group faces together and simplify the meshing.  The virtual topology tool is been used to:  Reduce the number of elements in the model,  Simplify small features out of the model,  Simplify load abstraction.

34. 34 Load model  Load the “Cap Fillets.x_t” file (last week’s file)

35. 35 Virtual topology  Highlight the model in the tree outline  Select the virtual topology tool from the menu above the tree

36. 36 Selecting surfaces  In the model, select the three connected surfaces as shown in the following figure:

37. 37 Virtual cell  Highlight the “virtual topology” in the tree outline, RMB  “insert”  virtual cell  Highlight the “Mesh” in the tree, RMB  “Generate Mesh”

38. 38  Note that: The mesh was changed, The elements in the horizontal plane and the vertical one are now continues