Chapter 5 Tetrahedral Mesh with Inflation

1. Chapter 5Tetrahedral Meshwith Inflation ANSYS MeshingApplication Introduction

2. Overview • Tetrahedral Meshing Algorithms • Inflation Options for Patch Conforming • Algorithms • Pre and Post • Advanced Options • Collision Avoidance • Patch Independent Meshing • Defeaturing • Proximity refinement • Curvature refinement • Workshop 5.1 Tetrahedral Mesh with Inflation for a Tee Mixer (Patch Conforming) • Workshop 5.2 Fluid and Structural Meshes for an Auto Manifold (Patch Independent)

3. Tetrahedral Meshing Algorithms • Patch Conforming • All faces and edges are respected by default (although this can be changed with pinch controls and virtual topology and there is default defeaturing based on the minimum size limit) • For moderately clean CAD (i.e. native CAD, Parasolid, ACIS, Etc.) • Possible to combine with sweeps in a multibody-part to generate conformalhybrid tet/prism and hex meshes • Works with advanced size functions • Surface mesh Volume mesh • Patch Independent • Useful for CAD with sliver faces, many surface patches, short edges, etc. • Built in defeaturing/simplification based on meshing technology • Based on ICEM CFD Tetra/Prism Octree method • Volume mesh Surface mesh

4. Inflation for Patch Conforming Tetrahedrons • Basic settings include Inflation Option as well as Pre and Post Inflation Algorithms

5. Inlation Option – Smooth Transition • Smooth Transition (Default) • Uses the local tetrahedral element size to compute each local initial height and total height so that the rate of volume change is smooth. Each triangle that is being inflated will have an initial height that is computed with respect to its area, averaged at the nodes. This means that for a uniform mesh, the initial heights will be roughly the same, while for a varying mesh, the initial heights will vary. • Transition Ratio • Volume-based size change between the last layer of elements in the inflation layer and the first elements in the tetrahedron region. • When the Solver is set to CFX, the default for Transition Ratio is 0.77. For all other physics preferences, including CFD when Solver Preference is set to Fluent, the default is 0.272. • The difference in treatment arises because the Fluent solver is cell-centered so that the mesh element is equal to the solver element, while the CFX solver is vertex-centered with the solver element constructed from the mesh duals about a node.

6. Inflation Option – Thickness Options • Total Thickness • Creates constant inflation layers using the values of the Number of Layers and Growth Rate controls to obtain a total thickness as defined by the value of the Maximum Thickness control. Unlike inflation with the Smooth Transition option, with the Total Thickness option the thickness of the first inflation layer and each following layer is constant • First Layer Thickness • creates constant inflation layers using the values of the First Layer Height, Maximum Layers, and Growth Rate controls to generate the inflation mesh. Unlike inflation with the Smooth Transition option, with the First Layer Thickness option the thickness of the first inflation layer and each following layer is constant.

7. Inflation Algorithms • Pre • TGrid algorithm • Default setting for all physics type. The surface mesh will be inflated first, and then the rest of the volume mesh will be generated. • Does not support different number of layers on adjacent faces. • Also applicable to Sweep and 2D meshing. • Post • ICEM CFD algorithm • A post processing technique that works after the tetrahedral mesh is generated is used. Valid only for patching conforming and patch independent tetrahedrons.

8. Advanced Inflation Options • Visible if View Advanced Options under the Global Inflation Options under Mesh is set to Yes • Collison Avoidance • Layer Compression (Default for Fluent) • Stair Stepping (Default for CFX) • Growth Rate Type • Maximum Angle • Fillet Ratio • Use Post Smoothing • Smoothing Iterations

9. Collision Avoidance • Layer Compression • If advancing inflated fronts from differentfaces are about to collide, the inflation layers are compressed in order to leave enough room for a layer of tets • If layer compression cannot resolve collision, layers may be removed as in stair stepping described below. A warning message may be generated and the quality of the mesh may be impacted,which is of special concern for FLUENTusers • Stair Stepping • Inflation layers are “peeled off” toprevent collision of advancing fronts in order to leave enough room for a layerof tets

10. Inflation: Compression vs. Stair-stepping Layer Compression: Stair-stepping:

11. Patch Independent Tetrahedrons • The Patch Independent Tetrahedral methods has controls similar to the Advanced Size Function for Curvature and Proximity as well as an explicit tolerance for defeaturing geometry. • Remember that the volume mesh is created first and then projected to vertices, edges, and faces to create the surface mesh. You can alwaysforce faces, edges, or points to be respected by creating named selections or by setting Define Defeaturing Tolerance to No

12. “Filters” in/out edges based on size and angle. If set to Yes, a Define Defeaturing Tolerance field appears where you enter a numerical value. There are several basic cases, including the following: Two approximately parallel spaced edges (fillet or chamfer) closer than the tolerance, as shown in Fig. 1 If the face (fillet or chamfer) between spans by more than 15 degrees, one edge is kept and the other is dropped. Nodes will only line up along one edge. If the face between spans by less than 15 degrees, both edges may be dropped and patch independent mesh will walk over this feature without capturing it explicitly. If the tolerance is less than the fillet/chamfer size, and the deflection is greater than 15 degrees, both edges are kept. A small hole with a diameter smaller than the tolerance as shown in Fig. 2. No edges are dropped. You should defeature manually in this case. Defeaturing Tolerance Fig. 1 Fig. 2

13. Examples of Defeaturing Geometry No Defeaturing Defeaturing Tolerance of 1

14. Proximity Refinement – Cells in Gap • Num Cells Across Gap • (displayed only when Curvature and Proximity Refinement is set to Yes). This is the number of cells desired in narrow gaps. This sets the goal for the proximity based refinement. The mesh will subdivide in tight regions toward this goal, but the refinement is limited by the Min Size Limit is reached. It will not override this limit. The default is 1.

15. Curvature Refinement – Span Angle • Span Angle • (displayed only when Curvature and Proximity Refinement is set to Yes). Sets the goal for the curvature based refinement. Similar to setting for the Advanced Size Function This refinement is also limited by the Min Size Limit. The following choices are available: • Coarse – 91 degrees to 60 degrees • Medium – 75 degrees to 24 degrees • Fine – 36 degrees to 18 degrees

16. Inflation for Patch Independent Tetrahedrons • Settings similar to those for Patch Conforming, but only Post algorithm since the surface mesh does not exist before the volume mesh is created.

17. Workshop 5.1 Tetrahedral Mesh with Inflationfor a Tee Mixer

18. Goals This workshop demonstrates the creation of a mesh for the fluid portion ofa mixing tee using the patch conforming tetrahedral mesher with an inflation layer to resolve the wall boundary layer. This mesh will be used later in the course to set up a CFD simulation so the workshop also demonstrateshow to export a mesh database for future analysis.

19. Importing Geometry Start Workbench and select the Import option in the menu bar and change the filter to Geometry File. Specify the mixer-tee.agdb file from the Tutorials folder and note that an entry appears in the Project Schematic with a green check mark. Expand the Component Systems entry at the left and drag Meshing onto the DM instance in the project schematic. Note the linkage that appears.

20. Supressing Solid Parts and Setting the Method • Double click the Mesh entry in System B on the Project Schematic to open up ANSYS Meshing. • Note that there are 5 parts and 5 solid bodies. The four Solid entries comprise the solid portion of the mixing tee while the body named Fluid is the fluid region • Since we will focus first on the fluid region, right-click and suppress the four solid bodies under geometry in the Outline • Right-click on Mesh and select Insert Method. Select the fluid body and set the Method to Tetrahedrons and the Algorithm to Patch Conforming

21. Physics Preference • Set the Physics Preference to CFD and the Solver Preference to Fluent • Expand the Sizing entry and set the Max Face Size to 0.015 [m] and the Max Tet Size to 0.03 [m]. • Expand the Inflation entry and set Use Automatic Tet Inflation to None. This means that you will need to define inflation layers manually

22. Previewing the Surface Mesh • Right click on Mesh and select Preview Surface Mesh. The mesh resolution of the surfaces appears to be reasonable

23. Inflating the Method • Right click on the Patch Conforming Method and choose Inflate this Method • Pick the five side surfaces of the modelas shown below and set the Inflation Option to First Layer Thickness and enter a value of 0.001 m. Set the Maximum Layers to 5.

24. Generating the Inflated Mesh • Right click on the mesh and chooseGenerate Mesh to create the inflated volume mesh.

25. Skewness Mesh Metric • Expand the Statistics Entry and set the Mesh Metrics Option to Skewness. The maximum value of 0.742 is suitable for the Fluent Solver

26. Unsuppressing the Solids • Select the four solid parts under geometry in the project outline and right-click to unsuppress them. You might want to mesh the solids for a conjugate heat transfer calculation in either CFX or FLUENT or perhaps for a one-wayFSI calculation.

27. Mesh Method for the Solid Parts • Insert a Patch Conforming Tetrahedral Method and assign it to the four solid parts

28. Body Sizing for the Solid Parts • Right-click on Mesh in the Outline and insert a Sizing. Select the 4 solid bodies in the Model View (set the selection filter to bodies if needed) and apply the selection to the geometry. Enter a sizing of 0.04 [m].

29. Combined Mesh for Fluid and Solid Parts • Regenerate the mesh. Note the new mesh count and quality metric

30. Named Selections for CFD • You will use the fluid portion of the mesh to set up a CFD tutorial later. Since the solid bodies are not needed for this, suppress the four solid bodies again. • To help prepare the mesh for CFD, you will create named selections for the 3 end faces. To create a named selection, set the selection filter to Faces, pick a face in the Model View, right-click and choose Create Named Selection. Do this for the low-y face in the model using inlet-y as the Name for the Selection.

31. Preparing the Mesh for CFD • Repeat this for the high-Z face (inlet-z) and the high-Y face (outlet)

32. Exporting the Mesh File • While still in ANSYS Meshing, click on File/Export and save the file as a meshdatfile. Note the location as you will import this file later in the course when setting up a fluid flow simulation using the fluid mesh. • Save the Project and exit Workbench.

33. Workshop 5.2 Fluid and Structural Meshes for an Auto Manifold

34. Goals This workshop demonstrates the creation of a mesh suitable for a conjugate heat transfer (CHT) flow simulation, or a fluid-structure interaction (FSI) simulation. However, the geometry presents potential difficulties. • The geometry contains two bodies. One represents a solid manifold and the other the fluid region. • The mesh in the fluid body will be of CFD quality, with inflation, whilst the solid mesh will be of structural quality. • The Patch Independent mesh method is used to avoid problems arising from the nature of the CAD (see later). • This same geometry will later be meshed using with the Patch Conforming Method with Virtual Topology in Workshop A.1.

35. Open Workbench Launch ANSYS 12.0 Workbench (WB) from the START menu Click on Component Systems in the Toolbox on the LHS of the WB main panel Double click the Mesh option

36. Geometry Import Right click on the Geometry button in the RHS of the WB panel and select Import geometry. Import the Auto-manifold.agdb file Double click on the Mesh button (in cell A3) to launch the Meshing Application

37. Geometry Review • The geometry was created by importing an IGES file for the manifold into DesignModeler and extracting the fluid region. • On the right-hand-side of the screen, Select ‘Mechanical’ for the Physics • Select ‘Automatic’ for the Meshing Method, then ‘OK’ that window. • The units of the geometry should be set to mm. • Named Selections were created in DesignModeler. Expand the Named Selections object and click on each to see where they have been applied. • If you cannot see the Named Selections in the Meshing Application, see next slide.

38. Named Selections If the Named Selections don’t appear in the Meshing Application, it is probably because the option to bring them in is switched off. Activate the option by right clicking on the Geometry button on the Project Page, and then select Properties. Ensure Named Selections is checked, and the Selection Key is blank. Right-Click on Geometry and select “Update” Right-Click on Mesh and select “Refresh”

39. Problem Geometry • The geometry includes many faces of various sizes and shapes and this would lead to problems for Patch Conforming methods. Virtual Topology could be an option to address this, but instead a Patch Independent approach will be used. Short edge Narrow sliver faces cusps

40. Surface Meshes • Patch Conforming Method • Short edges – unwanted refinement and too many elements. • Cusps and narrow faces – poor quality elements with small angles. refinement small angles • Patch Independent Method • Mesh not constrained by geometry. • Coarser mesh possible. • Elements are more regular in size and shape.

41. Inserting the Mesh Method Left click on Mesh in the tree and check its details Make sure the Physics preference is set to Mechanical This ensures that the solid body will have a mesh suitable for structural mechanics Assign the Meshing method: Set the Cursor Mode to Body RMB (Window) select Select All RMB select Insert -> Method Depending on your Workbench settings, sometimes a default Mesh Method is already created for you. You can either delete it and create the new one, or modify its details as follows. Set Details of Method Set the Method to Tetrahedrons Set Algorithm to Patch Independent Set Max Element Size to 6 mm Set Min Size Limit to 2 mm Cursor Modes

42. Setting Element Size for Fluid Region Body Sizing Maintain the Cursor Mode of Body Selection Select the Fluid body RMB (Window) select Insert -> Sizing Set Details of Body Sizing Set Element Size to 5 mm

43. Adding a Boundary Layer Mesh to the Fluid Insert Inflation Maintain the Cursor Mode of Body Selection Select the Solid Body RMB (Window) select Suppress Body RMB (Window) select Select All RMB (Window) select Insert Inflation Set Details of Inflation Set the Cursor Mode to Face selection To select Inflation on all wall surfaces: Pick one face Drop down the Extendmenu and Extend to Limits Apply selection 126 Faces Change Inflation Option Total Thickness Set Maximum Thickness to 5 mm

44. Volume Mesh Generation Mesh the Bodies Set the Cursor Mode to Body selection RMB (in Window) select Unsuppress all Bodies RMB (in Tree) select Generate Mesh In Statistics set Mesh Metrics to Skewness Around 150 000 elements were created with a worstskewness of about 0.9

45. Review Volume Mesh Review the Mesh Examine the surface mesh of the fluid region to see that it does not conform to the underlying surface topology You can Hide the solid mesh region to make this easier by right clicking on it in the geometry part of the Tree Try using a Section Plane ( ) to look at the interior of the mesh

46. Conclusion The mesh is now complete RMB (Tree) select Update This ensures everything in the project so far is up to date Select File > Close Mesh to close the Mesh application In the WB panel select File > Save Project As… and give the project a name Exit from ANSYS Workbench by selecting File > Exit Note: Because the Mechanical mesh preference was used, the mesh elements will contain midside nodes. This is a benefit for mechanical analysiswhich can use higher order tetrahedral elements. If the mesh is then used for CFD, these midside nodes will be automatically ignored.