Chapter 2 Introduction to the ANSYS Meshing Application

1. Chapter 2Introduction to theANSYS Meshing Application ANSYS MeshingApplication Introduction

2. Overview • Introduction to the ANSYS Meshing Application • Meshing Requirements for Different Physics • ANSYS Meshing Workflow • Meshing Methods for 3D and 2D geometries • Workshop 2.1 • Automatic Meshing for a Multibody Part • Program Controlled Inflation • Transferring Mesh to CFX or FLUENT

3. Workbench Guiding Principles • Parametric: Parameters drive system • Persistent: Model updates passed through system • Highly-automated: Baseline simulation w/limited input • Flexible: Able to add controls to influence resulting mesh (complete control over model/simulation) • Physics aware: Key off physics to automate modeling and simulation throughout system • Adaptive architecture: Open system that can be adapted to a customer’s process • CAD neutral, meshing neutral, solver neutral, etc.

4. What is the “ANSYS Meshing Application”? • ANSYS has been working to integrate “best in class” technologies from several sources: • ICEM CFD • TGrid • GAMBIT • CFX • ANSYS Prep/Post • Etc.

5. ANSYS Meshing Application Overview The objective of the ANSYS Meshing Application in Workbench is to provide access to common ANSYS Inc. meshing tools in a single location, for use by any analysis type: FEA Simulations Mechanical Dynamics Simulation Explicit Dynamics Simulation AUTODYN ANSYS LS DYNA Electromagnetic Simulation CFD Simulation ANSYS CFX ANSYS FLUENT

6. Mesh Specification Purpose For both CFD (fluid) and FEA (solid) modelling, the software performs the computations at a range of discrete locations within the domain. The purpose of meshing is to decompose the solution domain into an appropriate number of locations for an accurate result. The basic building-blocks for a 3D mesh are: Hexahedrons (usually structured) Tetrahedrons (unstructured) Prisms (formed when a tet mesh is extruded) Pyramids (where tet. and hex. cells meet) Manifold Example: Outer casting and internal flow region are meshed for coupled thermal/stress gas flow simulation

7. Mesh Specification Considerations • Detail: • How much geometric detail is relevant to the simulation physics. • Including unnecessary detail can greatly increase the effort required for the simulation. • Refinement • Where in the domain are the most complex stress/flow gradients? These areas will require higher densities of mesh elements. Is it necessary to resolve this recess? Refined mesh around bolt-hole Extra mesh applied across fluid boundary layer

8. Mesh Specification • Efficiency • Greater numbers of elements require more compute resource (memory / processing time). Balance the fidelity of the simulation with available resources.

9. Mesh Specification • Quality • In areas of high geometric complexity mesh elements can become distorted. Poor quality elements can lead to poor quality results or, in some cases, no results at all! • There are a number of methods for measuring mesh element quality (mesh metrics*). For example, one important metric is the element ‘Skewness’. Skewness is a measure of the relative distortion of an element compared to its ideal shape and is scaled from • 0 (Excellent) to 1 (Unacceptable). *Further information on mesh metrics is available in the documentation and training lecture appendices

10. Mesh Specification Example showing difference between good and poor meshes: This example illustrates an unconverged thermal field in a manifold solid casting. On closer inspection it is clear that the simulation is unable to resolve a sensible data field in the region of poor quality elements. The example with good quality elements demonstrates no problems in the solution field. The ANSYS Meshing Application provides many tools to help maximise mesh quality

11. FEA Meshing Issues • StructuralFEA • Refine mesh to capture gradients of concern • E.g. temperature, strain energy, stress energy, displacement, etc. • tet mesh dominated, but hex elements still preferred • some explicit FEA solvers require a hex mesh • tet meshes for FEA are usually second order (include mid-side nodes on element edges)

12. CFD Meshing Issues • CFD • Refine mesh to capture gradients of concern • E.g. Velocity, pressure, temperature, etc. • Mesh quality and smoothness critical for accurate results • This leads to larger mesh sizes, often millions of elements • tet mesh dominated, but hex elements still preferred • tet meshes for CFD are usually first order (no mid-side nodes on element edges)

13. Mesh Types • Tet Mesh and Tet/Prism hybrid

14. Mesh Types • Hex Mesh

15. Mesh Types • Tet Mesh 1) Can be generated quickly, automatically, and for complicated geometry Mesh can be generated in 2 steps: Step 1: Define element sizing Step 2: Generate Mesh

16. Mesh Types • Tet Mesh 2) Isotropic refinement – in order to capture gradients in one direction, mesh is refined in all three directions – cell counts rise rapidly Perforated plate resulting in pressure drop in x direction x

17. Mesh Types • Tet Mesh 3) Inflation layer helps with refinement normal to the wall, but still isotropic in 2-D (surface mesh)

18. Mesh Types • Hex Mesh • Fewer elements required to resolve physics for most CFD applications • This hexahedral mesh, which provides the same resolution of flow physics, has LESS than half the amount of nodes as the tet-mesh) TET HEX

19. Mesh Types • Hex Mesh • Fewer elements required to resolve physics for most CFD applications. • Anisotropic elements can be aligned with anisotropic physics (boundary layers, areas of tight curvature like wing leading and trailing edges)

20. Mesh Types • Hex Mesh • For arbitrary geometries, hex meshing may require a multi-step process which can yield a high quality/high efficiency mesh • For many simpler geometries, sweep techniques can be a simplerway to generate hex meshes • Sweep • MultiZone

21. ANSYS Meshing Application Workflow The ANSYS Meshing Application uses a ‘divide & conquer’ approach A different ‘Meshing Method’ can be applied to each part in the geometry Meshes between bodies in different parts will be non-matching or non-conformal Matched or conformal meshes will be generated for bodies in a single part All meshes are written back to a common central database A number of different methods are available for 3D and2D geometry

22. Meshing Methods for 3D Geometry There are six different meshing methods in the ANSYS Meshing Application for 3D Geometry: Automatic Tetrahedrons Patch Conforming Patch Independent (ICEM CFD Tetra algorithm) Swept Meshing MultiZone Hex Dominant CFX-Mesh

23. Meshing Methods for 2D Geometry • There are four different meshing methods in the ANSYS Meshing Platform for 2D Geometry which can be applied to Surface Bodies or Shells: • Automatic Method (Quadrilateral Dominant) • All Triangles • Uniform Quad/Tri • Uniform Quad

24. Patch Conforming Tetrahedrons Tetrahedrons Method with Patch Conforming Algorithm Faces and their boundaries (edges and vertices) are respected Includes the Expansion Factor setting, which controls the internal growth rate of tetrahedrons with respect to boundary size Includes inflation or boundary layer resolution for CFD Can be mixed with Sweep methods for bodies in a single part – conformal meshes will be generated Pyramid Prism Tet Element Shapes Tetrahedral Mesh Swept Mesh

25. Patch Independent Tetrahedrons Tetrahedrons Method with Patch Independent (ICEM CFD Tetra) Algorithm Faces and their boundaries (edges and vertices) are not necessarily respected unless there is a load, boundary condition, or other object scoped to them Useful for gross defeaturing or to produce a more uniformly sized mesh Simplified version of Tetra tightly integrated into the ANSYS Meshing Application Honors standard ANSYS Meshing Application mesh sizing controls Tetra parts can also have inflation applied Pyramid Prism Tet Coarse mesh ‘walks over’ detail in surface model Element Shapes Inflation layer applied for CFD

26. Sweep Method Produces Hexes and/or Prisms Body must be Sweepable Single Source, Single Target Inflation can yield pure hex or prisms Prism Hex Body split into 2 parts to allow for swept meshing Extrusion removed to allow for swept meshing Element Shapes Allows for inflation layer (boundary layer resolution) for CFD

27. Thin Solid Sweep Meshing • Multiple source/target faces • Works at body level with other methods • Multiple elements through thickness possible for single body parts

28. Automatic Method The Automatic setting toggles between Tetrahedral (Patch Conforming) and Swept Meshing, depending upon whether the body is sweepable. Bodies in the same part will have a conformal mesh. Tetrahedron (Patch Conforming) Swept Tetrahedron (Patch Conforming) Programmed Controlled Inflation No inflation

29. Inflation • Inflation is accomplished by extruding faces normal to a boundary to increase the boundary mesh resolution, typically for CFD • Smooth Transition from inflated layer to interior mesh • Collision avoidance: • Stair-stepping • Layer compression • Preview Inflation • Pre vs. Post inflation • All methods can be inflated exceptfor Hex-Dominant and Thin Sweep • Sweeping: • Pure hex or wedge

30. MultiZone Sweep Meshing • New feature for 12.0 • Automatic geometry decomposition • With the swept method, this part would have to be sliced into 3 bodies to get a pure hex mesh With MultiZone, it can be meshed directly!

31. Element Shapes Pyramid Prism Hex Tet Hex-Dominant Method • The hex-dominant meshing algorithm creates a quad-dominant surface mesh first, then hexahedral, pyramid and tetrahedral elements are filled in as needed. • Recommended when a hex mesh is desired for a body that cannot be swept • Useful for bodies with large amounts of interior volume • Not useful for thin complicated bodies where the ratio of volume to surface area is low • No boundary layer resolution for CFD • Mainly used for FEA analysis • Hex-dominant mesh shown above: • 19,615 Hex (60%) • 5,108 Tet (16%) • 211 Prisms (1%) • 7,671 pyramids (24%)

32. CFX-Mesh Method CFX-Mesh uses a ‘loose’ integration. No Meshing Application sizings are respected or transferred to CFX-Mesh Selecting Right Mouse ‘Edit…’ on the Method launches the CFX-Mesh GUI. Define mesh settings/controls/inflation Preview & generate volume mesh Commit the current mesh model Return to ANSYS Meshing Possible to ‘Generate Mesh’ on a CFX-Mesh method without opening the application Uses current or default settings Generate Volume Mesh Inflation layer

33. Workshop 2.1 Pipe Tee Mesh

34. Goals This workshop will illustrate the use of the Automatic Meshing Method for a single body part The transfer of the mesh toFLUENT and CFX is also demonstrated

35. Specifying Geometry Copy the pt.agdb file from the tutorial files folder to your working directory Start Workbench and double-click the Mesh entry in the Component Systems panel in the Toolbox Right-click on Geometry in the Mesh entry in the Project Schematic and select Import Geometry/Browse Browse to the pt.agdb file you copied and click Open Note that the Geometry entry in the Project Schematic now has a green check mark indicating that geometry has been specified

36. Initial Mesh • Double-click the Mesh entry in theschematic or right-click and select Edit. This will open the Meshing Application • In the Meshing Options panel set the Physics Preference to CFD, the Mesh Method to Automatic and press OK • Right click on Mesh and select Generate Mesh • Use the view manipulation tools and the axis triad to inspect the mesh Based upon choice of physics (CFD), the Meshing Application has produced a mesh accommodating curvature, a reasonable sizing strategy and automatic selection of optimal mesh methods with minimal user input. There are many ways in which the Meshing Application can control and improve the mesh. Some further mesh controls will now be demonstrated.

37. Named Selections velocity-inlet-1 velocity-inlet-2 • Set the Selection Filter to Faces and select one of the pipe end faces as shown. Right-click in the Model View and choose Create Named Selection. Enter velocity-inlet-1 for the Selection Name • Repeat for the other two pipe end faces using the naming as shown • The Named Selections just created are listed in the Outline by expanding Named Selections. The names assigned here will be transferred to the CFD solver so the appropriate flow conditions can be applied on these surfaces. pressure-outlet

38. Inflation • Select Mesh in the Outline and expand Inflation in Details • Set Use Automatic Tet Inflation to Program Controlled, leave other settings • Right click on Mesh and select Generate Mesh. Note the inflation layers are grown from all boundaries not assigned a Named Selection. The thickness of the inflation layers is calculated as a function of the surface mesh and applied fully automatically.

39. Section Planes • Orient the model by clicking on the axis triad (+X Direction) • Click on the New Section Plane icon in the menu bar. Left click, hold and drag the cursor in the direction of the arrow as illustrated to create the Section Plane • Created Section Planes are listed (bottom left). Planes can be individually activated using the checkbox, deleted and toggled between 3D element view and 2D slice view. Try this now (you will need to rotate the model to see the cross-section) After the Section Plane has been created the Section Plane cursor tool will still be active. Left clicking in the viewport and dragging will slide the Section Plane along its axis. Clicking on either side of the Plane tool will cut the mesh on each side respectively. Clicking twice on one side will change the view to a planar slice. When the position is finalized, select a view manipulation tool

40. Mesh Statistics • If you expand the Statistics entry under Mesh, it will summarize the number of nodes and elements in the mesh • Under Mesh Metric select Skewness. Note the reported mesh quality

41. Transferring Mesh to CFD • After the mesh has been generated, you can transfer it to a new CFD simulation • In the main Workbench Window, right click on the Mesh entry in the Meshing instance you created on the Project Schematic and observe that you can transfer the mesh to a new FLUENT or CFX simulation (Transfer Data To New >). Select either FLUENT or CFX • Note that the Mesh entry now has an Update symbol, right click the Mesh entry and select Update. This will pass data to the new FLUENT/CFX instance.

42. Fluent with Workbench Mesh If FLUENT was selected - Double click the Setup entry and accept the default options in the FLUENT Launcher FLUENT will start with the mesh loaded Save the project from the Workbench File Menu

43. CFX with Workbench Mesh If CFX was selected - Double click the Setup entry, CFX Pre will launch with the mesh loaded Save the project from the Workbench File Menu