1. Chapter 2 Introduction to the ANSYS Meshing Application
ANSYS Meshing Application Introduction

2. Introduction to the ANSYS Meshing Application
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 5

6. Pyramids (where tet. and hex. cells meet)
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:
Tetrahedrons
(unstructured)
Pyramids (where tet. and hex. cells meet)
Prisms (formed when a tet mesh is extruded)
Hexahedrons
(usually structured)
Manifold Example: Outer casting and internal flow region are meshed for coupled thermal/stress gas flow simulation 6

7. Mesh Specification Considerations Detail: Refinement
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 7

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

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).
Excellent very good good acceptable bad Unacceptable
*Further information on mesh metrics is available in the documentation and training lecture appendices 9

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 10

11. FEA Meshing Issues Structural FEA
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)
Meshing issues are very different for CFD and structural FEA cases.
For both cases you want to refine the mesh to capture gradients of concern
However for FEA cases, one is often concerned with strain energy, stress energy, displacement, and so forth. Also, 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)
For CFD cases, one is often concerned with velocity, total pressure, turbulence, and so forth. Because CFD involves the fluid domain, mesh sizes tend to be larger often millions of elements.
Most CFD solvers use mix of tet/hex/prism and pyramid elements
In the next few slides we will look at the advantages of different mesh types.

13. Tet Mesh and Tet/Prism hybrid
Mesh Types
Tet Mesh and Tet/Prism hybrid
The other common meshing type is tet or tet/prism hybrids.
In these figures, you can see that tet elements fill the body of the domain while prism elements are placed along the walls.

14. Mesh Types
Hex Mesh
Hexahedral Meshes…..

15. Mesh Types Tet Mesh Mesh can be generated in 2 steps:
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)
One region where we definitely do not want isotropic refinement is near the wall. For this reason tet meshes are almost always combined with a prism layer at the wall. Let’s take a look at how this prism layer is formed using the Advancing Front Method.
CLICK we start with a surface
CLICK which is then turned into a surface mesh. What you should note is that refinement of the surface mesh is still isotropic.
CLICK Prisms are then created
CLICK by inflating the surface
CLICK mesh
CLICK the prism layer then transitions to tetrahedral elements
CLICK this transition sometimes including pyramidal elements
CLICK

18. Mesh Types Hex Mesh TET HEX
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)
The two most common meshes involve tetrahedral and hexahedral elements. The most significant advantage of hexahedral elements is that fewer elements are 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.
MJC: note correction
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)
The reason why hexahedral elements allow for this is that anisotropic elements can be aligned with anisotropic physics. For example,
CLICK
There is not much variation along the wall so elements can be long without degrading the solution.
However, there IS significant variation in velocity away from the wall so the element height must be small to capture the gradients.
Essentially, hexahedral elements can more efficiently account for such anisotropic physics.

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 simpler way to generate hex meshes
Sweep
MultiZone
The downside of hexahedral meshes is the labor required to generate them. As shown here, one way of generating a hex mesh is the ‘blocking technique’. Here we start off with an encompassing block and remove portions until it is representative of the geometry. The block edges are projected onto the geometry edges and then meshing parameters are set. For complex geometries, this task can be time consuming and challenging.

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 and 2D geometry 21

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 22

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
Element Shapes
Prism
Pyramid
Tetrahedral Mesh
Tet
Swept Mesh 24

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
Coarse mesh ‘walks over’ detail in surface model
Element Shapes
Prism
Pyramid
Tet
Inflation layer
applied for CFD 25

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

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. Programmed Controlled Inflation
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)
No inflation
Programmed Controlled Inflation 28

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 except for 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. Hex-dominant mesh shown above:
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
Prism
Hex
Tet
Pyramid
Element Shapes
Hex-dominant mesh shown above:
19,615 Hex (60%)
5,108 Tet (16%)
211 Prisms (1%)
7,671 pyramids (24%)

32. CFX-Mesh Method Generate Volume Mesh
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 32

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 to FLUENT and CFX is also demonstrated 34

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 35

36. Initial Mesh
Double-click the Mesh entry in the schematic 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-2
velocity-inlet-1
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