ANSYS Meshing Application Introduction

ANSYS Meshing Application Introduction
Appendix B CFX-Mesh ANSYS Meshing Application Introduction

Introduction CFX-Mesh provides automated mesh generation
Unstructured triangular surface mesh generation Volume mesh is created from the surface mesh Tetrahedral/prismatic/pyramidal volume mesh generation Extruded meshes can also be created If quad faces exist on the extruded face due to inflation, hex elements will be created for those quad elements Advancing Front and Inflation (AFI)

Element Types Valid element types for the CFX-Solver include tetrahedra, prisms (wedges), pyramids, and hexes

Accessing CFX Mesh Launch ANSYS Workbench
Double click on Mesh under component systems. This will create a ‘Mesh component’ in the Project Schematic area. Right click on select “Import Geometry” and click on “Browse…” to load a previously created geometry or click “New Geometry” to open DesignModeler and create a new geometry. Once the geometry is loaded double click on to open the meshing application.

Accessing CFX Mesh In the Project environment go to Tools > Options… Select “Geometry Import” Select Analysis Type as “3D” Ensure “Solid Bodies” is chosen Only solid bodies are relevant to CFX Mesh Check the “Named Selection” box to get Design Modeler defined named selections Set the filtering prefix (keep the “Filtering Prefixes” box blank to import all named selections regardless of prefix)

Accessing CFX Mesh Right-click on Mesh and Insert Method
Select the Body of interest Now edit the method and choose CFX Mesh Then right Click on resulting CFX-Mesh Method and Choose Edit in CFX-Mesh

Accessing CFX Mesh Note that the meshing environment is now modified

Geometry Requirements
Geometry used for meshing in CFX-Mesh must consist of one or more Solid Bodies In CFX-Mesh, the body will have the units specified in DM Surface Bodies and Line Bodies are not supported in CFX-Mesh On import of certain file formats, Workbench will convert sets of surfaces which fully enclose to a volume into Solid Bodies (see DM documentation for details) Solid Bodies must not overlap each other Where Solid Bodies in a multi-body part touch, they must have common faces Bodies which are Frozen in DM will appear in CFX-Mesh and can be meshed To exclude a Solid Body from meshing, you can either suppress/delete it in DM, or suppress it in CFX-Mesh

Example 1: When Solid Bodies in a multi-body part touch, they must have common faces If two bodies contact as shown, the face at the end of pipe is not one of the faces of the cylinder, CFX-Mesh will fail in generating mesh if the two bodies are in a single part How to meet CFX-Mesh topology requirements? wrong

To make a common face between pipe and cylinder, the cylinder needs to have the cylinder face that touches the pipe split into two: one face is the circular face which matches the end of the pipe, the other face is the remaining annular ring. This can be done with an Imprint Face body operation in DM. right

Example 2: When part of pipe intrudes into the cylinder, part of the side surface is external to the cylinder, while the other part is internal to it. What should the two bodies look like if they are in a single part?

Again, the rule to remember is that adjacent solid bodies in a multi-body part must meet at shared faces If two bodies contact as shown, where the side surface of the pipe is a single face, it does not match up with cylindrical cut-out in the bottom cylinder and CFX-Mesh will fail in generating mesh. Single Side Surface Cylindrical Cut-Out wrong

To make sure the pipe and cylinder meet at a shared face, the pipe needs to have its side face segmented into the part that’s external to the bottom cylinder and the part that’s internal to it (via an Imprint Face body operation in DM). External Side Surface Cylindrical Cut-Out Internal Side Surface right

Other Geometry Requirements
The CFX-Mesh Help provides many useful examples of what can and cannot be handled in CFX-Mesh, and some ways around difficult geometries, including: Bodies Joined by a Common Face Bodies Touching at a Face Body with a Hole Body with an Enclosed Body Bodies with an Enclosed Body and a Hole Body with an Enclosed Body Touching the Face Non-Manifold Geometry Closed Faces (ie. Cylinders) Thin Surface Topology Poorly Parameterized Surfaces Degenerate Geometry

Right-click on Geometry in Tree View
Geometry Update Geometry Update allows for quick modification of geometry and mesh regeneration. Updates geometry while retaining most or all CFX-Mesh settings. Updates from CAD systems in plug-in mode is faster and cleaner. If importing in reader mode, then you must save the new geometry into the appropriate file before updating. Most geometry updates work with the minimum required modification to your mesh settings Depends on the complexity of the changes made to the geometry, the CAD format and the method of import Look at status symbols on each entity at the end of the update. If there are problems, you should correct them before regenerating the mesh. or Right-click on Geometry in Tree View Status Symbols Error OK

Geometry Checking Geometry Checking checks for the presence of certain undesirable features in faces and edges which can cause poor mesh quality or failure of the mesher. Can be accessed from the Go menu, by right-clicking on Geometry in Tree View, or in the top right toolbar. Note: the “lock” symbol means the item must remain. Results of check can be viewed under Errors in Tree View If a Warning or Error refers to a specific curve or face, it will be highlighted when selected Last warning gives a summary of the checks

Geometry Checking Failed check does not necessarily result in poor mesh Worth checking the mesh on any faces which failed the checks Doesn’t check for ALL problems which can be present, just a few specific problems: Sliver Edge Checking Sliver Face Checking Parameterization Face Checking Verify Options determine values which generate errors

Sliver Edge Checking Looks for short edges in the geometry
Short edges can produce a mesh which is over-refined in regions near the short edges To remove short edges, change the default from NO to YES for Remove Short Edges in Fix Options You can change the tolerance used for the check by using Verify Options

Sliver Face Checking Computes a ratio of perimeter length to area for each face Faces with a high sliver factor can result in a poor quality surface mesh You can change the limit used for the check by using Verify Options Default of 25 is usually sensible Each face identified will be highlighted when the individual warning message is selected

Parameterization Face Checking
Provides guidance on the parameterization of the surfaces Each potentially poorly parameterized surface will be highlighted when the individual warning message is selected

78 Surfaces represent car body
Virtual Topology By Default CFX-Mesh resolves every edge using a minimum of 3 vertices and meshes every face Results is large mesh when there are many short edges and narrow faces in the CAD data May not require a fine mesh in these areas for CFD If proper mesh controls are not used in these areas, the resulting mesh may be of poor quality or the mesher might fail Virtual Topology allows users to combine faces and edges into Virtual Faces and Virtual Edges. Can be added in CFX-Mesh or the Meshing Application. 78 Surfaces represent car body

A single virtual surface
Virtual Topology CFX-Mesh only sees the combined Virtual Face or Virtual Edge Mesher does not resolve the constituent faces or edges, giving higher quality mesh with the required refinement Does NOT modify the underlying CAD Virtual topology will be discussed in more detail later A single virtual surface

Geometry Display To change the appearance of your geometry, left-click on Geometry in the Tree View Transparency (%) 100% means completely transparent 0% means completely opaque Shine (%) Controls how much light is reflected by the faces of the mesh 0% gives lowest reflection and looks matt 100% gives highest reflection and looks very bright Transparency can be very useful for selecting hidden surfaces since there isn’t a wireframe view

Composite 2D Regions You can use 2D Regions to give meaningful names to parts of the geometry which may comprise many faces Composite Regions can be used for: Specifying Locations in CFX-Mesh Defining Boundary Conditions in CFX-Pre Default and additional Regions available To create a new Region, right-click on Regions and choose Insert>Composite 2D Region No primitive 2D Region can be assigned to more than one Composite 2D Region

Composite 2D Regions Named Selections are imported from DM as Composite Regions Select Named Selection under Default Geometry Options on the Project tab before proceeding to CFX-Mesh. Can be set as default option in the Geometry Import options panel Composite 2D Regions can be hidden!! Removes the constituent faces from the viewer Hidden faces cannot be selected

2D Regions and Faces Where two Solid Bodies meet at a common face:
There is just one face present in the geometry There are two 2D Regions Each meshing feature that requires you to specify a location has its own rules about 2D Regions on the same face Ex. Face Spacing: Do not try to apply different Face Spacings to 2D Regions which are the two sides of a common face (surface mesh is generated on the common face, not 2D Regions) Ex. Inflated Boundary: You can have different settings for the two different 2D Regions which make up a common face

2D Regions and Faces Use attached Selection Rectangles to select individual 2D Regions easily and accurately CFX-Mesh will not allow you to select locations for meshing features which break the rules given for each feature

Saving the Volume Mesh Two formats Access Options from the Tools Menu
.CMDB file Contains mesh and mesh settings Larger file which takes longer to generate for large meshes .GTM file Suitable for import directly into CFX-PRE Access Options from the Tools Menu The right panel will show various CFX options.

Saving the Volume Mesh You may choose to write .cmdb or .gtm or both
User Defined location for .gtm will produce a dialog box to save choose a location when you Generate the Volume Mesh

Length Scales The process of setting an element length scale for CFX-Mesh can be viewed as a 3 step process Default Body Spacing Face Spacing Other Mesh Controls (Point Spacing, Periodicity, Inflation, etc) Smallest effecting length scale is chosen

Body Spacing Body Spacing specifies the background mesh length scale
Currently all that can be set is the Default Body Spacing which applies to the overall geometry Should be set to the coarsest length scale required anywhere since no elements can be created that are larger than this spacing Maximum Spacing: the maximum element size to be used when creating triangles on the faces of the body and tets in the volume of the body

Face Spacing Face Spacing specifies the mesh length scale on a face (or faces) and in the volume adjacent to the selected faces Default and additional faces available To create a new Face Spacing, right-click on Spacing and choose Insert>Face Spacing

Face Spacing Face Spacing can be set to one of 4 types:
Angular resolution - curvature sensitive, discussed next Relative error - curvature sensitive, discussed next Constant - constant length scale, overriding the Body Spacing (must be less than Default Body Spacing) Volume Spacing - uses the same spacing on the face as the Body Maximum Spacing

Face Spacing Face spacings have a volumetric effect. The region over which they act are determined by the following settings: Radius of Influence: extent of the Face Spacing influence, after which it will expand according to the Expansion Factor Expansion Factor: rate of expansion of mesh scale from surface to interior Location: Faces where the Face Spacing values will be applied Can be selected from the Model View or Tree View Regions Unnecessary for Default Face Spacing

Curvature Sensitive Mesh
Angular Resolution [Degrees] CFX-Mesh chooses edge length such that the set angle is subtended at the center of circle with radius equal to smallest radius of curvature Default is 30 degrees (recommended 5 to 60 degrees) Relative Error [Δr/r] Deviation of mesh from surface as a fraction of local radius of curvature Minimum edge length - lower bound on length scale Maximum edge length - upper bound on length scale (default same as volume background scale)

Curvature Sensitive Mesh
With surface curvature sensitive meshing Without surface curvature sensitive meshing

Edge Spacing Edge Spacing specifies the mesh length scale on an edge (or edges) and in the volume adjacent to the selected edges To create a new Edge Spacing, right-click on Spacing and choose Insert>Edge Spacing Parameters and effect on mesh are the same as with Face Spacing

Edge Spacing

Mesh Controls Mesh Controls are used to refine the surface and volume mesh in specific regions of your model Location can be defined using any point on the model or by specifying coordinates Can be located anywhere in the 3D space of model (inside, outside or on the edge) 3 types of volumetric Controls are available: Point Line Triangle Remember: Face Spacing also available for volumetric control

Point Spacing Each of the 3 volumetric Controls requires you to specify a Point Spacing for the control at appropriate points. Any number of mesh controls can reference the same point Spacing Length Scale For the mesh size where the Point Spacing is applied Must be less than Body Spacing Max Radius of Influence Radial extent of the fixed local length scale influence Expansion Factor Geometric rate of increase of local element length scale beyond radius

Point Control Point Control controls the mesh spacing in a spherical region Point Select either a vertex from the model or coordinates Spacing Select a Point Spacing which defines the attributes for the Point Control (Length Scale, Radius of Influence and Expansion Factor) Figure to right shows a Point Control on a 1m cube with: Length Scale=0.05m Radius of Influence=0.2m Expansion Factor=1.2

Line Control Line Control controls the mesh spacing in a region defined by a cylindrical volume between 2 spheres Point Select either a vertex from the model or coordinates for both Points Spacing Definitions Uniform requires only one Spacing Non Uniform requires a Spacing for each end Spacing Select a Point Spacing which defines the attributes for the Line Control (Length Scale, Radius of Influence and Expansion Factor) Figure to right shows a Line Control on a 1m cube with: Length Scale=0.05m Radius of Influence=0.2m Expansion Factor=1.2

Triangle Control Triangle Control controls the mesh spacing in a region defined by a prismatic volume between 3 spheres Point Select either a vertex from the model or coordinates for all 3 Points Spacing Definitions Uniform requires only one Spacing Non Uniform requires a Spacing for each corner of the triangle Spacing Select a Point Spacing which defines the attributes for the Triangle Control (Length Scale, Radius of Influence and Expansion Factor) Figure to right shows a Triangle Control on a 1m cube with: Length Scale=0.05m Radius of Influence=0.2m Expansion Factor=1.2

Periodicity Using Periodicity allows you to generate identical meshes for faces that will be specified as part of a periodic boundary condition in ANSYS CFX The CFX Solver makes more accurate calculations when meshes on periodic pairs are identical (one-to-one) Periodicity can be either Translation by a fixed vector or Rotation Rules/Limitations: Each face in the Location 1 face list must map to an equivalent face in the Location 2 face list Multiple faces can be selected for each of Location 1 and Location 2, provided each face in the Location 1 face list maps onto a face in the Location 2 face list using the specified transformation Inflation cannot be applied to a face which is part of a Periodic Pair See the documentation for further details on Periodicity

Periodic Pairs Periodic Pairs create identical meshes on the 2 locations selected Location Select face(s) either directly from the Model View or select a Composite 2D Region from the Tree View All faces selected must be on the external boundary of the model and must not be included in an Inflated Boundary Periodic Type Rotational requires 2 points to define an axis, and possibly an Angle of Rotation Points can be either a vertex from the model or coordinates Translational requires no further input

Inflation Inflation is the generation of prismatic element layers by “inflating” triangular surface elements Purpose: Prism elements more effectively and efficiently captures boundary layer effects Node density near the wall is increased Velocity profile is captured by the prism layer Tetrahedral elements efficiently fill the volume region

Inflation You can control the number, thickness and expansion rate of inflation layers You can inflate from any surface or boundary condition, except those included in a Periodic Pair Inflation layers can be viewed within CFX-Mesh

Inflation Number of Inflated Layers Expansion Factor
If First Layer Thickness Option is used, this is a maximum number of layers If Total Thickness Option is used, this is the actual number of layers (unless layers are removed to improve mesh quality) Expansion Factor Each layer, moving away from the face, is one Expansion Factor thicker than the previous. Number of Spreading Iterations Advanced quality control, see documentation for details Minimum Internal Angle Inflation Option Total Thickness First Layer Thickness

Inflation Option - Total Thickness
The total thickness of the inflation is controlled by the: Thickness Multiplier Local element edge length Determined by Face Spacing and Controls Maximum Thickness Set individually for each Inflated Boundary Creates a less smooth transition from the inflated prism mesh elements to the tetrahedral mesh elements The number of inflated layers is more constant, and you have some control over height of layers on face-by face basis

Inflation Option - Total Thickness
Process used for creating the layers of prisms when using the Total Thickness option is given below: CFX-Mesh calculates the total thickness of the inflation layers as follows: Multiply the Thickness Multiplier by the local element edge length Where this is less than the specified Maximum Thickness, then this gives the total thickness of the layers Where this is greater than the specified maximum Thickness, then the Maximum Thickness is taken to be the total thickness of the layers Use the specified Number of Inflated Layers and Expansion Factor to calculate the height of each layer, given the total thickness that has just been calculated Inflation thickness will not be constant over the inflated edge if the element edge length changes in the region of the inflation layer

Inflation Option - First Layer Thickness
Does not control the overall height of the inflation layers Prisms based on First Prism Height or y+, Expansion Factor and Number of Inflated Layers Creates smoother transition from inflated prism mesh elements to the tetrahedral mesh elements First Prism Height must be less than the Max Spacing under Body Spacing You should examine the mesh to visualize the extent of the inflation and the quality of the transition from prisms to tetrahedral elements

Inflation Option - First Layer Thickness
Define First Layer By y+ Computes First Prism Height based on user inputs Desired y+, Flow Reynolds Number and Reference Length Dy = LDy+ 80 Re(-13/14) First Prism Height = Reference Length * (Desired) y+ * 80 * Reynolds Number(-13/14)

Inflation Option – Extended Layer Growth
Process used for creating the layers of prisms when using the First Layer Thickness option is given below Put a single layer of prisms against the faces of the inflated boundary, of a height equal to the First Prism Height Extended Layer Growth = No Check the aspect ratio of the prisms If height < base length, add another layer of prisms of height (Previous Height) X (Expansion Factor) If height ≥ base length, stop adding prisms Repeat until aspect ratio for all the prisms ≈ 1 or until the Number of Inflated Layers is reached Extended Layer Growth = Yes Check the aspect ratio of the prisms If height < base length, add another layer of prisms of height (Previous Height) X (Expansion Factor) If height ≥ base length keep adding layers of unit aspect ratio until the Number of Inflated Layers is reached

Number of Inflated layers = 25
Inflation Option – Extended Layer Growth Number of Inflated layers = 25 Extended Layer Growth = No Extended Layer Growth = Yes

Inflation Option – Layer Smoothing
Available when using First Layer Thickness option Allows prisms to grow out normal to the surface, i.e. orthogonal to the surface Layer normals and heights are then progressively smoothed, during the creation of each layer Maximizes the number of layers obtained Result in longer mesh generation times

Inflation Option – Layer Smoothing
Prism growth is orthogonal Layer by Layer Smoothing = No Layer by Layer Smoothing = Yes

Inflated Boundary Creation of an Inflated Boundary is how you specify which faces you want Inflation to apply to Location Select face(s) either directly from the Model View or select a Composite 2D Region from the Tree View A face cannot be in more than one Inflated Boundary, or in both an Inflated Boundary and a Periodic Pair Maximum Thickness The Maximum Thickness for the whole inflation layer, when Inflation Option is set to Total Thickness Not used if Inflation Option is set to First Layer Thickness

Stretch Stretch can be used to expand or contract the mesh elements in a particular direction The geometry is expanded by the specified factors, meshing takes place, then the geometry is contracted back to its original size The max and min stretches allowed are 0.2 and 5 (factors below 0.6 are not recommended) Before Stretching Stretch in X = 1.0 Stretch in Y = 1.0 Stretch in Z = 2.0 Stretch in X = 0.5 Stretch in Y = 3.0 Stretch in Z = 1.0

Combined Mesh Control and Stretch
The effective influence of a Mesh Control, which is treated as a spherical mesh control while meshing takes place, will NOT be modified to elliptical Therefore, a Point Control will appear to influence an elliptical region when the mesh is examined x y z

Proximity Proximity settings control automatic refinement of the mesh when edges or faces are near to other edges or faces, but not connected Edge proximity ON by default Adjusts mesh based on mesh size on neighboring edges Surface proximity OFF by default Adjusts mesh based on gap between neighboring surfaces

Edge Proximity Edge Proximity is used to automatically modify mesh elements in regions where curves are in close proximity Bounding curves of surface “sense” nearby curves and increase mesh density locally Only available when Delaunay Surface Mesher is used (meshers discussed soon) Edge Proximity OFF Edge Proximity ON Edge Proximity OFF Edge Proximity ON

Surface Proximity Surface Proximity is used to automatically reduce the mesh size in regions where surfaces are in close proximity and the original mesh does not resolve the gap sufficiently Number of Elements Across Gap Recommend at least 4 Generates higher quality prismatic and tetrahedral elements in the gap region Maximum Number of Passes Number of times the surface mesher will run to try to meet the Number of Elements Across Gap Available for both Delaunay and Advancing Front Surface Meshers

Options – Global Mesh Scaling
Allows easy scaling of each length scale for the mesh, except those applied to Face Spacing’s Decreasing this factor decreases mesh length scales and increases number of elements Does not affect anything other than mesh length scales (i.e. Radius of Influence is not affected) Stretch affects all lengths (including Radius of Influence) Global Mesh Scaling factor is only applied during meshing Display of size of Controls will show the size as if the factor is 1

Options – Surface Meshing
Both methods are well recognized and have established track records Both mesh individual surfaces Delaunay (default) works on “closed” surfaces Delaunay mesh quality is not good on poorly parameterized surfaces Advancing Front produces higher quality elements at boundaries traditionally slower than Delaunay cannot mesh “closed” surfaces

Options – Meshing Strategy
Advancing Front and Inflation 3D Includes Inflation Quickly generates a mesh with tetrahedra, prisms and pyramids with low memory usage New elements created from advancing “front” of triangles Creates tetrahedral elements by point (node) placement Identify exposed faces which now form the new “front” Extruded 2D Mesh See next two slides

Extruded Meshes When “Extruded 2D Mesh” is selected, the user is prompted to define the “Extruded Periodic Pair” Pick the two sets of faces from the model view or the object tree You can also select composite 2D regions from the Tree View Select the “Periodic Type” – Translational or Rotational If there are no vertices on the selected faces, you will be asked for a translation distance or a rotation angle Extruded meshes in CFX-Mesh are not as flexible as those that the Swept Mesher can generate The difference in the Periodic Pair must be a simple translation or rotation However, the source and target faces can consist of multiple (matching) faces

Extruded Meshes Extrusion Options 2D Extrusion Option Number of Layers
Full = extrude through the full extent of the geometry Partial = thickness of elements determined automatically such that element quality is high. Will not necessarily fill geometry for a given number of layers Number of Layers Distribution distribution of element heights along the extrusion can be uniform or biased Expansion Factor Set the growth rate for the thickness of elements in non-uniform extrusion

Options – Volume Meshing
This option is only available with the Advancing Front and Inflation 3D meshing strategy Advancing Front options is default Runs as a single process on a single CPU Parallel Advancing Front Multiple processes (multiple CPU’s) on the same or different machines Faster mesh generation for large models Overcomes memory limitations of a single processor / machine, especially on 32 bit system Have at least 500,000 tetrahedral elements per partition. Do not run small models in parallel. Uses the CFX-Parallel (Solver) licenses if available. Else can be separately licensed.

Options – Volume Meshing
Set the Number of Partitions along the X,Y and Z coordinates Divides the geometry based on the number of partitions along each coordinate Each partition is meshed independently and then combined Combined mesh will be same as that generated by a single process Parallel Meshing can be: Local Parallel, on the same machine Distributed Parallel, on different machines Distributed Parallel requires a Hosts List Refer to CFX-Mesh Help for details on setup and limitations of Distributed Parallel Meshing

Mesh Preview Allows you to look at the mesh on a particular face or faces before creating the entire surface or volume mesh Select face(s) for Preview Group either directly from the Model View or select a Composite 2D Region from the Tree View Can choose whether to generate mesh on selected faces or all at once Can view only surface mesh in CFX-Mesh, volume mesh may be viewed in CFX-Post

Mesh Preview Display Mesh Render Mode Display Mesh Shine (%)
Wire on Face Mesh shows the mesh faces and the mesh lines Solid Face shows the mesh faces Wire Mesh shows just the mesh lines Display Mesh Mesh Before Inflation Mesh After Inflation Inflated Front shows triangles across the top of the inflated elements Inflated Mesh shows the inflation layers only Transparency (%) 100% means completely transparent 0% means completely opaque Shine (%) Controls how much light is reflected by the faces of the mesh 0% gives lowest reflection and looks matt 100% gives highest reflection and looks very bright Face Color Mode Body shows mesh the same colour as body Uniform allows you to pick a color Rainbow shows the mesh on each face in a different colour, as different as possible

Mesh Statistics Mesh Statistics Warning Messages or Errors
Shows Number of Quads and Triangles (Surface Elements) in the Preview Group Warning Messages or Errors Non-fatal warning messages or errors will be shown under the Errors item in the Tree View Fatal errors produce a pop-up message and are also shown under Errors Clicking on an Error or Warning highlights the related face or element if appropriate

Volume Mesh Generate Volume Mesh
Once mesh is set up, you can generate the Volume Mesh The Volume Mesh is written to the GTM file for import into CFX-Pre GTM file automatically written when volume mesh is generated Contains all the mesh and region information Uses double-precision coordinates Not viewable in CFX-Mesh, use CFX-Post Can be repeated after any change to the mesh settings

Stopping Mesh Generation
To abort surface mesh or volume mesh generation, use the Interrupt or Halt Current Processing button This button is active only during mesh generation and geometry verification Limitation: Interrupt takes effect only when underlying process exchanges data with user interface In some circumstances the mesh process may go on for a long time without exchanging data with the user interface In these cases, if you want to terminate the process immediately, you can use Task Manager (Windows) or kill command (Unix) to end the following processes. (Use with care) srfmsh_wb.exe nsurf3d_wb.exe inflate_wb.exe nvol3d.exe nvol2d_wb.exe

A single virtual surface 78 Surfaces represent car body
Virtual Topology By Default CFX-Mesh resolves every edge using a minimum of 3 vertices and meshes every face Results in a large mesh when there are many short edges and narrow faces in the CAD data Virtual Topology allows users to combine faces and edges into Virtual Faces and Virtual Edges CFX-Mesh only sees the combined Virtual Face or Virtual Edge A single virtual surface 78 Surfaces represent car body

Creating Virtual Topology
Virtual Topology includes Virtual Face and Virtual Edge Virtual Topology can be created either automatically or manually Virtual Topology can be created in CFX-Mesh or in the Meshing Application Automatic Virtual Topology Creation: CFX-Mesh automatically detect candidate edges and faces that could be merged based on geometric parameters such as contact angle between faces, relative areas of faces, aspect ratios and shared boundary ratio Once these candidates have been detected, virtual edges and faces are created automatically Where possible, external edges of Virtual Faces will be automatically merged together to form Virtual Edges Manual Virtual Topology Creation: User manually create Virtual Topology by inserting Virtual Faces or Virtual Edges In the Virtual Face creation, user can turn on and off the option of automatic merging possible external edges of Virtual Faces to from Virtual Edges Automatic Virtual Topology creation Manual Virtual Topology creation

Automatic Virtual Topology
Automatic Virtual Topology creation: User controls for this feature are very simple Automatic Merge Strategy controls the aggressiveness of the automatic Virtual Topology algorithm. The Low option merges the worst faces and edges in the model, while the High option attempts to merge much more of the geometry. Select Virtual Topology in the Tree View. Controls are available in the Details View Automatic Merge Option defines whether the automatic Virtual Topology operation should be applied to the whole model (the default) or whether it should only apply to a selection of faces. The face selection can be defined by selecting the faces directly from the graphics window or by selecting a Region name in the tree view.

Virtual Topology Example
Automatic Virtual Topology example: Create a Virtual Face which includes 3 faces at the top Several ways of doing this automatically Method 1: Generate Virtual Topology on Entire Model Select Automatic merge Option as Entire Model Right Click on Virtual Topology in the Model Tree and select Generate Virtual Topology on Entire Model

Method 2: Generate Virtual Topology on Selected Set Select Automatic Merge Option as Selected Set Select three top faces and apply Right Click on Virtual Topology in the Model Tree and select Generate Virtual Topology on Selected Set

Method 3: Generate Virtual Topology on on a control (Composite 2D region, inflated boundary, etc) Create a Composite 2D Region which contains 3 faces at the top Right Click on the created Composite 2D Region Select Simplify Location using Virtual Topology Virtual Edges Virtual Face Final results for these three methods are the same – One virtual face and two virtual edges will be created.

Fine mesh due to sliver surface
Virtual Face Example Manually creating a Virtual Face: Right Click on Virtual Topology in the Model Tree and Insert a Virtual Face Select the required faces from the graphics window and Apply Can select Composite 2D regions as well Selected faces must be adjacent Virtual Face example: Fine mesh due to sliver surface Select 3 faces Mesh on Virtual Face

Mesh with auto generation of Virtual Edge turned off.
Virtual Edges Virtual Face … Where possible, CFX-Mesh will automatically merge external edges to form Virtual Edges. This behavior can be turned off from the Options panel Single Edge Mesh with auto generation of Virtual Edge turned off.

Virtual Edge Example Creating a Virtual Edge: Virtual Edge example:
Right Click on Virtual Topology in the Model Tree and Insert a Virtual Edge Select the required edges from the graphics window and Apply Selected edges must be adjacent Virtual Edge example: Mesh with Virtual Edge

Virtual Topology Restrictions
Limited to “developable surfaces” A developable surface has the property that it can be made out of sheet metal A virtual surface can be created for a group of surfaces that can be unfolded or unrolled into a flat plane Virtual Faces cannot form a closed region All six sides of a cube cannot be combined into a Virtual Face

Virtual Topology Rules
Constituent faces of a Virtual Faces will not be available for selection. You can only select the Virtual Face. Should consider boundary conditions requirements before defining Virtual Faces Look for the status symbols of features in the Model Tree after creating or deleting virtual entities. Some features may become invalid or may require verification Virtual Topology definitions are persistent for geometry updates If a location or CAD face does not exist after geometry update, the virtual entity will become invalid You can add more faces/edges to an existing Virtual Face or Virtual Edge You can include an existing Virtual Face or Edge in a new Virtual Face or Edge

Workshop B.1 Aircraft Engine-Airframe

Goals This workshop will take you through the process of importing an aircraft engine and airframe model prepared in DesignModeler, setting the mesh spacings, and generating a surface mesh for a CFD analysis. You will return to this workshop later (Workshop A.4) and add virtual topology. Goals: Import the DM model file. Define 2D regions for boundary conditions. Define mesh spacings

Opening the Geometry File
Copy the file Aircraft_Engine-Airframe.agdb to your working directory Launch ANSYS Workbench Double click on Mesh under component systems. This will create a ‘Mesh component’ in the Project Schematic area. Right click on and “Import Geometry” and click on “Browse…”. Locate and open the file Aircraft_Engine-Airframe.agdb. Once the geometry is loaded double click on to open the meshing application.

Imported Geometry Only half the model will be meshed to take advantage of the symmetry in the flow field

Choosing the CFX-Mesh Method
Right-click on Mesh and select Insert Method Select the body Change the Method to CFX-Mesh Right-click on the method in the tree and select Edit Mesh in CFX-Mesh

Creating Composite Regions
Now create composite 2D regions: Right-click on Regions in the Tree View and Insert a Composite 2D Region called Symmetry on the upper- Y surface Create the remaining 2D Region's as shown in the right figure Symmetry Outlet Top Bottom Right Inlet

Hiding Composite Regions
Now hide the newly created 2D Regions: Under Tree View > Regions, right click on Symmetry and select Hide Similarly hide all other 2D Regions except the Default 2D Region. You can do them all at once. Note: Hiding the external boundaries makes it easier to see the aircraft surfaces and also makes it easier to pick the surfaces of the aircraft

Setting Global Spacings
Set the Default Body Spacing: Under Tree View > Mesh > Spacing, select Default Body Spacing and set Maximum Spacing to 0.08 [m] Set the Default Face Spacing: Under Tree View > Mesh > Spacing, select Default Face Spacing and set the parameters as shown Generate surface mesh: Under Tree View >Preview, right click on Default Preview Group and select Generate Surface Meshes

Surface Mesh Preview Review the surface mesh

CAD Model Issues The CAD model has many narrow surfaces which are not significant to the flow analysis The CAD model has many short edges because of the way the surfaces are constructed By default CFX-Mesh, resolves these narrow surfaces and short edges, resulting in unnecessary mesh refinement and poor quality elements We will revisit this geometry in Workshop B.4 and create virtual faces and virtual edges to remove the unnecessary narrow faces and edges, thereby by reducing the mesh size and improving quality For now, save the CFX-Mesh database (File > Save Project)

Workshop B.2 Static Mixer: Basic Settings, Mesh Controls and Inflation

Goals This workshop will take you through the process of meshing a Static Mixer geometry with CFX-Mesh. Line mesh controls and inflation layers will be added to better refine the mesh The basic steps involved in this workshop are: 1. Start a new instance of the ANSYS Meshing Application and open the geometry file to be meshed 2. Set the Mesh Method to CFX-Mesh and edit the Method 3. Define any desired composite regions 4. Set global mesh spacings (Body Spacing and Face Spacing) 5. Preview the initial surface mesh 6. Define Point Spacings and Line Mesh Controls 7. Define Inflation Boundaries 8. Generate the Volume Mesh and save the meshing database

Starting the Meshing Application
Copy the file staticmixer.agdb to your working directory Launch ANSYS Workbench Double click on Mesh under component systems. This will create a ‘Mesh component’ in the Project Schematic area. Right click on and “Import Geometry” and click on “Browse…”. Locate and open the file staticmixer.agdb. Once the geometry is loaded double click on to open the meshing application.

Meshing Options Form When the Meshing Application comes up, go to the Meshing Options Panel which appears at the right of the screen Set the Physics Preference to CFD Set the Mesh Method to CFX-Mesh Make sure that Set Meshing Defaults toggle is enabled Click OK

CFX-Mesh Note that the model is now displayed in the CFX meshing environment.

Making the Model Transparent
In CFX-Mesh, click on the Geometry entry in the Tree View. In the Details View and move the Transparency slider to 50% to make the model partially transparent This makes it easier to see hidden faces in the model

Defining Composite Region in1
Right-click on Regions in the Tree View and select Insert Composite Region Create a Composite Region named in1 at the side pipe inlet as shown

Defining Composite Region in2
Create a Composite Region named in2 at the other side pipe inlet as shown

Defining Composite Region out
Create a Composite Region named out at the bottom pipe outlet as shown

Setting the Global Body Spacing
Click on the + sign next to the Spacing entry in the Tree View to expand it Set the Default Body Spacing to 0.20 m Note the mesh size preview icon in the viewport

Setting the Global Face Spacing
Set the Default Face Spacing Option to Angular Resolution with a setting of 18° Set the Minimum Edge Length to m and the Maximum to 0.20 m Again note the mesh size preview icon

Initial Mesh Preview Click on the + sign next to Preview in the Tree View to expand it Right-click on the Default Preview Group and select Generate Surface Meshes

Generating a Volume Mesh
The initial mesh is rather coarse for CFD purposes although it illustrates the basics steps involved in generating a tetrahedral mesh. Right-click the Mesh entry in the Tree View and select Generate Volume Mesh CFX-Mesh will create the volume mesh The information panel at the bottom right will display the node and element count for the mesh

Mesh Refinement The first part of this tutorial resulted in a rather coarse mesh with no resolution of the boundary layer near walls Although a better quality mesh for CFD purposes could be generated by defining finer global mesh spacings, the global mesh spacings will be left as they are Instead, a mesh control will be defined to refine the mesh in the area of the two pipe inlets. Also, an inflation layer will be added to the all walls in the geometry to better resolve the boundary layer

Mesh Control: Point Spacing
In the tree view right click on Controls under the Mesh listing and Insert a Point Spacing In the Details View for the Point Spacing enter the following: Length Scale = 0.1 Radius of Influence = 0.5 Expansion Factor = 1.2 This defines a point spacing which describes the element size and the region of influence over which it will be applied

In the white text box, clear None and type in 1,-3,-1
Line Control 1 Right-click on Controls in the Tree View, and select Insert > Line Control In the Details View for the Line Control, click on Cancel in the box next to the first Point. Right-click the red bar in the box next to the first Point and select Edit in the pop-up menu In the white text box, clear None and type in 1,-3,-1 You can hit Enter from the keyboard or click in the model view to finish Units are entered automatically Similarly set the coordinates of the second Point to 1,-1,-1 Leave the Option as Uniform Click in the empty Spacing box and select Point Spacing 1 from the Tree View and then click Apply

Line Control 2 and Inflation
In the Tree View, right-click on Controls under the Mesh listing and Insert another Line Control For Line Control 2: Enter 1, 3 ,1 for the first Point Enter 1, 1 , 1 for the second Point Select Point Spacing 1 as the Spacing In the Tree View right-click on Inflation and Insert an Inflated Boundary In the Details View for Inflated Boundary 1, click in the Location box marked None, select Default 2D Region from the Tree View as the Location and click Apply This will inflate from all walls in the model Set the Maximum Thickness for the inflated boundary to 0.2 m

Mesh Preview for Refined Mesh
Right-click on Preview > Default Preview Group and select Generate This Surface Mesh Notice the finer mesh in the two side pipes You can modify the Length Scale of Point Spacing 1 to refine the mesh further Also note the quad faces on the faces normal to the inflated boundary

Final Volume Mesh You are now ready to create and save the volume mesh: Select Tools > Options > CFX-Mesh Options Check that Volume Mesh Output is set to Add to CMDB File Click OK Click on the Generate Volume Mesh icon on the task bar When the process finishes, save your CFX-Mesh database (File > Save) The volume mesh is now stored in the Meshing Application cmdb file Note the change in the node and element count in the Information window and the addition of prisms from inflation

Workshop B.3 Extruded Mesh

Goals This workshop will take you through the process of meshing a simple box geometry with an extruded 2D mesh. The Full extrusion option will be demonstrated. The basic steps involved in this workshop are: 1. Start a new instance of the ANSYS Meshing Application and open the geometry file to be meshed 2. Set the Mesh Method to CFX-Mesh and edit the Method 3. In CFX-Mesh, change the mesh options to Extruded 2D Mesh and set the extrusion options 4. Define the faces for the 2D periodic pair 5. Set global mesh spacings (Body Spacing and Face Spacing) 6. Define an inflation layer on the side walls 7. Preview the surface mesh 8. Generate the Volume Mesh and save the meshing database

Starting the Meshing Application
Copy the file box.agdb to your working directory Launch ANSYS Workbench Double click on Mesh under component systems. This will create a ‘Mesh component’ in the Project Schematic area. Right click on and “Import Geometry” and click on “Browse…”. Locate and open the file box.agdb. Once the geometry is loaded double click on to open the meshing application.

Meshing Options Form When the Meshing Application comes up, go to the Meshing Options Panel which appears at the right of the screen Set the Physics Preference to CFD Set the Mesh Method to CFX-Mesh Make sure that Set Meshing Defaults toggle is enabled Click OK

CFX-Mesh The model is now displayed in the CFX meshing environment.
Note that there are two faces on either end of the bar. As is, this would not be a general sweepable body in the Meshing Application Swept Mesher.

Mesh Options Click on the Options entry under Mesh in the Tree View
In the Details View, set the Meshing Strategy Option to Extruded 2D Mesh Leave the 2D Extrusion Option set to Full Change the Number of Layers to 50 with a Uniform distribution

Extruded Periodic Pair
Note the addition of an Extruded Periodic Pair in the Tree View. This entry has a red X next to it since the faces which comprise it have yet to be defined. Click on the Extruded Periodic Pair entry in the Tree View In the Details View, select the two faces at the high Z end of the box and click Apply in the Location 1 entry box Similarly select the two faces at the other side of the box and click Apply in the Location 2 entry box

Setting the Global Body Spacing
Click on the + sign next to the Spacing entry in the Tree View to expand it Set the Default Body Spacing to 0.10 in Note the mesh size preview icon in the viewport

Setting the Global Face Spacing
Set the Default Face Spacing Option to Constant with a setting of 0.10 in

Initial Mesh Preview Select Preview > Default Preview Group > Generate Surface Meshes Note the extrusion in the length direction

Adding Inflation In the Tree View right-click on Inflation and Insert > Inflated Boundary In the Details View for Inflated Boundary 1, select the four sides of the box from the viewport and click Apply in the Location box. This will inflate the mesh from the four sides. Set the Maximum Thickness to 0.20 in

Final Mesh Preview Right-click on the Default Preview Group and select Generate Surface Meshes Since there are now quad faces on the ends from the inflated layer, a combination of hex and prism elements will be generated when the mesh is extruded

Final Volume Mesh You are now ready to create and save the volume mesh: Click on the Generate Volume Mesh icon on the task bar When the process finishes, save your CFX-Mesh database (File > Save). The volume mesh is now stored in the Meshing Application cmdb file Note that the Mesh Information Window shows that the volume mesh contains a combination of hexahedral (extruded quads) and prismatic (extruded tris) elements

Workshop B.4 Virtual Topology for Geometry and Mesh

Goals This workshop will take you through the process of using virtual topology to create a better quality mesh for the aircraft engine geometry imported in Workshop B.1 Goals: Use Automatic Virtual Topology to improve mesh quality Open the CFX-Mesh database that you saved at the end of Workshop B.1

CAD Issues and Virtual Topology
The CAD model has many narrow surfaces which are not significant to the flow analysis CAD model has many short edges because of the way the surfaces are constructed By default CFX-Mesh, resolves these narrow surfaces and short edges, resulting in unnecessary mesh refinement and poor quality elements We will create virtual faces and virtual edges to remove the unnecessary narrow faces and edges, thereby by reducing the mesh size and improving quality The automatic method of creating virtual topology will be demonstrated in the workshop

Initial Surface Mesh (Before VT)

Automatic Virtual Topology
Select Virtual Topology in the Tree View Set the Automatic Merge Strategy to Low Set the Automatic Merge Option to Entire Model Right-click on Virtual Topology and select Generate Virtual Topology on the Entire Model

Viewing Virtual Faces You should see that a number of virtual faces and edges have been created These appear in the Tree View below the Virtual Topology object You can click on the various virtual faces and edges. They are color coded so that different faces and edges appear differently. The leading and trailing edge of the wing are areas of interest for CFD. You will find that they have been grouped into virtual faces which is not desirable

Deleting Virtual Faces
Find any virtual faces which include the wing leading edge faces and delete them These are Virtual Face 8 and Virtual Face 11

Deleting Virtual Faces
Find the virtual face which include the wing trailing edge and delete it This is Virtual Face 7

Preview Surface Mesh with VT
Regenerate the surface mesh to see the effect of adding virtual topology

Creating the Volume Mesh
You could further modify the mesh by creating virtual faces and edges in selected areas manually to further improve the mesh quality Generate the volume mesh and save the CFX-Mesh database

ANSYS Meshing Application Introduction

Similar presentations

Presentation on theme: "ANSYS Meshing Application Introduction"— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

ANSYS Meshing Application Introduction

Similar presentations

Presentation on theme: "ANSYS Meshing Application Introduction"— Presentation transcript:

Similar presentations

About project

Feedback