Release 11.0 Documentation for ANSYS Workbench
www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS Workbench
Now that you have a geometry, open the Project Page using the tabs at the top of the window, and click on New Mesh under DesignModeler Tasks to open CFX-Mesh.
You must configure the settings under Tools > Options to ensure that CFX-Mesh automatically opens whenever you choose to create a new mesh and that CMDB is the default file type for saving a volume mesh. For details, please refer to Settings for CFX-Mesh Tutorials for instructions on how to perform this one-time setup.
For details on importing Parasolid files, please refer to Tutorials Requiring Modifications When Importing CAD Files.
Create the 2D Regions:
Create a Composite 2D Region called rotwall on the inner wall, which will subsequently be rotating in the CFD simulation.
Create a Composite 2D Region called SymP1 on the planar face with the lowest Z-coordinate.
Create a Composite 2D Region called SymP2 on the planar face with the highest Z-coordinate.
Set the Maximum Spacing:
Click on Default Body Spacing in the Tree View, which is contained in Mesh > Spacing.
In the Details View, change Maximum Spacing to 0.02 ft, and press Enter on the keyboard to set this value. If you are using geometry which has come from the Parasolid import route, use the value 0.006 m.
This mesh will be used to simulate the flow of a non-Newtonian fluid in ANSYS CFX, with its viscosity depending upon the shear strain. A fine mesh is required on the inner and outer radius walls to resolve the shear layers and accurately predict the viscosity variation in the boundary layer regions. You will use inflation to create layers of prismatic elements on the Wall boundaries. For this tutorial, you will use the First Layer Thickness option, which allows you to set the height of the first prism layer (i.e. the one which actually touches the edge of the geometry). Successive prism layers are then added, each one of thickness equal to the thickness of the previous layer multiplied by the Expansion Factor, until the height of the next prism layer is approximately equal to its width/length. Since the last layer of prisms have approximately unit aspect ratio (side lengths approximately equal), the transition between the prism elements and the tetrahedral elements is smoother using this option. When the First Layer Thickness option is enabled, the Number of Inflated Layers is used as a maximum number of layers rather than an actual number of layers.
In addition, this tutorial will use the Extended Layer Growth parameter. This is only available when the First Layer Thickness option is selected, and it allows extra prism layers to be added beyond the point where unit aspect ratio prisms are reached. Each of these extra layers is of the same thickness as the previous layer, so that unit aspect ratio is maintained. Prisms continue to be added until either the Number of Inflated Layers is reached or the prism layers begin to collide with each other or with the geometry boundaries.
The Extended Layer Growth option is being used here to ensure that as much of the geometry as possible is filled with prisms. This results in a smoother flow pattern for a coarser mesh since the flow is mostly aligned with the prism layers.
Click on Inflation in the Tree View. In the Details View, set Number of Inflated Layers to 40.
Set Expansion Factor to 1.3.
Set Inflation Option > Option to First Layer Thickness and set First Prism Height to 0.0012 ft or 0.00037 m for Parasolid geometry.
Ensure that Extended Layer Growth is set to Yes.
In the Tree View, right-click on Inflation and select Insert > Inflated Boundary.
For Location, select Default 2D Region and rotwall from the Tree View.
Expand the Preview item in the Tree View, right-click over Default Preview Group, and select Generate Surface Meshes. You should be able to see that the prism layers almost fill the geometry.
CFX-Mesh has an Extruded 2D mesh capability which can be used to mesh two-dimensional geometries (such as this one) or to extrude a mesh on one face through a specified translation to form an extruded mesh consisting of triangular prisms and hexahedra. In each case, the geometry is created as a normal 3D geometry. Once you activate the Extruded 2D Meshing capability, you must specify a Periodic Pair which can be either translational or rotational: this identifies two sets of faces which map onto each other by the specified transformation. When you mesh, the surface mesh (including Inflation) is generated as usual. However, instead of volume meshing in the normal manner, all the mesh apart from the mesh on one nominated set of faces (Location 1) is removed, and the mesh on Location 1 is swept through the transformation specified for the Periodic Pair, giving the 2D or extruded mesh.
In order to set up the Extruded 2D mesh, you must first activate the capability, and then create an Extruded 2D Periodic Pair to define the direction of the extrusion.
Click on Options in the Tree View. In the Details View, set Meshing Strategy to Extruded 2D Mesh.
Set Number of Layers to 1. This will give a mesh which is just one layer thick along the Z-axis, so that the flow is truly two-dimensional. Higher values for the number of layers would give you an extruded mesh which could be used for three-dimensional flow, such as a pipe mesh with elements all aligned along the pipe direction.
After you have selected the Extruded 2D Mesh
option, a new item will appear in the Tree View: Extruded Periodic
Pair. At first this shows as being invalid 
because the locations have not yet been specified.
Click on Extruded Periodic Pair.
For Location 1, select SymP1 from the Tree View.
For Location 2, select SymP2 from the Tree View.
Leave Periodic Type > Option set to Translational.
Since the sketches which were used to produce this geometry in DesignModeler consist entirely of circles which have no vertices, CFX-Mesh is unable to determine the translation vector automatically, and you must enter this in the boxes which appear. Set Translation Along X Axis to 0 ft, Translation Along Y Axis to 0 ft, and Translation Along Z Axis to 0.1 ft or 0.03048 m for Parasolid geometry.
Next, take a look at the mesh which is produced.
Right-click over Default Preview Group, and select Generate Surface Meshes.
In order to view the mesh clearly, right-click over Preview in the Tree View, and select Insert > Preview Group. For Location, select Default 2D Region, rotwall, and SymP2 from the Tree View.
Click on Preview in the Tree View, and in the Details View, set Display Mode to Wire Mesh, Face Color Mode to Uniform, and Uniform Color to a dark color (double-click on the existing color to bring up a color selector).
Now click on Preview Group 1 in the Tree View to make it visible again.
You will be able to see that on the two curved surfaces, there are no triangles in the surface mesh. Instead, the mesh on these faces consists of quad elements (four-sided elements) produced by extruding the mesh from SymP1 to SymP2.
Finally, you can generate the volume mesh.
Right-click on Mesh in the Tree View and select Generate Volume Mesh.
Select File > Save As from the main menu.
Save as NonNewtonMesh.cmdb.
The mesh is now complete.
Switch to the Project Page using the tabs at the top of the window, and choose File > Save All to save the project files.
Exit from ANSYS Workbench by selecting File > Exit.