Engineering Solutions

CFD-1400: Wind Tunnel Mesh

CFD-1400: Wind Tunnel Mesh

 Previous topic Next topic Expand/collapse all hidden text  

CFD-1400: Wind Tunnel Mesh

 Previous topic Next topic JavaScript is required for expanding text JavaScript is required for the print function  

In this tutorial you will generate a wind tunnel type mesh for external CFD analysis. The mesh consists of a Cartesian hexa-mesh for the far field, and a hybrid grid (tetras with boundary layers) in the vicinity of the object.

The tutorial includes the following steps:

•Setting the user profile
•Opening the model file to be used
•Using the wind tunnel functionality
•Surface meshing
•Volume meshing using the CFD Tetramesh panel
•Organizing the model and preparation for CFD export
•Export for FLUENT
hmtoggle_plus1greyStep 1: Load the CFD User Profile
1.From the menu bar, select Preferences > User Profiles or click userProfile-24on the Standard toolbar.
2.Select Engineering Solutions > CFD > AcuSolve.  
3.Click OK.
hmtoggle_plus1greyStep 2: Open the Model File
1.From the Standard toolbar, click the Open Model icon fileOpenModel-24.
2.Select the airplane.hm file.
3.Click Open to load the file.  

wind_mesh_01
hmtoggle_plus1greyStep 3: Use the Wind Tunnel Mesh Tool
1.Click Mesh > Volume Mesh 3D > Wind Tunnel. The Wind-Tunnel tab opens, displaying instructions for using this tool.
2.Enter values for your model as shown in the following image:

wind_mesh_02

3.Click Generate. A pop-up message will display the estimated number of hexahedral elements that will be created with the specified minimum hex cell size.
4.Click Yes on the pop-up message. The Wind Tunnel Mesh tool generates hexa, pyramids and shell elements and groups them into several collectors.

wind_mesh_03

You may need to rotate the model to obtain this view
hmtoggle_plus1greyStep 4: Generate a Shell Mesh on the Airplane
1.In the Model browser, expand Component, right-click plane, and select Isolate.
2.Click Mesh > Surface Mesh 2D > Automesh. This automatically loads the surface deviation subpanel.
3.With surfs selected in the toggle, hold SHIFT and drag a box around the entire visible airplane geometry. You may need to resize the display first.
4.For element size =, enter 10.
5.For growth rate =, enter 1.2.
6.For min elem size =, enter 2.
7.For max deviation =, enter 0.1.
8.For max feature angle =, enter 15.
9.Set mesh type to trias.
10.Ensure toggles are set to elems to surf comp and first order.
11.Click mesh. A message on the status bar indicates the number of elements created.

wind_mesh_04
hmtoggle_plus1greyStep 5: Mesh the Box Sym Component With an Element Size of 20
1.In the Model browser, show the elements and geometry for box_sym.
2.In the Automesh panel, click the size and bias subpanel.
3.With the surfs toggle active, click any visible part of the box to select it.
4.For element size =, enter 20 and set the mesh type to trias.
5.For map, activate the checkboxes for size and skew.
6.Click mesh. The component is meshed. A message on the status bar indicates the number of elements created.
7.Double-click return to return to the main menu.

wind_mesh_05
hmtoggle_plus1greyStep 6: Equivalence Nodes in box_sym
1.In the Model browser, right-click the component symp and select Show.
2.Click BCs > Check > Edge.
3.Click comps and select the components box_sym and symp.
4.For tolerance =, enter 0.1.
5.Click preview equiv. A message in the status bar indicates the number of nodes found.
6.Click equivalence. The nodes are equivalenced.
7.Click return to close the panel.
hmtoggle_plus1greyStep 7: Create New Component box_ground
1.Click BCs > Components > Single.
2.In the Name field, enter box_ground.
3.Click Color and select magenta.
4.Click Create. The new collector has now been created.
5.Close the dialog.
hmtoggle_plus1greyStep 8: Generate a Surface and a Tria Mesh on the Bottom of the Box
1.In the Model browser, turn off the element display for symp and turn on the display for ground.
2.Click Mesh > Surface Mesh 2D > Surface/Mesh > Spline.
3.Set the selector toggle to nodes.
4.Click the nodes selector to open the extended entity selection menu and pick by path.
5.Set the second toggle to surface only.
6.Pick the nodes by path on the perimeter of the box bottom, as in the following image:

wind_mesh_06

7.Click create.
8.Click return.
9.Click Mesh > Surface Mesh 2D > Automesh.
10.Select the size and bias subpanel, ensure the selector is set to surfs and the element size field is set to 20.
11.In the graphics area, click the box_ground surface.
12.Click mesh. A message on the status bar will indicate the number of elements created.
13.Double-click return to return to the main menu.
hmtoggle_plus1greyStep 9: Equivalence Nodes to Achieve a Closed Volume
1.Click BCs > Check > Edge.
2.Click comps and select the components plane, box_sym, ground, trias_hexas_pyras, and box_ground.
3.Set the tolerance field to 0.1.
4.Click preview equiv.
5.Click equivalence.
6.Click return.
7.In the Model browser, turn off the display of ground, and turn on the element display of trias_hexas_pyras.

wind_mesh_07

8.Return to the Edges panel.
9.Hold SHIFT and drag a box around all the visible components to select them all.
10.Click find edges. A message on the status bar indicates that no edges were found.
11.Select the components again and click preview equiv. A message on the status bar indicates that 0 nodes were found. This ensures that the volume is enclosed, which is necessary for the following tetra meshing step.
12.Click return.
hmtoggle_plus1greyStep 10: Mesh the Closed Volume
1.Click Mesh > Volume Mesh 3D > CFD tetramesh.
2.Under the With BL (fixed) header, click the comps selector and select the component plane.
3.Under the W/o BL (fixed) header, click the comps selector and select the components box_sym, box_ground and trias_hexas_pyras.
4.Click the BL parameters subpanel.
5.For Number of Layers = enter 3.
6.For First layer thickness = enter 0.7.
7.On the Tetramesh parameters subpanel, set the toggle to Interpolate.
8.Click mesh. The mesh may take a few minutes. When the mesh is complete, a message in the status bar will indicate the number of nodes and elements created. Note that two new components, CFD_tetcore001 and CFD_bl001, appear in the Model browser.
9.Click return.
hmtoggle_plus1greyStep 11: Inspect the Mesh
1.Click Mesh > Check > Hidden Lines. In the panel, deactivate the clip boundary elements checkbox.
2.Click show plot and then check and then uncheck the xy plane, yz plane and xz plane checkboxes to display the model in different views.

wind_mesh_08

3.Rotate and inspect the mesh from the side of the model.
4.Click and hold one of the corners of the model. While keeping the mouse button down, drag the corner of the model forth and back to sweep the cutting plane.
5.Click return.
hmtoggle_plus1greyStep 12: Organize Faces
1.In the Model browser, turn off the display for plane, box_sym, trias_hexas_pyras and box_ground so that only CFD_tetcore001 and CFD_bl001 are visible.
2.Click BCs > Faces.
3.Hold SHIFT and drag a box around the visible components to select them.
4.Click find faces. Note that a new component named ^faces appears in the Model browser.
5.Click return.
6.In the Model browser, turn off the display of the elements of CFD_tetramesh_core and CFD_boundary_layer.
7.Click BCs > Organize.
8.Click elems and select on plane.
9.Pick three nodes on the ^faces component, on the face that intersects the airplane model. A good way to determine which area to select is to isolate the display of the box_sym geometry. This will show you the face to focus on. Turn the display of the ^faces component back on, and select your three nodes.

wind_mesh_09

10.Click select entities.
11.Click dest component = and select symp.
12.Click move.
13.Click elems >> on plane.
14.Pick three nodes on the bottom of the ^faces component. A good way to determine which area to select is to isolate the display of the box_ground geometry. This will show you the face to focus on. Turn the display of the ^faces component back on, and select your three nodes.

wind_mesh_10

15.Click select entities.
16.Click dest component = and select ground.
17.Click move.
18.Click return to close the panel.
hmtoggle_plus1greyStep 13: Delete Collectors
1.In the Model browser, right-click the component ^faces, and select Delete.
2.In the pop-up dialog, click Yes to confirm the deletion.
3.In the Model browser, turn on the display of CFD_tetcore001 and CFD_bl001.
4.Press the CTRL key and select edges_xz and edges_xy in the Model browser.
5.Right-click and select Delete.
6.In the pop-up dialog, click Yes to confirm the deletion.
7.In the same way, also delete trias_hexas_pyras, box_sym and box_ground.
hmtoggle_plus1greyStep 14: Organize Components
1.Click BCs > Organize.
2.Click elems and select by collector.
3.Select CFD_tetcore001 and CFD_bl001.
4.Click select.
5.Click dest component = and select fluid_hex.
6.Click move. When the move is complete, nothing should be visible in the graphic area.
7.Click return.
hmtoggle_plus1greyStep 15: Use the Model Browser to Rename and Delete Components
1.In the Model browser, display elements for fluid_hex.
2.Right-click fluid_hex in the Model browser and select Rename.
3.Enter the new name as fluid.
4.Select CFD_tetcore001 and CFD_bl001 and delete them using the process described in Step 14.
5.Right-click Component and select Show to show all remaining components in the graphic area.

wind_mesh_11
hmtoggle_plus1greyStep 16: Export the File as .cas
1.Click Export Solver Deck fileExportSolver-24.
2.Ensure that CFD is selected for the File Type, and pick Fluent for the Solver Type.
3.Use the File field to navigate to the destination folder and enter the name wind_tunnel_mesh.
4.Click Export. A dialog appears. After reading the dialog, click Yes.

wind_mesh_12

5.In the pop-up dialog that appears, you are asked whether to reuse the setup from an existing FLUENT file. Since you just generated the grid and do not have a set up file (*.cas), click No. It may take a few minutes for the file to be created.
6.When the file creation is complete, a pop-up window appears. Click OK.