Workshop 3: Cutcell Mesh Generation. Introduction to ANSYS Fluent Meshing Release. Release ANSYS, Inc.

Size: px

Start display at page:

Download "Workshop 3: Cutcell Mesh Generation. Introduction to ANSYS Fluent Meshing Release. Release ANSYS, Inc."

Marcia Wade
5 years ago
Views:

1 Workshop 3: Cutcell Mesh Generation 14.5 Release Introduction to ANSYS Fluent Meshing ANSYS, Inc. December 21, 2012

2 I Introduction Workshop Description: CutCell meshing is a general purpose meshing technique which is suitable for a large range of applications. Due to the large fraction of hex cells in the generated mesh, the CutCell mesh can often produce better results than regular tetrahedral meshes. This meshing method uses a direct surface and volume approach without needing cleanup or decomposition, thereby reducing the turnaround time required for meshing. This tutorial demonstrates the generation of the CutCell mesh for a manifold. Learning Aims: This workshop will cover how to Import the CAD geometry. - Examine the objects. Create capping surfaces for the inlet and outlets. - Define size functions. Create the CutCell mesh. Set parameters and generate prisms for the CutCell mesh. Improve the CutCell mesh quality ANSYS, Inc. December 21, 2012

5 program group. Enable Meshing Mode under Options.

3 Starting ANSYS Fluent in Meshing Mode Open the Fluent Launcher by clicking the Windows Start menu, then selecting Fluent in the Fluid Dynamics sub-menu of the ANSYS 14.5 program group. Enable Meshing Mode under Options. Set Working Directory to the area where files are Click OK to start Fluent in meshing mode ANSYS, Inc. December 21, 2012

Import the CAD Geometry File Import CAD... Ensure that Import Single file is enabled. Click and select the file WS3_manifold.igs. Enable Import Curvature Data from CAD.

Click the Advanced... button to open the CAD Advanced Options dialog box. Enable Save PMDB in the File group box. Select mm in the Length Unit drop-down list.

4 Import the CAD Geometry File Import CAD... Ensure that Import Single file is enabled. Click and select the file WS3_manifold.igs. Enable Import Curvature Data from CAD. Retain default of 40 degrees for Feature Angle. Enter solid for Zone Name Prefix. Retain the value of 1 for Scale Factor and the selection of body in the One zone per drop-down list, respectively. Click the Advanced... button to open the CAD Advanced Options dialog box. Enable Save PMDB in the File group box. Select mm in the Length Unit drop-down list. Choose Conformal Tessellation in the Tessellation group box. Specify values of 0.3 and 20 for Min and Max Size, respectively. Retain the selection of Import Named Selections in the Named Selection group box. Click Apply and close the CAD Advanced Options dialog box. Click Import in the Import CAD Geometry dialog box. Close the Import CAD Geometry dialog box ANSYS, Inc. December 21, 2012

5 Minimum Size and Tessellation Tolerance In this case, the smallest feature in the geometry is 30 mm in circumference. Hence the minimum size to be used would be approximately 3 mm. It is recommended that you use a Tolerance value 1/10th the intended minimum size (0.3) ANSYS, Inc. December 21, 2012

6 Display Grid... Displaying the Geometry Select solid-part-1 from the list of Face Zones. Enable Free From the list of Options. Click Display. Conformal faceting has brought the model in well connected and there are no blue free faces. It is not a prerequisite to have fully connected input surfaces for cutcell meshing but it improves robustness of the method, reducing the likelihood of leakages ANSYS, Inc. December 21, 2012

Create the capping surface for the inlet. part-1 in the Objects list and click Draw. Enter inlet for Object Name. Select internal in the Type drop-down list.

To allow the recovery of baffle surfaces by the CutCell mesher, the type must be set to internal, which will be recovered as a wall.

7 Create the capping surface for the inlet. part-1 in the Objects list and click Draw. Enter inlet for Object Name. Select internal in the Type drop-down list. Though the capping surfaces to be created represent an inlet/outlet zone, to the cutcell algorithm they are essentially zero-thickness baffle surfaces. To allow the recovery of baffle surfaces by the CutCell mesher, the type must be set to internal, which will be recovered as a wall. You can then change the type of recovered boundary zone to the appropriate type. Select Edge in the Entity Type list. Disable Remesh and enable Auto Redisplay. Select the edge as shown in the graphics with RMB Hit Create A wrap object (inlet) is created and added to the Objects selection list. Creating Capping Surface ANSYS, Inc. December 21, 2012

Capping Surface Created for Outlets Create the capping surface for the outlets.

As described, to allow the recovery of baffle surfaces by the CutCell mesher, the type must be

You can then change the type of recovered boundary zone to the appropriate type.

8 Capping Surface Created for Outlets Create the capping surface for the outlets. Enter outlet-1 for Object Name. Select internal in the Type drop-down list. As described, to allow the recovery of baffle surfaces by the CutCell mesher, the type must be set to internal, which will be recovered as a wall. You can then change the type of recovered boundary zone to the appropriate type. Select Edge in the Entity Type list. Select the edge as shown. Click Create. A wrap object (outlet-1) is created and added to the Objects selection list ANSYS, Inc. December 21, 2012

9 Capping Surface for Outlet 2 and 3 Similarly, create the capping surfaces outlet-2 and outlet-3. Close the Capping Surface dialog box. Select all the objects in the Objects selection list and click Draw. Close the Capping Surface dialog box. outlet-1 outlet-2 outlet-3 inlet ANSYS, Inc. December 21, 2012

Set Up Size Functions In the Mesh Generation task page, under Create group box, click Size Functions... Enter values of 3 and 12 for Min and Max, respectively in the Global Controls group box.

If not, the maximum size will be automatically set to a value close to but smaller than the specified maximum size, which is in the ratio of 2 n with the minimum size specified. Retain the value of 1.

10 Set Up Size Functions In the Mesh Generation task page, under Create group box, click Size Functions... Enter values of 3 and 12 for Min and Max, respectively in the Global Controls group box. Note: The minimum and maximum sizes should be in the ratio 2 n. If not, the maximum size will be automatically set to a value close to but smaller than the specified maximum size, which is in the ratio of 2 n with the minimum size specified. Retain the value of 1.2 for Growth Rate and click Apply. You can use the Draw Sizes option to display red boxes of the specified global minimum and maximum sizes over the selected zones. Click Create Defaults in the Define Size Function group box. The curvature and proximity size functions will be listed in the Size Functions selection list. Delete the face proximity size function. Select default-face-proximity in the Size Functions selection list. Click Delete. Close the Size Functions dialog box ANSYS, Inc. December 21, 2012

Define Material Point Define the material point for internal flow.

Enable Limit in Z in the Clipping Planes group box in the Mesh Generation task page and adjust the lower slider to see inside

Select the zone solid-part-1 using RMB in the graphics window.

11 Define Material Point Define the material point for internal flow. Click Material Point in the Create group box in the Mesh Generation task page. Enable Limit in Z in the Clipping Planes group box in the Mesh Generation task page and adjust the lower slider to see inside the geometry as shown. Ensure that the selection filter is set to zone by using hot keys (Ctrl+Z). Select the zone solid-part-1 using RMB in the graphics window. Click Compute in the Material Point dialog box to get the centroid coordinates of the selected zone. Enable Draw to view the material point computed. Select the Name fluid and click Create to create the point once it s position is correctly verified Close the Material Point dialog box. Material Point ANSYS, Inc. December 21, 2012

Generate the CutCell Mesh Save the surface mesh with all the settings applied before generating the CutCell mesh File Write Mesh manifold_setup_cutcell.

Select fluid in the Material points selection list. Retain the selection of Keep Solid Cell Zones. Click Create.

12 Generate the CutCell Mesh Save the surface mesh with all the settings applied before generating the CutCell mesh File Write Mesh manifold_setup_cutcell.msh.gz Click CutCell... in the Volume Mesh group box in the Mesh Generation task page. Select all the objects in the Objects selection list. Select fluid in the Material points selection list. Retain the selection of Keep Solid Cell Zones. Click Create. A Question dialog box appears, asking if you want to proceed even though some objects (capping face objects) do not comprise edges. Click Yes in the Question dialog box ANSYS, Inc. December 21, 2012

Examine the Mesh Open Display Mesh and in the Bounds tab enter

Cells tab in the Display Grid dialog box and enable All in the

Select all the cell zones in the Cell Zones selection list.

13 Examine the Mesh Open Display Mesh and in the Bounds tab enter -50 for Minimum and Maximum in the Z Range group box Click the Cells tab in the Display Grid dialog box and enable All in the Options group box. Select all the cell zones in the Cell Zones selection list. Click Display. Note it is always wise to set bounds before displaying any cell zones! ANSYS, Inc. December 21, 2012

Check the Quality For CutCell meshes we generally use orthoskew in the mesher as the quality check but we can check orthogonal quality as used in

14 Check the Quality For CutCell meshes we generally use orthoskew in the mesher as the quality check but we can check orthogonal quality as used in the solver mode by using Mesh Check Quality Min orthogonal quality is reported as ~0.141 which is reasonable ANSYS, Inc. December 21, 2012

Clean Up the CutCell Mesh Operations such as deleting dead zones, deleting geometry/wrap objects, deleting edge zones, removing face/cell zone name prefixes (cutcell-) and/or suffixes, deleting

15 Clean Up the CutCell Mesh Operations such as deleting dead zones, deleting geometry/wrap objects, deleting edge zones, removing face/cell zone name prefixes (cutcell-) and/or suffixes, deleting unused faces and nodes (original geometry) are performed during the cleanup operation. In the Mesh Generation task page under Volume Mesh group box click Cleanup. A Question dialog box appears, asking you to confirm that you want to proceed with the cleanup operation. Click Yes in the Question dialog box to perform the cleanup operation. The number of unused boundary faces deleted and the number of unused nodes deleted after performing the operation is printed in the console ANSYS, Inc. December 21, 2012

16 Change the Zone Types The inlet and outlet zones are recovered as wall zones. You will now change the boundary zone type to the appropriate type. Boundary Manage Select the inlet zone, inlet in the Face Zones selection list. Retain the selection of Change Type in the Options list. Select velocity-inlet in the Type drop-down list and click Apply. Similarly select the outlet zones, outlet-1, outlet-2, and outlet-3 in the Face Zones selection list. Retain the selection of Change Type in the Options list. Select pressure-outlet in the Type drop-down list and click Apply. Close the Manage Face Zones dialog box ANSYS, Inc. December 21, 2012

Generate Prism for CutCell Mesh Save the volume mesh. File Write Mesh manifold_cutcell_volume.

under the Volume Mesh group box, click CutCell. The Create Prisms.

We will now examine the face zone group created from the fluid boundaries and determine the

17 Generate Prism for CutCell Mesh Save the volume mesh. File Write Mesh manifold_cutcell_volume.msh.gz We will now generate post prisms for the CutCell Mesh In the Mesh Generation task page, under the Volume Mesh group box, click CutCell. The Create Prisms... button is now enabled in the CutCell dialog box. We will now examine the face zone group created from the fluid boundaries and determine the wall zones for which prism meshing parameters are to be specified. Select _fluid in the Boundary Zone Groups selection list and click Draw ANSYS, Inc. December 21, 2012

2 for Rate. Click Apply in the Zone Specific Growth group box. Click Apply and Create in the Prisms dialog box.

18 Generate Prism for CutCell Mesh Deselect all the zones corresponding to the inlets and outlets in the Boundary Zones selection list. Select aspect-ratio in the Offset Method drop-down list. Select geometric in the Growth Method drop-down list. Enter 5 for First Aspect Ratio. Set Number of Layers to 5. Enter 1.2 for Rate. Click Apply in the Zone Specific Growth group box. Click Apply and Create in the Prisms dialog box. A Question log box will appear, asking if you want to morph the existing volume mesh. Type Yes to generate the prism layers. Close the Prisms and CutCell dialog boxes. Note that these post prisms can be inserted on almost any input volume mesh in Fluent Meshing ANSYS, Inc. December 21, 2012

Check Quality of the CutCell Mesh After prism creation we get a summary in the console showing the max orthoskew: Use Mesh Check Quality again to give

19 Check Quality of the CutCell Mesh After prism creation we get a summary in the console showing the max orthoskew: Use Mesh Check Quality again to give min Orthogonal Quality Note Orthoskew = 1 Orthogonal Quality and is used in Fluent Meshing for Legacy TGrid reasons ANSYS, Inc. December 21, 2012

20 Improve Beyond Smoothing Quality Again, the mesh quality can be improved beyond the smoothing quality limits set as default. You will modify the improve parameters, specifying a tighter quality limit for the node movement operation. Set the parameters for mesh quality improvement. Enter the following text command in the console. >/mesh/cutcell/set/set-post-morph-parameters Quality limit for Auto Node Move [0.9] 0.75 Iterations for Auto Node Move [1] Iterations per node in Auto Node Move [50] Restrict nodes on surfaces [yes] no Dihedral angle for sharp feature angle [120] Quality limit for cavity remeshing [0.95] Note: The prism cap in this case is an internal boundary zone, and hence, you can allow full freedom of node movement to improve quality. Improve the mesh quality using the following command: >/mesh/cutcell/modify/post-morph-improve () Cell Zones(1) [()] fluid* Cell Zones(2) [()] () Face Zones(1) [()] *cap* Face Zones(2) [()] The worst quality is reported to be around ANSYS, Inc. December 21, 2012

21 Merge Cell Zones Open Mesh Manage Select fluid and prism-cellsfluid-# in the list Choose Merge under Options Tick Merge Sub Zones This will ensure that the imprinted quad boundaries are also merged with their tri neighbours Click Apply ANSYS, Inc. December 21, 2012

Display Cutplane of CutCell Mesh with Prisms Open Display Grid

Enter -50 for Minimum and retain the value of -50 for Maximum in

22 Display Cutplane of CutCell Mesh with Prisms Open Display Grid Click the Cells tab in the Display Grid dialog box and enable All in the Options group box. Select all the cell zones in the Cell Zones selection list. Enter -50 for Minimum and retain the value of -50 for Maximum in the Z Range group box in the Bounds tab. Click Display. Prism Layers ANSYS, Inc. December 21, 2012

Hit the Switch to Solution button to enable the solver Note that

to polyhedra in solution mode Scale the grid as we imported in mm

Hit Scale Close Switch to Solver Mode Save the case file File

23 Hit the Switch to Solution button to enable the solver Note that the parent-child hanging node regions are automatically converted to polyhedra in solution mode Scale the grid as we imported in mm Select the Scale button in task page Choose Mesh Was Created In mm Hit Scale Close Switch to Solver Mode Save the case file File Write Case Manifold_cutcell.cas.gz ANSYS, Inc. December 21, 2012

24 Summary This workshop demonstrated the procedure for generating the CutCell mesh for a manifold. You created capping surfaces and defined size functions and a material point for the CutCell mesh. You then created and examined the CutCell mesh, and used the cleanup operation. Further, you set parameters and generated prisms for the CutCell mesh. The tutorial also demonstrated the improvement of the CutCell mesh after prism generation, and changing to solution mode in ANSYS FLUENT ANSYS, Inc. December 21, 2012

Introduction to ANSYS FLUENT Meshing

Workshop 04 CAD Import and Meshing from Conformal Faceting Input 14.5 Release Introduction to ANSYS FLUENT Meshing 2011 ANSYS, Inc. December 21, 2012 1 I Introduction Workshop Description: CAD files will