Introduction to ANSYS Fluent Meshing

Transcription

1 Workshop 06: Mesh Creation Including Removal of Gaps and Baffle Thickness 14.5 Release Introduction to ANSYS Fluent Meshing ANSYS, Inc. December 21, 2012

2 I Introduction Workshop Description: Fluent meshing workflow will be used on imported CAD file to generate fluid surface mesh. Then volume mesh will be generated from this surface mesh. Learning Aims: This workshop aims to teach some advanced skills in the use of Fluent Meshing interface. Importing CAD geometry as Tessellation Refinement Extract mid surface for baffles Using improve-feature-capture for capturing sharp angles Using shrink-wrap and sew to get final surface mesh Create volume mesh ANSYS, Inc. December 21, 2012

3 Starting ANSYS Fluent in Meshing Mode Ensure that you have installed Workbench with CAD reader options. Fluent Meshing uses the Workbench CAD readers to import CAD and so this is a prerequisite. 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

4 Importing a CAD Model From the File menu select Import and then CAD. File > Import > CAD... In the Import CAD Geometry dialog box Browse and select the file WS6_Pipe_Geom.agdb. Check Import Curvature Data from CAD Click Advanced... to open CAD Advanced Options dialog box. Select mm from the Length Unit drop-down list. Uncheck Import Part Names and Import Body Names Change the tolerance to 0.01 mm Click Apply. Retain the other default settings and click Close. Click Import. Note that it can take almost 45 seconds to import the file ANSYS, Inc. December 21, 2012

5 Displaying and Inspecting Mesh Click Manage... under Object group box. In the Manage Objects dialog box select all in the list under Objects. Click Draw. All Face and Edge Zones within the Objects selected are shown graphically. Deselect all Face Zones and click Draw to see the feature edges which are also imported from the CAD curves. Re-Select all Face Zones and enable Free in the Face Options group box and click Draw. This will show faces with disconnected nodes i.e. free faces in cyan color in the graphics window. Note that there are lots of disconnected faces in the model. A wrapping option could be applied to this Geometry Object in order to make the faces conformal ANSYS, Inc. December 21, 2012

6 Geometry Issues Gap between two sections of the pipe Baffles in the geometry are required to modeled as zero thickness baffles Sharp angle to capture Geometry Gap Sharp Angle Baffles ANSYS, Inc. December 21, 2012

7 Merge Nodes As there are many free faces in the geometry, we will use Merge Nodes to connect those faces Go to Bouandary Merge Nodes Set Tolarance to 1% of the shortest connected edge length and click Merge ANSYS, Inc. December 21, 2012

8 Create Caps Open the Caps panel, from Create Group Select all Objects & Click Draw Provide Object Name as inlet Change Type to inlet-vent Change Entity Type as Edge Check Create Edges and Auto Redisplay Uncheck Remesh Now select a circumfirential Edge of the pipe in GUI with RMB Click Create A capping surface will be created Similarly create another cap for outletvent (Refer to figure) ANSYS, Inc. December 21, 2012

9 Sizing Function Click Size Functions... in Create group Apply following Global Controls: Min Size: 0.15 Max Size : 1.5 Click Apply Use Create Defaults Button to create default sizing function Select all Face Zones in the list and click on Draw Sizes Use the slider bars to look inside to see the Min, Max sizes displayed in the graphics ANSYS, Inc. December 21, 2012

10 Create Material Point In Create group click on Material Point Change the selection filter to zone (Short-cut key ctrl+z ) and select one of the pipe sections and click compute Click on Draw to see and verify the position for the material point If the position looks correct, specify Name as Fluid and click Create ANSYS, Inc. December 21, 2012

11 Wrap Click on the Wrap... In the Objects Group Select all Objects except inlet and outlet and change wrap type to shrink-wrap Click Wrap. Ignore warnings about empty face zones. Click on Manage... In Objects Group and select all wrap* objects and click Draw We now have conformal wrap type Objects and can utilize the Remove Gaps and Sew functionality Write the mesh File Write Mesh pipe_geom_wrapped.msh.gz ANSYS, Inc. December 21, 2012

12 Sharp Angle Feature Capture In the Manage Object panel select the central thin pipe section wrapobj.1 and Draw We used shrink-wrap here for speed but the sharp angles in this object are not caught well Open the Wrap panel, select obj.1 and re-wrap but this time select cut-wrap then click Wrap A new object named wrap-obj.1-# is created. Select the new Object and click Draw. Note the improved feature capture in the cut-wrap representation. Shrink-wrapped object Cut-wrapped object ANSYS, Inc. December 21, 2012

13 Discard Shrink-Wrap Object As the cut-wrapped object we created is much better than the shrink wrapped object we will delete the latter. Open Manage under Objects in the task page Select wrap-obj.1 in the Objects list Check on Include Faces and Edges so as to delete the object definition and the entities within Click Delete to remove this Object Select wrap-obj.1-12:13 and input wrap-obj.1 into Object name and click Change. This makes our names consistent ANSYS, Inc. December 21, 2012

14 Improve feature capture Observe the mesh at the sharp angle. Although improved with cut-wrap there are still some kinks in the features. To capture these features better, use the TUI command as shown in the image. Input the name of your cutwrap object for imprinting. Accept the default of 3 iterations of imprinting. Write the mesh File Write Mesh pipe_geom_wrapped-2.msh.gz Before improve-feature-capture After improve-feature-capture ANSYS, Inc. December 21, 2012

15 Remove Gap Now we will calculate the gap size between the two solids For this switch to node selection (ctrl+n) and select two nodes on the two pipe sections as shown in the image and then click (ctrl+d) This will show the distance in TUI It will be around 0.5 Similarly calculate thickness of the baffles using the two extreme nodes on the baffle in a single direction It will be around ANSYS, Inc. December 21, 2012

16 Select Remove Gaps... In Objects Group. Select zone filter Ctrl-z and RMB to select Face Zones shown Use hot key Ctrl-B to select objects those face zones belong to in the Remove Gaps list Click List to display the object priorities in the console Enter Gap Distance of 0.75 Retain other default parameters Note we could choose to move high to low priority if we would prefer the higher priority object to move Click Mark and Draw to see the faces marked for gap removal (pink with yellow edges) Click Remove Remove Gap Again select wrap-obj and wrap-obj.1 and Click Draw Marked faces ANSYS, Inc. December 21, 2012

17 Display the baffles (i.e. wrap-obj.3 and wrap-obj.4) in GUI Change Operation to Remove Thickness In Objects Change Gap Distance to 1.25 (slightly larger than baffle thickness) Click on Remove Remove thickness of the baffles This will pop-up a Warning, Click Yes after reading it ANSYS, Inc. December 21, 2012

18 Sew In the TUI change process-slits-as-baffles? to yes as shown in image and accept the other defaults This will avoid us having to set the baffles as internal type and will detect them automatically Click on Sew in Surface Mesh Group and select all objects Enter New Object name as sew and click on Sew button After the sew operation is completed a new object named as sew will appear in the Objects list Select sew object and Draw ANSYS, Inc. December 21, 2012

19 Improve Select Improve... in the Surface Mesh Group Select the sew Object and then select Improve This will improve the surface mesh quality from around 0.95 to around 0.85 Note: Default quality criteria is skewness ANSYS, Inc. December 21, 2012

20 Volume mesh Click on Auto Mesh in the Volume Mesh Group Change the Object to sew in dropdown menu Select Material Points as fluid Uncheck Keep Solid Cell Zones, This will initialize and improve the mesh only in the Fluid zone Click on Mesh Click on the Cleanup button in the Volume Mesh Group ANSYS, Inc. December 21, 2012

21 Cleanup and Export to the Solver Mode To transfer the mesh to the solver, click on the icon on the upper left corner of the Fluent window Click Yes to the pop-up window ANSYS, Inc. December 21, 2012