Chapter 7 Introduction to MultiZone Meshing

1. Chapter 7Introduction toMultiZone Meshing ANSYS MeshingApplication Introduction

2. Overview • Comparing Sweep and MultiZone • Comparing Thin Sweep and MultiZone • Example for Sweep, Thin Sweep, and Multizone Methods • Approach for the MultiZone Method • MultiZone Method Settings • Mapped Mesh Type • Free Mesh Type • Source Selection • Defeaturing • Inflation and MultiZone • Workshop 7.1 MultiZone Meshing for a Block Geometry with Pipes • Workshop 7.2 MultiZone Meshing for a Tank Geometry with Piping

3. Comparing the Sweep and MultiZone Methods Some models can be meshed with either approach • Sweep Method: • Sweeps a single source/face to a single target/face. • Does a good job of handling multiple side faces along sweep • Geometry needs to be decomposed so that each sweep path is represented by 1 body. • MultiZone Method: • Free decomposition approach • Multiple sources to multiple targets

4. Sweep or MultiZone? Use Sweep Method when: You have a multibody part where some bodies should be meshed with Sweep, and some with Patch Conforming Tet If you want to use advanced size function Preview Sweepable bodies shows that all bodies are sweepable Use MultiZone when: You are meshing single body parts that are too complicated for traditional sweep approach. You have multiple sources and targets you need to respect (can’t use VTs to group into a single source/target) You need to inflate off source and side faces

5. Comparing Thin Sweep and MultiZone • Thin Sweep Method: • Sweeps multiple sources to • paired multiple targets • Good substitute for midsurfacing shell models to get a pure hex mesh • MultiZone Method: • Free decomposition approach • Multiple sources to multiple targets Some models can be meshed with either approach

6. Thin Sweep or MultiZone? Use Thin Sweep Method when: You have a “thin” solid part where the source and target faces don’t exactly match, and you don’t care about the features on the target side. Use MultiZone When: You have a “thin” solid part where the source and target faces don’t exactly match, and you care about the features on both sides.

7. Different Sweep Methods Example • Thin Sweep Method: Sweep Method: • MultiZone Method: ForExample

8. Sweep Method Treatment Use VTs to merge multiple targets into 1 target Use VTs to merge multiple sources into 1 source Multiple sources ignored Multiple targets ignored

9. Thin Solid Sweep Treatment Multiple target Multiple source Multiple sources captured Multiple targets ignored

10. MultiZone Method Sweep treatment Multiple target Multiple source Multiple sources captured Multiple targets captured Note, MultiZone will ignore the internal cutouts unless they are in a Named Selection

11. Multizone Method Approach • Multizone features automatic geometry decomposition which avoids the need to slice a body up into sweepable bodies to get a hex mesh with the sweep method • For example, the geometry shown at right would need to be sliced into three bodies to get a hex mesh with sweep. With the Multizone method, a hex mesh could be generated directly • Based on ICEM CFD Hexa blocking • O-grids can be extruded to createinflation • Unstructured regions can be filled with hex-dominant, hex-core, or tetrahedral mesh

12. Multizone Method Settings • Multizone will not utilize the Advanced Size Function (Patch Conforming Tet andSweep Methods only) • Source selection is not mandatory, but may be helpful • Can exclude or allow free mesh blocks

13. Multizone Method Settings • Mapped Mesh Type • Hexa • Hexa/Prism • Free Mesh Type • Not Allowed • Tetra • Hexa Dominant • Hexa Core • Source/Target Selection • Automatic • Manual Source • Advanced • Defeaturing Tolerance • Minimum Edge length

14. Multizone Method and Inflation • Algorithm different from other inflation methods (extruded o-grid) • Scoped to bodies, defined for faces • Only First Layer or Total Thickness options

15. Workshop 7.1 Multizone Meshing for aBlock Geometry with Pipes

16. Goals This tutorial will illustrate basic use of the Multizone method to create a Hex mesh for a simple geometry with the addition of an inflation layer. Source selection for the multizone sweep will be doneautomatically by the mesher when the mesh is generated.

17. Importing Geometry Copy the blockandpipes.agdb file from the Tutorial Files folder to your working directory Start Workbench and double-click the Mesh entry in the Component Systems panel Right-click on Geometry in the Mesh entry in the Project Schematic and select Import Geometry/Browse Browse to the block and pipes.agdb file you copied and click Open. Note that the Geometry entry in the Project Schematic now has a green check mark.

18. Insert Multizone Method • Double click the Mesh entry in the Mesh object on the Project Schematic to open ANSYS Meshing • Close the Meshing Options Panel at the right without setting anything. • Right-click on Mesh and insert a Method. Select the body and set the method to Multizone. Leavethe settings as the defaults as shown

19. Mesh Sizing and Metric Click on Mesh in the Outline Change the Physics Preference to CFD and the Solver Preference to Fluent Expand the Sizing Entry and turn off the Advanced Size Function (it will not be used for Multizone anyway) Set the Element Size to 0.20 [in]. (Note: if the units are set to some other system, click on Units in the Menu Bar and change to U.S. Customary (in, lbm, …) Expand the Statistics entry and set the Mesh Metric to Skewness

20. Mesh and Mesh Quality • Generate the Mesh. Note the Mesh count and Skewness metric

21. Inflating the Multizone Method • Insert Inflation for the Multizone Method. Pick the outer cylindrical faces of the pipes and the 4 side faces of the block as the Boundary. Set the Inflation Option to Total Thickness with a value of 0.20 [in]. • Generate the mesh.

22. Workshop 7.2 Multizone Meshing for aTank Geometry with Piping

23. Goals This tutorial will show how to use the Meshing Application in ANSYS 12 to generate a mesh suitable for a CFD simulation of a chemical process flow. The geometry, consists of three bodies representing a tank together with a single inlet and outlet pipe. The goal is to produce an Hex mesh throughout the domain without any further decomposition of the geometry using the Multizone Method.

24. Creating a Standalone Meshing System Launch ANSYS 12.0 Workbench from the START menu Open the Component Systems section of the Toolbox on the LHS of the WB GUI. Double click the Mesh option

25. Importing the Geometry Right click on the Geometry button in the RHS of the WB panel and select Import geometry (the question mark on the button turns to a tick once a geometry file is imported) Import the 2-pipe-tank.agdb file Double click on the Mesh button to launch the Meshing Application

26. Geomety The original geometry was modified in DesignModeler The tank was split into three bodies and some simplification was made to remove small faces that are not important to the analysis One multi-body “Part” was created and a given the name “Fluid” and the material type “Fluid” Individual bodies were re-named

27. In the Meshing Options panel to the RHS of the main window select the following meshing options: Physics Preference CFD Mesh Method Automatic Click OK after youmade the selections In Units, make sure it is set to Metric, mm Meshing Options

28. Named Selections Named Selections are used to assign Fluent name and zone types Set the Cursor Mode to Face selection Select the inlet face RMB select Create Named Selection Assign the name Inlet Repeat for Outlet A naming convention hasbeen established to automatically assign zone types in Fluent For example - “Inlet” Velocity-inlet zone “Outlet” Pressure-outlet zone See Fluent Mesh export section of the manual for all options.

29. Global Mesh Settings Set Global Size and Quality control Click on Mesh in the Model Tree to open up the Details of “Mesh” panel Sizing Turn Off Use Advanced Size Function Multizone does not use this option Change the Relevance Center Fine Recommended for most CFD applications that apply the Multizone Method Statistics Assign Mesh Metric Option Skewness Maintain all other defaults

30. Inserting a Multizone Method Insert Mutizone Meshing control Set the Cursor Mode to Body selection RMB (in Window) – Select All the bodies RMB (in Tree) – Insert – Method Select Multizone

31. Setting Multizone Sources Select Mutizone Source faces Change Src/Trg Selection – Manual Source To ensure the middle section can be swept Set the Cursor Mode to Face Pick the five green source faces(see top image) Rotate the model to look at therear of the tank Pick the additional fivered source faces(see bottom image) Apply

32. Generating the Initial Mesh Create an initial Mesh of the model RMB (in Tree) – Generate Mesh The mesh is successfully created – but refinement is clearly needed The mesh at the inlet and outlet pipes and close to the pipe/tank intersection is insufficient to capture the physics correctly This can be achieved by inserting some additional meshing instructions such as Inflation, Sizing and Biased Sizing to improve the pipe/tank meshing

33. Face Sizing Add Face Sizing for the pipes to control the size of elements Start by removing the mesh RMB (in Tree) – Clean and confirm Make sure you’re using Face Selection and pick the four faces shown in Green RMB (in Tree) – Insert – Sizing Set Sizing Details:Set Element Size 1 mm

34. Adding Inflation Add Inflation (boundary layers) Set the Cursor Modeto Body Selection Select the centralgreen body RMB (in Tree) – Insert – Inflation Set Inflation Details Switch to Face selection Select the four green cylindrical faces and Apply Set Inflation Control Number of Layers 2 Maximum thickness 1 mm

35. Edge Sizing Add Edge Sizing Change Cursor Modeto Edge Selection Select two green edges on one side Rotate the model Repeat the selection RMB (in Tree) – Insert – Sizing Set Sizing Details Element Size 1mm Behaviour Hard Bias type _ __ ___ __ _ Bias Factor 6

36. Generating the Final Mesh Generate the mesh RMB (in Tree) – Generate Mesh Statistics Elements ~45,000 Max Skewness Below 0.8 Overall a good Quality mesh

37. Examining the Mesh Examine the Mesh Sizing – 4 elements on face Inflation – on the pipe walls Sizing – element size 1mm across pipe and biasing to increase density at transition

38. Saving the Project The mesh is now complete RMB (Tree) select Update Select File > Close Mesh to close the Mesh application In the WB panel select File > Save Project As… and give the project a name Exit from ANSYS Workbench by selecting File > Exit Further Work Change the mesh settings for each of the additional parameters How do each of these parameters influence the mesh?