CFD-1000: Creating a Hybrid Grid Using the CFD Mesh Panel

In this tutorial, you will learn to:

•	Generate meshes for CFD applications (for example FLUENT, StarCD) using the CFD Tetramesh panel

•	Generate boundary layer type meshes with an arbitrary number of layers and thickness distribution

•	Specify/identify boundary regions for CFD simulations

•	Export a mesh with boundary regions for FLUENT

•	Import the model into FLUENT

The model file used in this exercise can be found in the es.zip file. Copy the file(s) from this directory to your working directory.

1.	From the menu bar, select Preferences > User Profiles or click on the Standard toolbar.

2.	Select Engineering Solutions > CFD > AcuSolve.

Click OK.

4.	Inspect the surface elements that will be used to generate the volume mesh. The boundary mesh can have any combination of tria/quad elements. You will generate boundary layers on all the surface elements contained in the collector named wall.

1.	Click the Open Model icon on the Standard toolbar.

2.	Select the manifold_surf_mesh.hm file.

3.	Click Open to load the file containing the surface mesh.

CFD-1000-01

1.	Click Mesh > Check > Component > Edges to open the Edges panel.

2.	Click comps and select the collectors wall, inlet and outlets.

3.	Click select, and then click find edges. A message indicating that no edges were found will appear on the status bar.

4.	Toggle free edges to T-connections.

5.	Select the three components again and then click find edges. The status bar will display: "No T-connected edges were found."

6.	Click return to close the panel.

1.	Click Mesh > Volume Mesh 3D > CFD Tetramesh to open the CFD Tetramesh panel.

2.	Click the Boundary selection subpanel. You will need to first select all the elements/components that define the surface area on which you need to generate boundary layers. This is done by selecting the elements/components under the With BL (float) and With BL (fixed) selectors.

3.	Under the heading With BL (fixed), click comps and select the collector wall. Next, select the remaining elements/components which define the volume but where a boundary layer is not desired. This is done by selecting the elements/components under the W/o BL (float) and W/o BL (fixed) selectors.

4.	Under the heading W/o BL (float), click comps and select the collectors inlet and outlets.

5.	Verify that the switch below the W/o BL (float) selector is set to Remesh. This means that the meshes in the zones defined by collectors inlet and outlets will be remeshed after being deformed by the boundary layer growth from adjacent surface areas.

6.	Select Smooth BL. This option is strongly recommended for most cases because it produces boundary layers with more uniform thickness and better element quality.

HM_3230_2a

7.	Click the BL parameters subpanel. All the data that has been entered in the Boundary selection subpanel is stored.

8.	Select the options to specify the boundary layer and tetrahedral core:

•	Number of Layers = 5

•	First layer thickness = 0.5

•	BL growth rate= 1.1 (This non-dimensional factor controls the change in layer thickness from one layer to the next).

9.	Under the BL hexa transition mode header, verify that selection is set to Simple Pyramid. The default, Simple Pyramid, uses one pyramid element to transition from a BL hexahedral’s quad face to the tetrahedral core mesh.

10.

Leave the BL only checkbox unchecked. This option generates the boundary layer alone and stops before generating the tetrahedral core. This option modifies adjacent surface meshes to reflect changes introduced by the boundary layer thickness, and creates a collector named ^CFD_trias_for_tetramesh, that is used to generate the inner core tetrahedral mesh using the Tetramesh parameters subpanel.

HM_3230_3a

11.	Click the Tetramesh parameters subpanel.

12.	There are three different tetrameshing algorithms available. Select Optimize Mesh Quality. For a detailed explanation of each option, please refer to the online help.

13.	Set the tetrahedral core growth rate to Interpolate. This avoids the problem of generating tetrahedral elements that are too large at the center of the core mesh.

14.	Click mesh to create the CFD mesh. When this task is finished, two collectors are automatically created: CFD_bl001 and CFD_tetcore001.

cfd_mesh

15.	Click return to close the panel.

You can mask the mesh by using the shortcut key F5, and select elements to be masked. The following is a snapshot. Observe the excellent mesh quality produced.

hm-3230S5

2.	You can also use the Hidden Line panel to view the interior of a solid mesh. Click BCs > Check > Hidden Lines to access the panel.

3.	Leave the title field blank and check the option for yz plane. This defines the yz plane as the cutting plane.

4.	Leave the options for trim planes and clip boundary elements checked on and click show plot.

HM_3230_4b

This automatically places the cutting plane at the center of the model. Notice that the display of the elements has been collapsed so that the nodes lie on the cutting plane.

5.	Left-click in the graphics area where the cutting plane is, hold down the left mouse button, and drag the mouse. Notice that the cutting plane moves.

6.	Next, uncheck the option for clip boundary elements and click show plot.

HM_3230_4c

Notice how the elements are displayed completely.

7.	Drag the placement of the cutting plane. Experiment with the other cutting planes and the trim planes option to see how they affect the plot.

8.	Click return to exit the panel and clear the plot.

In this section, you will define mesh surface regions used to specify boundary conditions in any CFD code (FLUENT, StarCD, CFX, and so on). For example, assume that you are going to export the mesh for FLUENT. For this model, you need to create three collectors to place the boundaries: inflow, outflow, and wall. You have selected two new names that are not already in your database and at the same time are compatible with the prefixes required by FLUENT to recognize boundary types according to their names.

You are going to reuse the surface mesh contained in collector wall because this mesh remained unchanged by the CFD mesh process as this component was specified as “fixed with boundary layer.” However, the surface areas associated with the original collectors inlet and outlets have been completely regenerated and you need to create new components that will be named inflow and outflow, respectively.

1.	Using the Model browser, rename the collector CFD_tetcore001 to fluid. This collector will hold all the 3D volume elements.

2.	Click BCs > Organize to move all the elements from the collector CFD_bl001 to collector fluid.

3.	Click BCs > Faces to automatically generate the collector ^faces containing all the external faces of the elements in collector fluid.

4.	Click BCs > Components > Single to create two new components named inflow and outflow.

HM_3230_5a

Now you are going to move some of the elements from the collector ^faces to the collectors inflow and outflow.

5.	In the Model browser, isolate the ^faces component.

6.	Click BCs > Organize and click one element on the inlet/inflow plane (the element will become highlighted).

7.	Click elems >> by face. All the elements in the collector ^faces on the inlet/inflow plane will be selected.

8.	Set the dest comp as inflow, and click move. Similarly, move the elements from ^faces associated with the outlets to the collector outflow.

9.	Show the inflow and outflow components in the Model browser. When done, you will have all the exterior surfaces colored according to the collectors where they have been placed as shown in the following image.

exterior_surfaces_colored

10.	The remaining elements in the collector ^faces are the same as in wall and you can discard them.

11.	Delete both collectors ^faces and collector CFD_boundary_layer, which is now empty.

1.	Display only the components containing elements that have to be exported for FLUENT, the components are: fluid, inflow, outflow and wall. All other components should not be visible.

export_fluent_only

2.	Click the Export Solver Deck icon to open the Export tab.

3.	Notice that the File Type is set to CFD. Set the Solver Type to Fluent.

4.	In the File field, click the file icon and specify a name and location for the file.

5.	Click Export to export the file.

6.	Select Yes to the first message that appears and No to the second message.

If you have access to FLUENT, you can import manifold.cas to create a new FLUENT simulation case as follows

1.	Start FLUENT 3d or 3ddp.

2.	From the File menu, select Read, then Case.

3.	Select manifold.cas.

4.	Click OK. After importing this file, you will observe that FLUENT has recognized the boundary zones outflow, inflow and wall by name, and the 3D volume zone fluid. Zone interior-* is automatically created by FLUENT containing all the interior faces shared by two 3D cells.

fluent_file

5.	Select Define, then select Boundary Conditions.

6.	Select zone inflow, and set the appropriate boundary condition such as mass-flow-inlet and velocity inlet.

7.	Change the boundary condition type for the remaining surface zones, outflow and wall.

Engineering Solutions allows you to perform the most time consuming tasks of generating the volume mesh and identifying the boundary zones. Now inside FLUENT the rest of the simulation tasks can be executed easily.

The boundary layer type mesh generated in this tutorial was generated with uniform thickness. This is OK for a model like this manifold as long as the total boundary layer thickness does not lead to collision or interference that can occur when the sum of the BL thickness is close to or larger than the distance separating boundary layer walls. When such collision or interference occurs you have the following options:

•	Decrease the global boundary layer thickness (throughout / for all the BL surfaces)

•

Use distributed boundary layer thickness ratios on nodes or collectors/components. This is a capability in HyperMesh that allows you to specify a local value of boundary layer thickness by specifying the ratio of the local value to the global value. For example, if the ratio specified on certain nodes or all the nodes belonging to a collector is equal to 0.1, then the boundary layer thickness generated around those nodes will be only 10 percent of the global boundary layer thickness.

•

The CFD user profile has a tool (Generate BL Thickness) to generate automatically “distributed boundary layer thickness ratios” at each node of the surface mesh so that boundary layer collision is avoided when using the global or nominal boundary layer thickness. The usage of this tool is explained in Tutorial CFD-1100.

In this appendix you are going to use option B to manually change the BL thickness ratio.

Step A: Prepare data to generate a CFD mesh (boundary layer and core mesh) using a distributed boundary layer thickness

1.	Create a new component named wall_thinner_bl, and move elements from wall to this new collector as shown in the following image.

wall_thinner

2.	Click BCs > Check > Edge, then select the collectors wall, wall_thinner_bl, inlet and outlets.

3.	Click find edges. A message indicating that no edges were found will appear on the status bar.

4.	Click Mesh > Volume Mesh 3D > CFD tetramesh to access the CFD Tetramesh panel.

5.	Leave the default Smooth BL option unchanged.

6.	In the BL parameters subpanel, select the options to specify the boundary layer and tetrahedral core:

•	Number of Layers = 5

•	First layer thickness = 0.5

•	BL growth rate= 1.1

7.	Select the type of tetrameshing algorithm: Simple Pyramid, Smooth Pyramid, All Prism or All Tetras

8.	Ensure the BL only checkbox is not checked.

9.	In the Tetramesh parameters subpanel, set the Pyramid transition ratio = 0.8

10.	Select the tetrahedral core growth rate switch to Interpolate. This avoids the problem of generating tetrahedral elements that are too large at the center of the core mesh.

Step B: Define a distributed boundary layer thickness on certain components

1.	In the BL parameters subpanel, ensure that the BL reduction and Pre calc checkboxes are checked and click Manual.

2.	The Distributed BL Thickness Ratio dialog opens. This dialog enables you to specify distributed thickness ratios for groups of nodes or whole components. You can choose either Nodes or Components by selecting the associated radio button.

3.	Select Components.

4.	Click Select Components and select the component wall_thinner_bl.

5.	Specify a thickness ratio of value 0.3 and click Assign.

6.	Notice that the summary message now indicates the number of BL thickness ratio loads on components:

HM_3230_7a

When the models are more complex it is useful to display surface contours of BL thickness ratio values.

7.	Click Contours of BL Thickness Ratio, and the Contour panel will be automatically displayed.

8.	Click contour to inspect the distribution of BL Thickness Ratio on the surface of your domain and click return when you are finished. Click Close to close the dialog.

9.	Go to the CFD Tetramesh panel, Boundary selection subpanel. Here all the elements/components that define the surface area on which you need to generate boundary layers will be selected. This selection is done with the With BL (fixed) selector.

10.	Click comps under With BL (fixed) and select the collectors wall and wall_thinner_bl.

11.	Select all the elements/components that define the surface area on which you do not want to generate boundary layers. This selection is done with the W/o BL (float) selector.

12.	Click comps and select the collectors, inlet and outlets.

13.	The switch below the W/o BL (float) selector is set to Remesh. This means that the meshes in the zones defined by collector’s inlet and outlets will be remeshed after being deformed by the boundary layer growth from adjacent surface areas.

14.	Click mesh to create the CFD mesh. When this task is finished, note the two collectors automatically created: CFD_boundary_layer and CFD_Tetramesh_core.

cfd_two_collectors

15.	Inspect the relative size of the boundary layer thickness by masking some of the elements as shown in the following image. This image shows that the BL thickness on component wall_thinner_bl is only 30 percent of the global BL thickness.

mask_elems_boundary_layer

The manual approach followed previously is useful when you need to reduce the BL thickness throughout a component, or at a clearly identified group of nodes.

When you have a very complicated geometry and BL collision is likely to occur, the best approach is to use the Generate BL Thickness tool to generate automatically “distributed boundary layer thickness ratios” at each node of the surface mesh. This tool performs a collision study and assigns a BL thickness ratio to each node of the surface mesh that requires a reduction of the baseline BL thickness to avoid collision. Usage of this tool is explained in Tutorial CFD-1100.

The previous steps illustrate simple and effective steps to reduce the BL thickness on surface components. This approach is very easy to use and effective when you know how much you want to increase or decrease the BL thickness all over a component. A similar approach is followed to increase/decrease BL thickness on groups of nodes.

CFD-1000: Creating a Hybrid Grid Using the CFD Mesh Panel

CFD-1000: Creating a Hybrid Grid Using the CFD Mesh Panel

CFD-1000: Creating a Hybrid Grid Using the CFD Mesh Panel

See Also: