CFD-1200: CFD Meshing with Automatic BL Thickness Reduction

In this tutorial, you will learn to:

•	Generate meshes for most CFD codes, for example, Acusolve, CFD++, CFX, FLUENT, StarCD and SC/Tetra, using the CFD Tetramesh panel.

•

Generate boundary layer type meshes with arbitrary number of layers and thickness distribution in domains defined by surfaces that are very close to one another in some areas. More specifically, in some areas the clearance or separation of bounding surfaces is not enough to accommodate the user specified nominal boundary layer thickness.

•	Generate a distributed thickness “loading” that prevents boundary layer interference/collision in zones where the distance between opposing walls is too small to accommodate the baseline or nominal boundary layer thickness.

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.

1.	On the Standard toolbar, click the Open Model icon.

2.	Select the manifold_inner_cylinder.hm file.

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

tut_man_inn_cyl

Inspect the surface elements that will be used to generate the volume mesh. You would like to generate boundary layers on all the surface elements contained in components wall and wall_cyl. However, there is an area close to the end of wall_cyl where the clearance between wall and wall_cyl is very small. This can be easily observed in this case by changing the visibility of component wall, as shown in the following image.

tut_change_visability

In more complex models it is not possible to visually identify all the zones where there is not enough space to growth the “baseline” or nominal boundary layer as specified in terms of the number of layers, first layer thickness and growth rate. This is not a problem because the automatic distributed thickness “loading” computation takes into account all possible interference cases. This is demonstrated in this tutorial.

1.	Click Mesh > Check > Components > Edges.

2.	Click comps and select all collectors that define the domain’s surface, namely inlet, outlets, wall and wall_cyl.

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

4.	Toggle the free edges switch to T-connections.

5.	Select the components again and click find edges. The status bar will display, “No T-connected edges were found.”

1.	Click Mesh > Volume Mesh 3D > CFD Tetramesh.

2.	Click the Boundary selection subpanel.

HM_3250_04a

3.	Under the heading With BL (fixed), click comps and select the collectors wall and wall_cyl.

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

5.	Ensure that the switch below the W/o BL (float) selector is set to Remesh. This means that the surface meshes associated with those components will be remeshed or rebuilt after shrinking due to boundary layer growth from adjacent boundary layer components.

6.	Select Smooth BL.

7.	Click the BL parameters subpanel.

HM_3250_04b

8.	Set the following fields:

•	Number of Layers = 5

•	First layer thickness = 0.5

•	BL growth rate = 1.2 (This non-dimensional factor controls the change in layer thickness from one layer to the next).

•

BL hexa transition mode = All Prisms (Prism to all Layers). This means that if there are any quad elements in the surface mesh, those will be split into two trias each so that there is no need to transition from quad faces to tria faces when transitioning from the last boundary layer to the tetrahedral core. This option is very important when there are quad elements on areas with (low) distributed BL thickness ratio, because in such areas the thickness of the transition elements (for example, simple pyramid) was not taken into account when doing the interference study to assign distributed BL thickness ratio to those elements.

9.	Check the box for Pre calc and then click Auto. The Generate Boundary Layer distributed thickness values dialog opens. Notice that the four components selected in the Boundary selection subpanel are already added.

10.	Set the correct Bound Type for each one of the selected components. You want to generate a boundary layer from components wall and wall_cyl, therefore, you will leave wall as their Bound Type. Also verify that the Bound Type of components inlet and outlets is set to in/outlet as shown, following:

HM_3250_06

A component with Bound Type: wall indicates that you are going to generate a boundary layer mesh on the component later on when you generate the mesh. Therefore, the same component should be consistently specified with the comps selector for the With BL (fixed or float) in the Boundary selection subpanel.

A component with a Bound Type: slip, symmetry, in/outlet, or farfield indicates that you are NOT going to generate a boundary layer mesh on the component. Therefore, when you generate the mesh this component should be consistently specified with the comps selector for the W/o BL (fixed or float) in the Boundary selection subpanel.

11. Specify the Boundary Layer options as shown in the following image.

•	The first three fields are set in the BL parameters subpanel and cannot be changed here. All layers will have the same thickness except in area affected by the distributed thickness "loading" and also mesh smoothing operations such as hyperbolic smoothing at corners.

•

Specify a Minimum (Tetrahedral-Core / Boundary-Layer) thickness ratio value of 2.0. This means that in areas where there is not enough room to grow the nominal BL (5 layers starting with a thickness of 0.5 and increasing with a grow rate of 1.2), the boundary layers’ thickness will be reduced so that the tetrahedral core thickness is approximately at least 2.0 times the total boundary layer thickness, except for mesh smoothing operations such as hyperbolic smoothing at corners and convex/concave areas.

•

The last option, Bound Layer thickness at corners, is a coefficient that controls the hyperbolic growth where walls make an angle. The smaller this value is, the thinner the total BL thickness is in such areas; values less than 1 produce thinner layers and values greater than 1 produce thicker layers.

HM_3250_07

Now you are ready to generate the Distributed BL Thickness loading. Make sure that none of the elements specified in the boundary collectors are masked. If they are masked an error message will indicate that there is a discrepancy between the total number of elements in the components that you specified and the number of tria3/quad4 elements found (displayed). If you have masked elements, you can use mask (F5), and press unmask all.

12. Click Generate Distributed BL Thickness Ratio. If the model already contains boundary layer thickness ratios, then a pop-up message box will ask you if you want to keep such loads or if you want to clear/discard them. Most of the time you will want to clear the existing boundary layer thickness ratios; click Yes. In some special cases you may want to keep them, if more than one loading value is specified for a node, the minimum value is used when generating the mesh.

HM_3250_08

13. After a few seconds you will see a pop-up message indicating the number of distributed boundary layer thickness values included in collector ^CFD_BL_Thickness.

14. Click Close in the Generate Boundary Layer distributed thickness values dialog.

1.	In the CFD Tetramesh panel, click the Tetramesh parameters subpanel.

HM_3250_09

2.	Set the switch for the tetrahedral mesh generation algorithm to Optimize Mesh Quality.

3.	Ensure that the tetrahedral grow rate is switched to Interpolate.

4.	Click mesh to generate the mesh. If collectors CFD_bl001 and CFD_tetcore001 are present, you will be asked if you want to delete the elements in those collectors. Almost always you select Yes. When this task is finished two collectors are created: CFD_bl001 and CFD_tetcore001.

1.	Select the XZ Left Plane View icon .

2.	Access the Mask panel by using the shortcut key F5.

3.	Select elements to be masked by pressing SHIFT and the left mouse button, then move the cursor so that the rubber band covers the upper half of the model.

4.	Click mask.

5.	Click the XY Top Plane View icon .

6.	Zoom in into the area where the bounding surfaces come close together. The following image illustrates how BL interference has been avoided by reducing the BL thickness.

7.	Click return to close the Mask panel.

tut_reduce_blt_1.zoom74 tut_reduce_blt_2.zoom80

First you need to put in the same component all the elements that represent a single fluid and/or solid domain. In this case you have a single fluid domain, therefore you proceed as follows:

1.	Rename the CFD_Tetramesh_core component. Typically, select a name “fluid*,” for example, fluid. In the Model browser, select CFD_tetcore001, right-click, select Rename, and then type the new name, fluid.

2.	Click BCs > Organize.

3.	Click elems >> by collector and select the collector CFD_bl001.

4.	In the dest component field, select fluid.

Click move and then click return. Now you have all the volume elements in component fluid. The surface mesh of this component is typically different from the surface mesh that was used to define the boundary of the domain. For this reason, and to have consistent surface zones to impose boundary conditions in most CFD solvers, you are going to create new boundary components that will be used when exporting the mesh for the CFD solver of your choice. To accomplish this you first extract the surface mesh of component fluid. You do this by generating the surface elements.

6.	Click BCs > Faces.

7.	Select the component fluid, and click find faces. All boundary faces are placed in the component ^faces.

8.	Create new, empty components to place the elements from ^faces so that when these components are later exported, they can be used to set a boundary condition in your CFD solver. In the Model browser, right-click Component, and then select Create. The Entity Editor opens.

9.	For Name enter wall_exterior. Leave the Type as None.

HM_3250_10

10.	Create three more empty components with the names wall_cylinder, inlet_annulus and outlets3.

11.

Move the elements from component ^faces into the newly created components. This is done for clarity; however, most of the time you create one fewer component and you rename ^faces which retains the remaining elements after you move elements to the newly created surface components. Organize the components by using the Organize panel. Select BCs > Organize.

12.	Set dest component to wall_exterior, then pick one element on the exterior wall surface in the ^faces component.

13.

Click the elems switch and select by face. This will recursively select all the elements attached to the picked element as long as the adjacent elements are within a break angle less or equal to the value specified in the feature angle field (Preferences > Geometry Options > Mesh subpanel). The surface mesh in ^faces is such that the zones that you want to organize/move make an angle close to 90 degrees and their boundaries, therefore this is a very easy job to do with a default feature angle of 20 or 30 degrees.

HM_3250_11

14. Having selected all the elements that should go to component wall_exterior, click move.

15. Now set the dest component to outlets3 and pick at least one element on each one of the three separate outlets as shown in the following image.

HM_3250_12

16.	Click the elems switch and select by face.

17.	Having the elements on the three outlets selected, press move and those elements are moved to component outlets3. Set dest component to inlet_annulus and pick one element, as shown in the following image.

HM_3250_13

18. Right-click the elems switch and select by face.

19. Having all the elements on the inlet annulus selected, press move and those elements are moved to component inlet_annulus. Now that all the remaining elements in component ^faces are the elements that you want to move to component wall_cylinder.

20.	Set dest component to wall_cylinder.

21.	Click elems and in the panel area and select by collector.

22.	Select the component ^faces.

23.	Click move and then click return. The elements are moved to component wall_cylinder as shown in the following image.

HM_3250_14

As mentioned previously, more often than not it is easier to rename/recolor component ^faces.

1.	Verify that only the components that you want to export are displayed. All other components should NOT be displayed, as illustrated in the following image of the Model browser.

tut_faces_only_export

2.	Click the Export Solver Deck icon to open the Export tab. Select the CFD file format of your choice (such as Acusolve, CFD++, CFX, CGNS, FLUENT, or StarCD) to export the grid or mesh.

Note:

Solvers like Acusolve and FLUENT have certain requirements when the domain contains different fluids and/or solids. This is described in other sections of the Engineering Solutions Help system.

Engineering Solutions allowed you to generate high-quality boundary layer meshes on parts where the clearance or separation of the bounding surfaces is not enough to accommodate the user specified nominal boundary layer thickness. To accomplish this you first used the CFD utility Generate Distributed BL Thickness Ratio to generate load collector ^CFD_BL_Thickness. This load collector is then used when you enable distributed thickness. As shown in the cross-sectional images, the mesh is very smooth, free of collisions, and is of excellent quality.