5.1. 2D Meshing Workflow

The 2D Meshing workflow is available from the list of meshing workflows for perform common meshing operations on 2D geometries.

Note:  When edges are drawn as part of the updating a task within the 2D workflow, they are colored based on their connectivity according to the following rules:

  • Edges adjacent to one face: red

  • Edges having the same face on both sides: cyan

  • Edges having two different faces on both sides: black

  • Edges connected to three faces: magenta

  • Edges connected to four faces: yellow

 

5.1.1. Loading the CAD Geometry

Use the Load CAD Geometry task to designate a geometry or surface mesh for your simulation.

Note:  2D CAD geometries can not be connected/transferred into the 2D meshing workflow from within a SpaceClaim (or Discovery) session.

  1. Browse for a specific File Name.

    Supported file types are SpaceClaim (.scdoc), Discovery (.dsco), and Workbench (.agdb) files and also .fmd and .pmdb files.

    Note:  When a SpaceClaim (.scdoc) file is imported into Fluent while in meshing mode, Fluent also creates an intermediary .pmdb file that can be imported. The .pmdb file should always reside alongside the .scdoc file. When changes are made to the geometry in SpaceClaim, and the file is reimported into Fluent, the original .pmdb file is overwritten. The .pmdb file can be more easily and quickly read into Fluent for additional processing and should be used as long as the .scdoc file has not changed.

    Note:  SpaceClaim (.scdoc) files are only supported on Windows. When working on Linux systems, however, you can use the intermediary .pmdb file as your geometry file for the workflows.

    On Windows, use the Import CAD Geometry dialog to import the CAD file into Fluent, and enable the Save PMDB (Intermediary File) option in the Import Options dialog. After the file is imported, you can move the generated .pmdb file over to your Linux system to use in your workflow.

  2. Choose a suitable option for the Units. You should work in units where the minimum size of the mesh is of the order of one. The mesh will automatically be scaled to meters while transferring the mesh to the Fluent solver

  3. Select an appropriate Import Route option, or keep the default value, depending on your requirements and platform. In most cases, the default value is recommended and should lead to the desired data being imported, however, you should be aware of and verify the CAD configurations being made because they may be considered during import. See CAD Integration for details.

    The workflow uses an .fmd file to extract and persist CAD information for this task. To generate an appropriate .fmd file, the available options for the Import Route depend on the selected CAD File, and your particular platform (Windows or Linux). The various Import Route options include:

    • The Native option loads the CAD file natively into FM, and internally generates an FMD file that is then loaded into the workflow. This option is available for .fmd, .fmdb, and .stl file formats.

      Note:  Using this import route, the CAD data should not differ across Windows and Linux for default settings.

    • The SCDM option uses ANSYS SpaceClaim Direct Modeler to read the CAD file and internally generates an .fmd file that is then loaded into the workflow. You may also want to note any SpaceClaim file options that you may have configured.

      Note:  This route is only available on Windows, and is not available on Linux.

    • The DSCO option, available only when Discovery is installed, allows you to import Discovery (.dsco) files.

    • The Workbench option uses Ansys Workbench CAD readers or plug-ins to attach or load the given CAD file and generates an .fmd file that is then loaded into the workflow.

      Note:  This route is available on Windows and Linux., though not all formats are supported on Linux when compared to Windows. Also, third-party add-on modules can lead to slightly different CAD data upon import (for example, names, assembly hierarchy, etc.).

  4. Use the Refacet check box to enable or disable additional faceting refinement in this task. When enabled, you can change the faceting of the CAD geometry. Only the faceted CAD model is used during the meshing process. In either case, when disabled, normal CAD faceting is performed as defined by the imported CAD file(s).

    • The Deviation controls how far facet edges are away from the model.

    • The Normal Angle also controls how far facet edges are away from the model. Decreasing the normal angle will result in more facets along the curved edges.

    • The Max Size controls the maximum size of the facets after the deviation and the normal angle are respected.

  5. Once all selections have been made, click Load CAD Geometry.

    If you need to make adjustments to any of your settings in this task, click Edit, make your changes and click Update, or click Cancel to cancel your changes.

  6. Proceed to the next step in the workflow.

 

5.1.2. Updating Regions

You can update the properties of any defined region using the Update Regions task. This task can be added to the workflow as many times as you require.

The table contains a list of all of the defined regions, and their assigned types.

  1. (optional) Use the Filter button to filter the table contents based on a particular column.

  2. Assign a Region Type as needed using the corresponding drop-down menu. Available region types include:

    • fluid

    • solid

    • dead

    Multiple regions can be assigned a specific type all at once by selecting them in the table, right-click, and select Set Region Type in the context menu, then designate a type for the selected regions directly in the menu.

  3. Use the Draw Regions button to display the available regions in the graphics window.

    Multiple regions can be visualized all at once by selecting them in the table, right-click, and select Draw Selections in the context menu.

  4. When you are satisfied with the region assignments, click Update Regions.

    If you need to make adjustments to any of your settings in this task, click Revert and Edit, make your changes and click Update, or click Cancel to cancel your changes.

  5. Once all regions have been updated, proceed to the next step in the workflow.

 

5.1.3. Updating Boundaries

You can update the properties of any defined boundary using the Update Boundaries task. This task can be added to the workflow as many times as you require.

  1. Choose a Selection Type as either by label or by zone.

  2. (optional) Use the Filter button to filter the table contents based on a particular column.

  3. (optional) Rename any Boundary Name by double-clicking the label in the table and entering a new name.

  4. (optional) Re-assign any Boundary Type to another value by selecting a type in the table and using the corresponding drop-down menu. Choices include:

    • velocity-inlet

    • pressure-outlet

    • pressure-inlet

    • pressure-far-field

    • mass-flow-inlet

    • mass-flow-outlet

    • outflow

    • symmetry

    • wall

    • internal

    • interface

    • overset

    • outlet-vent

    • intake-fan

    • inlet-vent

    • exhaust-fan

    • fan

    • porous-jump

    • radiator

    • axis

    Multiple boundaries can be assigned a specific type all at once by selecting them in the table, right-click, and select Set Boundary Type in the context menu, then designate a type for the selected boundaries directly in the menu.

  5. When you are satisfied with the boundary assignments, click Update Boundaries.

    If you need to make adjustments to any of your settings in this task, click Revert and Edit, make your changes and click Update, or click Cancel to cancel your changes.

  6. Multiple boundaries can be visualized all at once by selecting them in the table, right-click, and select Draw Selections in the context menu.

    Use the Draw Boundaries button to visualize all boundaries or just wall boundaries.

  7. Once all boundaries have been updated, proceed to the next step in the workflow.

 

5.1.4. Defining Global Sizing

Use this task to specify various global mesh sizing features for the imported geometry.

  1. Specify a value for the Minimum Size for the global size control.

  2. Specify a value for the Maximum Size for the global size control.

  3. Specify a value for the Growth Rate for the global size control.

  4. Choose a Size Function for the new global size control.

    • The Curvature size function can be used for refining the surface mesh based on the underlying curve and surface curvature.

      For this option, you can also specify the Curvature Normal Angle for the curvature size function. The default value of 18 degrees should approximately produce 20 facets in the circumferential direction of a cylinder.

    • The Proximity size function can be used for creating the surface mesh, based on the number of cells per gap specified.

      For this option, you can also specify the Cells Per Gap for the proximity size function. This value is the number of element layers to be generated in a gap for the edge proximity size function. Note that for proximity size functions, the number of cells per gap can be a real value, with a minimum value of 0.01. See Proximity for more information.

    • By default, a Curvature and Proximity size function is assigned based on both curvature and proximity.

      For this option, you can also specify the Curvature Normal Angle for the curvature size function. The default value of 18 degrees should approximately produce 20 facets in the circumferential direction of a cylinder.

      In addition, you can also specify the Cells Per Gap for the proximity size function. This value is the number of element layers to be generated in a gap for the edge proximity size function. Note that for proximity size functions, the number of cells per gap can be a real value, with a minimum value of 0.01. See Proximity for more information.

    Note:  If local sizing has been added, these curvature and proximity size controls are appended to the local sizes and the resulting size field is used to dictate the sizes during surface meshing.

    For additional information, see Size Functions and Scoped Sizing.

  5. Once your selections are made, click Define Global Sizing and proceed onto the next task.

    If you need to make adjustments to any of your settings in this task, click Edit, make your changes and click Update, or click Cancel to cancel your changes.

  6. Once you are satisfied with your changes, proceed to the next step in the workflow.

 

5.1.5. Adding Local Sizing

You can gain better control over the mesh size distribution by using the Add Local Sizing task. Using this task, you can define specific mesh size controls that operate on specific, localized, portions of the geometry and mesh. Using this task, you can add as many localized size controls to the workflow as you need, depending on the requirements and details of your geometry. Note that this task can only be added to the workflow prior to the Generate Initial Surface Mesh task.

For the Would you like to add local sizing? field, select yes if you need to define local sizing parameters using the following steps. Otherwise, if you do not need to define local sizing controls, keep the default of no, click Update and proceed to the next task.

  1. Provide a Name for the new size control, or use the default name. The default name changes depending on the assigned Size Control Type.

  2. Provide a Growth Rate.

  3. Choose the Size Control Type. Choices include:

    • Use the Edge Size setting for refining the local sizing based on the edge size. This option is only available if the imported geometry contains one or more named edges (for example, an ANSYS SpaceClaim Design Modeler CAD geometry with one or more edges explicitly using named selections). For this setting, you can also provide a Target Mesh Size.

    • Use the Face Size setting for refining the local sizing based on the face size. For this setting, you can also provide a Target Mesh Size.

    • Use the Body of Influence setting, or BOI, to assign a maximum size on all parts of your geometry that falls within the boundaries of the body of influence. For this setting, you can also provide a Target Mesh Size.

    • Use the Curvature setting for refining the local sizing based on the underlying curve and surface curvature. This size control type is useful, for instance, in models with a combination of large and small scales. For this option, you have the following additional settings:

      • Specify a value for the Local Min Size for the curvature size control.

      • Specify a value for the Max Size for the curvature size control.

      • Specify a value for the Curvature Normal Angle for the curvature.

      • Specify a value for the Scope to field, where you can localize the size control to faces, edges, faces and edges, or edge labels. Edge selection selects the edges of a particular face.

    • Use the Proximity setting for refining the local sizing based on the number of cells per gap specified. For this option, you have the following additional settings:

      • Specify a value for the Local Min Size for the proximity size control.

      • Specify a value for the Max Size for the proximity size control.

      • Specify a value for the Cells Per Gap. This value is the number of element layers to be generated in a gap for the edge proximity size function. Note that for proximity size functions, the number of cells per gap can be a real value, with a minimum value of 0.01.

      • Specify a value for the Scope to field, where you can localize the size control to faces, edges, faces and edges, or edge labels. Edge selection selects the edges of a particular face.

  4. You can select an available zone or label to apply your local sizing changes. Choose whether to Select By the zone name, or the label name in the list below.

  5. Select the Draw Size Boxes field to visualize the size control's minimum and maximum sizes in the graphics window (in the form of red cubes).

  6. Once your selections are made, click Add Local Sizing and proceed onto the next task.

    You can add as many local sizing controls as you require for your workflow, each operating on different zones and/or with different sizing parameters. The size controls will appear as sub-tasks under the parent task.

    If you need to make adjustments to any of your settings in this task, select the specific size control sub-task, click Revert and Edit, make your changes and click Update, or click Cancel to cancel your changes.

    Note:  If you need to add another local sizing control after you have already created a surface mesh, you need to revert and edit at least one existing local size control in order to properly see and use the available geometry objects in the graphics window and the object listing. Alternatively, you can also re-import your geometry and update the Add Local Sizing task.

  7. Once you are satisfied with your changes, proceed to the next step in the workflow.

 

5.1.6. Adding 2D Boundary Layers

You can define 2D shell boundary layers along various regions using the Add 2D Boundary Layers task. This task can be added to the workflow as many times as you require.

Use this task to create a layered mesh on the surface mesh from certain edges. This, together with boundary layer mesh, can create an anisotropic mesh.

For the Add 2D Boundary Layers? field:

  • Select yes if you need to specify boundary layers using this task.

  • Select no if you do not need to account for boundary layers. Click Update and proceed to the next task.

  1. Specify a Name for the shell boundary layer, or use the default value. Note that the default name is dependent on the value of the Offset Method Type.

  2. Choose an Offset Method Type. The offset method that you choose determines how the mesh cells closest to the boundary are generated. See Offset Distances for more information. Choices include:

    • aspect-ratio: allows you to control the aspect ratio of the boundary layer cells (or prism cells) that are extruded from the base boundary zone. The aspect ratio is defined as the ratio of the prism base length to the prism layer height.

      In this case, you can also specify the First Aspect Ratio. You can control the heights of the inflation layers by defining the aspect ratio of the inflations that are extruded from the inflation base. The aspect ratio is defined as the ratio of the local inflation base size to the inflation layer height. The value for the First Aspect Ratio allows you to specify the first aspect ratio to be used.

    • uniform: allows you to generate every new node (child) to be initially the same distance away from its parent node (that is, the corresponding node on the previous layer, from which the direction vector is pointing).

      In this case, you can also specify the First Height for the height of the first layer of cells in the boundary layer.

    • smooth-transition: allows you to use the local tetrahedral element size to compute each local initial height and total height so that the rate of volume change is smooth. Each triangle that is being inflated will have an initial height that is computed with respect to its area, averaged at the nodes. This means that for a uniform mesh, the initial heights will be roughly the same, while for a varying mesh, the initial heights will vary

  3. Specify the Number of Layers. This value determines the maximum number of boundary layers to be created in the mesh.

  4. Specify the Growth Rate for the boundary layer. This value determines the relative thickness of adjacent inflation layers. As you move away from the face to which the inflation control is applied, each successive layer is approximately one growth rate factor thicker than the previous one. For example, a growth rate of 1.2 will expand each layer of the extrusion by 20 percent of the previous length.

  5. For the Edge Selection Type field, specify whether to select edges by label or zone. Select items in the list, or use the Filter Text option in the drop-down to provide text and/or regular expressions in filtering the list (for example, using *, ?, and []). You can also choose the Use Wildcard option in the drop-down to provide wildcard expressions in filtering the list. When you use either ? or * in your expression, the matching list item(s) are automatically selected in the list. Use ^, |, and & in your expression to indicate boolean operations for NOT, OR, and AND, respectively.

  6. For the Grow on field, specify where you would like to develop the boundary layers.

    • Use the all adjacent faces option to grow the boundary layer along all adjacent surfaces.

    • Use the selected-zones option to select from the Zones list of available named zone(s) in your geometry.

    • Use the selected-labels option to select from the Labels list of available named label(s) in your geometry.

  7. Click Advanced Options to access additional controls prior to performing this task.

    • Use the Gap Factor option to specify the relative gap between two boundary layer caps in a narrow channel. A value of 1 indicates a gap that is of the same order as the boundary layer cap triangle size in the inflation layer.

    • Use the Max Aspect Ratio option to specify the maximum aspect ratio for the boundary layer when proximity compression is applied.

    • Use the Min Aspect Ratio option to specify the minimum aspect ratio for the boundary layer.

    • Use the Local Remesh? prompt to specify whether or not you want to apply remeshing to the adjacent triangles after the shell boundary layer.

    • Use the Remesh Growth Rate field to specify the growth rate for the local remeshing.

    • Use the Refine Stretched Quads? prompt to specify whether or not you want to refine any stretched quadrilateral cells.

    • Use the Max Projection Angle to control the projection of sides on adjacent edges. If the angle is above this threshold, it does not imprint.

    • Use the Max Face Skewness field to specify the target skewness that you want to achieve.

  8. Click Add 2D Boundary Layers to generate the appropriate boundary layers for the imported CAD geometry.

    If you need to make adjustments to any of your settings in this task, click Revert and Edit, make your changes and click Update, or click Cancel to cancel your changes.

 

5.1.7. Generating the Surface Mesh

Use the Generate the Surface Mesh task to create a conformal, connected surface on all of the objects of an imported geometry, or remesh all or parts of an imported surface mesh. Use this task to identify regions that will later be filled with the volume mesh. In many cases, the default values will be sufficient for a useful CFD surface mesh.

  1. Use the Generate Quads? option to determine whether or not to generate quadrilateral cells in the initial surface mesh.

    Note:  After enabling the Generate Quads? option, the Split Quads? option will no longer be available.

  2. Use the Project on Geometry check box to determine whether, after surface meshing, Fluent will project the mesh nodes back onto to the original CAD model. This option is not available when multi-threading.

  3. Use the Enable Multi Threading option to determine whether or not to use more than one thread in generating the initial surface mesh (enabled by default). If enabled, you can set the Number of Multi Threads, or use the default value of 4. This option is not available when projecting onto the geometry.

  4. Click Advanced Options to access additional controls prior to performing this task.

    • Use the Merge edge zones based on labels option to merge all labeled edge zones into a single cell zone after generating the surface mesh.

    • Use the Merge face zones based on labels option to merge all labeled face zones into a single cell zone after generating the surface mesh.

  5. Click Generate Initial Surface Mesh to generate a CFD surface mesh for the imported CAD geometry.

    If you need to make adjustments to any of your settings in this task, click Edit, make your changes and click Update, or click Cancel to cancel your changes.

  6. Proceed to the next step in the workflow.

 

5.1.8. Exporting the Fluent 2D Mesh

Since this 2D meshing workflow exists in the normal (3D) Fluent meshing environment, it is not possible to directly switch to the 2D Fluent solver. Instead, you can create a special 2D mesh file that can only be loaded into the 2D Fluent solver.

When you have completed setting up the 2D meshing workflow details, specify the File Name (or use the default name that is based on the imported CAD file) and click the Write 2D Mesh button to create the 2D mesh file.

Note:  You cannot read this 2D mesh back into the 2D meshing workflow.

From here, you can go on to add more tasks to the workflow, if required, and/or proceed to performing any mesh checking or diagnostics.