When beta features are enabled, the Topology Based Meshing workflow is available from the list of meshing workflows. Topology-based meshing is advantageous for handling models that exhibit geometric and topological complexity, providing targeted refinement and precise control over mesh density in critical areas. Additionally, this approach allows for the strategic alignment of mesh elements with essential features, which is particularly beneficial when dealing with complex surfaces.
- 35.5.1. Loading the CAD Geometry
- 35.5.2. Adding Virtual Topology
- 35.5.3. Defining Global Sizing
- 35.5.4. Adding Local Sizing
- 35.5.5. Generating the Initial Surface Mesh
- 35.5.6. Adding Layered Shell Mesh Controls
- 35.5.7. Generating the Layered Shell Mesh
- 35.5.8. Creating Mesh Objects
- 35.5.9. Updating Regions
- 35.5.10. Updating Boundaries
- 35.5.11. Add Boundary Layers
- 35.5.12. Generating the Volume Mesh
Use the Load CAD Geometry task to designate a geometry for your simulation.
Browse for a specific File Name.
Supported file types are SpaceClaim (
.scdoc), Discovery (.dsco), and Workbench (.agdb) files and also.fmdand.pmdbfiles.Other CAD formats are also supported, including
.CATPart,.CATProduct,.asm.prt,.x_t,.sat,.sab,.stp,.step,.iges, and.igs.Note: When a SpaceClaim (
.scdoc) file is imported into Fluent while in meshing mode, Fluent also creates an intermediary.pmdbfile that can be imported. The.pmdbfile should always reside alongside the.scdocfile. When changes are made to the geometry in SpaceClaim, and the file is reimported into Fluent, the original.pmdbfile is overwritten. The.pmdbfile can be more easily and quickly read into Fluent for additional processing and should be used as long as the.scdocfile has not changed.Note: SpaceClaim (
.scdoc) files are only supported on Windows. When working on Linux systems, however, you can use the intermediary.pmdbfile 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
.pmdbfile over to your Linux system to use in your workflow.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
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
.fmdfile to extract and persist CAD information for this task. To generate an appropriate.fmdfile, 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.stlfile 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
.fmdfile 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
.fmdfile 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.).
When the Import Route is set to Workbench, the Use Prime Geometry Kernel option becomes available. If enabled, this option employs the prime geometry kernel for topology-based meshing, which may enhance efficiency compared to the standard geometry engine in Workbench.
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. Facets represent the curved surfaces of the CAD model in the mesh and are used to approximate the geometry during the meshing process.
Specify the resolution of facets as Coarse, Medium, Fine, or Custom. Finer facet resolution means more facets are used, which can better capture the curvature and details of the original CAD model but at the cost of increased computational resources.
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 in curved areas.
The Facet Max Edge Length controls the method for specifying the maximum edge length:
The Relative (Bounding Box) option allows you to specify a Max Edge Length Factor to be applied to the overall bounding box size of the geometry.
The Absolute option allows you to enter an absolute dimension value (Max Edge Length) for the overall geometry bounding box size.
Choosing None will not enforce any maximum facet length.
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.
Proceed to the next step in the workflow.
In the Add Virtual Topology? task you can create a "virtual" topology that effectively merges topological faces by suppressing non-essential edges. Adding a virtual topology prevents nodes from being placed on non-essential model edges, avoiding the creation of unnecessarily refined or poor-quality cells.
For the Add Virtual Topology? prompt, select yes if you need to define a virtual topology using the following steps. Otherwise, if you do not need to define a virtual topology, keep the default of no, click Update and proceed to the next task.
Specify a Name for the virtual topology, or use the default name (
mesh-topology-1).You can select an available zone or label to apply the virtual topology. Choose whether your Selection Type will be the face labels, or the face zones in the list below.
Click Merge to generate the appropriate virtual topology.
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.
Use this task to specify various global mesh sizing features for the imported geometry.
Specify a value for the Minimum Size for the global size control.
Specify a value for the Maximum Size for the global size control.
Specify a value for the Growth Rate for the global size control.
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.
Use the Multi Threaded Size Field Computation option to determine whether or not to use more than one thread when computing the size field. If enabled, you can set the Number of Multi Threads, or use the default value of 1.
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.
Once you are satisfied with your changes, proceed to the next step in the workflow.
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.
Provide a Name for the new size control, or use the default name. The default name changes depending on the assigned Size Control Type.
Provide a Growth Rate.
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 or edges. Edge selection will select 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 or edges. Edge selection selects the edges of a particular face.
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.
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).
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.
Once you are satisfied with your changes, proceed to the next step in the workflow.
Use the Generate Initial Surface Mesh task to create a conformal, connected surface on all of the objects of an imported geometry. 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.
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 with multi-threading.
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 1. This option is not available when projecting onto the geometry.
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.
Proceed to the next step in the workflow.
You can use the Add Layered Shell Mesh Controls task for adding layers of elements along shell mesh regions. This, together with boundary layer mesh, can create an anisotropic mesh. This task can be added to the workflow as many times as you require.
For the Add Shell 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.
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.
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.
last-ratio: allows you to control the aspect ratio of the boundary layer cells (or prism cells) that are extruded from the base boundary zone.
In this case, you can also specify the First Height for the height of the first layer of cells in the boundary layer. In addition, you can specify the Last 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 Last Aspect Ratio allows you to specify the last aspect ratio to be used.
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
Specify the Number of Layers. This value determines the maximum number of boundary layers to be created in the mesh.
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.
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.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.
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 Adjacent Attach Angle option to specify the maximum angle between the layers and an adjacent edge that will permit the layers to be stretched to attach to the adjacent edge. If this angle is exceeded the layers will either terminate or stairstep according to the setting of Stairstep Exposed Sides?.
Set the Stairstep Exposed Sides? option (no by default). When set to yes unattached layers will stairstep to the adjacent edge.
Click Add Shell 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.
Use the Generate Layered Shell Mesh task for generating additional structured mesh layers along the surface of shell mesh regions.
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 Refine Stretched Quads? prompt to specify whether or not you want to refine any stretched quadrilateral cells.
Use the Number of Orthogonal Layers option to specify the number of layers of mesh elements placed orthogonally to the surface of the geometry.
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 Create Mesh Objects task to manage and organize the mesh according to your simulation requirements.
When enabled (default), the Merge face zones based on labels option will consolidate multiple face zones into a single zone based on specified labels.
When enabled (default), the Create a face zone per body option will automatically assign a face zone for each distinct body in the geometry.
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.
(optional) Use the Filter button to filter the table contents based on a particular column.
Assign a Region Name as needed by double-clicking the current name.
You can also rename one or more regions by selecting them in the table, right-click, and select Set Region Name in the context menu, and provide a new name directly in the menu.
Assign a Region Type as needed using the corresponding drop-down menu. Available region types include:
fluid
solid
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.
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.
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.
Once all regions have been updated, proceed to the next step in the workflow.
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.
Choose a Selection Type as either by label or by zone.
(optional) Use the Filter button to filter the table contents based on a particular column.
(optional) Rename any Boundary Name by double-clicking the label in the table and entering a new name.
You can also rename a boundary by selecting it in the table, right-click, and select Set Boundary Name in the context menu, and provide a new name directly in the menu.
(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.
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.
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.
Once all boundaries have been updated, proceed to the next step in the workflow.
You can define boundary layers along various regions using the Add Boundary Layers task. This task can be added to the workflow as many times as you require.
For the Add 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.
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.
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.
last-ratio: allows you to control the aspect ratio of the boundary layer cells (or prism cells) that are extruded from the base boundary zone.
In this case, you can also specify the First Height for the height of the first layer of cells in the boundary layer. In addition, you can specify the Last 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 Last Aspect Ratio allows you to specify the last aspect ratio to be used.
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
Specify the Number of Layers. This value determines the maximum number of boundary layers to be created in the mesh.
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.
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.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.
Click Add 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.
You can generate a computational mesh for your fluid volume(s) using the Generate the Volume Mesh task. In many cases, the default values will be sufficient.
Choose the Solver for which you wish to generate the volume mesh. The default is Fluent, however you can also choose CFX.
Note: When CFX is chosen as the target Solver, the following settings in this task are changed to ensure a compatible volume mesh:
For Volume Fill, you can only choose tetrahedral and hexcore.
When using hexcore, then Avoid 1/8 octree transition is set to yes by default.
Sets the Use default stair-step handling? prompt to No, Exclude both checks, essentially keeping stair-step handling to a minimum.
Choose the type of Fill With that you require. Available options are:
tetrahedral
hexcore
polyhedra
poly-hexcore
Indicate whether to Mesh Fluid Regions or not. This is enabled by default, and can be enabled along with the Mesh Solid Regions option, however, both options cannot be disabled at the same time.
Indicate whether to Mesh Solid Regions or not. This is enabled by default, and can be enabled along with the Mesh Fluid Regions option, however, both options cannot be disabled at the same time.
If the Fill With method is set to tetrahedral or polyhedra, specify the Growth Rate. This value determines the relative length-based size change of cells from the boundary (or the boundary layer cap) towards the interior of the domain.
If the Fill With method is set to hexcore or poly-hexcore, specify the number of Buffer Layers and Peel Layers. The buffer layers are additional layers of cells to alleviate a rapid transition from finer cells to coarser cells. The peel layers are additional layers that control the gap between the hexahedra core and the geometry.
If the Fill With method is set to hexcore or poly-hexcore, specify the Min Cell Length field to determine the minimum length of the volume mesh cell.
Note: Clicking in this field displays red boxes in the graphics window, providing a visual representation of the field value. Use the Clear Preview button to hide the visualization display.
Specify the Max Cell Length field to determine the maximum length of the volume mesh cell.
Note: Clicking in this field displays red boxes in the graphics window, providing a visual representation of the field value. Use the Clear Preview button to hide the visualization display.
If, when generating your surface mesh, you elected to separate zones based on angle, you will see the Merge Back the Separated Boundary Zones? prompt. Here, you can elect to re-merge the zones prior to creating the volume mesh. By default, this option is set to No.
Note: You should not invoke this option if you want to use body labels on multiple bodies to merge cell zones, or if you plan on using the Manage Zones task.
For the Sizing Method, choose how the cell sizing will be evaluated.
Select Global (the default) to assign global sizing controls such as Growth Rate and the Max Cell Length.
Select Region-based Sizing to display a table of available regions where you can assign local sizing controls on a per-region basis.
For imported CAD geometries that include body labels (and if you have set the Use Body Labels field to Yes in the Import Geometry task), body label names are also listed alongside region names in the table (though their names cannot be edited).
When Fill With is set to tetrahedral or polyhedra, you can specify the Max Cell Length and Growth Rate for specific region(s), whereas when Fill With is set to hexcore or poly-hexcore, you can specify the Max Cell Length for specific region(s).
Note: A body's target mesh size in the context of local sizing and a region's maximum cell length in the context of volume meshing are not identical. When performing local sizing, the body's target mesh size sets the size on both the boundaries and the interior of the region and should be used to set small sizes within a region. Performing local sizing impacts the surface mesh, and it therefore is performed prior to surface meshing. Setting the region's maximum cell length size only controls the size on the interior of the body and should be used to control the maximum cell length of a region, and has no impact on the surface mesh.
A recommended approach would be to provide a face size control on a body (rather than a body size control) and, for the target mesh size, provide the same value for the region's maximum cell length, therefore providing the same result as if you were to perform body sizing.
Apply parallel processing of the volume mesh using the Enable Parallel Meshing option (enabled by default). This option is available when the Number of Layers for the boundary layer is greater than 1, and when the number of parallel processors is greater than 1. The option is applicable for any Fill With method, such as polyhedra, poly-hexcore, hexcore, or tetrahedral. Disable this option if you are interested in only generating the volume mesh in serial mode.
Click Advanced Options to access additional controls prior to performing this task. Options include:
Use the Quality Method option to choose from several different types of mesh quality controls (skewness, aspect ratio, change in size, and so on). Choices include Orthogonal (the default for the workflows), Enhanced Orthogonal, and Skewness. The quality method chosen here will also be used in the Improve Volume Mesh task if you later add that task to the workflow, however, you can still choose a different quality method for that task if desired.
Use the Invoke Persistent Renaming option to allow the volume mesh components to use persistent and unique names for the solver. This will make zone names equivalent to region names, and will make cell and face zone names unique. Using this field is highly recommended for any parametric study.
Note: Persistent renaming only works if all body names are unique.
If multiple body labels (named selections) are defined in your imported CAD geometry, you can use the Merge Body Label Bodies field to determine if you would like to merge such bodies or not upon meshing the volume (the default is yes).
Important: Body names between each Body Label should be unique, while inside a Body Label they can be the same.
If set to yes, after volume meshing, the following occurs:
All cell zones within a body label will be merged into a single cell zone and take the name of the body label.
All face zones adjacent to the merged cell zones will also be merged.
Interior face zones between cells will be renamed. For instance, those between "
cell-a" and "cell-b" will be renamed to "cell-a-cell-b".All face labels will always be preserved, and automatic renaming does not change the face labels. Face labels that have been separated are also automatically remerged.
If set to no, you can insert the Manage Zone task and perform the same merging operations by selecting Body Labels as the Type and select all body labels in the list.
Use the Use Size Field? option to determine whether or not to use size fields as part of generating the volume mesh.
Use the Polyhedral Mesh Feature Angle option to set the angle to preserve features when using a polyhedral-based mesh.
Use the Avoid 1/8 Octree Transition? option to determine whether or not you want to avoid any potential 1:8 cell transition in the hexcore region of the volume mesh, replacing any abrupt change in the cell size with polyhedral cells.
Use the Fill Polyhedra in Solids? option to fill only polyhedra cells in all solid regions during volume meshing using the poly-hexcore volume fill method. This option is available when there is at least one solid region and one fluid region. The workflow assumes that the largest volume represents a fluid region such that, when using this option, you achieve a higher quality volume mesh by filling the largest (fluid) region with poly-hexcore cells.
When using the poly-hexcore volume fill method, use the Use Size Field in Solids? option to use size-field-based sizing for polyhedra regions during volume meshing. This setting is available when the Use Size Field? and Fill Polyhedra in Solids? options are enabled and is recommended when BOI(s) are defined that include polyhedra regions. Size-field based sizing is required for BOI(s) to be respected inside all polyhedra regions.
Use the Solid Region Growth Rate field to control the growth rate of all solid regions in the volume mesh. Note that this field is only available for poly-hexcore volume meshes and when the Fill Polyhedra in Solids? option is set to yes. By default, the growth rate is set to a value of 1.5.
Use the Quality Improve Limit option to set the threshold for when mesh quality improvements are automatically invoked that employ the orthogonal quality limit.
Use the Check Self Proximity option to determine whether or not you are going to check for any proximity issues (such as overlapping surfaces, very small gaps between surfaces, very sharp angles, etc.) while generating the volume mesh. If set to yes, problematic areas will be highlighted in the graphics window.
If you have added (or read in) any boundary layers to your workflow, you can write out a boundary layer (prism) control file to save their settings to use later. Use the Write Prism Control File option to specify whether or not you want to save a boundary layer control file that contains your boundary layer specifications. If you select yes, a
.pzmcontrolfile (based on the CAD file name) will be written to your working directory during volume mesh creation. If the file already exists, you will be notified and you can choose to overwrite the file or not.Note: Advanced options (such as acute angles, invalid normals, etc.) are not supported and cannot be saved to the prism control file.
Click Global Boundary Layer Settings to access additional boundary layer controls prior to performing this task. These options are only available when you have defined a boundary layer using the Add Boundary Layer task. Options include:
Use the Merge Boundary Layer Cells Within Regions? to determine whether or not you want to have the boundary layer mesh merged into the bulk mesh.
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 Keep First Boundary Layer Height? option to retain the initial boundary layer's height.
Use the Adjacent Attach Angle option to set the angle for which the boundary layer would imprint on an adjacent boundary.
Use the Use default stair-step handling? option to reduce the stair-stepping at certain locations based on quality or proximity criteria. By default, Yes allows you to retain the default stair-step handling, otherwise you can also choose No, Exclude proximity check, No, Exclude quality check and No, Exclude both checks.
Stairstep Exposed Quads can be used when generating a tetrahedral mesh with prism cells and is set to No by default. Selecting Yes for this option will enable stair-stepping for exposed quadrilateral faces (exposed quads) on prism cells. Stair-stepping these exposed quads can prevent the mesh generation from "hanging" or becoming unresponsive during pyramid creation and can enhance pyramid quality.
Click Generate the Volume Mesh to generate a volume 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.
Use the Draw Mesh button to display the fluid and/or solid meshes.
When you are satisfied with the volume mesh, you can proceed to setting up your CFD simulation in Fluent solver mode.
Note: When using the meshing workflows, after generating the volume mesh, the default quality measure is set to Orthogonal Quality, and will be reported as such when querying the mesh quality.