Using the Thin Mesh Features in Fluent Meshing

Meshing Strategies For Models With Thin Bodies

Thin body meshing is highly advantageous for efficiently simulating thin-walled structures or geometries with significantly smaller thickness compared to their other dimensions. When working with such geometries, conventional volume meshing techniques can lead to a high element count as they attempt to capture the thin dimensions with many unnecessary elements. Thin body meshing solves this problem by refining the mesh specifically along the thin direction, ensuring an accurate resolution of important physical phenomena without the need for excessive mesh density. This approach reduces computational costs while maintaining the fidelity of the simulation. Thin meshing is particularly useful for applications like thermal analysis, structural simulations, and fluid-structure interactions, where thin surfaces or regions have a critical role. Furthermore, thin meshing can be paired with multizone meshing techniques for complex geometries, where structured and efficient mesh generation is required across various regions, resulting in a high-quality mesh with a reduced number of elements.

Here, we will outline the differences between the thin body mesh tools and the multizone mesh tools in Ansys Fluent to help provide an understanding of their individual workflows and the differences between them.

Thin Body Meshing

Thin body meshing is an efficient meshing strategy used for geometries with regions where one dimension (the thickness) is significantly smaller than the others. This technique refines the mesh along the thin dimension, allowing for high-resolution capturing of critical physical phenomena without generating an excessive number of elements in the other directions. Thin meshing reduces the computational cost while preserving the accuracy required to simulate thin-walled structures like shells, plates, or thin-walled containers. This method is particularly useful for thermal analysis, where heat transfer through thin regions is critical, as well as structural and fluid flow simulations, where the material behavior in thin bodies plays an essential role.

Thin meshing is well-suited for models that include thin geometries like stacked plates or thin-walled structures. In these cases, using a traditional volume meshing technique would generate unnecessary elements, resulting in increased computation time without added accuracy. By focusing mesh refinement in the thin regions only, thin meshing achieves the necessary resolution while maintaining efficiency. Additionally, thin body meshing can work with features like side imprints and bias growth rates to further improve the fidelity of the mesh where necessary, ensuring smooth transitions between regions of different thicknesses.

Steps for Using Thin Body Meshing Tools in Fluent Mesh:

1. Create Your CAD Model: For this example, we will be using a simple case. The model will consist of 2 large fluid domains with 1 thin plate in between, which will be treated as a solid body in Fluent. Shared topology is active between each fluid domain and the thin plate. In this model, we have created named selections for: The thin plate, the top shared surface of the thin plate, the bottom shared surface of the thin plate and the inlet/outlet of each fluid domain.
   
   
   
   
2. Import Geometry: Import the CAD model into a watertight meshing workflow.
    
   
   
   
3. Add Local Sizing: Here, we can add any local mesh size controls we wish for our model. In this example, since this is a simple case, we will choose not to add any local mesh controls.
   
   
4. Insert Thin Volume Meshing Controls: Add the thin volume meshing controls before inserting boundary layers in your workflow. To insert the thin mesh controls, you can right click on Generate Surface Mesh --> Insert New Task --> Add Thin Volume Meshing Controls. A new object will appear underneath Generate the Surface Mesh, and you can control the settings there.
   
   
   
   
5. Select Regions or Surfaces: Use the graphical interface to choose specific surfaces or regions where thin meshing should be applied. In the first window, you will need to define which solids will have the thin mesh option applied to them. In our example, "thinplate" represents the named selection we created for the thin plate. Next, we'll need to select a "seed" surface for the thin mesh algorithm to start from. From this seed surface, Fluent mesh will extrude the elements until it reaches it's counterpart, similar to the way the swept mesh algorithm works in Workbench Mesh. Since we have a named selection created for the top and bottom shared surfaces of the plate, we can utilize those. 
   
   Alternatively, if we did not have named selections, we could choose to select a surface from either the list of faces (who's names will be automatically created by Fluent), or from the GUI. If you have several thin plates oriented in the same direction, you can utilize the Select Parallel Zones option to automatically assist with the thin mesh creation for each body.
   
   
   
   
6. Select the Number of Layers: You can choose how many layers of elements you would like to have through the thickness of your plate. For solid bodies, the best practice is to have no fewer than 3 elements through the thickness, especially for applications involving heat transfer. This will help ensure a smooth gradient through your solid. For this example, we will use 3 as shown above.
   
   
7. Define Growth Rate: Specify the growth rate for element size transition. The Growth Rate controls how much each thin volume mesh layer expands during extrusion and is set to 1 by default. A growth rate of 1 keeps all layers the same thickness, while a growth rate of 1.2, for example, increases each subsequent layer's thickness by 20% of the previous layer's length.
   
   
8. Choose the Stair Step Option: Stair stepping refers to the jagged or stepped appearance of mesh elements along curved or sloped surfaces, where the mesh fails to follow the contours smoothly. In Fluent Mesh, the standard option for stair stepping minimizes this effect by creating more gradual transitions between mesh elements, ensuring smoother surface representation. The aggressive option, on the other hand, allows for more pronounced steps in the mesh, prioritizing speed and simplicity over surface accuracy. This is typically used in cases where mesh quality is less critical or where computational resources are limited. See the example below from the Fluent User Guide.
   
   
9. Use Parallel Zones Option: The Use Parallel Zones option in ANSYS Fluent Mesh is a tool that helps streamline the mesh generation process by automatically selecting zones that are aligned with a global plane (such as XY, XZ, or YZ). This option is particularly useful when working with geometries that have multiple regions or surfaces parallel to a specific plane, as it simplifies zone selection by allowing the software to group them together. This reduces manual selection effort, ensuring a more efficient meshing workflow and helping maintain alignment and consistency in the mesh across similar regions.

Multizone Meshing

Multizone meshing is a highly versatile approach used to generate structured, hexahedral-dominant meshes for complex geometries. It automatically decomposes a geometry into multiple zones or regions and sweeps the mesh through the geometry in one or more directions. This method is particularly effective for creating high-quality, structured meshes in geometries that are difficult to mesh with conventional techniques, such as those that involve multiple bodies or require a sweepable mesh along specific axes. Multizone meshing is beneficial for complex industrial geometries, where maintaining a structured, high-quality mesh across the entire domain is crucial for accurate results.

One of the key advantages of multizone meshing is its ability to handle varying body shapes and configurations. The method allows for the generation of different types of mesh elements, such as Hex-Pave, Hex-Map, Prism, or Mixed, depending on the geometry and the desired level of mesh resolution. This flexibility ensures that multizone meshing can be applied across various types of geometries without compromising mesh quality. 

Steps for Multizone Meshing in Fluent Mesh:

1. Create Your CAD Model: For this example, we will be using a simple case similar to the example from the Fluent User Guide (see below). 
   
   
   
   
2. Import Geometry: Import the CAD model into a watertight meshing workflow.
   
   
3. Add Local Sizing: Here, we can add any local mesh size controls we wish for our model. In this example, since this is a simple case, we will choose not to add any local mesh controls.
   
   
4. Generate the Surface Mesh: Here, we will choose to generate the surface mesh with the default mesh settings.

6. Activate Multizone Meshing: Here in the details of the "Describe Geometry" item in the tree is where we will be able to enable Multizone Meshing. In the details box, we will want to choose the settings below.

7. Create Regions: Here is where we determine how many fluid regions we are estimated to have in our model. In this example, we only have one solid body, so we can set the number of estimated Fluid Regions to 0.

8. Update Regions: After determining how many fluid regions you have in your model, here is where we can confirm whether each body is a fluid, solid or dead zone. In this example, we only have one solid region.

9. Add Boundary Layers: If you have fluid regions in your model, you will almost certainly need to add an algorithm to insert boundary layers into your model to adequately capture the flow. This branch on the tree is where we can choose to add an algorithm to insert boundary layers into our fluid domain(s). However, in this example, because we only have a solid body, we do not need to insert any boundary layers. To move past this branch in the tree, we can right click "Add Boundary Layers" and simply mark this branch as updated.

10. Add Multizone Mesh Controls: This branch allows us to select the specific body or bodies to apply multizone mesh controls. Here are the main options available:

• Name: Specify the name of the multizone object for easy identification.

• Mesh Method: Choose the meshing algorithm for the multizone object. The Standard method is the default, breaking the model into sweepable regions whenever possible. For example, in this model, it will detect the two extruded rectangular sections and begin a sweep from each end toward the main base, applying a similar sweeping approach for the base itself. The Thin method is best for parts that, although thin, don't meet the criteria for thin meshing, such as components with surface imprints that prevent a standard sweep.

• Fill With: Decide how elements are distributed within the body to which multizone controls are applied. Options include Hex-Pave, Hex-Map, Prism, and Mixed. Each choice creates a unique mesh structure—see the example below from the Fluent User Guide for more on how these selections impact the final mesh layout.

• Use Max Sweep Size - Determines whether or not a variable (no) or a fixed (yes) sweep size is to be applied to the multizone mesh control.