Meshing Process for AEC Applications in Simulation CFD
For this module, focus will be placed on two essential automatic meshing tools, mesh size adjustment and refinement regions. A complete understanding of these two meshing options will enable the development of a suitable quality mesh for any AEC application, regardless of size and complexity.
However, there are a number of alternate meshing schemes and advanced options that should be explored once basic meshing skills have been established. Advanced meshing topics, which will not be covered in full detail here, include:
These advanced options have the potential of further improving both the meshing process and the mesh, but typically require some experience to adjust the settings appropriately for each application.
Building the Initial Mesh
Before proceeding, please review the following videos which provide a concise overview of the meshing process:
As depicted in the videos, the development of the mesh starts with clicking on the Autosize button. Autosize evaluates the geometry and then applies a mesh distribution which is previewed with cyan dots known as mesh seeds. The distribution algorithm will place more elements (mesh seeds) where there are finer geometric details and less elements in areas that have no small features.
Mesh seeds are spaced further apart since there are no fine geometric details in this area. Element size is larger (element count is smaller) in this local region.
|2||Mesh seeds are closely spaced on the occupant due to short edges and curved surfaces. Element size is smaller (element count is larger) in this local region.|
TIP: In addition to the mesh seeds, the surface mesh can be quickly viewed using the Preview command, which is documented here.
The Autosize algorithm references the shortest edges in the model to establish a meshing parameter known as the Minimum Refinement Length (MRL), which is detailed in the following references:
For certain AEC models, it may be strategic to modify the MRL to avoid the finer meshing of areas in the CAD model that have undesirable short edges. Consider the occupant in the office space which is depicted above. If the occupant is in the model to just show a sense of scale or to create a marketing image, then a higher level of mesh detail would not necessarily be warranted. By increasing the default MRL value, less elements would be placed around the occupant.
TIP: CAD models of occupants for simulation are kept as simplistic as possible to minimize element count. Facial features, fingers and toes are typically omitted. More information on representing occupants can be found in the Occupants section of Component Characterization module.
NOTE: Increasing the MRL from the default value could result in a failure if the mesher has a difficult time placing elements into areas of fine detail or small gaps.
Volumes which are not expected to play a role in the simulation may optionally be suppressed using the techniques detailed here. This has the benefit of reducing mesh size and solution time since a suppressed volume is not meshed. For example, a table which is not expected to conduct or radiate heat can be suppressed without impacting the results. Even though it is suppressed, the volume representing the table will still obstruct the flow of fluid since it remains as a void in the space.
Reviewing the Mesh
To fully examine the internal mesh quality (not just the seeds or surfaces) and obtain the actual element count, it will be necessary to generate the mesh. The mesher is part of the solver process and can be initiated by either of the following two options:
- Right click on the Mesh Size node in the Design Study Bar and click Generate Mesh, or
- Click on Solve in the Setup ribbon, specify 0 for the Iterations to Run and then click the Solve button.
In both of these cases, the solver generates the mesh and then automatically stops before performing any CFD calculations. The actual mesh statistics (element and node count for fluids and solids) will be printed to the Message Window of the Output Bar and the Status File.
In Results mode, the mesh on surfaces can be shown by changing the Visual Style to Shaded Mesh. Hiding volumes or surfaces will allow components immersed in the fluid domain to be visualized.
|1||Visual Style pulldown menu|
|3||Shaded Mesh style|
|4||Shaded Mesh style (main air domain hidden)|
The most useful results visualization tool for evaluating the mesh is the plane since it can reveal internal mesh details. By adding a plane and setting the appearance to Shaded Mesh, a cross-section of the mesh is revealed. The plane can be reoriented to inspect the mesh at all locations as documented in the video located here Online Help: Using Results Planes.
Refining the Mesh
Once the initial mesh has been generated and reviewed, it will typically need to be refined (i.e., adjusting the mesh settings to add more elements). Although the Autosize option is a powerful meshing feature, it is rarely capable of developing an optimal mesh in only one step. Also, adhering to the best practices for mesh convergence will require at least one refinement iteration to validate the mesh quality.
Two of the essential tools for refining the mesh are:
Adjusting the mesh size is achieved by clicking on Edit in the Automatic Sizing ribbon menu, selecting the volume(s) that are targeted for refinement, moving the Size adjustment slider (or typing in a value) and then clicking the Apply button. This process is repeated as necessary to achieve the desired mesh refinement.
|1||Default Autosize mesh seeds|
|2||Selected volume with refined mesh seeds. Size adjustment slider bar was moved to the left to approximately a factor of 0.25. This equates to about 4 times as many elements in the volume. Notice the more closely spaced mesh seeds.|
When adjusting the size of the volume with this method, the refinement is applied to the entire volume. This technique will be inefficient if the intent is only to refine a small portion of the volume. This will be common in many AEC applications (e.g., warehouses) which have large, relatively empty fluid spaces with details (diffuser inlets) that require localized refinement.
Mesh refinement regions are a convenient method of precisely targeting specific areas that require a finer mesh. Region shapes include boxes, cylinders, or spheres to match a variety of geometric conditions. Regions can be accessed in the Automatic Sizing ribbon or by clicking the Edit button to launch the Mesh Sizes dialog.
|1||Default autosize mesh|
|2||Mesh refinement region dialog and box mesh refinement region positioned in the corner.|
|3||Refined mesh. Note that the outline of the refinement region box can be seen in the mesh.|
|4||Plane cutting through the region to reveal inner details of the mesh refinement region.|
Multiple regions can be defined across the domain, as needed, to complete the necessary refinement.
Mesh size adjustment and mesh refinement regions are flexible and scalable to meet even the most demanding meshing situations.