Customize and Visualize the Mesh

Customize the mesh that you created when you defined the fluid domain, and inspect its quality.

A mesh is an alternative representation of a 1D, 2D, or 3D geometry. The app provides default mesh values based on the dimensions of the fluid domain's geometry. The default mesh's element size aims to balance the desired accuracy of the results against the time it takes to run the simulation. If desired, you can change both the size and type of the elements within the mesh. Typically, a smaller element size yields more accurate results but increases the run time. After you mesh the fluid domain, you can use visualization tools to inspect the quality of your mesh. Based on your inspection, you can change the mesh specifications to update the existing mesh or to create multiple meshes for use with the simulation.

In this example, you first define a coarse mesh for the entire fluid domain. Then, you refine the mesh along the surface of the drone and in a subregion of the fluid domain to improve the accuracy of the results in the immediate space around the drone. By refining only a portion of the mesh, you can simulate reasonably accurate results without significantly increasing the time required to mesh. Finally, you use visualization tools to inspect a cross-section of the mesh at the boundary layer of the drone.

This task shows you how to:

Customize the Mesh

  1. Define a coarse mesh for the entire fluid domain.
    1. From the tree, expand Nodes and Elements, and double-click Hex Mesh.1.
    2. Enter 500mm as the Maximum size, and enter 20mm as the Minimum size.
    3. Enter 30deg as the Minimum angle between faces.
    4. Select Add boundary layers to specify the distribution of elements at the surface of the fluid domain.
    5. Enter 4mm as the First layer thickness, and enter 3 as the Number of layers.
    6. Expand the Options section, and clear all selections.
  2. Refine the mesh along the surface of the drone.
    1. Expand the Local Specifications section, and click Local Mesh Size on Face and Edge .
    2. From the context toolbar, click Select faces by propagation .
    3. Select any surface of the drone.
      A second context toolbar appears.
    4. Enter 180deg in the context toolbar, and click Propagate.
      You have selected the entire surface of the drone for surface mesh refinement. Refining the surface mesh improves the accuracy of your results at the surface. This is especially useful when your model includes curvy geometries like the surfaces of this drone.

    5. In the Local Mesh Size on Geometry dialog box, enter 10mm as the Size, and click OK.
  3. Refine a portion of the overall mesh by creating a Cartesian box around the drone.
    1. From the Local Specifications section, click Local Mesh Size in Cartesian Box .
    2. Enter the following values for the Origin (X,Y,Z) and Size (X,Y,Z) of the Cartesian box:

      X Y Z
      Origin -4000 -3000 -1000
      Size 5000 3000 1800

      These Cartesian values create a smaller box within the bounding box. The smaller box serves to bound the refined section of the mesh. Like the bounding box, it divides the drone into two symmetrical parts.

    3. In the Local Mesh Size in Cartesian Box dialog box, enter 100mm as the Mesh size, and click OK.
  4. Click Mesh to start the meshing process.

    Note: Clicking Mesh starts the meshing process immediately; clicking OK saves the dialog box settings and closes the dialog box without meshing.

    The PLM Update... window appears and displays the meshing progress. This window closes automatically when the app completes the meshing process.

  5. Click OK.
  6. Save your work.

Visualize the Mesh

  1. Hide the bounding box.
    1. From the tree, expand Model > Drone A.1 > Airflow Mesh A.1 > Abstractions > Physical Environment.1.
    2. Right-click Bounding Box.1, and select Hide/Show .


  2. Display a cross-section of the mesh.
    1. From the Display section of the Assistant, click Sectioning .
    2. From the Plane options, select X-axis, Y-axis, or Z-axis to specify the cutting plane.

      The cutting plane is the plane normal to the selected axis.

    3. If desired, click Reverse to display the mesh on the other side of the cutting plane.
    4. Clear Exact mesh cut to show whole elements on the cutting plane.
    5. Move the cutting plane in the direction of the selected axis by dragging the cutting section with your pointer.


  3. Inspect the density of the mesh in critical areas of the model.
    1. From the Display section of the action bar, click Visualization Management .
    2. From the Shape options, select Hide to hide the drone.
      The mesh appears fine at the surface of the drone, and it coarsens outside of the Cartesian box that you defined earlier. You can verify the number of boundary layer elements that you specified when creating the mesh.

    3. From the Shape options, select Show .
  4. Close both the Visualization Management and Sectioning dialog boxes.