Skip to end of metadata
Go to start of metadata

Mesh

The following video shows how to create a regular mesh for the rectangle using "Mapped face meshing".

Summary of steps in the above video:

  1. In Workbench, double-click on Model cell A4.
  2. To view the default mesh:
    1. Highlight Mesh in the Project Tree.
    2. Click Update. 
  3. To make a regular mesh:
    1. Right click on Mesh > Insert > Mapped Face Meshing.
    2. Using the Face Selection Tool, click on the rectangular geometry. Click Geometry > Apply.
    3. Click Update. 
  4. To change the element size:
    1. Highlight Mesh in the Project Tree. Right click on Mesh > Insert > Sizing.
    2. Using the Face Selection Tool, click on the rectangular geometry. Click Geometry > Apply.
    3. Next to Element Size, type the following to insert an expression:  = 8/3
    4. Hit Enter. 
  5. Save Project. 

 

For this example, we would like to use "Q4" elements i.e. quadrilateral elements with 4 nodes for every element, one at each corner. It turns out that the quadrilateral elements in the mesh obtained above have mid-side nodes in addition to the corner nodes. So these elements are "Q8" elements with a total of 8 nodes for each element. In the video below, we drop mid-side nodes to get "Q4" elements (in the ANSYS element library, these are referred to as PLANE 182). Note that the mid-side nodes provide higher accuracy, so in the real world, you would not drop mid-side nodes unless you had a compelling reason to do so. Here we do it for learning purposes.

Summary of steps in the above video:

  1. To double check on mid-side nodes:
    1. Zoom in to top left corner of rectangle by holding down the right mouse button and drawing a box over the area to which you want to zoom into.
    2. In the toolbar menu, click on Select Type (Geometry/Mesh) > Select Mesh.
    3. In the toolbar menu, click on Select Mode > Select Box Select.
    4. Draw a box over a few elements in the mesh by holding down the right mouse button.
  2. To get rid of midside nodes:
    1. Highlight Mesh in the Project Tree.
    2. In Details of ‘Mesh’, expand Advanced. Element Midside Nodes > Dropped.
    3. Click Update.
    4. Repeat steps 1a-d to check that midside nodes have been dropped. 
  3. Save Project. 

 

Go to Step 4: Physics Setup

Go to all ANSYS Learning Modules

  • No labels