...
...
...
...
2D Beam: Mesh
Mesh
The following video shows how to create a regular mesh for the rectangle using "Mapped face meshing".
HTML |
---|
<iframe width="600" height="338" src="//www.youtube.com/embed/9GOxpcILyVM?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of steps in the above video:
- In Workbench, double-click on Model cell A4.
- To view the default mesh:
- Highlight Mesh in the Project Tree.
- Click Update.
- To make a regular mesh:
- Right click on Mesh > Insert > Mapped Face Meshing.
- Using the Face Selection Tool, click on the rectangular geometry. Click Geometry > Apply.
- Click Update.
- To change the element size:
- Highlight Mesh in the Project Tree. Right click on Mesh > Insert > Sizing.
- Using the Face Selection Tool, click on the rectangular geometry. Click Geometry > Apply.
- Next to Element Size, type the following to insert an expression: = 8/3
- Hit Enter.
- 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.
HTML |
---|
<iframe width="600" height="338" src="//www.youtube.com/embed/UxJtAwVM8Lo?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of steps in the above video:
- To double check on mid-side nodes:
- 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.
- In the toolbar menu, click on Select Type (Geometry/Mesh) > Select Mesh.
- In the toolbar menu, click on Select Mode > Select Box Select.
- Draw a box over a few elements in the mesh by holding down the right mouse button.
- To get rid of midside nodes:
- Highlight Mesh in the Project Tree.
- In Details of ‘Mesh’, expand Advanced. Element Midside Nodes > Dropped.
- Click Update.
- Repeat steps 1a-d to check that midside nodes have been dropped.
- Save Project.
Go to Step 4: Continue to Step 4 - Physics Setup
Go to all ANSYS Learning Modules