Author: John Singleton, Cornell University

Problem Specification
1. Pre-Analysis & Start-Up
2. Geometry
3. Mesh
4. Setup (Physics)
5. Solution
6. Results
7. Verification and Validation
Exercises
Comments

3. Mesh

In the step, we'll discretize or chop up the domain to create a mesh containing many "elements". During the numerical solution, ANSYS will obtain a discrete version of our boundary value problem on this mesh. We will generate a regular face mesh with 200 elements. The horizontal edges will have 10 divisions and the vertical edges will have 20 divisions.

Launch ANSYS Mechanical

ANSYS Mechanical is the application where we'll generate a mesh, apply the material properties and boundary conditions, and obtain a numerical solution to our boundary value problem. In order to start ANSYS Mechanical (Double Click) Model, .

Create a Regular Mesh

We will create a nice, regular mesh which is done using the "mapped face meshing" option. A mapped face mesh is a mesh that can be mapped to a rectangular domain, hence the name. Our domain is already rectangular, thus mapped faced meshing will yield a rectangular grid as the mesh.

First (Click) Mesh, in the model tree. Next, (Click) Mesh Control > Mapped Face Meshing, as shown below. 


https://confluence.cornell.edu/download/attachments/146918513/MFM_Full.png


Then, click on the rectangle and it should be highlighted in green. If it does not highlight in green, click on the face selection filter button, at the top of the GUI,then click on the rectangle. Once the rectangle has been selected, (Click) Apply in the "Details of Mapped Face Meshing" table as shown below. 


https://confluence.cornell.edu/download/attachments/146918513/DMFM_Full.png


ANSYS now knows that a mapped face mesh has to be generated for the rectangle. Next, (Click) Update, , in order to generate the mesh. You should obtain the following mesh. 


https://confluence.cornell.edu/download/attachments/146918513/GenMesh_Full.png


Edge Sizing

Let's specify the number of divisions to be used along each edge rather than have ANSYS pick them automatically. ANSYS calls this step "edge sizing". We will use 20 divisions along the vertical edges and 10 divisions along the horizontal edges. We will work with the horizontal edge first. In order to implement the edge sizing, first (Click) Mesh, . Next, (Click) Mesh Control > Sizing, as shown below. 


https://confluence.cornell.edu/download/attachments/146918513/InsSizing_Full.png


Next, click on the edge selection filter, , located at the top of the GUI. Then click on the bottom edge of the rectangle, ctrl-click on the top of the rectangle (to select both of them), and (Click) Apply in the "Details of Sizing" table as shown below. 


https://confluence.cornell.edu/download/attachments/146918513/DetSizing_Full.png


Next, set Type to Number of Divisions and set Number of Divisions to 10, as shown below. 


https://confluence.cornell.edu/download/attachments/146918513/detdet_full.png

You will notice that under Number of Divisions there is a row labeled Behavior which is defaulted to Soft.  Change this option to Hard.  Soft Behavior means that the mesher will take your sizing just as a guideline, not an absolute law.  For our simple geometry, we know exactly what the mesh should look like, and don't want the mesher taking any creative interpretations of our sizing options.

 
This completes the sizing for the horizontal edge. Now, create a new edge sizing, apply it to the right and left vertical edges  (ctrl-click to keep both of them selected.) And set the Number of Divisions to 20. After, you have properly implemented the two edge sizing commands, (Click) Update, , in order to generate the new mesh. You should then obtain the following mesh. Important note: If ANSYS modifies the number of divisions you give it, change the setting for Behavior in the above menu from Soft to Hard.


This completes the meshing process for this problem.

Save

Save the project. Do not close Mechanical yet.


Go to Step 4: Setup (Physics)

See and rate the complete Learning Module

Go to all ANSYS Learning Modules