In this 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.
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, . When Mechanical opens, make sure that the units are properly defined to be in metric. Do this by clicking on Units, in the top toolbar, and selecting Metric (m, kg, N, s, V, A).
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 |
https://confluence.cornell.edu/download/attachments/146918513/DMFM_Full.png |
https://confluence.cornell.edu/download/attachments/146918513/GenMesh_Full.png |
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 |
https://confluence.cornell.edu/download/attachments/146918513/DetSizing_Full.png |
https://confluence.cornell.edu/download/attachments/146918513/detdet_full.png |
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 the project. Do not close Mechanical yet.
Go to Step 4: Physics Setup
Go to all ANSYS Learning Modules