Step 6: Specify boundary conditions
Next, we step up to the plate to define the displacement constraints and loads. Recall that in ANSYS terminology, the displacement constraints are also "loads". As in the truss tutorial, we'll apply the loads to the geometry rather than the mesh. That way we won't have to reapply the loads on changing the mesh.
Apply Symmetry Boundary Conditions
ANSYS provides the option of applying a "symmetry boundary condition" along lines of symmetry.
Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > Symmetry B.C. > On Lines
Select the straight lines corresponding to the left and bottom edges (which are the lines of symmetry for this problem) by clicking on them. Click OK in the pick menu. The symbol s appears along these lines indicating that the symmetry B.C. is applied along these lines.
Main Menu > Preprocessor > Loads > Define Loads > Apply > Structural > Pressure > On Lines
Select the circular arc and click OK. This brings up the Apply Pressure on Lines menu. Enter p for Value and click OK. A single red arrow denotes the pressure and the direction in which it is acting.
Let's check that the displacement constraints have been applied correctly.
Utility Menu > List > Loads > DOF constraints > On All Lines
Symmetry BCs are applied on lines 8 and 9. Turn on line numbering:
Utility Menu > PlotCtrls > Numbering
Turn on Line numbers and click OK. Are lines L8 and L9 the ones on which you want the symmetry BCs?
Similarly, check that the pressure is applied correctly using Utility Menu > List > Loads > Surface Loads > On All Lines. Note that VALI and VALJ would be different if the applied pressure were linearly varying along the line.
Turn off line numbering: Utility Menu > PlotCtrls > Numbering. Turn off Line numbers and click OK.
Save Your Work
Toolbar > SAVE_DB