Apply Boundary Conditions

First we will create boundary conditions that prevent the left end of the beam from displacing in the global x-direction. Since we are using a half-symmetry model, we must enforce this condition.

1. Select Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Areas.
2. Use the graphics window to select the end surface of the beam and the end surface of the rubber pad and click OK.
3. In the dialog that appears, select UX and enter a displacement of 0 and click OK.

Now we will prevent the entire model from displacing in the global z-direction. This enforces a plane strain condition.

1. Select Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Nodes.
2. Use the graphics window to select all nodes of the model and click OK.
3. In the dialog that appears, select UZ and enter a displacement of 0 and click OK.

Next, we can apply a displacement constraint to simulate the support for the 3-point bending test.

1. Select Preprocessor > Loads > Define Loads > Apply > Structural > Displacement > On Nodes.
2. Use the graphics window to select the nodes shown below and click OK (If you followed all of the steps thus far, the appropriate nodes to select are numbered: 1392, 1393, 18869, and 18870).
3. In the dialog that appears, select UY and enter a displacement of 0 and click OK.

The final boundary condition will tie the rubber pad to the beam.

1. Select Preprocessor > Coupling / Ceqn > Couple DOFs.
2. Select all of the nodes on the bottom of the rubber pad and click OK.
3. Assign a reference number of 1 and select the UY degree-of-freedom label. Click OK.