A boundary condition can be applied to nodes, edges or surfaces of a model.
What Does a Boundary Condition Do?
- A boundary condition holds a node and prevents it from translating and/or rotating. It acts like a rigid support between the model and the ground.
- An edge or surface boundary condition applies nodal boundary conditions to each node on the edge or surface.
- When the model is being analyzed, an equation is generated for each degree of freedom of each node. If a boundary condition is applied to a node no equation is generated for that node because it experiences no translation or rotation.
- To model a cantilever beam, constrain both the translation and rotation at the fixed end.
- To model a simply supported beam (using beam elements), constrain the three translations and axial rotation at one end and constrain the two transverse translations at the opposite end. (If the beam were parallel to the X axis, the constraints are TxTyTzRx at one end and TyTz at the other. The Rx constraint is necessary to provide torsional stability. Freeing Tx at one end is optional for a linear static analysis, since this analysis type does not account for large displacement effects. So, the two supports do not move closer together regardless of the amount of deflection.)
- Each element type supports certain degrees of freedom (DOF). If you apply a boundary condition to a DOF on an element that does not support that particular DOF, the boundary condition is ignored. For example, truss elements cannot resist rotation because they have no rotational DOF. They behave as if both ends are ball-joint connections. If you place a fixed boundary condition on an end of a truss element, the three rotational constraints are ignored. Similarly, brick and tetrahedral elements have only translational DOF. Rotational constraints are ignored for these solid elements too.
Apply Boundary Conditions
If you have nodes, edges or surfaces selected, you can right-click in the display area and select the Add pull-out menu. Select the Nodal Boundary Condition, Edge Boundary Condition or Surface Boundary Condition command. This command can also be accessed via the ribbon (Setup 
Constraints General Constraints). Edge boundary conditions can only be applied to parts that originated from CAD solid models or the 2D Mesh Generation.
Either press one of the buttons in the Predefined section or activate the appropriate check boxes in the Constrained DOFs section. The Fixed button activates all six check boxes. The Free button deactivates all six check boxes. The No Translation button activates the Tx, Ty, and Tz check boxes. The No Rotation button activates the Rx, Ry, and Rz check boxes.
The remaining six buttons apply symmetric or antisymmetric boundary conditions. See the Model Symmetry page for more information.