This section discusses converting structural boundary conditions on the geometry to constraints on the mesh for analyses targeting the Mechanical APDL solver.
In the Mechanical APDL application, structural degree-of-freedom constraints can be defined at individual nodes. Specifically, you can choose to constrain each node along any of the three axis directions (x, y, z) of its local coordinate system to simulate the kinds of supports your model requires. In the Mechanical application, however, you specify boundary conditions on the geometry, so the program must automatically convert them into nodal constraints prior to solution. Ordinarily, this process is straightforward and the boundary conditions can be transcribed directly onto the nodes. In certain cases, however, the Mechanical application may be confronted with combinations of boundary conditions that require negotiation to produce an equivalent rendition of the effective constraints acting on the nodes. A common case occurs in structural analyses where two or more boundary conditions are applied to neighboring topologies, for example, Frictionless Supports applied to neighboring faces that meet at an angle: the nodes on the edge are subject to two separate combinations of DOF constraints, one from each Frictionless Support. The Mechanical application attempts to identify a suitable orientation to the nodal coordinate system that accommodates both frictionless supports and, if successful, constrain its axes accordingly. Should this attempt ever fail, the solution will be prevented and an error will be issued to the Message Window (See The Solver Has Found Conflicting DOF Constraints in the Troubleshooting section.)
Supported Boundary Conditions
The following boundary conditions support conversion:
Fixed Supports (Fixed Face, Fixed Edge, Fixed Vertex).
Simply Supported (Edge or Vertex)
Displacements (Displacements for Faces, Displacement for Edges, Displacements For Vertices)
Note: By default, if you apply a displacement using a cylindrical coordinate system, and if there is a displacement applied in either the radial (X Component) and/or tangential (Y Component) direction, the application applies a zero displacement on the nodes located on the cylindrical axis (Z) for both radial and tangential directions or both components. The application displays an informational message to indicate this situation. You can specify a preference to make sure the application uses the setting for the radial/tangential components by default when it encounters this condition. See the Loads and Boundary Conditions category of the Options dialog.
Calculation Processes
The calculations that convert the boundary conditions into nodal constraints involve:
The identification of the linear span contributed by each of the boundary conditions
The combination of the individual spans into a final nodal constraint choice.
Angular tolerances are involved in distinguishing and combining the spans. A program controlled tolerance of 0.01 degrees will be used.
Note: The calculations have a built in preference for producing nodal coordinate systems that are closest in orientation to the global coordinate system.