Release 11.0 Documentation for ANSYS
www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS
Rigid target surfaces are defined in their original configuration, and the motion of the entire surface is then defined by the imposed displacements on the pilot node (or the different nodes of the target surface if no pilot node was defined).
You must use a pilot node in any of the following situations to control the boundary conditions (and motion) of the entire target surface:
The target surface is subjected to applied forces.
The target surface is subjected to rotations.
The target surface is connected to other elements (e.g., structural mass element MASS21).
The motion of the target surface is adjusted by the equilibrium condition.
The degrees of freedom of the pilot node represent the motion of the entire rigid surface, including two translational and one rotational degree of freedom in 2-D, and three translational and three rotational degrees of freedom in 3-D. You can apply boundary conditions (displacement, initial velocity), concentrated loads, rotations, etc. to the pilot node. To account for a rigid body's mass, define a mass element (MASS21) on the pilot node. You can also define a follower element (FOLLW201) on the pilot node; the element-specified external forces and moments will follow the motion of the pilot node.
Keep in mind the following restrictions on the target surface when using a pilot node:
Each target surface can have only one pilot node.
ANSYS ignores all boundary conditions on all nodes other than the pilot node.
Only the pilot node can connect to other elements. If you need to attach the rigid surface to another element, you must use the pilot node to do so.
You cannot use constraint equations (CE) or node coupling (CP) to control the degree of freedom of the target surface when a pilot node has been defined. If you want to apply any loads or constraints on the rigid target surface, you must define a pilot node and apply the loads to that pilot node. If you do not use a pilot node, you can have rigid body motions only.
The pilot node can be one of the nodes on the target elements or a node at any arbitrary location. However, it should not be the node on the contact element. The location of the pilot node becomes important only when rotations or moments are to be applied. For each pilot node, ANSYS will automatically define an internal node and an internal constraint equation. The rotational DOF of the pilot node is connected to the translational DOF of the internal node by the internal constraint equation.
By default, KEYOPT(2) = 0 for the target element, ANSYS checks the boundary conditions for each target surface. If all of the following conditions are met, then ANSYS treats the target nodes along the respective degree of freedom as fixed:
There are no explicit boundary conditions or prescribed forces for target surface nodes.
Target surface nodes are not connected to other elements.
Neither constraint equations nor node coupling have been used to constrain such nodes.
At the end of each load step, ANSYS releases the constraint conditions that were set internally.
The constraint conditions stored in the results file (Jobname.RST) and the database file (Jobname.DB) may be updated due to this change. You should carefully verify whether the current constraint conditions are expected before restarting an analysis or resolving the problem in interactive mode.
If you wish, you can control the constraint conditions of target nodes by setting KEYOPT(2) = 1 in the target element definition.