MPC184
Multipoint Constraint Element
MPC184 Element Description
MPC184 represents a general class of multipoint constraint elements that apply kinematic constraints between nodes. The elements are loosely classified here as constraint elements (rigid link, rigid beam, etc.) and joint elements (revolute, universal, etc.).
The constraint may be as simple as that of identical displacements between nodes. Constraints can also be more complicated, such as those modeling rigid parts, or those transmitting motion between flexible bodies in a particular way. For example, a structure may consist of rigid parts and moving parts connected together by rotational or sliding connections.
The rigid part of the structure can be modeled with the MPC184 link/beam elements, while the moving parts can be connected with any of the MPC184 joint elements.
The kinematic constraints are imposed using one of the following methods:
Direct-elimination method -- The kinematic constraints are imposed by internally generated constraint equations. The degrees of freedom of a dependent node in the equations are eliminated in favor of an independent node.
The dependent degrees of freedom are eliminated. Therefore, the constraint forces and moments are not available from the element output table (ETABLE) for output purposes. However, the global constraint reaction forces are available at independent nodes in the results file, Jobname.rst (PRRSOL, etc.).
Use the direct-elimination method whenever it is available, as the degrees of freedom at the dependent nodes are eliminated, thereby reducing the problem size and solution time.
Lagrange multiplier method -- The kinematic constraints are imposed using Lagrange multipliers. In this case, all the participating degrees of freedom are retained.
Use the Lagrange multiplier method when the direct elimination method is not available or not suitable for the analysis.
The constraint forces and moments are available from the element output table (ETABLE).
Because the Lagrange multipliers are additional solution variables, the problem size is larger and the solution time increases.
Penalty-based method -- The kinematic constraints are imposed via penalty stiffness factors. As in the Lagrange multiplier method, all participating degrees of freedom are retained.
The constraint forces and moments are available from the element output table (ETABLE).
No solution variables are added.
If the penalty factors are too high, the system of equations becomes ill-conditioned. Low-value penalty factors can result in a violation of constraint conditions.
The MPC184 rigid link/beam elements can use the direct-elimination method or the Lagrange multiplier method. All other MPC184 element options use the Lagrange multiplier method or the penalty-based method.
Joint Elements
Numerical simulations often involve modeling the joints between two parts. The joints or connections may require simple kinematic constraints such as identical displacements between the two parts at the junction, or more complicated kinematic constraints allowing for motion transmission between two flexible bodies.
Complex joints may also include some sort of control mechanism such as limits or stops, and locks on the components of relative motion between the two bodies. Often, such joints may also have stiffness, damping, or friction forces based on the unconstrained components of relative motion between the two bodies.
The following joint elements are available:
The elements are well suited for linear, large rotation, and/or large strain nonlinear applications. If finite rotations and/or large-strain effects are to be considered, issue NLGEOM,ON; otherwise, linear behavior is assumed. For example, if a revolute joint element is used in an analysis without NLGEOM,ON, the calculations occur in the original configuration and the end result may not reflect the expected deformed configuration. With NLGEOM,ON, the calculations account for the rotation of the revolute joint element.
Two nodes define the joint elements. Depending on the joint to be defined, the kinematic constraints are imposed on some of the quantities that define the relative motion between the two nodes. These kinematic constraints are applied using Lagrange multipliers. In some instances, one of the nodes is required to be grounded (attached to a ground) or other static reference location. In such cases, only one of the two nodes can be specified. The specified node and the grounded node are assumed to be coincident in the element calculations.
The joint element has six degrees of freedom at each node, defining six components of relative motion: three relative displacements and three relative rotations. The six components are of primary interest in simulations involving joint elements. Some components may be constrained by the kinematic constraints relevant to a particular joint element, while other components are free (unconstrained). For example, in the case of universal and revolute joint elements, the two nodes are assumed to be connected; therefore, the relative displacements are zero. For the revolute joint, only one rotational component of the relative motion (rotation about the revolute axis) is unconstrained, while for the universal joint two such components are available.
Joint elements include control features (such as stops, locks, and actuating loads/boundary conditions) that can be imposed on the components of relative motion between the two nodes of the element. For example, in a revolute joint, stops can be specified for the rotation about the revolute axis, limiting the rotation around the revolute axis to be within a certain range. Displacement, force, velocity, and acceleration boundary conditions can be imposed on the components of relative motion between the two nodes allowing for actuation of the joints. The driving force or displacements arise from the actuating mechanism (such as an electric or hydraulic system) that drives the joint.
You can impose linear and nonlinear elastic stiffness and damping behavior or hysteretic friction behavior on the available components of relative motion of a joint element. The properties can be made temperature-dependent if necessary.
In addition to the existing output options available in Mechanical APDL, outputs related to the components of relative motion are available for joint elements.
Joint Input Data
Some input requirements are common to most MPC184 joint elements. Any specific requirements for an individual joint element are highlighted in the element description.
The following types of input data are typical:
Element Connectivity Definition -- A joint element is usually defined by specifying two nodes, I and J. One of the nodes may be a grounded node.
Section Definition -- Each joint element must have an associated section definition (SECTYPE command).
Local Coordinate System Specification -- Local coordinate systems at the nodes are often required to define the kinematic constraints of a joint element (SECJOINT command).
Stops or Limits -- You can impose stops or limits on the available components of relative motion between the two nodes of a joint element (SECSTOP).
Locks -- Locking limits may also be imposed on the available components of relative motion between the two nodes of a joint element to "freeze" the joint in a desired configuration (SECLOCK).
Material Behavior -- The JOIN material option (TB) enables linear and nonlinear elastic stiffness and damping behavior or hysteretic friction behavior on the available components of relative motion of a joint element.
Reference Lengths and Angles -- These correspond to the free relative degrees of freedom in a joint element for which constitutive calculations are performed and are used when stiffness, damping, or hysteretic friction are specified for the joint elements (SECDATA).
Boundary Conditions -- You can impose boundary conditions (DJ) or apply concentrated forces (FJ) on the available components of relative motion of the joint element.
MPC184 Input Data
Specify the MPC184 constraint or joint element form that you want to use via KEYOPT(1).
Specify the constraint-imposition method via KEYOPT(2).
The remaining input data depends on the given constraint or joint element form. The description of each MPC184 element form contains an input summary applying only to that particular element. Review the element-specific input summaries after you determine which constraint or joint element form that you want to use.
- KEYOPT(1)
Element behavior:
- 0 --
Rigid link (default)
- 1 --
- 3 --
- 6 --
- 7 --
- 8 --
- 9 --
- 10 --
- 11 --
- 12 --
- 13 --
- 14 --
- 15 --
- 16 --
- 17 --
- 18 --
- 19 --
- KEYOPT(2)
The constraint imposition method. Values depend on the joint type.
For Rigid link/beams (KEYOPT(1) = 0 or 1), KEYOPT(2) settings are:
- 0 --
Direct elimination method (default)
- 1 --
Lagrange multiplier method
For all other MPC184 elements, KEYOPT(2) settings are:
- 0 --
Lagrange multiplier method (default)
- 1 --
Penalty-based method
MPC184 Output Data
The solution output associated with the constraint and joint elements is in two forms:
Nodal displacements included in the overall nodal solution.
Additional element output as shown in the individual constraint and joint element descriptions. This output is available via ETABLE using the Sequence Number method.
Refer to the individual element descriptions for complete listings of the output for each element.
MPC184 Assumptions and Restrictions
The following restrictions apply to all forms of the MPC184 constraint and joint element:
The element coordinate system (/PSYMB,ESYS) is not relevant.
Only damping defined via TB,JOIN is supported. All other damping specifications (Rayleigh damping, DMPSTR, and so on) are not supported.
Additional assumptions and restrictions apply to each form of the MPC184 constraint and joint element. For details, see Assumptions and Restrictions within the documentation for each of the MPC184 element forms.