MPC184
## MPC184 Element Description

### Joint Elements

### Joint Input Data

## MPC184 Input Data

## MPC184 Output Data

## MPC184 Assumptions and Restrictions

## MPC184 Product Restrictions

**Multipoint Constraint Element**

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

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 may be modeled with the MPC184 link/beam elements, while the moving parts may be connected with any of the MPC184 joint elements.

The kinematic constraints are imposed using one of the following two methods:

The

**direct elimination method**, wherein 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**command, etc.).The direct elimination method should be used whenever it is available since the degrees of freedom at the dependent nodes are eliminated, thereby reducing the problem size and solution time.

The

**Lagrange multiplier method**, wherein the kinematic constraints are imposed using Lagrange multipliers. In this case, all the participating degrees of freedom are retained.The Lagrange multiplier method should be used when the direct elimination method is not available or not suitable for the analysis purposes.

In this method, the constraint forces and moments are available from the element output table (

**ETABLE**).The disadvantage of the Lagrange multiplier method is that the Lagrange multipliers are additional solution variables and, hence, the problem size and solution time become larger when compared with the direct elimination method.

Currently, 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 only.

Numerical simulations often involve modeling of joints between two parts. These
joints or connections may need simple kinematic constraints such as identical
displacements between the two parts at the junction or more complicated kinematic
constraints that allow for transmission of motion between two flexible bodies. These
complex joints may also include some sort of control mechanism like limits or stops,
and locks on the components of relative motion between the two bodies. In many
instances, these joints may also have stiffness, damping, or friction forces based
on the unconstrained components of relative motion between the two bodies. For
detailed information on how to use joint elements, see Connecting Multibody Components with Joint Elements in the *Multibody Analysis Guide*.

The following types of joint elements are available:

These 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, the **NLGEOM**,ON command must be used; otherwise, linear
behavior is assumed. For example, if a revolute joint element is used in an analysis
and **NLGEOM**,ON is not set, the calculations are carried out in the
original configuration and the end result may not reflect the expected deformed
configuration. However, if the **NLGEOM**,ON command is used, the
calculations will take into account the rotation of the revolute joint element.

Two nodes define these 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" or attached to "ground" or some other reference location that is not moving. In such cases, only one of the two nodes may 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. These six components of relative motion are of primary interest in simulations that involve joint elements. Some of these components may be constrained by the kinematic constraints relevant to a particular joint element, while the other components are "free" or "unconstrained". For example, in the case of universal and revolute joint elements the two nodes are assumed to be connected, and 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.

The capabilities of these elements include certain 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. This limits the rotation around the revolute axis to be within a certain range. Displacement, force, velocity, and acceleration boundary conditions may 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 mechanisms like an electric or hydraulic system that drives these joints.

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 ANSYS, outputs related to the components of relative motion are available for joint elements.

Certain input requirements are common to most MPC184 joint elements. Any specific requirements for individual joint elements are highlighted in the description for that element.

The following types of input data should be considered:

Element Connectivity Definition - A joint element is typically defined by specifying two nodes, I and J. One of these 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**command).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**command).Material Behavior - The JOIN material option on the

**TB**command allows you to impose 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**command).Boundary Conditions - You can impose boundary conditions (

**DJ**command) or apply concentrated forces (**FJ**command) on the available components of relative motion of the joint element.

Use KEYOPT(1) to specify the type of MPC184 constraint or joint element you want to use. The remaining input data will vary depending on the type of constraint or joint element specified. The individual MPC184 element descriptions each contain an input summary that applies only to that particular element. You should review these element-specific input summaries after you determine which constraint or joint element you will be using.

**KEYOPT(1)**Element behavior:

**0 --**Rigid link (default)

**1 --****3 --****6 --****7 --****8 --****9 --****10 --****11 --****12 --****13 --****14 --****15 --****16 --****17 --**

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 the

**ETABLE**command using the Sequence Number method.

Refer to the individual element descriptions for complete listings of the output for each element.

The following restrictions apply to all forms of the MPC184element:

For MPC184, the element coordinate system (

**/PSYMB**,ESYS) is not relevant.

There are additional assumptions and restrictions for each type of constraint and joint element. For details, see the Assumptions and Restrictions section in the individual constraint and joint element descriptions.

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

**ANSYS Mechanical Pro **

Birth and death is not available.

Linear perturbation is not available.

**ANSYS Mechanical Premium **

Birth and death is not available.