MPC184-Link/Beam## MPC184 Rigid Link/Beam Element Description

## MPC184 Rigid Link/Beam Input Data

### MPC184 Rigid Link/Beam Input Summary

## MPC184 Rigid Link/Beam Output Data

## MPC184 Rigid Link/Beam Assumptions and Restrictions

## MPC184 Rigid Link/Beam Product Restrictions

**Multipoint Constraint Element: Rigid Link or Rigid Beam**

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

The MPC184 rigid link/beam element can be used to model a rigid constraint between two deformable bodies or as a rigid component used to transmit forces and moments in engineering applications. This element is well suited for linear, large rotation, and/or large strain nonlinear applications.

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 MPC (multipoint constraint) equations. The degrees of freedom of a dependent node in the MPC equations are eliminated in favor of an independent node.The

**Lagrange multiplier method**, wherein the kinematic constraints are imposed using Lagrange multipliers. In this case, all the participating degrees of freedom are retained.

Figure 184link.1: MPC184 Rigid Link/Beam Geometry shows the geometry, node locations, and the coordinate system for this element. Two nodes define the element. The element x-axis is oriented from node I toward node J. The cross-sectional area of the element is assumed to be one unit. ANSYS selects the cross-section coordinate system automatically. The cross-section coordinate system is relevant only for the output of bending moments when the element is used as a rigid beam.

If KEYOPT(1) = 0 (default), the element is a rigid link with two nodes and three degrees of freedom at each node (UX, UY, UZ). If KEYOPT(1) = 1, the element is a rigid beam with two nodes and six degrees of freedom at each node (UX, UY, UZ, ROTX, ROTY, ROTZ).

If KEYOPT(2) = 0 (default), then the constraints are implemented using the direct elimination method. If KEYOPT(2) = 1, then the Lagrange multiplier method is used to impose the constraints.

The MPC184 rigid link/beam element with KEYOPT(2) = 1 can also be used in applications that call for thermal expansion on an otherwise rigid structure. The direct elimination method cannot be used for thermal expansion problems.

Because the element models a rigid constraint or a rigid component, material stiffness properties are not required. When thermal expansion effects are desired, the coefficient of thermal expansion must be specified. Density must be specified if the mass of the rigid element is to be accounted for in the analysis. If density is specified, the program calculates a lumped mass matrix for the element. The cross-sectional area is always assumed to be 1 (irrespective of the unit system used); therefore, the density should be suitably specified to account for the proper mass of the rigid link or beam in the appropriate unit system.

The element supports the birth and death options using **EALIVE** and **EKILL**.

Nodal Loading describes element loads. You can input temperatures as element body loads at the nodes. The node I temperature T(I) defaults to TUNIF. The node J temperature defaults to T(I).

This input summary applies to the rigid link and rigid beam options of MPC184: KEYOPT(1) = 0 and 1.

**Nodes**I, J

**Degrees of Freedom**UX, UY, UZ if KEYOPT(1) = 0

UX, UY, UZ, ROTX, ROTY, ROTZ if KEYOPT(1) = 1

**Real Constants**None

**Material Properties**ALPX (or CTEX

*or*THSX), DENS**Surface Loads**None

**Body Loads****Temperatures --**T(I), T(J)

**Element Loads**None

**Special Features**Birth and death Large deflection Linear perturbation **KEYOPT(1)**Element behavior:

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

**1 --**Rigid beam

**KEYOPT(2)**Reduction method:

**0 --**Direct elimination method (default)

**1 --**Lagrange multiplier method

The solution output associated with the element is in two forms:

Nodal displacements included in the overall nodal solution

Additional element output as shown in Table 184link.1: MPC184 Rigid Link/Beam Element Output Definitions.

Table 184link.1: MPC184 Rigid Link/Beam Element Output Definitions uses the following notation:

A colon (:) in the Name column indicates the item can be accessed
by the Component Name method [**ETABLE**, **ESOL**]. The O column indicates the availability of the
items in the file **Jobname.OUT**. The R column indicates
the availability of the items in the results file.

In either the O or R columns, Y indicates that the item is *always* available, a number refers to a table
footnote that describes when the item is *conditionally* available, and a - indicates that the item is *not* available.

**Table 184link.1: MPC184 Rigid Link/Beam Element Output Definitions**

Name | Definition | O | R |
---|---|---|---|

Link/Beam Elements (KEYOPT(1) = 0 or 1, and KEYOPT(2) = 0 or 1) | |||

EL | Element number | - | Y |

NODES | Element node numbers (I and J) | - | Y |

Link/Beam Elements (KEYOPT(1) = 0 or 1, and KEYOPT(2)
= 1) | |||

MAT | Material number for the element | - | Y |

TEMP | Temperature at nodes I and J | - | Y |

FX | Axial force | - | Y |

MY, MZ | Bending moments | - | Y |

SF:Y, Z | Section shear forces | - | Y |

MX | Torsional moment | - | Y |

Table 184link.2: MPC184 Rigid Link/Beam Item and Sequence Numbers lists output available via
the **ETABLE** command using the Sequence Number method.
See The General Postprocessor
(POST1) in the *Basic Analysis Guide* and The Item and Sequence Number Table for
further information. The table uses the following notation:

**Name**output quantity as defined in the Element Output Definitions table.

**Item**predetermined Item label for

**ETABLE**command**E**sequence number for single-valued or constant element data

The following restrictions apply to both the direct elimination method and the Lagrange multiplier method (KEYOPT(2) = 0 and 1):

A finite element model cannot be made up of only rigid elements in a static analysis. At a minimum, a deformable element (or elements) must be connected to one of the end nodes of a rigid element.

The cross-sectional area of the element is assumed to be unity.

The element coordinate system (

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

**Direct Elimination Method (KEYOPT(2) =
0)**

These additional restrictions apply to the direct elimination method:

The MPC184 rigid link/beam using the direct elimination method can be used in static, transient, modal, and buckling analyses.

This element cannot be used in a distributed solution when the direct elimination method is used.

Displacement boundary conditions on the nodes of rigid link/beams must be applied prudently. In a rigid linkage (structure) made of a number of rigid link/beam elements, if displacement boundary conditions are applied at more than one location, ANSYS will use the first encountered displacement boundary condition to constrain the entire rigid linkage according to rigid kinematic conditions. In some cases where the applied displacements may be redundant or self-contradictory, ANSYS will issue warning or error messages.

The direct elimination method cannot be used in problems involving thermal expansion. Use the Lagrange Multiplier method instead.

Reaction forces at the constrained nodes of a rigid link/beam may not always be available since the dependent and independent nodes are determined by ANSYS internally. We recommend that you check the interface nodes which connect rigid and deformable elements since reaction forces are available on these nodes.

The nodes of a rigid link/beam using the direct elimination method should not be linked with a node of an element implemented via the Lagrange multiplier method. For example, a rigid beam implemented using the direct elimination method (KEYOPT(2) = 0) should not be linked to a rigid beam implemented via the Lagrange multiplier method (KEYOPT(2) = 1). Or, a rigid beam implemented via the direct elimination method should not be linked to a node of a contact element that is implemented via the Lagrange multiplier method (KEYOPT(2) = 2 on the contact element).

Coupling constraints (

**CP**command) cannot be applied to nodes of rigid links/beams using the direct elimination method.Nodes of rigid links/beams cannot be part of the retained nodes (nodes specified by the

**M**command) in a substructure. However, the rigid links/beams can be entirely within the substructure.Rigid links/beams should be not used in cyclic symmetry analyses.

**Lagrange Multiplier Method (KEYOPT(2)
= 1)**

These additional restrictions apply to the Lagrange Multiplier method:

To employ this feature successfully, use as few of these elements as possible. For example, it may be sufficient to overlay rigid line elements on a perimeter of a rigid region modeled with shell elements, as opposed to overlaying rigid line elements along each element boundary of the interior.

Modeling that avoids overconstraining the problem is necessary. Overconstrained models may result in trivial solutions, zero pivot messages (in a properly restrained system), or nonlinear convergence difficulties.

The temperature is assumed to vary linearly along the spar of the rigid link or rigid beam element.

If constraint equations are specified for the DOFs of a rigid element, it may be an overconstrained system. Similarly, prescribed displacements on both ends of the element is an indication of overconstraint.

When used as a link element, exercise the same precautions that you would when using a truss element (for example, LINK180).

The equation solver (

**EQSLV**) must be the sparse solver or the PCG solver. The command**PCGOPT**,,,,,,,ON is also required in order to use the PCG solver.The element is valid for static and transient analyses (linear and nonlinear), and rigid beam is valid for harmonic analyses. The element is not supported for buckling analyses.

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.