Manual coupling

Use the Manual Coupling command to manually create either multi-point constraint equations (MPCs) or coupled degrees-of-freedom between selected nodes.

In Simcenter Nastran, MSC Nastran, or Simcenter Samcef environments, a manual coupling is categorized as a constraint. In the Abaqus and ANSYS environments, it is categorized as a solver-specific simulation object.

For more information about manual coupling in the Simcenter Samcef environment, see Manual coupling (Simcenter Samcef).

Types of Manual Couplings

The available manual coupling options depend on the solver and solution type.

Type of manual coupling	Solver and solution types	Description
Coupled DOF	Simcenter Nastran Structural	Lets you define coupled degrees-of-freedom (DOF) between a single independent node and any number of dependent nodes. Coupled DOF create multi-point constraint equations that relate the displacement DOF of the dependent node to those of the independent node. You can use the Coupled DOF option, for example, to model rigid links between nodes or to simulate rigid spider type elements.
MSC Nastran Structural
Abaqus Structural, Axisymmetric Structural, Thermal, Dynamic Explicit, Axisymmetric Dynamic Explicit, Coupled Thermal-Structural, and Dynamic Coupled Thermal-Structural
ANSYS Structural
ANSYS Axisymmetric Structural
Simcenter Samcef Structural and Axisymmetric and Other 2D Structural
MPC	Simcenter Nastran Structural and Axisymmetric Structural	Lets you define a multi-point constraint equation. Each MPC is described by a single equation that specifies a linear relationship for two or more DOF. You can use the MPC option, for example, to join dissimilar elements, or to describe rigid elements and mechanisms.The MPC constrains one DOF of the dependent node to the DOF of one or more independent nodes. If you want to constrain all six DOF for the dependent node, you must create six MPCs.See Multipoint Constraints in the Simcenter Nastran User's Guide for more information.
MSC Nastran Structural and Axisymmetric Structural (in MSC Nastran 2007 and later)
Simcenter Samcef Structural and Axisymmetric and Other 2D Structural
MPCY	MSC Nastran Structural and Axisymmetric Structural	Lets you define an MPC with a non-zero right-hand value for the MPC equation.See the MPCY bulk data entry in the MSC Nastran Quick Reference Guide for more information.
Multi MPC	Simcenter Nastran and MSC Nastran Structural	Lets you apply constraints to Constraint Equation type of elements.See Defining constraint equations as elements for more information.
CE	ANSYS Structural, Axisymmetric Structural,	Lets you define a multi-point constraint equation with a non-zero right hand value.See Coupling and Constraint Equations in the ANSYS Modeling and Meshing Guide.
*EQUATION	Abaqus Structural, Axisymmetric Structural, Thermal, Dynamic Explicit, Axisymmetric Dynamic Explicit, Coupled Thermal-Structural, and Dynamic Coupled Thermal-Structural	Lets you define a linear multi-point constraint equation.See Linear constraint equations in the Abaqus Analysis User’s Guide for more information.
Beam	Abaqus Structural, Axisymmetric Structural, Thermal, Dynamic Explicit, Axisymmetric Dynamic Explicit, Coupled Thermal-Structural, and Dynamic Coupled Thermal-Structural	Creates a rigid beam between two nodes. This beam constrains the displacement and rotation at the first node to the displacement and rotation at the second node, corresponding to the presence of a rigid beam between the two nodes.
Link	Abaqus Structural, Axisymmetric Structural, Thermal, Dynamic Explicit, Axisymmetric Dynamic Explicit, Coupled Thermal-Structural, and Dynamic Coupled Thermal-Structural	Creates a pinned, rigid link between two nodes that keeps the distance between the nodes constant. The software modifies the displacements of the first node to enforce this constraint.Note: Any rotational DOF for the two nodes are not included in this constraint.
Tie	Abaqus Structural, Axisymmetric Structural, Thermal, Dynamic Explicit, Axisymmetric Dynamic Explicit, Coupled Thermal-Structural, and Dynamic Coupled Thermal-Structural	Makes the global displacements and rotations as well as all other active degrees of freedom equal at two nodes. If there are different degrees of freedom active at the two nodes, the software only constrains those DOF in common. Typically, you use the TIE option when you need to fully connect corresponding nodes on two different portions of a mesh.
Pin	Abaqus Structural, Axisymmetric Structural, Thermal, Dynamic Explicit, Axisymmetric Dynamic Explicit, Coupled Thermal-Structural, and Dynamic Coupled Thermal-Structural	Creates a pinned joint between two nodes. With a Pin type of constraint, the software makes the global displacements of the two nodes equal.Note: Any rotational DOF for the two nodes are not included in this constraint.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and the displayed partNastran, Abaqus, ANSYS, or Simcenter Samcef as the specified solver Structural, Axisymmetric Structural, Axisymmetric and Other 2D Structural (Simcenter Samcef only), Thermal (Abaqus only), Dynamic Explicit (Abaqus only), Axisymmetric Dynamic Explicit (Abaqus only), Coupled Thermal-Structural (Abaqus only), or Dynamic Coupled Thermal-Structural (Abaqus only), as the specified analysis type
Command Finder	Manual Coupling
Simulation Navigator	Under a solution, right-click Constraints→New Constraint→Manual CouplingFor Abaqus and ANSYS, under a solution, right-click Simulation Objects→New Simulation Object→Manual Coupling

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Manual coupling, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });