Chapter 12: Coupling and Constraint Equations

Go to the Next Chapter
Go to the Previous Chapter
Go to the Table of Contents for This Manual
Go to the Guides Master Index

Chapter 1 * Chapter 2 * Chapter 3 * Chapter 4 * Chapter 5 * Chapter 6 * Chapter 7 * Chapter 8 * Chapter 9 * Chapter 10 * Chapter 11 * Chapter 12 * Chapter 13 * Chapter 14

12.1 Introduction

When generating your model, you typically define the relationships among different degrees of freedom by using elements to connect the nodes. However, you sometimes need to be able to model distinctive features (rigid regions, pinned structural joints, sliding symmetry boundaries, periodic conditions, and other special internodal connections) which cannot be adequately described with elements. You can establish such special associations among nodal degrees of freedom by using coupling and constraint equations. Using these techniques enables you to link degrees of freedom in ways that elements cannot.

12.2 What Is Coupling?

When you need to force two or more degrees of freedom (DOFs) to take on the same (but unknown) value, you can couple these DOFs together. A set of coupled DOFs contains a prime DOF, and one or more other DOFs. Coupling will cause only the prime DOF to be retained in your analysis' matrix equations, and will cause all the other DOFs in a coupled set to be eliminated. The value calculated for the prime DOF will then be assigned to all the other DOFs in a coupled set.

Typical applications for coupled DOFs include: 1) maintaining symmetry on partial models, 2) forming pin, hinge, universal, and slider joints between two coincident nodes, and 3) forcing portions of your model to behave as rigid bodies (see this chapter's discussion of constraint equations for more general rigid region capability).

12.3 How to Create Coupled Degree of Freedom Sets

12.3.1 Creating and Modifying Coupled Sets at Specified Nodes

To define (or modify) a set of coupled degrees of freedom, use one of these methods:

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Couple DOFs

After creating a coupled set of nodes, you can include more nodes in that set by simply performing an additional coupling operation (be sure to use the same set reference number). You can also use selecting logic to couple "ALL" of the selected nodes. Nodes can be deleted from a coupled set by inputting them as negative node numbers on the CP command. To modify a coupled DOF set (that is, add or delete nodes, or change the DOF label), use the CPNGEN command. (You cannot access the CPNGEN command directly in the GUI.)

12.3.2 Coupling Coincident Nodes

The CPINTF command couples coincident nodes in a model by generating one coupled set for each specified DOF label at every pair of coincident nodes. This operation is useful for "buttoning" together several pairs of nodes (such as at a seam).

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Coincident Nodes

Instead of coupling coincident nodes, you can use one of these alternative methods to force the nodes to behave in the same way:

12.3.3 Generating More Coupled Sets

Once one or more coupled sets exist, additional sets can be generated using these methods:

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Gen w/Same Nodes

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Gen w/Same DOF

12.3.4 Listing and Deleting Coupled Sets

You can perform two other operations to help you manage your coupled sets:

Command(s):

GUI:

Utility Menu>List>Other>Coupled Sets>All CP nodes selected
Utility Menu>List>Other>Coupled Sets>Any CP node selected

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Del Coupled Sets

12.4 Additional Considerations for Coupling

Coupling operates in the nodal coordinate system of each node coupled. You should usually keep your nodal coordinate systems consistent.

Degrees of freedom are coupled within a set but are not coupled between sets. You must not allow a degree of freedom to appear in more than one coupled set.

"Grounded" degrees of freedom (that is, DOFs with values specified by D or other constraint commands) must not be included in the coupled set.

In a reduced analysis, if master degrees of freedom are to be chosen from coupled DOF sets, only prime DOFs may be designated as master degrees of freedom. (You must not designate any eliminated DOF in a coupled set as a master degree of freedom.)

In a structural analysis, coupling DOFs to create a rigid region can sometimes cause apparent violations of equilibrium. A set of coupled nodes which are not coincident or are not in line with the coupled displacement direction may produce an applied moment that will not appear in the reaction forces.

12.5 What Are Constraint Equations?

Linear constraint equations provide a more general means of relating degree of freedom values than is possible with simple coupling. Constraint equations must have the form:

where U(I) is the degree of freedom of term (I), and N is the number of terms in the equation.

12.6 How to Create Constraint Equations

12.6.1 The Direct Method

You can create constraint equations directly, using one of these methods:

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Constraint Eqn

The following example illustrates a typical application of a constraint equation, in which moment transfer capability is created for a connection between a BEAM3 element and PLANE42 elements (PLANE42 elements have no in-plane rotational degree of freedom):

Figure 12-1 Establishing relationships between rotational and translational degrees of freedom

In this example, node 2 acts as a hinge if no constraint equations are used. To transfer moment between the beam and the plane-stress elements, you can use the following equation:

ROTZ2 = (UY3 - UY1)/10

This equation would be rewritten in the required format and entered into the program as:

0 = UY3 - UY1 - 10*ROTZ2 

CE,1,0,3,UY,1,1,UY,-1,2,ROTZ,-10
The first unique degree of freedom in the equation is eliminated in terms of all other degrees of freedom in the equation. A unique degree of freedom is one which is not specified in any other constraint equation, coupled node set, specified displacement set, or master degree of freedom set. You should make the first term of the equation be the degree of freedom to be eliminated. Although you may, in theory, specify the same degree of freedom in more than one equation, you must be careful to avoid over-specification. You must also take care to ensure that each node and degree of freedom exists in the model. (Remember that for a degree of freedom to be present at a node, that node must be connected to an element which supplies the necessary degree of freedom.)

12.6.1.1 Periodic Conditions

Often in field analysis, it is desirable to take advantage of antisymmetric or periodic field variation to limit the model size. This can be accomplished by coupling nodal potential values, and/or by writing constraint equations. Both these options are available in the ANSYS/EMAG program using the CP and CE commands, respectively.

A periodic condition is a boundary for which neither the flux-parallel nor flux-normal conditions hold, but rather the potential at one point is of equal magnitude but of opposite sign to that of a point in another location. This condition arises in the analysis of symmetry sectors of motors, for example, where the potentials one pole pitch apart are equal but opposite in sign. In Figure 12-2, suppose node 129 in the outlined symmetry sector is to be constrained as described above with node 363 on the opposite pole pitch.

Figure 12-2 Example of specifying a periodic condition

The constraint equation would read:

The CE command used to input this constraint equation would appear as follows: 

CE,1,0,129,MAG,1,363,MAG,1
To automatically apply groups of periodic boundary conditions (CP and CE commands) for 2-D magnetic analyses, use the PERBC2D command macro (refer to Chapter 11 of the ANSYS Electromagnetic Field Analysis Guide for a discussion of this modeling aide):

Command(s):

GUI:

Main Menu>Preprocessor>Loads>Apply>Periodic BCs
Main Menu>Solution>Apply>Periodic BCs

Note-Periodic boundary conditions can also be represented in a structural analysis (for example, in a turbine blade model) using CP commands on nodes rotated into the cylindrical coordinate system.

12.6.2 Modifying Constraint Equations

To change the constant term of a constraint equation in either PREP7 or SOLUTION, use one of these methods:

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Modify ConstrEqn
Main Menu>Preprocessor>Loads>Other>Modify ConstrEqn
Main Menu>Solution>Other>Modify ConstrEqn

If you need to change any of the other terms of a constraint equation, you must use the CE command (or the corresponding GUI path) in PREP7, before you start your solution.

12.6.3 Direct vs. Automatic Constraint Equation Generation

An example that appeared earlier in this chapter illustrated how you can use the CE command to create constraint equations directly, one at a time.

Three other operations, described below, automatically generate multiple constraint equations for you.

12.6.3.1 Creating a Rigid Region

The CERIG command defines a "rigid region" by writing constraint equations to define rigid lines linking a designated retained (or "master") node to a number of removed (or "slave") nodes. (The term "master node" as applied to this operation is not the same as a master degree of freedom for a reduced analysis.)

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Rigid Region

By setting Ldof to ALL on the CERIG command (default), this operation will generate three equations for each pair of constrained nodes in 2-D space. These equations define the three rigid body motions in global Cartesian space (UX, UY, ROTZ). In order to create a rigid region on a 2-D model, you must make sure that the X-Y plane is the rigid plane and that UX, UY, and ROTZ degrees of freedom are available at each constrained node. This operation will similarly generate six equations for each pair of constrained nodes in 3-D space. All six degrees of freedom (UX, UY, UZ, ROTX, ROTY, and ROTZ) must be available at each constrained node.

Entering other labels in the Ldof field will create different effects. If this field is set to UXYZ, the program will write two constraint equations in 2-D (X,Y) space and three constraint equations in 3-D (X,Y,Z) space. These equations will be written in terms of the slave nodes' translational degrees of freedom, and in terms of the master node's translational and rotational degrees of freedom. Similarly, the RXYZ label allows you to generate a partial set of equations that omit the slave nodes' translational degrees of freedom. The other available Ldof labels will generate other types of constraint equations.

In general, your slave nodes need have only the degrees of freedom called for by Ldof, but your master node must have all applicable translational and rotational degrees of freedom (that is, UX, UY, ROTZ for 2-D; UX, UY, UZ, ROTX, ROTY, ROTZ for 3-D). For models that are made up of elements having no rotational degree of freedom, you might consider adding a dummy beam element to provide rotational degrees of freedom at the master node.

12.6.3.2 Tying Dissimilarly Meshed Regions Together

You can generate constraint equations connecting the selected nodes of one region to the selected elements of another region by using the CEINTF command (Main Menu>Preprocessor>Coupling / Ceqn>Adjacent Regions). This operation "ties" together regions with dissimilar mesh patterns. At the interface location between two regions, select the nodes from the denser mesh region, A, and select the elements from the sparser mesh region, B. The degrees of freedom of region A nodes are interpolated with the corresponding degrees of freedom of the nodes on the region B elements, using the shape functions of the region B elements. Constraint equations are then written that relate region A and B nodes at the interface. ANSYS allows two tolerances on the location of these nodes. Nodes which are outside the element by more than the first tolerance are not accepted as being on the interface. Nodes that are closer than the second tolerance to an element surface are moved to that surface. See Section 15.8.3 of the ANSYS Theory Reference for details.

Certain limitations affect the CEINTF command: stress or thermal flux might not be continuous across the interface. Nodes in the interface region must not have specified displacements. You can interface 6-DOF solids only with other elements having six degrees of freedom per node.

12.6.3.3 Generating Sets of Constraint Equations from Existing Sets

You can issue the CESGEN command to generate sets of constraint equations from existing sets. All node numbers within the existing sets are then incremented to generate the additional sets. The labels and coefficients of the additional sets remain the same as those of the original sets.

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn >Gen w/same DOF

12.6.4 Listing and Deleting Constraint Equations

You can list and delete your constraint equations.

Command(s):

GUI:

Utility Menu>List>Other>Constraint Eqns>All CE nodes selected
Utility Menu>List>Other>Constraint Eqns>Any CE node selected

Command(s):

GUI:

Main Menu>Preprocessor>Coupling / Ceqn>Del Constr Eqn

12.7 Additional Considerations for Constraint Equations

All constraint equations are based on small rotation theory. Therefore, their use in large-rotation analyses [NLGEOM] should be restricted to cases where the directions of the DOF included in constraint equations do not change significantly.

The presence of constraint equations can produce unexpected reaction and nodal force results. Please see the related discussion in Chapter 5 of the ANSYS Basic Analysis Procedures Guide.

Go to the beginning of this chapter