www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS

You can use several different methods to create constraint equations.
These include the **CE** command (the direct method) and other
commands such as **CEINTF**, **CERIG**, and **RBE3**.
These methods of generating constraint equations are discussed in the following
sections.

In addition to the methods discussed here, you
can use the internal multipoint constraint (MPC) feature of certain contact
elements (CONTA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, and CONTA177)
to model contact assemblies and kinematic constraints. By this method, the
program builds MPC equations internally based on the contact kinematics. See "Multipoint Constraints and Assemblies" in the *Contact Technology Guide* for more information on how to
use this feature.

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

Command(s): | CE |

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):

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:

ROTZ

_{2}= (UY_{3}- UY_{1})/10

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

0 = UY

_{3}- UY_{1}- 10*ROTZ_{2}

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.)

Often in field analysis, it is desirable to take advantage of antisymmetric or periodic field variation to limit the model size. For static magnetic analyses, this can be accomplished by using ANSYS cyclic symmetry capabilities. See Solving a Magnetic Cyclic Symmetry Analysis for more information. For harmonic or transient magnetic analyses, use the constraint equation method explained here.

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: "Example of Specifying a Periodic Condition", suppose node 129 in the outlined symmetry sector is to be constrained as described above with node 363 on the opposite pole pitch.

The constraint equation would read:

A

_{129}= - A_{363}0 = A

_{129}+ A_{363}

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 "Electric and Magnetic Macros" in the *Low-Frequency Electromagnetic Analysis Guide* for a discussion of
this modeling aide):

Command(s): | PERBC2D |

GUI: | Main Menu> Preprocessor> Loads> Define Loads> Apply> Magnetic>
Boundary> Flux Normal> Periodic BCs Main Menu> Solution>
Define Loads> Apply> Magnetic> Boundary> Flux Normal> Periodic BCs |

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.

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

Command(s): | CECMOD |

GUI: | Main Menu> Preprocessor> Coupling/Ceqn> Modify ConstrEqn Main
Menu> Preprocessor> Loads> Load Step Opts> Other> Modify ConstrEqn Main
Menu> Solution> Load Step Opts> 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.

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.

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): | CERIG |

GUI: | Main Menu> Preprocessor> Coupling/Ceqn> Rigid Region |

By setting * Ldof* to ALL on the

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

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.

You can tie dissimilarly meshed regions together via the **CEINTF** command,
or you can use contact elements with the internal multipoint constraint (MPC)
algorithm.

You can generate constraint equations connecting the selected nodes
of one region to the selected elements of another region via 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 the *Theory Reference for ANSYS and ANSYS Workbench* 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.

To learn more about tying dissimilarly meshed regions together via contact elements and the internal MPC algorithm, see "Multipoint Constraints and Assemblies".

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): | CESGEN |

GUI: | Main Menu> Preprocessor> Coupling/Ceqn > Gen w/same DOF |

You can list and delete your constraint equations.

To list constraint equations, use one of these methods:

**Command(s):****CELIST****GUI:****Utility Menu> List> Other> Constraint Eqns> All CE nodes selected****Utility Menu> List> Other> Constraint Eqns> Any CE node selected**To delete constraint equations, use one of these methods:

**Command(s):****CEDELE****GUI:****Main Menu> Preprocessor> Coupling/Ceqn> Del Constr Eqn**

During the solution, the user-defined constraint equations (CEs) may be modified as follows:

CEs that are applied to DOFs which are not active (for example, a CE relating rotational DOFs on nodes with only translational DOFs) are deleted.

CEs for which all DOFs are constrained (

**D**command) are deleted.CEs that have DOFs in another equation have their terms reordered so that they all have a common retained DOF.

CEs which are chained together are merged into a single CE.

CEs which are internal to the solution process are generated by MPC contact and by cyclic symmetry. These CEs cannot be listed or deleted.

Overconstrained problems for which there is no unique DOF that can be solved typically generate an error message similar to one of the following:

`Constraint equation set is defective.``Constraint equation is circular.``Constraint equation has no unique degree of freedom.``Contact overconstraint may occur.`

In addition to CE-specific error messages, you may also notice "small (or zero) pivot" messages from the solver. Such overconstraints may be caused by one of the following conditions:

**Duplicate CEs are specified for the same DOFs.***Work-around:*Delete any duplicate specifications, or issue an**NUMMRG**,CE command to compress them out.**DOFs in a CE are also present in a coupled (CP) set.***Work-around:*Delete the CP set and include the DOF in the CE to obtain the desired response.**CEs are chained together in such a way that they form a "circular" set.**Typically, this condition occurs when you define

**CEINTF**and/or MPC contact on adjacent surfaces.*Work-around:*Perform the**CEINTF**operation, or specify the contact region encompassing both surfaces simultaneously rather than individually.