The methods for setting a constraint condition of a model are Basic, Advanced and Auto.

Basic

Select the target and assign a [Fixed], [Pinned] or [No Rotation] that fits the behavior of the analysis model.

Advanced

The 6 degrees of freedom of a node can be fully or partially constrained.

Tx, Ty, Tz are the displacement constraints in the x, y, z direction and Rx, Ry, Rz are the rotational constraints in the x, y, z direction.

The constraint conditions can be input for a desired boundary condition (Point, Edge, Face, Node, Free face node).

The constraint conditions are assigned to the element node and reflected in the analysis. Setting the constraint conditions on a point, edge, face etc. is a convenient method of selecting element nodes included in the selected geometry shape

Auto

Select the target mesh set to automatically create constraint conditions. The ground conditions for general stress analysis are set automatically. The x direction displacement is constrained for the left/right side, the y direction displacement is constrained for the front/back side and the x,y direction displacement is constrained for the bottom of a model.

Boundary set

Register the set constraint conditions on the desired boundary set. The user can specify the name of the boundary set.

Symmetric and inverse symmetric constraints

Boundary conditions can be largely divided into two conditions;

1. Constraint conditions of the analysis target are specified

2. Symmetry of the structure is used to analyze the symmetric area only, not the entire model.

Applying symmetry is a very effective way to increase the convenience of modeling and decrease the analysis time. If the geometry of the structure and loading is symmetrical, a 1/2 model or 1/4 model can be used to decrease the number of elements and create an economic model that reduces analysis time. However, constraints exist when checking the deformed shape or stress distribution for the entire model because the analysis results from the symmetric model cannot be shown on the entire model. Here, use the View symmetric model function on the Additional view control toolset to expand the analysis results of the 1/2 or 1/4 model onto the entire model.

• How to apply symmetric boundary conditions

If one or more of the geometry shapes, materials, loads or boundary conditions is symmetrical about a plane or axis, the symmetric boundary condition can be used. The View symmetric model function can output, expand a 1/2, 1/4, 1/8 symmetric model onto the entire model. To assign a symmetric boundary condition, a boundary condition needs to be set such that the structure does not invade the symmetry plane.

The figure below is an example of symmetric constraint conditions applied to a solid model. To apply the symmetric constraint conditions in the YZ plane, the Translation degree of freedom Tx is constrained. For the XY plane, the Tz needs to be constrained and for the ZX plane, the Ty needs to be constrained.

Because Solid elements do not have a rotational degree of freedom, only the displacement boundary condition of the symmetric model is constrained. However, the rotational degree of freedom needs to be constrained for a Shell model such that the symmetry plane is not invaded. In other words, Tx,Ry,Rz need to be constrained for the XY plane, Tz,Rx,Ry for the XY plane and Ty,Rx,Rz for the ZX plane.

When applying a symmetric boundary condition, the loading size needs to be converted to fit the symmetric condition. Also, the symmetric condition cannot be applied to the model shape and buckling shape because of the asymmetric vibration mode or the possibility of asymmetric buckling.