You can define a boundary condition by selecting one of the common types listed in the symmetry/antisymmetry/encastre boundary condition editor.
To create or edit a symmetry/antisymmetry/encastre boundary condition:
Display the symmetry/antisymmetry/encastre boundary condition editor using one of the following methods:
To create a new symmetry/antisymmetry/encastre boundary condition, follow the procedure outlined in “Creating boundary conditions,” Section 16.8.2 (Category: Mechanical; Types for Selected Step: Symmetry/Antisymmetry/Encastre).
To edit an existing symmetry/antisymmetry/encastre boundary condition using menus or managers, see “Editing step-dependent objects,” Section 3.4.12. You can edit the symmetry/antisymmetry/encastre boundary condition only in the step in which it was created.
If you are creating the boundary condition in a buckling step, select the Use BC for option that specifies the calculations for which you want the boundary condition used. For more information, see “Boundary conditions,” in “Eigenvalue buckling prediction,” Section 6.2.3 of the ABAQUS Analysis User's Manual.
Select one of the following options:
XSYMM Symmetry about a plane X = constant (U1 = UR2 = UR3 = 0).
YSYMM Symmetry about a plane Y = constant (U2 = UR1 = UR3 = 0).
ZSYMM Symmetry about a plane Z = constant (U3 = UR1 = UR2 = 0).
XASYMM Antisymmetry about a plane with X = constant (U2 = U3 = UR1 = 0;ABAQUS/Standard only).
YASYMM Antisymmetry about a plane with Y = constant (U1 = U3 = UR2 = 0;ABAQUS/Standard only).
ZASYMM Antisymmetry about a plane with Z = constant (U1 = U2 = UR3 = 0;ABAQUS/Standard only).
PINNED Pinned (U1 = U2 = U3 = 0).
ENCASTRE Fully built-in (U1 = U2 = U3 = UR1 = UR2 = UR3 = 0).
Click OK to save your data and to exit the editor.
