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

The generalized plane strain option is a feature developed for PLANE182 and PLANE183. The generalized plane strain feature assumes a finite deformation domain length in the Z direction, as opposed to the infinite value assumed for standard plane strain. Generalized plane strain, therefore, will give more practical results for deformation problems where the Z-direction dimension is not long enough. It will also give users a more efficient way to simulate certain 3-D deformations using 2-D element options.

The deformation domain or structure is formed by extruding a plane area along a curve with a constant curvature, as shown in Figure 2.2: "Generalized Plane Strain Deformation". The extruding begins at the starting (or reference) plane and stops at the ending plane. The curve direction along the extrusion path is called the fiber direction. The starting and ending planes must be perpendicular to this fiber direction at the beginning and ending intersections. If the boundary conditions and loads in the fiber direction do not change over the course of the curve, and if the starting plane and ending plane remain perpendicular to the fiber direction during deformation, then the amount of deformation of all cross sections will be identical throughout the curve, and will not vary at any curve position in the fiber direction. Therefore, any deformation can be represented by the deformation on the starting plane, and the 3-D deformation can be simulated by solving the deformation problem on the starting plane. The existing plane strain and axisymmetric options will be particular cases of the generalized plane strain option.

All inputs and outputs are in the global Cartesian coordinate system. The starting plane must be the X-Y plane, and must be meshed. The applied nodal force on the starting plane is the total force along the fiber length. The geometry in the fiber direction is specified by the rotation about X and Y of the ending plane and the fiber length passing through a user-specified point on the starting plane called the starting or reference point. The starting point creates an ending point on the ending plane through the extrusion process. The boundary conditions and loads in the fiber direction are specified by applying displacements or forces at the ending point. This ending point can be different from regular nodes, in that it is designated by the same X - Y coordinates that are fixed in plane during deformation.

The generalized plane strain option introduces three new degrees of freedom for each element. Two internal nodes will be created automatically at the solution stage for the generalized plane strain option to carry the extra three DOF's. Users can apply boundary conditions and loads and check the results of the fiber length and rotation angle changes, and reaction forces, using the commands GSBDATA, GSGDATA, GSSOL, and GSLIST. The results of the fiber length change, rotation angle change, and reaction forces can also be viewed through OUTPR.

The fiber length change is positive when the fiber length increases. The sign of the rotation angle or angle change is determined by how the fiber length changes when the coordinates of the ending point change. If the fiber length decreases when the X coordinate of the ending point increases, the rotation angle about Y is positive. If the fiber length increases when the Y coordinate of the ending point increases, the rotation angle about X is positive.

In Eigenvalue analyses, such as Eigen buckling and modal analysis, the generalized plane strain option usually reports fewer Eigenvalues and Eigenvectors than you would obtain in a 3-D analysis. Because it reports only homogenous deformation in the fiber direction, generalized plane strain employs only three DOFs to account for these deformations. The same 3-D analysis would incorporate many more DOFs in the fiber direction.

Because the mass matrix terms relating to DOFs in the fiber direction are approximated for modal and transient analyses, you cannot use the lumped mass matrix for these types of analyses, and the solution may be slightly different from regular 3-D simulations when any of the three designated DOFs is not restrained.