EENS

EENS, Elem, Fname, --, KOut
Evaluates element solutions based on assumed element deformation.

PREP7: Elements

Elem: Element to be included in the evaluation. If ALL, the command evaluates the element solutions for all selected elements (ESEL). A component name is also valid.

Fname

Result file name..

File name and directory path (248 characters maximum, including the characters needed for the directory path). An unspecified directory path defaults to the working directory; in this case, you can use all 248 characters for the file name.

The file name defaults to Jobname. Applicable only when evaluated element results are output to a result file (KOut = 0 or blank).

--

Unused field.

KOUT

Definition of KOut

0	—	Or blank. Evaluated element results are saved in the result file (default).
1	—	Evaluated element results are converted to initial-state data at the integration points.

Notes

This action command calculates element results (such as strains and stresses) based on the curvature that is caused by bending or twisting. Membrane deformation is ignored. This command can be used to evaluate element solutions without running a regular finite element simulation, which may be useful during the design phase of a product that requires frequent shape changes.

EENS supports structural 3D shell elements SHELL181 and SHELL281 with regular stiffness option (KEYOPT(1) = 0).

EENS evaluates element results based on the element definition and assumed element deformation. The assumptions are:

The selected elements are part of a slender structure with a large span-to-thickness ratio.
The structure is initially flat and subjected predominantly to bending and twisting deformation. The membrane and transverse deformations are negligible.
Material behaviors are mostly linear.

With these assumptions, the element deformation can be adequately represented with the curvature of the element. For a SHELL281 element, the element curvature is computed directly with element geometry. For SHELL181 elements, the curvature is computed from the surface normal of a slender structure.

The recovered element results can be output in one of two forms, either saved to the result (RST) file or converted to initial-state data, controlled with KOut.

EENS can be issued multiple times, with behavior as follows:

When KOut = 0, the newly issued EENS command overwrites the previously generated result file if Fname is not specified or if the same Fname is used. Multiple result files can be generated by specifying a new Fname for each EENS command.
When KOut = 1, the newly issued EENS command causes the accumulation of initial state data for the same elements as in the previous EENS command.

Element outputs to the result file (KOut = 0)

The following table shows the element outputs saved in the result file. The items are available for both printing (PRESOL) and plotting (PLESOL) commands for postprocessing. The RSYS command can be used to transform the coordinate system.

Name	Definition
EL	Element number and name
NODES	Nodes I, J, K, L
MAT	Material number
XC, YC, ZC	Location where results are reported^[a]
S: X, Y, Z, XY, YZ, XZ	Stresses^[b]^[c]
EPEL:X, Y, Z, XY, YZ, XZ	Elastic strains^[b]^[c]

^[a]Available only at the centroid as a *GET item.

^[b]Stresses and strains in the element coordinate system are available at all section points through the thickness. If layers are in use, the results are in the layer coordinate system.

^[c]The shear components of stress and strain are always close to zero.

Conversion of the evaluated result to initial-state data (KOut = 1)

The stresses at the integration points can be converted to the initial-state data under the following conditions:

Stresses are in the element solution coordinate systems.
Initial-state data are at the element integration points.

The converted data is saved in the database and can be used in a subsequent analysis with additional user defined solution controls, loads, and boundary conditions.

The INISTATE command can be used to write, read, list, and delete the converted data.

The following limitations for EENS apply:

To obtain detailed element results in both in-plane and thickness directions, consider using advanced layer data storage option (KEYOPT(8) = 1 or 2) and full integration option (KEYOPT(3) = 2) for SHELL181.
When meshed with SHELL181 elements, the surface normal directions are approximated by averaging the element normal directions at the shared nodes. The advanced curved-shell formulation (KEYOPT(5) = 1) is required to incorporate the computation of surface normal directions. A refined SHELL181 mesh may be required at the high curvature regions.
The recovered curvatures at a SHELL181 element with degenerated triangular shape may not be accurate, especially when these elements are located at the structure's boundaries.
The stresses are computed with elastic material properties. If nonlinear materials are defined, only the linear material behaviors are accounted for in the EENS command.
Both isotropic and orthotropic materials are supported. See the Element Reference for more details on the element coordinate systems in which the material properties are evaluated.
The EMODIF command is not recommended for the generation of SHELL181 elements due to the insufficient geometric information for the EENS command.

Menu Paths

This command cannot be accessed from a menu.