For surface bodies, stress and strain results at the top and bottom faces are displayed simultaneously, by default. (See Understanding Surface Body Shell Offsets for information on identifying the top and bottom faces.) The contours vary linearly through the thickness from the top face to the bottom face. However you can choose to display only the , , or stress/strains in the Details view of the result item. Selecting Top, Middle, or Bottom will display the result at the selected location as a uniform contour through the thickness.
Middle Stresses
Normal and Shear results
The middle stresses are calculated at the shell mid-surface or at each layer mid-surface if layers are present. The Middle option for Shell gives the actual result values at the mid-surface if the solver was directed to calculate these results. In Mechanical APDL terminology, the solver computes results at mid-surface if KEYOPT(8) for the shell element is set to at the time of element creation. Otherwise, the results are computed as the average of the and results, that is, ( + ) / 2. Note that these results are valid only for linear analyses.
Equivalent and Principal results
These results are derived from the Normal and Shear results. Hence the Normal and Shear component results for are computed first, and then the Equivalent and Principal results are derived.
Element Nodal results (like stress/strain), as well as EDIR- and PNUM-type Elemental results, can be plotted on a specific layer or on a specific ply by entering the desired Layer number (Layer only) or by scoping the result to a specific Ply using the Sub Scope By property in the Details view of the result object. Elemental results outputting volume or energy are calculated for the entire element, regardless of the requested layer.
If the Layer specified does not exist for a particular surface body, the display of the result will be translucent with zero values for minimums and maximums on that body. If you enter 0 for Layer, it defaults to the Entire Section.
Note:
A Layer number must be specified to calculate the Middle stresses and strains. If you set Layer to 0 (Entire Section) while Shell is Middle, the Shell option will become invalid. Similarly, if you have Layer set to Entire Section and you try to set Shell to Middle, Shell will become invalid.
If there is a Layered Section in the model, convergence is not supported for results.
If Layer is Entire Section, Top stresses and strains are for the top surface of the topmost layer and the Bottom stresses and strains are for the outer surface of the bottom layer.
If a Layered Section is present in the model and you enter a number larger than the maximum number of layers that exists in the model, the Layer field will become invalid.
All stress tool results and all fatigue tool results are unsupported if Layered Sections are present in the model.
Only results from the section top and bottom are available on hyperelastic layered shells. Thus no results will be reported on such bodies if the layer is not set to 0 "Entire Section".
Imported Plies are not supported for an Explicit Dynamics analysis.
Layered Solid Body Results
Certain solid elements in the Mechanical APDL element library (including SOLID185, SOLID186, and SOLSH190) support stress and strain results on layers. These layered solid elements are created on solid bodies.
At Release 16.0, these elements support the Layer property, which specifies the layer to calculate Shell result values. This property specifies a Layer number. In addition, the Position property appears only for stress and strain results scoped to surface bodies or to a layer. This property is specified as either , , , or .
For the elements, the convention is that the Bottom corresponds to nodes I-J-K-L and the Top corresponds to nodes M-N-O-P.
Note: If the model does not include surface bodies or layered sections, the Layer and Position properties do not display in the Details view and the application displays layer results in format.
For Explicit Dynamics Layer Results
Normal/shear stresses and strains are available in global and solution coordinate systems.
Stress and strain results for individual layers may be selected by using the Layer property in the result’s Details view. Only a single result is available per layer.