Generates elements by symmetry reflection.
Increment to be added to element numbers in existing set.
Increment nodes in the given pattern by
Reflect elements from pattern beginning with
IEL1) in steps of
to 1). If
IEL1 = ALL,
ignored and pattern is all selected elements [ESEL]. If
P, graphical picking is enabled and all remaining command fields are ignored
(valid only in the GUI). A component name may also be substituted for
IEINC are ignored).
This command is the same as the ESYM command except
it allows explicitly assigning element numbers to the generated set (in terms
of an increment
IINC). Any existing elements already
having these numbers will be redefined.
The operation generates a new element by incrementing the nodes on the original element, and reversing and shifting the node connectivity pattern. For example, for a 4-node 2-D element, the nodes in positions I, J, K and L of the original element are placed in positions J, I, L and K of the reflected element.
Similar permutations occur for all other element types. For line elements, the nodes in positions I and J of the original element are placed in positions J and I of the reflected element. In releases prior to ANSYS 5.5, no node pattern reversing and shifting occurred for line elements generated by ENSYM. To achieve the same results as you did in releases prior to ANSYS 5.5, use the ENGEN command instead.
See the ESYM command for additional information about symmetry elements.
The ENSYM command also provides a convenient way
to reverse shell element normals. If the
fields are left blank, the effect of the reflection is to reverse the direction
of the outward normal of the specified elements. You cannot use the ENSYM command
to change the normal direction of any element that has a body or surface load.
We recommend that you apply all of your loads only after ensuring
that the element normal directions are acceptable. Also note that real constants
(such as nonuniform shell thickness and tapered beam constants) may be invalidated
by an element reversal. See Revising
Your Model in the Modeling and Meshing Guide for more information about
controlling element normals.