Create and mesh a pretension section
Unique section number. This number must not already be assigned to a section.
Unique eight character descriptive name, if desired.
Pretension node number. The node will be defined if it doesn't exist and the number defaults to the highest node number plus one.
Element group on which PSMESH will
Egroup = P, graphical picking
is enabled and
NUM is ignored (valid only
in the GUI).
L (or LINE)
PSMESH operates on all elements in the line specified by
A (or AREA)
PSMESH operates on all elements in the area specified by
V (or VOLU)
PSMESH operates on all elements in the volume specified by
PSMESH operates on
elements selected through the subsequent picking operations, and
The command operates on all selected
Coordinate system number for the separation surface and normal direction.
Direction (x, y, or z) normal to separation surface
KCN coordinate system.
KCN is cartesian, the pretension section
normal will be parallel to the
regardless of the position of the pretension node.
KCN is non-cartesian, the pretension
section normal will be aligned with the
KDR direction of system
KCN at the position
of the pretension node.
Point along the
at which to locate the separation surface. Ignored if
NDPLANE is supplied.
Existing node that PSMESH will
use to locate the separation surface. If
NDPLANE is supplied, the location of the separation surface is defined by
KDIR coordinate of
Optional tolerance below
VALUE. Allows nodes occurring precisely at or slightly below the separation
to be identified properly as above the plane. Has the effect of shifting
the plane down by
PSTOL. The following
expression represents the default value:
where ΔX, ΔY,
and ΔZ are the dimensions of the model based on nodal locations
(that is, ΔX = X
max - X
If specified, this value is the type number for pretension elements. (If not specified, ANSYS defines this value.) If already defined, it must be of type PRETS179.
If specified, the name of a component to be composed of new pretension elements and existing elements modified by the PSMESH command.
Name of a component to be composed of nodes on new pretension elements.
The PSMESH command creates a pretension section
normal to the pretension load direction by cutting the mesh along
existing element boundaries at the point defined by
NDPLANE and inserting PRETS179 elements. The PSMESH command
PSTYPE is PRETS179; if it is not, the command finds the lowest available
ITYPE that is PRETS179, or
if necessary will create a new one.
When it is necessary to define the pretension node, ANSYS uses
NDPLANE. If the
NDPLANE value is not specified, ANSYS defines the pretension node at:
The centroid of geometric entity
Egroup = LINE, AREA or VOLU
The centroid location of all selected elements, if
Egroup = ALL or if graphical picking is used.
If the elements to which the pretension load is to be applied have already been meshed in two groups, PSMESH cannot be used to insert the pretension elements. The EINTF command must be used to insert the PRETS179 elements between the two meshed groups.
The PSMESH operation copies any nodal temperatures you have defined on the split surface of the original mesh from the original nodes to the newly created coincident duplicate nodes. However, displacements, forces, and other boundary conditions are not copied.
By mathematical definition, the pretension surface must always
be a flat plane. In a non-Cartesian coordinate system, the PSMESH command creates that plane at the indicated position,
oriented with respect to the specified direction of the active system
(in the same manner that the NROTAT command orients
a nodal system with respect to a curved system). For example, assuming
a X = 1 and Y = 45 in a cylindrical coordinate system with Z as the
axis of rotation (
KCN = 1), a pretension
surface normal to X tilts 45 degrees away from the global X axis.
The PSMESH command is valid for structural analyses only.