PSMESH
PSMESH, SECID, Name, P0, Egroup, NUM, KCN, KDIR, VALUE, NDPLANE, PSTOL, PSTYPE, ECOMP, NCOMP
Creates and meshes a pretension section
(PRETS179) or a preload section
(MPC184).
-
SECID Unique section number. This number must not already be assigned to a section.
-
Name Unique eight character descriptive name, if desired.
-
P0 Pretension node number (for a pretension section using PRETS179) or joint element number (for a preload section using MPC184).
For a pretension element, the node is defined if it doesn't exist, and the number defaults to the highest node number plus one.
For a joint element, a unique element number is assigned by default.
-
Egroup,NUM Element group on which PSMESH will operate. If
Egroup= P, graphical picking is enabled andNUMis ignored (valid only in the GUI).L (or LINE)
—
PSMESH operates on all elements in the line specified by
NUM. New pretension nodes are associated withNUMor entities below it. Any subsequent LCLEAR operation ofNUMdeletes the pretension elements and nodes created by PSMESH. (MPC184 joint elements and associated contact pairs of a preload section are not deleted by LCLEAR.)A (or AREA)
—
PSMESH operates on all elements in the area specified by
NUM. New pretension nodes are associated withNUMor entities below it. Any subsequent ACLEAR ofNUMdeletes the pretension elements and nodes created by PSMESH. (MPC184 joint elements and associated contact pairs of a preload section are not deleted by ACLEAR.)V (or VOLU)
—
PSMESH operates on all elements in the volume specified by
NUM. New pretension nodes are associated withNUMor entities below it. Any subsequent VCLEAR ofNUMdeletes the pretension elements and nodes created by PSMESH. (MPC184 joint elements and associated contact pairs of a preload section are not deleted by VCLEAR.)P
—
PSMESH operates on elements selected through the subsequent picking operations, and
NUMis ignoredALL
—
The command operates on all selected elements, and
NUMis ignored.-
KCN Coordinate system number for the separation surface and normal direction.
-
KDIR Direction (x, y, or z) normal to separation surface in the
KCNcoordinate system.If
KCNis Cartesian, the pretension section normal will be parallel to theKDIRaxis regardless of the position of the pretension node.If
KCNis non-Cartesian, the pretension section normal will be aligned with theKDIRdirection of systemKCNat the position of the pretension node.For an MPC184 joint element defined as part of a preload section,
KDIRis used to define the normal of the separation surface and does not affect the axis direction of the joint element.-
VALUE Point along the
KDIRaxis at which to locate the separation surface. Ignored ifNDPLANEis supplied.-
NDPLANE Existing node that PSMESH will use to locate the separation surface. If
NDPLANEis supplied, the location of the separation surface is defined by theKDIRcoordinate ofNDPLANE.-
PSTOL 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 byPSTOL. The following expression represents the default value:where ΔX, ΔY, and ΔZ are the dimensions of the locally selected region of the model based on nodal locations (that is, ΔX = X
max- Xmin).-
PSTYPE Type of pretension or preload section to be generated.
If a positive value is specified (or if this argument is left blank), a pretension section that includes PRETS179 elements is generated. The value entered is the element type number for PRETS179. If no number is specified, the program defines the element type number.
If TORQUE is specified, a preload section that includes a cylindrical joint element (MPC184) is generated as follows:
For a 2D model: An x-axis cylindrical joint element is generated along with two force-distributed surface-based constraints. A local Cartesian coordinate system is created at the first node of the joint element such that the local x- axis is the axis of that element (KEYOPT(4) = 0 for the MPC184 element).
For a 3D model: A z-axis cylindrical joint element is generated along with two force-distributed surface-based constraints. A local Cartesian coordinate system is created at the first node of the joint element such that the local z- axis is the axis of that element (KEYOPT(4) = 1 for the MPC184 element).
For a 3D model that contains beam elements: A z-axis cylindrical joint element is generated between the endpoints of two beam elements. (No force-distributed surface-based constraints are needed.) A local Cartesian coordinate system is created at the first node of the joint element such that the local z- axis is the axis of that element (KEYOPT(4) = 1 for the MPC184 element).
If a negative value is specified, a preload section that includes a screw joint element (MPC184) is created with the absolute value of
PSTYPEused as the pitch value for the joint. This option is only valid for 3D models. Two force-distributed surface-based constraints are generated at the cutting surfaces, except for the case of a beam model which does not need the force-distributed constraints. A local Cartesian coordinate system is created at the first node of the joint element such that the local z- axis is the axis of that element.-
ECOMP If specified, the name of a component to be composed of new pretension elements and existing elements modified by the PSMESH command. This argument is not used with the MPC184 joint element.
-
NCOMP Name of a component to be composed of nodes on new pretension elements. This argument is not used with the MPC184 joint element.
Notes
PSMESH generates a pretension section
(PRETS179) or a preload section (MPC184) for
modeling bolt fastener preloads. The type of section is specified by the
PSTYPE argument.
The PSMESH command is valid for structural analyses only.
Pretension Section (PRETS179)
When PSTYPE is a positive value or blank,
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
VALUE or NDPLANE and inserting
PRETS179 elements. The PSMESH command verifies that
PSTYPE is a PRETS179 element type; if it is
not, the command finds the lowest available ITYPE
(ET) that is PRETS179, or it creates a new one if
necessary.
When it is necessary to define the pretension node, the program uses node
NDPLANE. If the NDPLANE value is not
specified, the program defines the pretension node at:
The centroid of geometric entity
NUM, ifEgroup= LINE, AREA, or VOLU; orThe 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 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.
A pretension section can be defined for fastener models made up of any 2D or 3D structural solid, beam, shell, pipe, or link element type. The elements can be low- or high-order.
The pretension section is also supported for general axisymmetric elements (SOLID272 and SOLID273). PSMESH cuts the model and generates PRETS179 elements between all Fourier nodes in the circumferential direction.
For more information, see Defining Pretension in a Joint Fastener in the Basic Analysis Guide.
Preload Section (MPC184)
When PSTYPE is a negative value or set to
TORQUE, the PSMESH command defines an MPC184 joint
element for applying a preload to a bolt undergoing large rotation or large deformation.
PSMESH cuts the mesh in two parts along existing element boundaries at the
point defined by VALUE or NDPLANE. It
generates force-distributed surface-based constraints
(remote points) on the cutting surfaces, inserts an MPC184 joint element
that connects the two pilot nodes, and creates a local Cartesian coordinate system at the first
node of the joint element to define the normal direction. If the joint is between beam elements,
no force-distributed constraints are generated. For more information, see Defining Preload in a Joint Fastener Undergoing Large Rotation in the Basic Analysis Guide.
The preload section based on MPC184 is not supported for general axisymmetric elements (SOLID272 and SOLID273).