step11.ORIENT子程序的使用说明

1.1.15 ORIENT
User subroutine to provide an orientation for defining local material directions or local directions for kinematic coupling constraints or local rigid body directions for inertia relief.
Product: Abaqus/Standard
References
∙“Orientations,” Section 2.2.5 of the Abaqus Analysis User's Manual ∙*ORIENTATION
∙“Eigenvalue analysis of a piezoelectric transducer,” Section 7.1.1 of the Abaqus Example Problems Manual
Overview
User subroutine ORIENT:
∙will be called at the start of the analysis at each location (material point, special-purpose element, coupling node, or
reference point for inertia relief) for which local directions are defined with a user-subroutine-defined orientation;
∙is used to define the direction cosines of a local system of (material) directions with respect to the default basis directions (default basis directions are defined as the global directions for continuum elements and as the default surface directions for shell, membrane, and surface elements, as described in “Conventions,”
Section 1.2.2 of the Abaqus Analysis User's Manual);
∙can be used to define the direction cosines orienting the layer of reinforcing material in membrane, shell, or surface elements (see “Defining reinforcement,” Section 2.2.3 of the Abaqus Analysis
User's Manual);
∙can be used to provide a local system for defining the direction of action of rotary inertia, spring, dashpot, flexible join t, and elastic-plastic joint elements;
∙can be used with gasket elements to define the local in-plane directions for three-dimensional area and three-dimensional link elements that consider transverse shear and membrane deformations
(see “Defining the gasket behavior directly using a gasket behavior model,” Section 31.6.6 of the Abaqus Analysis User's Manual);
∙can be used to define a local system in which coupling constraints are applied (see “Coupling constraints,” Section 33.3.2 of the
Abaqus Analysis User's Manual, and “Kinematic coupling
constraints,” Section 33.2.3 of the Abaqus Analysis User's Manual);
∙can be used to define a local system at the reference point for the rigid body directions in which inertia relief loads are applied for the entire model (see “Inertia relief,” Section 11.1.1 of the Abaqus Analysis User's Manual);
∙will ignore rotation angles defined for layers of composite solids (see “Solid (continuum) elements,” Section 27.1.1 of the Abaqus Analysis User's Manual) but will take into account rotation angles defined for layers of composite shells (see “Using a shell section integrated during the analysis to define the section behavior,”
Section 28.6.5 of the Abaqus Analysis User's Manual, and “Using a general shell section to define the section behavior,” Section
28.6.6 of the Abaqus Analysis User's Manual); and
∙ignores any data specified for the associated orientation definition outside the user subroutine.
The local directions defined by user subroutine ORIENT must be specified relative to the default basis directions.
User subroutine interface
SUBROUTINE ORIENT(T,NOEL,NPT,LAYER,KSPT,COORDS,BASIS,
1 ORNAME,NNODES,CNODES,JNNUM)
C
INCLUDE 'ABA_PARAM.INC'
C
CHARACTER*80 ORNAME
C
DIMENSION T(3,3),COORDS(3),BASIS(3,3),CNODES(3,NNODES)
DIMENSION JNNUM(NNODES)
user coding to define T
RETURN
END
Variable to be defined
T
An array containing the direction cosines of the preferred orientation in terms of the default basis directions. T(1,1), T(2,1), T(3,1) give the (1, 2, 3) components of the first direction; T(1,2), T(2,2), T(3,2) give the second direction; etc. For shell and membrane elements only the first and second directions are used. The directions do not have to be normalized. If the second direction is not orthogonal to the first direction, Abaqus/Standard will orthogonalize and normalize the second direction with respect to the first. The third direction is then determined by taking the cross product of the first and second directions. For planar elements the first two directions must lie in the plane of the element.
For use with coupling constraints (“Coupling constraints,” Section 33.3.2 of the Abaqus Analysis User's Manual), the local basis directions are used as the local constraint directions for application of the kinematic constraint.
For use with inertia relief loads, the local basis directions are used as the rigid body direction vectors for computing the loads.
Variables passed in for information
NOEL
Element number. This value is zero when the subroutine is called for use with coupling constraints or inertia relief loads.
NPT
Integration point number. This variable is set only for relevant uses. LAYER
Layer number (for composite shells and layered solids). This variable is set only when relevant. It is equal to zero when it is irrelevant, such as in a regular solid element or in a shell element when transverse shear stiffness calculations are performed.
KSPT
Section point number within the current layer. This variable is set only when relevant. It is equal to zero when it is irrelevant, such as in a regular solid element or in a shell element when transverse shear stiffness calculations are performed.
COORDS
An array containing the initial coordinates of this point. This array contains the coordinates of the reference point for inertia relief loads.
BASIS
An array containing the direction cosines of the normal material basis directions in terms of the global coordinates in the original configuration. BASIS(1,1), BASIS(2,1), BASIS(3,1) give the 1-direction, etc. This is useful only in shells or membranes since in all other cases the basis is the global coordinate system.
ORNAME
User-specified orientation name, left justified, with one exception. When an overall section orientation is specified for a composite solid or shell section and the individual layer orientations are specified by an orientation angle, Abaqus defines an internal orientation name to represent the actual orientation of the layer. To avoid internal names, provide an orientation name rather than an orientation angle as part of the layer definition for each individual layer of a composite section.
NNODES
Number of element nodes. This value is two when the subroutine is called for use with a kinematic coupling definition, where the two nodes are the reference and current coupling node. When used with a distributing coupling definition, this number is equal to the number of coupling nodes plus one for the reference node. It is one when used with inertia relief loads since the local basis is defined at the reference point.
CNODES
An array containing the original coordinates of the nodes. When used with a kinematic coupling definition, the first entry defines the reference node coordinates, and the second entry defines the coupling node coordinates. When used with a distributing coupling definition, the first
entry defines the reference node coordinates, and the subsequent entries define the coupling node coordinates in the order defined by the JNNUM array. When used with inertia relief loads, this array is not used. For all other uses the entry order follows that of the element definition node ordering.
JNNUM
An array containing the NNODES node numbers. When used with a kinematic coupling definition, the first entry is the reference node number, and the second entry is the node number for the current coupling node. When used with a distributing coupling definition, the first entry is the reference node number followed by the node numbers of all coupling nodes. When used with inertia relief loads, this array is not used. For all other uses the entry order follows that of the element definition node ordering.。