SIGINI
User subroutine to define an initial stress field.
Product: Abaqus/Standard
References
“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1 of the Abaqus Analysis User's Manual
*INITIAL CONDITIONS
Overview
User subroutine SIGINI:
will be called for user-subroutine-defined initial stress fields at particular material points (these are the effective stress values for soils analysis);
is called at the start of the analysis for each applicable material calculation point in the model; and
can be used to define all active initial stress components at material points as functions of coordinates, element number, integration point number, etc.
Stress components
The number of stress components that must be defined depends on the element type for which this call is being made. Part VI, “Elements,” of the Abaqus Analysis User's Manual,” describes the element stresses. The order in which the components must be defined is the same as in the element definition. For example, in three-dimensional continuum elements six stress components must be defined in the order
Initial stress field equilibrium
You should ensure that the initial stress field is in equilibrium with the applied forces and distributed loads by using a static step or a geostatic step to check the equilibrium of the initial stress field before starting the response history. See “Geostatic stress state,” Section 6.8.2 of the Abaqus Analysis User's Manual, for a discussion of defining initial equilibrium conditions for problems that include pore fluid pressure.
User subroutine interface
SUBROUTINE SIGINI(SIGMA,COORDS,NTENS,NCRDS,NOEL,NPT,LAYER,
1 KSPT,LREBAR,NAMES)
C
INCLUDE 'ABA_PARAM.INC'
C
DIMENSION SIGMA(NTENS),COORDS(NCRDS)
CHARACTER NAMES(2)*80
user coding to define SIGMA(NTENS)
RETURN
END
Variables to be defined
SIGMA(1)
First stress component.
SIGMA(2)
Second stress component.
SIGMA(3)
Third stress component.
Etc.
Only NTENS stress values should be defined, where NTENS depends on the element type.
Variables passed in for information
COORDS
An array containing the initial coordinates of this point.
NTENS
Number of stresses to be defined, which depends on the element type.
NCRDS
Number of coordinates.
NOEL
Element number.
NPT
Integration point number in the element.
LAYER
Layer number (for composite shells and layered solids).
KSPT
Section point number within the current layer.
LREBAR
Rebar flag. If LREBAR=1, the current integration point is associated with element rebar. Otherwise, LREBAR=0.
NAMES(1)
Name of the rebar to which the current integration point belongs, which is the name given in the rebar or rebar layer definition (“Defining reinforcement,” Section 2.2.3 of the Abaqus Analysis User's Manual, or “Defining rebar as an element prop
erty,” Section 2.2.4 of the Abaqus Analysis User's Manual). If no name was given in the rebar or rebar layer definition, this variable will be blank. This variable is relevant only when LREBAR=1.
NAMES(2)
Element type name (see Section EI.1, “Abaqus/Standard Element Index,” of the Abaqus Analysis User's Manual).