Product: ABAQUS/Standard
User subroutine DLOAD:
can be used to define the variation of the distributed load magnitude as a function of position, time, element number, load integration point number, etc.;
will be called at each load integration point for each element-based or surface-based nonuniform distributed load definition during stress analysis;
will be called at each stiffness integration point for computing the effective axial force, ESF1, for pipe elements subjected to nonuniform load types PENU and PINU;
cannot be used in mode-based procedures to describe the time variation of the load; and
ignores any amplitude references that may appear with the associated step definition or nonuniform distributed load definition.
SUBROUTINE DLOAD(F,KSTEP,KINC,TIME,NOEL,NPT,LAYER,KSPT,
1 COORDS,JLTYP,SNAME)
C
INCLUDE 'ABA_PARAM.INC'
C
DIMENSION TIME(2), COORDS (3)
CHARACTER*80 SNAME
user coding to define F
RETURN
ENDF
Magnitude of the distributed load. Units are FL–2 for surface loads and FL–3 for body forces. F will be passed into the routine as the magnitude of the load specified as part of the element-based or surface-based distributed load definition. If the magnitude is not defined, F will be passed in as zero. For a static analysis that uses the modified Riks method (“Static stress analysis,” Section 6.2.2 of the ABAQUS Analysis User's Manual) F must be defined as a function of the load proportionality factor, 
. The distributed load magnitude is not available for output purposes.
KSTEP
Step number.
KINC
Increment number.
TIME(1)
Current value of step time or current value of the load proportionality factor, , in a Riks step.
TIME(2)
Current value of total time.
NOEL
Element number.
NPT
Load integration point number within the element or on the element's surface, depending on the load type. (Stiffness integration point number while computing effective axial force, ESF1, for pipe elements subjected to load types PENU and PINU.)
LAYER
Layer number (for body forces in layered solids).
KSPT
Section point number within the current layer.
COORDS
An array containing the coordinates of the load integration point. These are the current coordinates if geometric nonlinearity is accounted for during the step (see “Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis User's Manual); otherwise, the array contains the original coordinates of the point. For axisymmetric elements that allow nonaxisymmetric deformation, COORDS(3) is the angular position of the integration point, in degrees.
JLTYP
Identifies the load type for which this call to DLOAD is being made. The load type may be a body force, a surface-based load, or an element-based surface load. For element-based surface loads, this variable identifies the element face for which this call to DLOAD is being made. This information is useful when several different nonuniform distributed loads are being imposed on an element at the same time. See Part VI, “Elements,” of the ABAQUS Analysis User's Manual for element face identification. The key is as follows:
SNAME
Surface name for a surface-based load definition (JLTYP=0). For a body force or an element-based surface load the surface name is passed in as blank.