<!-- source-page: 41 -->

# JDOF

Degree of freedom.

# COORDS

An array containing the current coordinates of this point. These are the coordinates at the end of the prior increment if geometric nonlinearity is accounted for during the step (see “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User’s Guide); otherwise, the array contains the original coordinates of the node. This array cannot be used if user subroutine DISP is used to prescribe connector motions.

<!-- source-page: 42 -->

<!-- source-page: 43 -->

# 1.1.5 DLOAD: User subroutine to specify nonuniform distributed loads.

# Product: Abaqus/Standard

# References

• “Distributed loads,” Section 34.4.3 of the Abaqus Analysis User’s Guide   
• \*DLOAD   
• \*DSLOAD   
• “Nonuniform crack-face loading and J -integrals,” Section 1.16.7 of the Abaqus Benchmarks Guide   
• “Pure bending of a cylinder: CAXA elements,” Section 1.3.33 of the Abaqus Verification Guide   
• “Cylinder subjected to asymmetric pressure loads: CAXA elements,” Section 1.3.35 of the Abaqus Verification Guide   
• “Patch test for axisymmetric elements,” Section 1.5.4 of the Abaqus Verification Guide   
• “Transient internal pressure loading of a viscoelastic cylinder,” Section 2.2.9 of the Abaqus Verification Guide   
• “DLOAD,” Section 4.1.3 of the Abaqus Verification Guide

# Overview

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.

# User subroutine interface

```txt
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) 
```

<!-- source-page: 44 -->

# CHARACTER\*80 SNAME

user coding to define F

# RETURN

# END

# Variable to be defined

F

Magnitude of the distributed load. Units are $\mathrm { F L } ^ { - 2 }$ for surface loads and $\mathrm { F L } ^ { - 3 }$ for body forces. F will be passed into the routine as the magnitude of the load specified as part of the element-based or surfacebased 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 Guide) F must be defined as a function of the load proportionality factor, . The distributed load magnitude is not available for output purposes.

# Variables passed in for information

# 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.

<!-- source-page: 45 -->

# 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 “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User’s Guide); 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 Guide for element face identification. The key is as follows:

<table><tr><td>JLTYP</td><td>Load type</td></tr><tr><td>0</td><td>Surface-based load</td></tr><tr><td>1</td><td>BXNU</td></tr><tr><td>1</td><td>BRNU</td></tr><tr><td>2</td><td>BYNU (except for axisymmetric elements)</td></tr><tr><td>2</td><td>BZNU (for axisymmetric elements only)</td></tr><tr><td>3</td><td>BZNU (for three-dimensional elements and asymmetric-axisymmetric elements)</td></tr><tr><td>20</td><td>PNU</td></tr><tr><td>21</td><td>P1NU</td></tr><tr><td>22</td><td>P2NU</td></tr><tr><td>23</td><td>P3NU</td></tr><tr><td>24</td><td>P4NU</td></tr><tr><td>25</td><td>P5NU</td></tr><tr><td>26</td><td>P6NU</td></tr><tr><td>27</td><td>PINU</td></tr><tr><td>28</td><td>PENU</td></tr><tr><td>41</td><td>PXNU</td></tr><tr><td>42</td><td>PYNU</td></tr><tr><td>43</td><td>PZNU</td></tr></table>

<!-- source-page: 46 -->

# 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.

<!-- source-page: 47 -->

# 1.1.6 FILM: User subroutine to define nonuniform film coefficient and associated sink temperatures for heat transfer analysis.

# Product: Abaqus/Standard

# References

• “Thermal loads,” Section 34.4.4 of the Abaqus Analysis User’s Guide   
• \*CFILM   
• \*FILM   
• \*SFILM   
• “Temperature-dependent film condition,” Section 1.3.42 of the Abaqus Verification Guide

# Overview

# User subroutine FILM:

• can be used to define a node-based, element-based, or surface-based nonuniform film coefficient;   
• can be used to define sink temperatures as functions of position, time, temperature, node number, element number, integration point number, etc.;   
• will be called during procedures that allow heat transfer analysis at each node or surface integration point of those surfaces and elements for which node-based, element-based, or surface-based nonuniform film conditions are defined;   
• ignores any amplitude references for the sink temperature or film coefficient that may appear with the associated nonuniform film definition; and   
• uses the nodes for first-order heat transfer elements as surface integration points for both elementbased and surface-based films.

# User subroutine interface

```fortran
SUBROUTINE FILM(H, SINK, TEMP, KSTEP, KINC, TIME, NOEL, NPT, 1 COORDS, JLTYP, FIELD, NFIELD, SNAME, NODE, AREA)
C
INCLUDE 'ABA_PARAM.INC'
C
DIMENSION H(2), TIME(2), COORDS(3), FIELD(NFIELD)
CHARACTER*80 SNAME
user coding to define H(1), H(2), and SINK
RETURN
END 
```

<!-- source-page: 48 -->

# Variables to be defined

# H(1)

Film coefficient at this point. Units are $\mathrm { J } \mathrm { T } ^ { - 1 } \mathrm { L } ^ { - 2 } \theta ^ { - 1 }$ . H(1) will be passed into the routine as the magnitude of the film coefficient specified as part of the node-based, element-based, or surface-based film condition definition. If the magnitude is not defined, H(1) will be initialized to zero.

# H(2)

$d h / d \theta _ { ; }$ , rate of change of the film coefficient with respect to the surface temperature at this point. Units are $\mathrm { J } \mathrm { T } ^ { - 1 } \mathrm { L } ^ { - 2 } \theta ^ { - 2 }$ . The rate of convergence during the solution of the nonlinear equations in an increment is improved by defining this value, especially when the film coefficient is a strong function of surface temperature.

# SINK

Sink temperature. SINK will be passed into the routine as the sink temperature specified as part of the node-based, element-based, or surface-based film condition definition. If the sink temperature is not defined, SINK will be initialized to zero.

# Variables passed in for information

# TEMP

Estimated surface temperature at this time at this point.

# KSTEP

Step number.

# KINC

Increment number.

# TIME(1)

Current value of step time.

# TIME(2)

Current value of total time.

# NOEL

Element number. This variable is passed in as zero for node-based films.

# NPT

Surface integration point number. This variable is passed in as zero for node-based films.

# COORDS

An array containing the coordinates of this point. These are the current coordinates if geometric nonlinearity is accounted for during the step (see “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User’s Guide); otherwise, the array contains the original coordinates of the point.

<!-- source-page: 49 -->

# JLTYP

Identifies the element face for which this call to FILM is being made for an element-based film coefficient specification. This information is useful when several different nonuniform film conditions are being imposed on an element at the same time. See Part VI, “Elements,” of the Abaqus Analysis User’s Guide for element face identification. The key is as follows:

<table><tr><td>JLTYP</td><td>Film type</td></tr><tr><td>0</td><td>Node-based or surface-based loading</td></tr><tr><td>11</td><td>F1NU (FNEGNU for heat transfer shells)</td></tr><tr><td>12</td><td>F2NU (FPOSNU for heat transfer shells)</td></tr><tr><td>13</td><td>F3NU</td></tr><tr><td>14</td><td>F4NU</td></tr><tr><td>15</td><td>F5NU</td></tr><tr><td>16</td><td>F6NU</td></tr></table>

# FIELD

Interpolated values of field variables at this point.

# NFIELD

Number of field variables.

# SNAME

Surface name for which this call to FILM is being made for a surface-based film coefficient specification (JLTYP=0). This variable is passed in as blank for both node-based and element-based films.

# NODE

Node number. This variable is passed in as zero for both element-based and surface-based films.

# AREA

Nodal area for node-based films. AREA will be passed into the routine as the nodal area specified as part of the node-based film coefficient specification. This nodal area is not available for output purposes. This variable is passed in as zero for both element-based and surface-based films.

<!-- source-page: 50 -->
