Abaqus Keywords Reference Guide  
How to find keyword examples

*DLOAD
Specify distributed loads.

This option is used to prescribe distributed loading. It is also used to apply concentrated or distributed wind, wave, or buoyancy loading in an Abaqus/Aqua analysis or to apply general body, buoyancy, or porous drag force loading in Abaqus/CFD.

Products: Abaqus/Standard  Abaqus/Explicit  Abaqus/CFD  Abaqus/CAE  Abaqus/Aqua  

Type: History data

Level: Step

Abaqus/CAE: Load module

References:


Applying distributed loads

Required parameter for cyclic symmetry models in steady-state dynamics analyses: 

CYCLIC MODE

Set this parameter equal to the cyclic symmetry mode number of loads that are applied in the current steady-state dynamics procedure.

Optional parameters:

AMPLITUDE

Set this parameter equal to the name of the amplitude curve that defines the variation of the load magnitude during the step.

If this parameter is omitted for uniform load types in an Abaqus/Standard analysis, the reference magnitude is applied immediately at the beginning of the step or linearly over the step, depending on the value assigned to the AMPLITUDE parameter on the *STEP option (see “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User's Guide). If this parameter is omitted in an Abaqus/Explicit or an Abaqus/CFD analysis, the reference magnitude is applied immediately at the beginning of the step.

Amplitude references are ignored for nonuniform loads given by user subroutine DLOAD in an Abaqus/Standard analysis. Amplitude references are passed into user subroutine VDLOAD in an Abaqus/Explicit analysis.

Only the load magnitude is changed with time. Quantities such as the direction of an applied gravity load and the fluid surface level in hydrostatic pressure loading are not changed.

CONSTANT RESULTANT

Set CONSTANT RESULTANT=NO (default) if surface traction vectors, edge traction vectors, or edge moments are to be integrated over the surface in the current configuration.

Set CONSTANT RESULTANT=YES if surface traction vectors, edge traction vectors, or edge moments are to be integrated over the surface in the reference configuration.

The CONSTANT RESULTANT parameter is valid only for uniform and nonuniform surface tractions and edge loads (including edge moments); it is ignored for all other load types.

FOLLOWER

Set FOLLOWER=YES (default) if a prescribed traction or shell-edge load is to rotate with the surface or shell edge in a large-displacement analysis (live load).

Set FOLLOWER=NO if a prescribed traction or edge load is to remain fixed in a large-displacement analysis (dead load).

The FOLLOWER parameter is valid only for traction and edge load labels TRVECn, TRVEC, TRVECnNU, TRVECNU, EDLDn, and EDLDnNU. It is ignored for all other load labels.

OP

Set OP=MOD (default) for existing *DLOADs to remain, with this option modifying existing distributed loads or defining additional distributed loads.

Set OP=NEW if all existing *DLOADs applied to the model should be removed. New distributed loads can be defined.

ORIENTATION

Set this parameter equal to the name given for the *ORIENTATION option (“Orientations,” Section 2.2.5 of the Abaqus Analysis User's Guide) used to specify the local coordinates in which components of traction or shell-edge loads are specified.

The ORIENTATION parameter is valid only for traction and edge load labels TRSHRn, TRSHR, TRSHRnNU, TRSHRNU, TRVECn, TRVEC, TRVECnNU, TRVECNU, EDLDn, and EDLDnNU. It is ignored for all other load labels.

REF NODE

This parameter applies only to Abaqus/Explicit analyses and is relevant only for viscous and stagnation body force and pressure loads when the velocity at the reference node is used.

Set this parameter equal to either the node number of the reference node or the name of a node set containing the reference node. If the name of a node set is chosen, the node set must contain exactly one node. If this parameter is omitted, the reference velocity is assumed to be zero.

REGION TYPE

This parameter applies only to Abaqus/Explicit analyses.

This parameter is relevant only for pressure loads applied to the boundary of an adaptive mesh domain. If a distributed pressure load is applied to a surface in the interior of an adaptive mesh domain, the nodes on the surface will move with the material in all directions (they will be nonadaptive). Abaqus/Explicit will create a boundary region automatically on the surface subjected to the defined pressure load.

Set REGION TYPE=LAGRANGIAN (default) to apply the pressure to a Lagrangian boundary region. The edge of a Lagrangian boundary region will follow the material while allowing adaptive meshing along the edge and within the interior of the region.

Set REGION TYPE=SLIDING to apply the pressure load to a sliding boundary region. The edge of a sliding boundary region will slide over the material. Adaptive meshing will occur along the edge and in the interior of the region. Mesh constraints are typically applied on the edge of a sliding boundary region to fix it spatially.

Set REGION TYPE=EULERIAN to apply the pressure to an Eulerian boundary region. This option is used to create a boundary region across which material can flow. Mesh constraints must be used normal to an Eulerian boundary region to allow material to flow through the region. If no mesh constraints are applied, an Eulerian boundary region will behave in the same way as a sliding boundary region.

Optional, mutually exclusive parameters for matrix generation and steady-state dynamics analyses (direct, modal, or subspace): 

IMAGINARY

Include this parameter to define the imaginary (out-of-phase) part of the loading.

REAL

Include this parameter (default) to define the real (in-phase) part of the loading.

Data lines to define all distributed loads except those special cases described below: 

First line:

  1. Element number or element set label.

  2. Reference load magnitude, which can be modified by the use of the *AMPLITUDE option. For nonuniform loads the magnitude must be defined in user subroutine DLOAD for Abaqus/Standard and VDLOAD for Abaqus/Explicit. If given, this value will be passed into the user subroutine in an Abaqus/Standard analysis.

Repeat this data line as often as necessary to define distributed loads for different elements or element sets.

Data lines to define mechanical pore pressure loads (Abaqus/Standard only): 

First line:

  1. Element number or element set label.

  2. Distributed load type label PORMECHn.

  3. Scaling factor.

Repeat this data line as often as necessary to define mechanical pore pressure loading for different elements or element sets.

Data lines to define a general surface traction vector, a surface shear traction vector, or a general shell-edge traction vector: 

First line:

  1. Element number or element set label.

  2. Distributed load type label TRVECn, TRVEC, TRSHRn, TRSHR, EDLDn, TRVECnNU, TRVECNU, TRSHRnNU, TRSHRNU, or EDLDnNU.

  3. Reference load magnitude, which can be modified by using the *AMPLITUDE option.

  4. 1-component of the traction vector direction.

  5. 2-component of the traction vector direction.

  6. 3-component of the traction vector direction.

For a two-dimensional or axisymmetric analysis, only the first two components of the traction vector direction need to be specified. For the shear traction load labels TRSHRn, TRSHR, TRSHRnNU, or TRSHRNU, the loading direction is computed by projecting the specified traction vector direction down upon the surface in the reference configuration. For nonuniform loads in Abaqus/Standard the magnitude and traction vector direction must be defined in user subroutine UTRACLOAD. If given, the magnitude and vector will be passed into the user subroutine in an Abaqus/Standard analysis.

Repeat this data line as often as necessary to define traction vectors for different elements or element sets.

Data lines to define a surface normal traction vector, a shell-edge traction vector (in the normal, transverse, or tangent direction), or a shell-edge moment: 

First line:

  1. Element number or element set label.

  2. Distributed load type EDMOMn, EDNORn, EDSHRn, EDTRAn, EDMOMnNU, EDNORnNU, EDSHRnNU, or EDTRAnNU.

  3. Reference load magnitude, which can be modified by using the *AMPLITUDE option. For nonuniform loads in Abaqus/Standard the magnitude must be defined in user subroutine UTRACLOAD. If given, the magnitude will be passed into the user subroutine in an Abaqus/Standard analysis.

Repeat this data line as often as necessary to define traction vectors for different elements or element sets.

Data lines to define centrifugal loads and Coriolis forces (Abaqus/Standard only): 

First line:

  1. Element number or element set label.

  2. Distributed load type label CENTRIF, CENT, or CORIO.

  3. Actual magnitude of the load, which can be modified by the use of the *AMPLITUDE option.

  4. Coordinate 1 of a point on the axis of rotation.

  5. Coordinate 2 of a point on the axis of rotation.

  6. Coordinate 3 of a point on the axis of rotation.

  7. 1-component of the direction cosine of the axis of rotation.

  8. 2-component of the direction cosine of the axis of rotation.

  9. 3-component of the direction cosine of the axis of rotation.

For axisymmetric elements the axis of rotation must be the global y-axis, which must be specified as 0.0, 0.0, 0.0, 0.0, 1.0, 0.0.

Repeat this data line as often as necessary to define centrifugal or Coriolis forces for different elements or element sets.

Data lines to define rotary acceleration loads (Abaqus/Standard only): 

First line:

  1. Element number or element set label.

  2. Distributed load type label ROTA.

  3. Actual magnitude of the load, which can be modified by the use of the *AMPLITUDE option.

  4. Coordinate 1 of a point on the axis of rotary acceleration.

  5. Coordinate 2 of a point on the axis of rotary acceleration.

  6. Coordinate 3 of a point on the axis of rotary acceleration.

  7. 1-component of the direction cosine of the axis of rotary acceleration.

  8. 2-component of the direction cosine of the axis of rotary acceleration.

  9. 3-component of the direction cosine of the axis of rotary acceleration.

For two-dimensional elements the axis of rotation direction must be the global z-axis (out of the plane of the model), which must be specified as 0.0, 0.0, 1.0.

Repeat this data line as often as necessary to define rotary acceleration loading for different elements or element sets.

Data lines to define rotordynamic loads (Abaqus/Standard only): 

First line:

  1. Element number or element set label.

  2. Distributed load type label ROTDYNF.

  3. Actual magnitude of the load, which can be modified by the use of the *AMPLITUDE option.

  4. Coordinate 1 of a point on the axis of rotation.

  5. Coordinate 2 of a point on the axis of rotation.

  6. Coordinate 3 of a point on the axis of rotation.

  7. 1-component of the direction cosine of the axis of rotation.

  8. 2-component of the direction cosine of the axis of rotation.

  9. 3-component of the direction cosine of the axis of rotation.

Rotordynamic loads are supported only for three-dimensional continuum and cylindrical elements, shell elements, membrane elements, beam elements, and rotary inertia elements. The spinning axis defined as part of the load must be the axis of symmetry for the structure. Therefore, beam elements must be aligned with the symmetry axis. In addition, one of the principal directions of each loaded rotary inertia element must be aligned with the symmetry axis, and the inertia components of the rotary inertia elements must be symmetric about this axis.

Repeat this data line as often as necessary to define rotordynamic loads for different elements or element sets.

Data lines to define gravity loading: 

First line:

  1. The element number or element set label is optional for gravity loads. If this field is left blank in an Abaqus/Standard or Abaqus/Explicit analysis, all elements in the model that have mass contributions (including point mass elements) are automatically included in an element set called _Whole_Model_Gravity_Elset and the gravity load is applied to all elements in this element set. If this field is left blank in an Abaqus/CFD analysis, the gravity load is applied to all user-defined element sets.

  2. Distributed load type label GRAV.

  3. Actual magnitude of the load, which can be modified by the use of the *AMPLITUDE option.

  4. 1-component of the gravity vector.

  5. 2-component of the gravity vector.

  6. 3-component of the gravity vector.

For axisymmetric elements the gravity load must be in the z-direction; therefore, only component 2 should be nonzero. For Abaqus/CFD gravity loading defines the gravity vector used with a Boussinesq-type body force in buoyancy driven flow (see “Specifying gravity loading” in “Distributed loads,” Section 34.4.3 of the Abaqus Analysis User's Guide).

Repeat this data line as often as necessary to define gravity loading for different elements or element sets.

Data lines to define porous drag load (Abaqus/CFD only): 

First line:

  1. Element number or element set label.

  2. Distributed load type label PDBF.

  3. Value of the porosity, which can be modified by the use of the *AMPLITUDE option.

Repeat this data line as often as necessary to define porous drag body force loads for different elements or element sets.

Data lines to define external and internal pressure in pipe or elbow elements: 

First line:

  1. Element number or element set label.

  2. Distributed load type label PE, PI, PENU, or PINU.

  3. Actual magnitude of the load, which can be modified by the use of the *AMPLITUDE option. For nonuniform loads the magnitude must be defined in user subroutine DLOAD.

  4. Effective inner or outer diameter.

Repeat this data line as often as necessary to define internal or external pressure loading for different pipe or elbow elements or element sets.

Data lines to define hydrostatic pressure (Abaqus/Standard only): 

First line:

  1. Element number or element set label.

  2. Distributed load type label HPn or HP.

  3. Actual magnitude of the load, which can be modified by the use of the *AMPLITUDE option.

  4. Z-coordinate of zero pressure level in three-dimensional or axisymmetric cases; Y-coordinate of zero pressure level in two-dimensional cases.

  5. Z-coordinate of the point at which the pressure is defined in three-dimensional or axisymmetric cases; Y-coordinate of the point at which the pressure is defined in two-dimensional cases.

Repeat this data line as often as necessary to define hydrostatic pressure loading for different elements or element sets.

Data lines to define external and internal hydrostatic pressure in pipe or elbow elements: 

First line:

  1. Element number or element set label.

  2. Distributed load type label HPE (external) or HPI (internal).

  3. Actual magnitude of the load, which can be modified by the use of the *AMPLITUDE option.

  4. Z-coordinate of zero pressure level in three-dimensional or axisymmetric cases; Y-coordinate of zero pressure level in two-dimensional cases.

  5. Z-coordinate of the point at which the pressure is defined in three-dimensional or axisymmetric cases; Y-coordinate of the point at which the pressure is defined in two-dimensional cases.

  6. Effective inner or outer diameter.

Repeat this data line as often as necessary to define internal or external pressure loading for different pipe or elbow elements or element sets.

Data lines to define viscous body force, stagnation pressure, or stagnation body loads (Abaqus/Explicit only): 

First line:

  1. Element number or element set label.

  2. Distributed load type label VBF, SPn, SP, or SBF.

  3. Reference load magnitude, which can be modified by the use of the *AMPLITUDE option.

Repeat this data line as often as necessary to define viscous body force, stagnation pressure, or stagnation body loads for different elements or element sets.


Loads used by Abaqus/Aqua

Optional parameters:

AMPLITUDE

Set this parameter equal to the name of the amplitude curve that defines the variation of the load magnitude during the step. If this parameter is omitted for uniform load types, the reference magnitude is applied immediately at the beginning of the step or linearly over the step, depending on the value assigned to the AMPLITUDE parameter on the *STEP option (see “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User's Guide). Amplitude references are ignored for nonuniform loads given by user subroutine DLOAD.

Only the load magnitude is changed with time. Quantities such as the fluid surface level in hydrostatic pressure loading are not changed.

OP

Set OP=MOD (default) for existing *DLOADs to remain, with this option modifying existing loads or defining additional loads.

Set OP=NEW if all existing *DLOADs applied to the model should be removed. New distributed loads can be defined.

Data lines to define distributed buoyancy forces: 

First line:

  1. Element number or element set label.

  2. Distributed load type label PB.

  3. Magnitude factor, M (default value is 1.0). This factor will be scaled by any *AMPLITUDE specification associated with this *DLOAD option.

  4. Effective outer diameter of the beam, truss, or one-dimensional rigid element (not used for rigid surface elements R3D3 and R3D4).

    5. The following data must be provided only when it is necessary to model the fluid inside an element:

  5. Density of fluid inside the element.

  6. Effective inner diameter of the element.

  7. Free surface elevation of the fluid inside the element.

    8. The following data should be provided only if it is necessary to change the fluid properties provided on the *AQUA option, as described in “Buoyancy loads” in “Abaqus/Aqua analysis,” Section 6.11.1 of the Abaqus Analysis User's Guide. Gravity waves do not affect the buoyancy loading when any external fluid property is overridden.

  8. Density of the fluid outside the element.

  9. Free surface elevation of the fluid outside the element.

  10. Constant pressure, added to the hydrostatic pressure outside the element.

Repeat this data line as often as necessary to define buoyancy loading for various elements or element sets.

Data lines to define distributed transverse fluid or wind drag: 

First line:

  1. Element number or element set label.

  2. Distributed load type label FDD (fluid) or WDD (wind).

  3. Magnitude factor, M (default value is 1.0). This factor will be scaled by any *AMPLITUDE specification associated with this *DLOAD option.

  4. Effective outer diameter of the member, D.

  5. Drag coefficient, .

  6. Structural velocity factor, . The default value is 1.0 if this entry is left blank or set equal to 0.0.

  7. For load type FDD, name of the *AMPLITUDE curve used for scaling steady current velocities (). For load type WDD, name of the *AMPLITUDE curve used for scaling the local x-direction wind velocity (). If this entry is blank, the velocities are not scaled ( or ).

  8. For load type FDD, name of the *AMPLITUDE curve used for scaling wave velocities (). For load type WDD, name of the *AMPLITUDE curve used for scaling the local y-direction wind velocity (). If this is blank, the velocities are not scaled ( or ).

Repeat this data line as often as necessary to define distributed transverse fluid or wind drag on various elements or element sets.

Data lines to define distributed tangential fluid drag: 

First line:

  1. Element number or element set label.

  2. Distributed load type label FDT.

  3. Magnitude factor, M (default value is 1.0). This factor will be scaled by any *AMPLITUDE specification associated with this *DLOAD option.

  4. Effective outer diameter of the member, D.

  5. Drag coefficient, .

  6. Structural velocity factor, . The default value is 1.0 if this entry is left blank or set equal to 0.0.

  7. Exponent h. The default value is 2.0 if this entry is left blank or set equal to 0.0.

  8. Name of the *AMPLITUDE curve () used for scaling steady current velocities. If this entry is blank, the current velocities are not scaled ().

  9. Name of the *AMPLITUDE curve () used for scaling wave velocities. If this entry is blank, the wave velocities are not scaled ().

Repeat this data line as often as necessary to define distributed tangential fluid drag on various elements or element sets.

Data lines to define distributed fluid inertia loading: 

First line:

  1. Element number or element set label.

  2. Distributed load type label FI.

  3. Magnitude factor, M (default value is 1.0). This factor will be scaled by any *AMPLITUDE specification associated with this *DLOAD option.

  4. Effective outer diameter of the member, D.

  5. Transverse fluid inertia coefficient, .

  6. Transverse added-mass coefficient, .

  7. Name of the *AMPLITUDE curve used for scaling fluid particle accelerations (). If this entry is blank, the fluid particle accelerations are not scaled ().

Repeat this data line as often as necessary to define fluid inertia loading for various elements or element sets.

Data lines to define concentrated fluid and wind drag loading on the ends of elements: 

First line:

  1. Element number or element set label.

  2. Distributed load type label FD1, FD2, WD1, or WD2.

  3. Magnitude factor, M (default value is 1.0). This factor will be scaled by any AMPLITUDE specification associated with this *DLOAD option.

  4. Exposed area, .

  5. Drag coefficient, C.

  6. Structural velocity factor, . The default value is 1.0 if this entry is left blank or set equal to 0.0.

  7. For load types FD1 or FD2, name of the *AMPLITUDE curve used for scaling steady current velocities (). For load types WD1 or WD2, name of the *AMPLITUDE curve used for scaling the local x-direction wind velocity (). If this entry is blank, the velocities are not scaled ( or ).

  8. For load types FD1 or FD2, name of the *AMPLITUDE curve used for scaling wave velocities (). For load types WD1 or WD2, name of the *AMPLITUDE curve used for scaling the local y-direction wind velocity (). If this entry is blank, the velocities are not scaled ( or ).

Repeat this data line as often as necessary to define concentrated fluid or wind drag loading on the ends of elements.

Data lines to define concentrated fluid inertia loading on the ends of elements: 

First line:

  1. Element number or element set label.

  2. Distributed load type label FI1 or FI2.

  3. Magnitude factor, M (default value is 1.0). This factor will be scaled by any AMPLITUDE specification associated with this *DLOAD option.

  4. Fluid inertia coefficient, .

  5. Fluid acceleration shape factor, .

  6. Added-mass coefficient, .

  7. Structural acceleration shape factor, .

  8. Name of the *AMPLITUDE curve used for scaling fluid particle accelerations. If this entry is blank, the fluid particle accelerations are not scaled.

Repeat this data line as often as necessary to define concentrated fluid inertia loading on the ends of elements.