27.4.3 Distributed loads

**Products: **ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE

“Defining a pressure load,” Section 16.9.3 of the ABAQUS/CAE User's Manual

“Defining a shell edge load,” Section 16.9.4 of the ABAQUS/CAE User's Manual

“Defining a surface traction load,” Section 16.9.5 of the ABAQUS/CAE User's Manual

“Defining a pipe pressure load,” Section 16.9.6 of the ABAQUS/CAE User's Manual

“Defining a body force,” Section 16.9.7 of the ABAQUS/CAE User's Manual

“Defining a line load,” Section 16.9.8 of the ABAQUS/CAE User's Manual

“Defining a gravity load,” Section 16.9.9 of the ABAQUS/CAE User's Manual

“Defining a rotational body force,” Section 16.9.11 of the ABAQUS/CAE User's Manual

Distributed loads:

can be prescribed on element faces, element bodies, or element edges;

can be prescribed over geometric surfaces or geometric edges; and

require that an appropriate distributed load type be specified—see Part VI, “Elements,” for definitions of the distributed load types available for particular elements.

In steady-state dynamic analysis both real and imaginary distributed loads can be applied (see “Direct-solution steady-state dynamic analysis,” Section 6.3.4, and “Mode-based steady-state dynamic analysis,” Section 6.3.8, for details).

Incident wave loading is used to apply distributed loads for the special case of loads associated with a wave traveling through an acoustic medium. Inertia relief is used to apply inertia-based loading in ABAQUS/Standard. These load types are discussed in “Acoustic loads,” Section 27.4.5, and “Inertia relief,” Section 11.1.1, respectively. ABAQUS/Aqua load types are discussed in “ABAQUS/Aqua analysis,” Section 6.10.1.

Defining time-dependent distributed loads

The prescribed magnitude of a distributed load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 27.1.1. If different variations are needed for different loads, each load can refer to its own amplitude definition.

Modifying distributed loads

Distributed loads can be added, modified, or removed as described in “Applying loads: overview,” Section 27.4.1.

Improving the rate of convergence in large-displacement implicit analysis

In large-displacement analyses in ABAQUS/Standard some distributed load types introduce unsymmetric load stiffness matrix terms. Examples are hydrostatic pressure, pressure applied to surfaces with free edges, Coriolis force, rotary acceleration force, and distributed edge loads and surface tractions modeled as follower loads. In such cases using the unsymmetric matrix storage and solution scheme for the analysis step may improve the convergence rate of the equilibrium iterations. See “Procedures: overview,” Section 6.1.1, for more information on the unsymmetric matrix storage and solution scheme.

Defining distributed loads in a user subroutine

Nonuniform distributed loads such as a nonuniform body force in the *X*-direction can be defined by means of user subroutine `DLOAD` in ABAQUS/Standard or `VDLOAD` in ABAQUS/Explicit. When an amplitude reference is used with a nonuniform load defined in user subroutine `VDLOAD`, the current value of the amplitude function is passed to the user subroutine at each time increment in the analysis. `DLOAD` and `VDLOAD` are not available for surface tractions, edge tractions, or edge moments.

In ABAQUS/Standard nonuniform distributed surface tractions, edge tractions, and edge moments can be defined by means of user subroutine `UTRACLOAD`. User subroutine `UTRACLOAD` allows you to define a nonuniform magnitude for surface tractions, edge tractions, and edge moments, as well as nonuniform loading directions for general surface tractions, shear tractions, and general edge tractions.

Nonuniform distributed surface tractions, edge tractions, and edge moments are not currently supported in ABAQUS/Explicit.

Specifying the region to which a distributed load is applied

As discussed in “Applying loads: overview,” Section 27.4.1, distributed loads can be defined as element-based or surface-based. Element-based distributed loads can be prescribed on element bodies, element surfaces, or element edges. Surface-based distributed loads can be prescribed directly on geometric surfaces or geometric edges.

Three types of distributed loads can be defined: body loads, surface loads, and edge loads. Distributed body loads are always element-based. Distributed surface loads and distributed edge loads can be element-based or surface-based. In ABAQUS/CAE pressure loads can be element-based or surface-based. All other distributed surface and edge loads are always surface-based; surfaces can be defined as collections of geometric faces and edges or collections of element faces and edges. Table 27.4.3–1 summarizes the regions on which each load type can be prescribed. In ABAQUS/CAE all distributed loads are specified by selecting the region in the viewport or from a list of surfaces. In the ABAQUS input file different options are used depending on the type of region to which the load is applied, as illustrated in the following sections.

**Table 27.4.3–1** Regions on which the different load types can be prescribed.

Load type | Load definition | Input file region | ABAQUS/CAE region |
---|---|---|---|

Body loads | Element-based | Element bodies | Volumetric bodies |

Surface loads | Element-based | Element surfaces | Surfaces defined as collections of geometric faces or collections of element faces (applicable only for pressure loads) |

Surface-based | Geometric element-based surfaces | Surfaces defined as collections of geometric faces or collections of element faces | |

Edge loads (including beam line loads) | Element-based | Element edges | N/A |

Surface-based | Geometric edge-based surfaces | Surfaces defined as collections of geometric edges or collections of element edges |

Body forces

Body loads, such as gravity, centrifugal, Coriolis, and rotary acceleration loads, are applied as element-based loads. The units of a body force are force per unit volume.

Table 27.4.3–2 lists all of the distributed body load types that are available in ABAQUS, along with the corresponding load type labels.

**Table 27.4.3–2** Distributed body load types.

Load description | Load type label for element-based loads | Load type label for surface-based loads | ABAQUS/CAE load type |
---|---|---|---|

Uniform body force in global X-, Y-, and Z-directions | BX, BY, BZ | N/A | Body force |

Nonuniform body force in global X-, Y-, and Z-directions | BXNU, BYNU, BZNU | N/A | |

Uniform body force in radial and axial directions (only for axisymmetric elements) | BR, BZ | N/A | |

Nonuniform body force in radial and axial directions (only for axisymmetric elements) | BRNU, BZNU | N/A | |

Viscous body force in global X-, Y-, and Z-directions (available only in ABAQUS/Explicit) | VBF | N/A | Not supported |

Stagnation body force in global X-, Y-, and Z-directions (available only in ABAQUS/Explicit) | SBF | N/A | |

Gravity loading | GRAV | N/A | Gravity |

Centrifugal load (magnitude is input as , where is the mass density per unit volume and is the angular velocity) | CENT | N/A | Not supported |

Centrifugal load (magnitude is input as , where is the angular velocity) | CENTRIF | N/A | Rotational body force |

Coriolis force | CORIO | N/A | Coriolis force |

Rotary acceleration load | ROTA | N/A | Rotational body force |

You can specify body forces on any elements in the global *X*-, *Y*-, or *Z*-direction. You can specify body forces on axisymmetric elements in the radial or axial direction.

Input File Usage: | Use the following option to define a body force in the global X-, Y-, or Z-direction: |

*DLOAD where Use the following option to define a body force in the radial or axial direction on axisymmetric elements: *DLOAD where |

ABAQUS/CAE Usage: | Load module: |

Viscous body force loads are defined by

where is the viscous force applied to the body; is the viscosity, given as the magnitude of the load; is the velocity of the point on the body where the force is being applied; is the velocity of the reference node; and is the element volume.

Viscous body force loading can be thought of as mass-proportional damping in the sense that it gives a damping contribution proportional to the mass for an element if the coefficient is chosen to be a small value multiplied by the material density (see “Material damping,” Section 20.1.1). Viscous body force loading provides an alternative way to define mass-proportional damping as a function of relative velocities and a step-dependent damping coefficient.

Input File Usage: | Use the following option to define a viscous body force load: |

*DLOAD, REF NODE= |

ABAQUS/CAE Usage: | Viscous body force loads are not supported in ABAQUS/CAE. |

Stagnation body force loads are defined by

where is the stagnation body force applied to the body; is the factor, given as the magnitude of the load; is the velocity of the point on the body where the body force is being applied; is the velocity of the reference node; and is the element volume. The coefficient should be very small to avoid excessive damping and a dramatic drop in the stable time increment.

Input File Usage: | Use the following option to define a stagnation body force load: |

*DLOAD, REF NODE= |

ABAQUS/CAE Usage: | Stagnation body force loads are not supported in ABAQUS/CAE. |

Gravity loading (uniform acceleration in a fixed direction) is specified by using the gravity distributed load type and giving the gravity constant as the magnitude of the load. The direction of the gravity field is specified by giving the components of the gravity vector in the distributed load definition. ABAQUS uses the user-specified material density (see “Density,” Section 16.2.1), together with the magnitude and direction, to calculate the loading. The magnitude of the gravity load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 27.1.1. However, the direction of the gravity field is always applied at the beginning of the step and remains fixed during the step.

You need not specify an element or an element set as is customary for the specification of other distributed loads. ABAQUS automatically collects all elements in the model that have mass contributions (including point mass elements) in an element set called `_Whole_Model_Gravity_Elset` and applies the gravity loads to the elements in this element set.

When gravity loading is used with substructures, the density must be defined and unit gravity load vectors must be calculated when the substructure is created (see “Defining substructures,” Section 10.1.2).

Input File Usage: | Use the following option to define a gravity load: |

*DLOAD |

ABAQUS/CAE Usage: | Load module: |

Centrifugal loads, Coriolis forces, and rotary acceleration loads can be applied in ABAQUS/Standard by specifying the appropriate distributed load type in an element-based distributed load definition.

Centrifugal load magnitudes can be specified as , where is the angular velocity in radians per time. ABAQUS/Standard uses the specified material density (see “Density,” Section 16.2.1), together with the load magnitude and the axis of rotation, to calculate the loading. Alternatively, a centrifugal load magnitude can be given as , where is the material density (mass per unit volume) for solid or shell elements or the mass per unit length for beam elements and is the angular velocity in radians per time. This type of centrifugal load formulation does not account for large volume changes. The two centrifugal load types will produce slightly different local results for first-order elements; uses a consistent mass matrix, and uses a lumped mass matrix in calculating the load forces and load stiffnesses.

The magnitude of the centrifugal load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 27.1.1. However, the position and orientation of the axis around which the structure rotates, which is defined by giving a point on the axis and the axis direction, are always applied at the beginning of the step and remain fixed during the step.

ABAQUS/CAE Usage: | Load module: |

Coriolis force is defined by specifying the Coriolis distributed load type and giving the load magnitude as , where is the material density (mass per unit volume) for solid and shell elements or the mass per unit length for beam elements and is the angular velocity in radians per time. The magnitude of the Coriolis load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 27.1.1. However, the position and orientation of the axis around which the structure rotates, which is defined by giving a point on the axis and the axis direction, are always applied at the beginning of the step and remain fixed during the step.

The Coriolis load formulation does not account for large volume changes.

Input File Usage: | Use the following option to define a Coriolis load: |

*DLOAD |

ABAQUS/CAE Usage: | Load module: |

Rotary acceleration loads are defined by specifying the rotary acceleration distributed load type and giving the rotary acceleration magnitude, , in radians/time^{2}, which includes any precessional motion effects. The axis of rotary acceleration must be defined by giving a point on the axis and the axis direction. ABAQUS/Standard uses the specified material density (see “Density,” Section 16.2.1), together with the rotary acceleration magnitude and axis of rotary acceleration, to calculate the loading. The magnitude of the load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 27.1.1. However, the position and orientation of the axis around which the structure rotates are always applied at the beginning of the step and remain fixed during the step.

Rotary acceleration loads are not applicable to axisymmetric elements.

Input File Usage: | Use the following option to define a rotary acceleration load: |

*DLOAD |

ABAQUS/CAE Usage: | Load module: |

Surface tractions and pressure loads

General or shear surface tractions and pressure loads can be applied in ABAQUS as element-based or surface-based distributed loads. The units of these loads are force per unit area.

Table 27.4.3–3 lists all of the distributed surface load types that are available in ABAQUS, along with the corresponding load type labels.

**Table 27.4.3–3** Distributed surface load types.

Load description | Load type label for element-based loads | Load type label for surface-based loads | ABAQUS/CAE load type |
---|---|---|---|

Uniform general surface traction | TRVECn | TRVEC | Surface traction |

Uniform shear surface traction | TRSHRn | TRSHR | |

Nonuniform general surface traction | TRVECnNU | TRVECNU | Not supported |

Nonuniform shear surface traction | TRSHRnNU | TRSHRNU | |

Uniform pressure | Pn | P | Pressure |

Nonuniform pressure | PnNU | PNU | |

Hydrostatic pressure (available only in ABAQUS/Standard) | HPn | HP | |

Viscous pressure (available only in ABAQUS/Explicit) | VPn | VP | |

Stagnation pressure (available only in ABAQUS/Explicit) | SPn | SP | |

Hydrostatic internal and external pressure (only for PIPE and ELBOW elements in ABAQUS/Standard) | HPI, HPE | N/A | Pipe pressure |

Uniform internal and external pressure (only for PIPE and ELBOW elements in ABAQUS/Standard) | PI, PE | N/A | |

Nonuniform internal and external pressure (only for PIPE and ELBOW elements in ABAQUS/Standard) | PINU, PENU | N/A |

By definition, the line of action of a *follower* surface load rotates with the surface in a geometrically nonlinear analysis. This is in contrast to a *non-follower* load, which always acts in a fixed global direction.

With the exception of general surface tractions, all the distributed surface loads listed in Table 27.4.3–3 are modeled as follower loads. The hydrostatic and viscous pressures listed in Table 27.4.3–3 always act normal to the surface in the current configuration, the shear tractions always act tangent to the surface in the current configuration, and the internal and external pipe pressures follow the motion of the pipe elements.

General surface tractions can be specified to be follower or non-follower loads. There is no difference between a follower and a non-follower load in a geometrically linear analysis since the configuration of the body remains fixed. The difference between a follower and non-follower general surface traction is illustrated in the next section through an example.

ABAQUS/CAE Usage: | Load module: |

General surface tractions allow you to specify a surface traction, , acting on a surface *S*. The resultant load, , is computed by integrating over *S*:

where is the magnitude and is the direction of the load. To define a general surface traction, you must specify both a load magnitude, , and the direction of the load with respect to the reference configuration, . The magnitude and direction can also be specified in user subroutine

ABAQUS/CAE Usage: | Load module: |

By default, the components of the traction vector are specified with respect to the global directions. You can also refer to a local coordinate system (see “Orientations,” Section 2.2.5) for the direction components of these tractions. See “Examples: using a local coordinate system to define shear directions” below for an example of a traction load defined with respect to a local coordinate system.

ABAQUS/CAE Usage: | Load module: |

The traction load acts in the fixed direction in a geometrically linear analysis or if a non-follower load is specified in a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state).

If a follower load is specified in a geometrically nonlinear analysis, the traction load rotates rigidly with the surface using the following algorithm. The reference configuration traction vector, , is decomposed by ABAQUS into two components: a normal component,

and a tangential component,

where is the unit reference surface normal and is the unit projection of onto the reference surface. The applied traction in the current configuration is then computed as

where is the normal to the surface in the current configuration and is the image of rotated onto the current surface; i.e., , where is the standard rotation tensor obtained from the polar decomposition of the local two-dimensional surface deformation gradient .

The following two examples illustrate the difference between applying follower and non-follower tractions in a geometrically nonlinear analysis. Both examples refer to a single 4-node plane strain element (element 1). In Step 1 of the first example a follower traction load is applied to face 1 of element 1, and a non-follower traction load is applied to face 2 of element 1. The element is rotated rigidly 90° counterclockwise in Step 1 and then another 90° in Step 2. As illustrated in Figure 27.4.3–1, the follower traction rotates with face 1, while the non-follower traction on face 2 always acts in the global *x*-direction.

**Figure 27.4.3–1** Follower and non-follower traction loads in a geometrically nonlinear analysis, load applied in Step 1: (a) beginning of Step 1; (b) end of Step 1, beginning of Step 2; (c) end of Step 2.

*STEP, NLGEOM Step 1 - Rotate square 90 degrees ... *DLOAD, FOLLOWER=YES 1, TRVEC1, 1., 0., -1., 0. *DLOAD, FOLLOWER=NO 1, TRVEC2, 1., 1., 0., 0. *END STEP *STEP, NLGEOM Step 2 - Rotate square another 90 degrees ... *END STEP

In the second example the element is rotated 90° counterclockwise with no load applied in Step 1. In Step 2 a follower traction load is applied to face 1, and a non-follower traction load is applied to face 2. The element is then rotated rigidly by another 90°. The direction of the follower load is specified with respect to the original configuration. As illustrated in Figure 27.4.3–2, the follower traction rotates with face 1, while the non-follower traction on face 2 always acts in the global *x*-direction.

**Figure 27.4.3–2** Follower and non-follower traction loads in a geometrically nonlinear analysis, load applied in Step 2: (a) beginning of Step 1; (b) end of Step 1, beginning of Step 2; (c) end of Step 2.

*STEP, NLGEOM Step 1 - Rotate square 90 degrees ... *END STEP *STEP, NLGEOM Step 2 - Rotate square another 90 degrees *DLOAD, FOLLOWER=YES 1, TRVEC1, 1., 0., -1., 0. *DLOAD, FOLLOWER=NO 1, TRVEC2, 1., 1., 0., 0. ... *END STEP

Shear surface tractions allow you to specify a surface force per unit area, , that acts tangent to a surface *S*. The resultant load, , is computed by integrating over *S*:

where is the magnitude and is a unit vector along the direction of the load. To define a shear surface traction, you must provide both the magnitude, , and a direction, , for the load. The magnitude and direction vector can also be specified in user subroutine

ABAQUS modifies the traction direction by first projecting the user-specified vector, , onto the surface in the *reference* configuration,

where is the reference surface normal. The specified traction is applied along the computed traction direction tangential to the surface:

Consequently, a shear traction load is not applied at any point where is normal to the reference surface.

The shear traction load acts in the fixed direction in a geometrically linear analysis. In a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state), the shear traction vector will rotate rigidly; i.e., , where is the standard rotation tensor obtained from the polar decomposition of the local two-dimensional surface deformation gradient .

ABAQUS/CAE Usage: | Load module: |

By default, the components of the shear traction vector are specified with respect to the global directions. You can also refer to a local coordinate system (see “Orientations,” Section 2.2.5) for the direction components of these tractions.

ABAQUS/CAE Usage: | Load module: |

It is sometimes convenient to give shear and general traction directions with respect to a local coordinate system. The following two examples illustrate the specification of the direction of a shear traction on a cylinder using global coordinates in one case and a local cylindrical coordinate system in the other case. The axis of symmetry of the cylinder coincides with the global *z*-axis. A surface named `SURFA` has been defined on the outside of the cylinder.

In the first example the direction of the shear traction, , is given in global coordinates. The sense of the resulting shear tractions using global coordinates is shown in Figure 27.4.3–3(a).

**Figure 27.4.3–3** Shear tractions specified using global coordinates (a) and a local cylindrical coordinate system (b).

*STEP Step 1 - Specify shear directions in global coordinates ... *DSLOAD SURFA, TRSHR, 1., 0., 1., 0. ... *END STEP

In the second example the direction of the shear traction, , is given with respect to a local cylindrical coordinate system whose axis coincides with the axis of the cylinder. The sense of the resulting shear tractions using the local cylindrical coordinate system is shown in Figure 27.4.3–3(b).

*ORIENTATION, NAME=CYLIN, SYSTEM=CYLINDRICAL 0., 0., 0., 0., 0., 1. ... *STEP Step 1 - Specify shear directions in local cylindrical coordinates ... *DSLOAD, ORIENTATION=CYLIN SURFA, TRSHR, 1., 0., 1., 0. ... *END STEP

You can choose to integrate surface tractions over the current or the reference configuration by specifying whether or not a constant resultant should be maintained.

In general, the constant resultant method is best suited for cases where the magnitude of the resultant load should not vary with changes in the surface area. However, it is up to you to decide which approach is best for your analysis. An example of an analysis using a constant resultant can be found in “Distributed traction and edge loads,” Section 1.4.17 of the ABAQUS Verification Manual.

If you choose not to have a constant resultant, the traction vector is integrated over the surface in the current configuration, a surface that in general deforms in a geometrically nonlinear analysis. By default, all surface tractions are integrated over the surface in the current configuration.

ABAQUS/CAE Usage: | Load module: |

If you choose to have a constant resultant, the traction vector is integrated over the surface in the reference configuration and then held constant.

ABAQUS/CAE Usage: | Load module: |

The constant resultant method has certain advantages when a traction is used to model a distributed load with a known constant resultant. Consider the case of modeling a uniform dead load, magnitude *p*, acting on a flat plate whose normal is in the -direction in a geometrically nonlinear analysis (Figure 27.4.3–4).

In this case a uniform traction leads to a resultant load that increases as the surface area of the plate increases, which is not consistent with a fixed snow load. With the constant resultant method, the total integrated load on the plate is

In this case a uniform traction leads to a resultant that is equal to the pressure times the surface area in the reference configuration, which is more consistent with the problem at hand.

Distributed pressure loads can be specified on any elements. Hydrostatic pressure loads can be specified in ABAQUS/Standard on two-dimensional, three-dimensional, and axisymmetric elements. Viscous and stagnation pressure loads can be specified in ABAQUS/Explicit on any elements.

Distributed pressure loads can be specified on any elements.

ABAQUS/CAE Usage: | Load module: |

To define hydrostatic pressure in ABAQUS/Standard, give the *Z*-coordinates of the zero pressure level (point *a* in Figure 27.4.3–5) and the level at which the hydrostatic pressure is defined (point *b* in Figure 27.4.3–5) in an element-based or surface-based distributed load definition. For levels above the zero pressure level, the hydrostatic pressure is zero.

In planar elements the hydrostatic head is in the *Y*-direction; for axisymmetric elements the *Z*-direction is the second coordinate.

ABAQUS/CAE Usage: | Load module: |

Viscous pressure loads are defined by

where

Viscous pressure loading is most commonly applied in structural problems when you wish to damp out dynamic effects and, thus, reach static equilibrium in a minimal number of increments. A common example is the determination of springback in a sheet metal product after forming, in which case a viscous pressure would be applied to the faces of shell elements defining the sheet metal. An appropriate choice for the value of is important for using this technique effectively.

To compute , consider the infinite continuum elements described in “Infinite elements,” Section 22.2.1. In explicit dynamics those elements achieve an infinite boundary condition by applying a viscous normal pressure where the coefficient is given by ; is the density of the material at the surface, and is the value of the dilatational wave speed in the material (the infinite continuum elements also apply a viscous shear traction). For an isotropic, linear elastic material

where and are Lamé's constants,

For typical structural problems it is not desirable to absorb all of the energy (as is the case in the infinite elements). Typically is set equal to a small percentage (perhaps 1 or 2 percent) of as an effective way of minimizing ongoing dynamic effects. The coefficient should have a positive value.

ABAQUS/CAE Usage: | Load module: |

Stagnation pressure loads are defined by

where is the stagnation pressure applied to the body; is the factor, given as the magnitude of the load; is the velocity of the point on the surface where the pressure is being applied; is the unit outward normal to the element at the same point; and is the velocity of the reference node. The coefficient should be very small to avoid excessive damping and a dramatic drop in the stable time increment.

ABAQUS/CAE Usage: | Load module: |

You can specify external pressure, internal pressure, external hydrostatic pressure, or internal hydrostatic pressure on pipe or elbow elements. When pressure loads are applied, the effective outer or inner diameter must be specified in the element-based distributed load definition.

The loads resulting from the pressure on the ends of the element are included: ABAQUS/Standard assumes a closed-end condition. Closed-end conditions correctly model the loading at pipe intersections, tight bends, corners, and cross-section changes; in straight sections and smooth bends the end loads of adjacent elements cancel each other precisely. If an open-end condition is to be modeled, a compensating point load should be added at the open end. A case where such an end load must be applied occurs if a pressurized pipe is modeled with a mixture of pipe and beam elements. In that case closed-end conditions generate a physically non-existing force at the transition between pipe and beam elements. Such mixed modeling of a pipe is not recommended.

For pipe elements subjected to pressure loading, the effective axial force due to the pressure loads can be obtained by requesting output variable ESF1 (see “Beam element library,” Section 23.3.8).

Input File Usage: | Use the following option to define an external pressure load on pipe or elbow elements: |

*DLOAD Use the following option to define an internal pressure load on pipe or elbow elements: *DLOAD Use the following option to define an external hydrostatic pressure load on pipe or elbow elements: *DLOAD Use the following option to define an internal hydrostatic pressure load on pipe or elbow elements: *DLOAD |

ABAQUS/CAE Usage: | Load module: |

Plane stress theory assumes that the volume of a plane stress element remains constant in a large-strain analysis. When a distributed surface load is applied to an edge of plane stress elements, the current length and orientation of the edge are considered in the load distribution, but the current thickness is not; the original thickness is used.

This limitation can be circumvented only by using three-dimensional elements at the edge so that a change in thickness upon loading is recognized; suitable equation constraints (“Linear constraint equations,” Section 28.2.1) would be required to make the in-plane displacements on the two faces of these elements equal. Three-dimensional elements along an edge can be connected to interior shell elements by using a shell-to-solid coupling constraint (see “Shell-to-solid coupling,” Section 28.3.3, for details).

Edge tractions and moments on shell elements and line loads on beam elements

Distributed edge tractions (general, shear, normal, or transverse) and edge moments can be applied to shell elements in ABAQUS as element-based or surface-based distributed loads. The units of an edge traction are force per unit length. The units of an edge moment are torque per unit length. References to local coordinate systems are ignored for all edge tractions and moments except general edge tractions.

Distributed line loads can be applied to beam elements in ABAQUS as element-based distributed loads. The units of a line load are force per unit length.

Table 27.4.3–4 lists all of the distributed edge and line load types that are available in ABAQUS, along with the corresponding load type labels.

**Table 27.4.3–4** Distributed edge load types.

Load description | Load type label for element-based loads | Load type label for surface-based loads | ABAQUS/CAE load type |
---|---|---|---|

Uniform general edge traction | EDLDn | EDLD | Shell edge load |

Uniform normal edge traction | EDNORn | EDNOR | |

Uniform shear edge traction | EDSHRn | EDSHR | |

Uniform transverse edge traction | EDTRAn | EDTRA | |

Uniform edge moment | EDMOMn | EDMOM | |

Nonuniform general edge traction | EDLDnNU | EDLDNU | Not supported |

Nonuniform normal edge traction | EDNORnNU | EDNORNU | |

Nonuniform shear edge traction | EDSHRnNU | EDSHRNU | |

Nonuniform transverse edge traction | EDTRAnNU | EDTRANU | |

Nonuniform edge moment | EDMOMnNU | EDMOMNU | |

Uniform force per unit length in global X-, Y-, and Z-directions (only for beam elements) | PX, PY, PZ | N/A | Line load |

Nonuniform force per unit length in global X-, Y-, and Z-directions (only for beam elements) | PXNU, PYNU, PZNU | N/A | |

Uniform force per unit length in beam local 1- and 2-directions (only for beam elements) | P1, P2 | N/A | |

Nonuniform force per unit length in beam local 1- and 2-directions (only for beam elements) | P1NU, P2NU | N/A |

By definition, the line of action of a *follower* edge or line load rotates with the edge or line in a geometrically nonlinear analysis. This is in contrast to a *non-follower* load, which always acts in a fixed global direction.

With the exception of general edge tractions on shell elements and the forces per unit length in the global directions on beam elements, all the edge and line loads listed in Table 27.4.3–4 are modeled as follower loads. The normal, shear, and transverse edge loads listed in Table 27.4.3–4 act in the normal, shear, and transverse directions, respectively, in the current configuration (see Figure 27.4.3–6).

The edge moment always acts about the shell edge in the current configuration. The forces per unit length in the local beam directions rotate with the beam elements.The forces per unit length in the global directions on beam elements are always non-follower loads.

General edge tractions can be specified to be follower or non-follower loads. There is no difference between a follower and a non-follower load in a geometrically linear analysis since the configuration of the body remains fixed.

ABAQUS/CAE Usage: | Load module: |

General edge tractions allow you to specify an edge load, , acting on a shell edge, *L*. The resultant load, , is computed by integrating over *L*:

To define a general edge traction, you must provide both a magnitude, , and direction, , for the load. The specified load directions are normalized by ABAQUS; thus, they do not contribute to the magnitude of the load.

If a nonuniform general edge traction is specified, the magnitude, , and direction, , must be specified in user subroutine `UTRACLOAD`.

ABAQUS/CAE Usage: | Load module: |

In a geometrically linear analysis the edge load, , acts in the fixed direction defined by

If a non-follower load is specified in a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state), the edge load, , acts in the fixed direction defined by

If a follower load is specified in a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state), the components must be defined with respect to the reference configuration. The reference edge traction is defined as

The applied edge traction, , is computed by rigidly rotating onto the current edge.

By default, the components of the edge traction vector are specified with respect to the global directions. You can also refer to a local coordinate system (see “Orientations,” Section 2.2.5) for the direction components of these tractions.

ABAQUS/CAE Usage: | Load module: |

The loading directions of shear, normal, and transverse edge tractions are determined by the underlying elements. A positive shear edge traction acts in the positive direction of the shell edge as determined by the element connectivity. A positive normal edge traction acts in the plane of the shell in the inward direction. A positive transverse edge traction acts in a sense opposite to the facet normal. The directions of positive shear, normal, and transverse edge tractions are shown in Figure 27.4.3–6.

To define a shear, normal, or transverse edge traction, you must provide a magnitude, for the load.

If a nonuniform shear, normal, or transverse edge traction is specified, the magnitude, , must be specified in user subroutine `UTRACLOAD`.

In a geometrically linear step, the shear, normal, and transverse edge tractions act in the tangential, normal, and transverse directions of the shell, as shown in Figure 27.4.3–6. In a geometrically nonlinear analysis the shear, normal, and transverse edge tractions rotate with the shell edge so they always act in the tangential, normal, and transverse directions of the shell, as shown in Figure 27.4.3–6.

Input File Usage: | Use one of the following options to define a directed edge traction: |

*DLOAD For element-based loads the For surface-based loads the |

ABAQUS/CAE Usage: | Load module: |

An edge moment acts about the shell edge with the positive direction determined by the element connectivity. The directions of positive edge moments are shown in Figure 27.4.3–7.

To define a distributed edge moment, you must provide a magnitude, , for the load.

If a nonuniform edge moment is specified, the magnitude, , must be specified in user subroutine `UTRACLOAD`.

An edge moment always acts about the current shell edge in both geometrically linear and nonlinear analyses.

In a geometrically linear step an edge moment acts about the shell edge as shown in Figure 27.4.3–7. In a geometrically nonlinear analysis an edge moment always acts about the shell edge as shown in Figure 27.4.3–7.

ABAQUS/CAE Usage: | Load module: |

You can choose to integrate edge tractions and moments over the current or the reference configuration by specifying whether or not a constant resultant should be maintained. In general, the constant resultant method is best suited for cases where the magnitude of the resultant load should not vary with changes in the edge length. However, it is up to you to decide which approach is best for your analysis.

If you choose not to have a constant resultant, an edge traction or moment is integrated over the edge in the current configuration, an edge whose length changes during a geometrically nonlinear analysis.

ABAQUS/CAE Usage: | Load module: |

If you choose to have a constant resultant, an edge traction or moment is integrated over the edge in the reference configuration, whose length is constant.

ABAQUS/CAE Usage: | Load module: |

You can specify line loads on beam elements in the global *X*-, *Y*-, or *Z*-direction. In addition, you can specify line loads on beam elements in the beam local 1- or 2-direction.

Input File Usage: | Use the following option to define a force per unit length in the global X-, Y-, or Z-direction on beam elements: |

*DLOAD where Use the following option to define a force per unit length in the beam local 1- or 2-direction: *DLOAD where |

ABAQUS/CAE Usage: | Load module: |