Distributed loads

Centrifugal loads

Centrifugal load magnitudes can be specified as ${\omega }^2$, where $\omega$ is the angular velocity in radians per time. Abaqus/Standard uses the specified material density (see Density), together with the load magnitude and the axis of rotation, to calculate the loading. Alternatively, a centrifugal load magnitude can be given as $\rho {\omega }^2$, where $\rho$ is the material density (mass per unit volume) for solid or shell elements or the mass per unit length for beam elements and $\omega$ 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; $\rho {\omega }^2$ uses a consistent mass matrix, and ${\omega }^2$ 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 About Prescribed Conditions. 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.

DLOAD
element number or element set, CENTRIF, ${\omega }^2$, coord1, coord2, coord3, comp1,
comp2, comp3
DLOAD
element number or element set, CENT, $\rho {\omega }^2$, coord1, coord2, coord3, comp1, 
comp2, comp3

Load module: Create Load: choose Mechanical for the Category and Rotational body force for the Types for Selected Step: Load effect: Centrifugal

Coriolis forces

Coriolis force is defined by specifying the Coriolis distributed load type and giving the load magnitude as $\rho \omega$, where $\rho$ is the material density (mass per unit volume) for solid and shell elements or the mass per unit length for beam elements and $\omega$ 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 About Prescribed Conditions. 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.

In a static analysis Abaqus computes the translational velocity term in the Coriolis loading by dividing the incremental displacement by the current time increment.

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

DLOAD
element number or element set, CORIO, $\rho \omega$, coord1, coord2, coord3, 
comp1, comp2, comp3

Load module: Create Load: choose Mechanical for the Category and Coriolis force for the Types for Selected Step

Rotary acceleration loads

Rotary acceleration loads are defined by specifying the rotary acceleration distributed load type and giving the rotary acceleration magnitude, $\alpha$, in radians/time², 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), 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 About Prescribed Conditions. 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.

DLOAD
element number or element set, ROTA, $\alpha$, coord1, coord2, coord3, 
comp1, comp2, comp3

Load module: Create Load: choose Mechanical for the Category and Rotational body force for the Types for Selected Step: Load effect: Rotary acceleration

Specifying general rigid-body acceleration loading in Abaqus/Standard

General rigid-body acceleration loading can be specified in Abaqus/Standard by using a combination of the gravity, centrifugal (${\omega }^2$), and rotary acceleration load types.

Rotordynamic loads in a fixed reference frame

Rotordynamic loads can be used to study the vibrational response of three-dimensional models of axisymmetric structures, such as a flywheel in a hybrid energy storage system, that are spinning about their axes of symmetry in a fixed reference frame (see Genta, 2005). This is in contrast to the centrifugal loads, Coriolis forces, and rotary acceleration loads discussed above, which are formulated in a rotating frame. Rotordynamic loads are, therefore, not intended to be used in conjunction with these other dynamic load types.

The intended workflow for rotordynamic loads is to define the load in a nonlinear static step to establish the centrifugal load effects and load stiffness terms associated with a spinning body. The nonlinear static step can then be followed by a sequence of linear dynamic analyses such as complex eigenvalue extraction and/or a subspace or direct-solution steady-state dynamic analysis to study complex dynamic behaviors (induced by gyroscopic moments) such as critical speeds, unbalanced responses, and whirling phenomena in rotating structures. You do not need to redefine the rotordynamic load in the linear dynamic analyses—the load definition is carried over from the nonlinear static step. The contribution of the gyroscopic matrices in the linear dynamic steps is unsymmetric; therefore, you must use unsymmetric matrix storage as described in Defining an analysis during these steps.

Rotordynamic loads are intended only for three-dimensional models of axisymmetric bodies; you must ensure that this modeling assumption is met. Rotordynamic loads are supported for all three-dimensional continuum and cylindrical elements, shell elements, membrane elements, cylindrical 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. Multiple spinning structures spinning about different axes can be modeled in the same step. The spinning structures can also be connected to non-axisymmetric, non-rotating structures (such as bearings or support structures).

Rotordynamic loads are defined by specifying the angular velocity, $\omega$, in radians per time. The magnitude of the rotordynamic load can vary with time during a step according to an amplitude definition, as described in About Prescribed Conditions. 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.

DLOAD
element number or element set, ROTDYNF, $\omega$, coord1, coord2, coord3, 
comp1, comp2, comp3

Defining the direction vector with respect to a local coordinate system

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) 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. When using local coordinate systems for tractions applied to two-dimensional solid elements, you must ensure that the nonzero components of the loads are applied only in the X- and Y-directions. Tractions loads in the third direction are not supported (Z-direction for plane strain and plane stress elements, $\theta$-direction for axisymmetric elements).

DLOAD, ORIENTATION=name
DSLOAD, ORIENTATION=name

Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: select CSYS: Picked and click Edit to pick a local coordinate system, or select CSYS: User-defined to enter the name of a user subroutine that defines a local coordinate system

Rotation of the traction vector direction

The traction load acts in the fixed direction $\widehat{\mathbf{t}}={\widehat{\mathbf{t}}}^o$ 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, ${\mathbf{t}}^o=\alpha {\widehat{\mathbf{t}}}^o$, is decomposed by Abaqus into two components: a normal component,

and a tangential component,

where $\mathbf{N}$ is the unit reference surface normal and $\mathbf{D}$ is the unit projection of ${\widehat{\mathbf{t}}}^o$ onto the reference surface. The applied traction in the current configuration is then computed as

where $\mathbf{n}$ is the normal to the surface in the current configuration and $\mathbf{d}$ is the image of $\mathbf{D}$ rotated onto the current surface; i.e., $\mathbf{d}=\mathbf{RD}$, where $\mathbf{R}$ is the standard rotation tensor obtained from the polar decomposition of the local two-dimensional surface deformation gradient $\mathbf{F}=\mathbf{RU}$.

Examples: follower and non-follower tractions

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 1, the follower traction rotates with face 1, while the non-follower traction on face 2 always acts in the global x-direction.

Figure 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 2, the follower traction rotates with face 1, while the non-follower traction on face 2 always acts in the global x-direction.

Figure 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

Defining the direction vector with respect to a local coordinate system

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) for the direction components of these tractions.

DLOAD, ORIENTATION=name
DSLOAD, ORIENTATION=name

Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: select CSYS: Picked and click Edit to pick a local coordinate system, or select CSYS: User-defined to enter the name of a user subroutine that defines a local coordinate system

Examples: using a local coordinate system to define shear directions

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, ${\mathbf{t}}_{user}=\left(0.,1.,0.\right)$, is given in global coordinates. The sense of the resulting shear tractions using global coordinates is shown in Figure 3(a).

Figure 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, ${\mathbf{t}}_{user}=\left(0.,1.,0.\right)$, 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 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

Choosing not to have a constant resultant

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.

DLOAD, CONSTANT RESULTANT=NO
DSLOAD, CONSTANT RESULTANT=NO

Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction is defined per unit deformed area

Maintaining a constant resultant

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

DLOAD, CONSTANT RESULTANT=YES
DSLOAD, CONSTANT RESULTANT=YES

Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction is defined per unit undeformed area

Example

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 ${\mathbf{e}}_2$-direction in a geometrically nonlinear analysis (Figure 4).

Figure 4. Dead load on a flat plate.

Such a model might be used to simulate a snow load on a flat roof. The snow load could be modeled as a distributed dead traction load $\mathbf{t}=-p{\mathbf{e}}_2$. Let $S_o$ and S denote the total surface area of the plate in the reference and current configurations, respectively. With no constant resultant, the total integrated load on the plate, $\mathbf{f}$, is

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

Distributed pressure loads can be specified on any elements. For beam elements, a positive applied pressure results in a force vector acting along the particular local direction of the section or a global direction, whichever is specified. For conventional shell elements, the force vector points along the element SPOS normal. For continuum solid or a continuum shell elements with the distributed load on an explicitly identified facet, the force vector acts against the outward normal of that facet. Distributed pressure loads are not supported for pipe and elbow elements.

Distributed pressure loads can be specified on a surface formed over elements; a positive applied pressure results in a force vector acting against the local surface normal.

DLOAD
element number or element set, load type label, magnitude

DSLOAD
surface name, P or PNU, magnitude

Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: select an analytical field or a discrete field

Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Uniform or User-defined

Hydrostatic pressure loads on two-dimensional, three-dimensional, and axisymmetric elements in Abaqus/Standard

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

Figure 5. Hydrostatic pressure distribution.

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

DLOAD
element number or element set, HPn or HP, magnitude, Z-coordinate of point a, 
Z-coordinate of point b

DSLOAD
surface name, HP, magnitude, Z-coordinate of point a, 
Z-coordinate of point b

Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Hydrostatic

Mechanical pore pressure loads on two-dimensional, three-dimensional, and axisymmetric coupled pore pressure elements in Abaqus/Standard

In a coupled pore fluid diffusion and stress analysis (see Coupled pore fluid diffusion and stress analysis) the pore pressure degrees of freedom, $P_{pore}$, can be applied automatically as mechanical surface pressures for two-dimensional, three-dimensional, and axisymmetric coupled pore pressure elements. Abaqus/Standard applies a mechanical pressure, $P_{mech}=P_{pore}$, onto the surfaces you prescribe. Since the mechanical pressure loads are determined by the solution pore pressures, Abaqus/Standard ignores any amplitude definition on the distributed load definition. You can include a nonzero scaling factor, $\alpha$, which will be applied to the pore pressures to give $P_{mech}=\alpha P_{pore}$. By default, the scaling factor is set to unity. This loading is supported only for continuum elements that have pore pressure degrees of freedom during a geostatic (Geostatic stress state) or coupled pore fluid diffusion and stress analysis (Coupled pore fluid diffusion and stress analysis).

DLOAD
 element number or element set, PORMECHn, scaling factor 

DSLOAD
surface name, PORMECH, scaling factor

Viscous pressure loads in Abaqus/Explicit

Viscous pressure loads are defined by

where p is the pressure applied to the body; $c_v$ is the viscosity, given as the magnitude of the load; $\mathbf{v}$ is the velocity of the point on the surface where the pressure is being applied; ${\mathbf{v}}_{ref}$ is the velocity of the reference node; and $\mathbf{n}$ is the unit outward normal to the element at the same point.

Viscous pressure loading is most commonly applied in structural problems when you want 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 $c_v$ is important for using this technique effectively.

To compute $c_v$, consider the infinite continuum elements described in Infinite elements. In explicit dynamics those elements achieve an infinite boundary condition by applying a viscous normal pressure where the coefficient $c_v$ is given by $\rho c_d$; $\rho$ is the density of the material at the surface, and $c_d$ 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 $\lambda$ and $\mu$ are Lamé's constants, E is Young's modulus, and $\nu$ is Poisson's ratio. This choice of the viscous pressure coefficient represents a level of damping in which pressure waves crossing the free surface are absorbed with no reflection of energy back into the interior of the finite element mesh.

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

DLOAD, REF NODE=reference_node
element number or element set, VPn or VP, magnitude
DSLOAD, REF NODE=reference_node
surface name, VP, magnitude

Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Viscous, toggle on or off Determine velocity from reference point

Stagnation pressure loads in Abaqus/Explicit

Stagnation pressure loads are defined by

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

DLOAD, REF NODE=reference_node
element number or element set, SPn or SP, magnitude
DSLOAD, REF NODE=reference_node
element number or element set, SP, magnitude

Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Stagnation, toggle on or off Determine velocity from reference point

Pressure on pipe and elbow elements

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 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).

DLOAD
element number or element set, PE or PENU, magnitude, effective outer diameter

DLOAD
element number or element set, PI or PINU, magnitude, effective inner diameter

DLOAD
element number or element set, HPE, magnitude, effective outer diameter

DLOAD
element number or element set, HPI, magnitude, effective inner diameter

Load module: Create Load: choose Mechanical for the Category and Pipe pressure for the Types for Selected Step: Side: External or Internal, Distribution: Uniform, User-defined, or select an analytical field

Load module: Create Load: choose Mechanical for the Category and Pipe pressure for the Types for Selected Step: Side: External or Internal, Distribution: Hydrostatic

Rotation of the load vector

In a geometrically linear analysis the edge load, $\mathbf{t}$, 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, $\mathbf{t}$, 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, $\mathbf{t}$, is computed by rigidly rotating ${\mathbf{t}}^o$ onto the current edge.

Defining the direction vector with respect to a local coordinate system

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) for the direction components of these tractions.

DLOAD, ORIENTATION=name
DSLOAD, ORIENTATION=name

Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: select CSYS: Picked and click Edit to pick a local coordinate system, or select CSYS: User-defined to enter the name of a user subroutine that defines a local coordinate system

Choosing not to have a constant resultant

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.

DLOAD, CONSTANT RESULTANT=NO
DSLOAD, CONSTANT RESULTANT=NO

Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction is defined per unit deformed area

Maintaining a constant resultant

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.

DLOAD, CONSTANT RESULTANT=YES
DSLOAD, CONSTANT RESULTANT=YES

Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction is defined per unit undeformed area