| Load description | Load type label for element-based loads |
| Body force in global X-, Y-, and Z-directions | BX, BY, BZ |
| Nonuniform body force in global X-, Y-, and Z-directions | BXNU, BYNU, BZNU |
| Body force in radial and axial directions (only for axisymmetric elements) | BR, BZ |
| Nonuniform body force in radial and axial directions (only for axisymmetric elements) | BRNU, BZNU |
| Viscous body force in global X-, Y-, and Z-directions (available only in Abaqus/Explicit) | VBF |
| Stagnation body force in global X-, Y-, and Z-directions (available only in Abaqus/Explicit) | SBF |
| Gravity loading | GRAV |
| Centrifugal load (magnitude is input as ρω2, where ρ is the mass density per unit volume and ω is the angular velocity) | CENT |
| Centrifugal load (magnitude is input as ω2, where ω is the angular velocity) | CENTRIF |
| Coriolis force | CORIO |
| Rotary acceleration load | ROTA |
| Load description | Abaqus/CAE load type |
| Body force in global X-, Y-, and Z-directions | Body force |
| Nonuniform body force in global X-, Y-, and Z-directions | Body force |
| Body force in radial and axial directions (only for axisymmetric elements) |
| Nonuniform body force in radial and axial directions (only for axisymmetric elements) |
| Viscous body force in global X-, Y-, and Z-directions (available only in Abaqus/Explicit) | Not supported |
| Stagnation body force in global X-, Y-, and Z-directions (available only in Abaqus/Explicit) |
| Gravity loading | Gravity |
| Centrifugal load (magnitude is input as ρω2, where ρ is the mass density per unit volume and ω is the angular velocity) | Not supported |
| Centrifugal load (magnitude is input as ω2, where ω is the angular velocity) | Rotational body force |
| Coriolis force | Coriolis force |
| Rotary acceleration load | Rotational body force |
| Rotordynamic load | Not supported |
| Porous drag load (input is porosity of the medium) | Porous drag body force |
# Specifying general body forces
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 Zdirection:
\*DLOAD
element number or element set, load type label, magnitude
where load type label is BX, BY, BZ, BXNU, BYNU, or BZNU.
Use the following option to define a body force in the radial or axial direction on axisymmetric elements:
\*DLOAD
element number or element set, load type label, magnitude
where load type label is BR, BZ, BRNU, or BZNU.
Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Body force for the Types for Selected Step
# Specifying viscous body force loads in Abaqus/Explicit
Viscous body force loads are defined by
$$
\mathbf {f} _ {\mathbf {v}} = - \mathbf {c} _ {\mathbf {v b}} \left(\mathbf {v} - \mathbf {v} _ {\mathrm{ref}}\right) \mathbf {V} _ {\mathrm{e}},
$$
where $\mathbf { f _ { v } }$ is the viscous force applied to the body; $c _ { v b }$ 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; $\mathbf { v } _ { r e f }$ is the velocity of the reference node; and $V _ { e }$ 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 $c _ { v b }$ is chosen to be a small value multiplied by the material density (see “Material damping,” Section 26.1.1). 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=reference\_node
element number or element set, VBF, magnitude
Abaqus/CAE Usage: Viscous body force loads are not supported in Abaqus/CAE.
# Specifying stagnation body force loads in Abaqus/Explicit
Stagnation body force loads are defined by
$$
\mathbf {f} _ {\mathrm{s}} = - \mathbf {c} _ {\mathrm{sb}} \left(\mathbf {v} - \mathbf {v} _ {\mathrm{ref}}\right) ^ {2} \mathbf {V} _ {\mathrm{e}},
$$
where $\mathbf { f _ { s } }$ is the stagnation body force applied to the body; $c _ { s b }$ 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; $\mathbf { v } _ { r e f }$ is the velocity of the reference node; and $V _ { e }$ is the element volume. The coefficient $c _ { s b }$ 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=reference\_node element number or element set, SBF, magnitude
Abaqus/CAE Usage: Stagnation body force loads are not supported in Abaqus/CAE.
# Specifying gravity loading
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 21.2.1), 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 34.1.1. 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/Standard and Abaqus/Explicit automatically collect all elements in the model that have mass contributions (including point mass elements but excluding rigid elements) in an element set called \_Whole\_Model\_Gravity\_Elset and apply the gravity loads to the elements in this element set. Abaqus/CFD applies the gravity loading to all user-defined elements.
In Abaqus/CFD gravity loading defines the gravity vector used with a Boussinesq-type body force in buoyancy driven flow. You must activate the energy equation for incompressible flow and define thermal expansion to specify the volumetric thermal expansion coefficient (see “Incompressible fluid dynamic analysis,” Section 6.6.2, and “Computation of buoyancy forces in Abaqus/CFD” in “Thermal expansion,” Section 26.1.2). Gravity loading can be used only in conjunction with the energy equation and will be ignored if used without the energy equation; general body forces can be defined for incompressible flow without the energy equation.
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
element number or element set, GRAV, gravity constant, comp1, comp2, comp3
Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Gravity for the Types for Selected Step
# Specifying loads due to rotation of the model in Abaqus/Standard
Centrifugal loads, Coriolis forces, rotary acceleration, and rotordynamic loads can be applied in Abaqus/Standard by specifying the appropriate distributed load type in an element-based distributed load definition. These loading options are primarily intended for replicating dynamic loads while performing analyses other than implicit dynamics using direct integration (“Dynamic stress/displacement analysis,” Section 6.3). In an implicit dynamic procedure inertia loads due to rotations come about naturally due to the equations of motion. Applying distributed centrifugal, Coriolis, rotary acceleration,
and rotordynamic loads in an implicit dynamic analysis may lead to non-physical loads and should be used carefully.
# 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,” Section 21.2.1), together with the load magnitude and the axis of rotation, to calculate the loading. Alternatively, a centrifugal load magnitude can be given as $\rho \omega ^ { 2 }$ , 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 “Prescribed conditions: overview,” Section 34.1.1. 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.
Input File Usage: Use either of the following options to define a centrifugal load:
\*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
Abaqus/CAE Usage: 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 “Prescribed conditions: overview,” Section 34.1.1. 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.
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.
Input File Usage: Use the following option to define a Coriolis load:
\*DLOAD
element number or element set, CORIO, , coord1, coord2, coord3, comp1, comp2, comp3
Abaqus/CAE Usage: 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, , 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,” Section 21.2.1), 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 34.1.1. 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
element number or element set, ROTA, , coord1, coord2, coord3, comp1, comp2, comp3
Abaqus/CAE Usage: 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 ( ), 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,” Section 6.1.2, 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, , 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 “Prescribed conditions: overview,” Section 34.1.1. 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.
Input File Usage: Use the following option to define a rotordynamic load:
\*DLOAD
element number or element set, ROTDYNF, , coord1, coord2, coord3, comp1, comp2, comp3
Abaqus/CAE Usage: Element-based rotordynamic loads are not supported in Abaqus/CAE.
# Specifying porous drag body force load in Abaqus/CFD
In Abaqus/CFD porous drag loading defines the porous drag body forces (Darcy and inertial drag forces) in flow through porous media (see “Incompressible fluid dynamic analysis,” Section 6.6.2). If the porous drag body forces are activated, permeability of the medium must be defined (see “Permeability,” Section 26.6.2). In addition, if the energy equation for incompressible flow is activated for porous flow problems involving heat transfer, the properties of both the solid and fluid phases of the porous medium must be defined using a fluid section definition. Porous drag loads are defined by specifying the dimensionless porosity, (ratio of the fluid to the total volume of the porous medium). The porosity value specified with the porous drag body load will override the porosity value specified with the permeability of the fluid material.
Input File Usage: Use the following option to define a porous drag body force load:
\*DLOAD
element number or element set, PDBF, porosity
Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Porous drag body force for the Types for Selected Step