Steady-state transport analysis

By default, the steady-state transport analysis procedure in Abaqus/Standard solves for a steady-state rolling and sliding solution directly as a series of increments, with iterations to obtain equilibrium within each increment. The solution in each increment is a steady-state solution corresponding to the loads acting on the structure at that instant. The steady-state transport analysis procedure also provides an alternative technique to obtain a quasi-steady-state rolling and sliding solution as a series of increments, with iterations to obtain equilibrium within each increment. However, the solution in each increment is usually not a steady-state solution corresponding to the loads acting on the structure at that instant. A steady-state solution is generally obtained in several increments, with each increment corresponding to a loading pass through the structure. Each loading pass through the structure can have a different magnitude.

The pass-by-pass analysis technique is relevant only when used with plasticity/creep models. It has no effect on a viscoelastic material model.

STEADY STATE TRANSPORT, PASS BY PASS

Local instabilities (e.g., surface wrinkling, material instability, or local buckling), can occur in a steady-state transport analysis. Abaqus/Standard offers the option to stabilize this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in Automatic stabilization of unstable problems.

You can generate a three-dimensional mesh by revolving a two-dimensional cross-section about a symmetry axis, so that the streamlines follow the mesh lines. In this case the symmetric model generation capability requires a two-dimensional cross-section of the body as a starting point. The cross-section, which must be discretized with axisymmetric finite elements, is defined in a separate input file. A data check analysis must be performed to write the model information to a restart file. The restart file is read in a subsequent run, and a three-dimensional model is generated by Abaqus/Standard by revolving the cross-section about the symmetry axis, starting at a reference plane. Both the symmetry axis and reference plane of the new three-dimensional model can be oriented in any direction in the global coordinate system. The symmetry axis also defines the axis of the spinning body. A nonuniform discretization in the circumferential direction can be specified to allow a finer mesh in the contact region than elsewhere in the model.

SYMMETRIC MODEL GENERATION, REVOLVE

Alternatively, you can generate a periodic three-dimensional mesh by revolving a single three-dimensional sector about its axis of symmetry. To accurately account for the material convection when the streamline integration is performed, the segment angle for the repetitive three-dimensional sector must be chosen small enough.

In this case the symmetric model generation capability requires a single three-dimensional sector as a starting point. The original three-dimensional sector is defined in a separate input file. A data check analysis must be performed to write the model information to a restart file. The restart file is read in a subsequent run, and a three-dimensional periodic model is generated by Abaqus/Standard by revolving the original three-dimensional sector about the symmetry axis. Both the symmetry axis and the original three-dimensional repetitive sector can be oriented in any direction in the global coordinate system. The symmetry axis also defines the axis of the spinning body. There is no restriction that the meshes on the two symmetry surfaces of the repetitive sector match in any way. If the surface meshes on either side of the original sector are not matched completely, constraints will be generated automatically to couple the opposing neighboring surfaces when revolving the original sector to create a periodic model.

SYMMETRIC MODEL GENERATION, PERIODIC

By default, the rigid body motion in the whole model will be described in a spatial or Eulerian manner. In some cases you may want only part of the model to be treated with the Eulerian method while the rest should be treated with the classical Lagrangian method. One typical example is a disc brake where the disc itself can be treated with the Eulerian method while the brake assembly (brake pads and caliper) is treated with the Lagrangian method. In this case you can specify the name of an element set for which the rigid body motion will be described in an Eulerian manner. The elements that are not included in the element set will be treated with the classical Lagrangian method. Only one Eulerian element set can be specified in the whole model. In a new steady-state transport step or upon restart (see Restarting an analysis) you can respecify a set of elements to be treated with the Eulerian method even after it has previously been treated with the Lagrangian method and vice versa. Elements treated with the Eulerian method and elements treated with the Lagrangian method cannot be mixed along a streamline.

STEADY STATE TRANSPORT, ELSET=name

The spinning motion of the deformable body around its own axis is described by a user-specified angular velocity, $\mathit{\omega }$ (see Figure 1). This angular velocity defines the transport of material through the mesh; you define the magnitude of the spinning rotation, $\omega$. The axis of revolution is the symmetry axis used for generating the mesh as described in Defining the model. The transport velocity must be defined for all nodes on the spinning body. The magnitude of the angular velocity can also be defined with user subroutine UMOTION.

The transport velocity can also be applied to a rigid body based on a three-dimensional surface of revolution. In that case the velocity is applied to the rigid body reference node to describe the transport of the (rigid) material relative to the reference node. Abaqus/Standard assumes that the rigid body spins around the axis of revolution of the rigid body. This option can, for example, be applied to the rigid body representing the rim on which a tire is mounted.

Abaqus/Standard will automatically update the position and orientation of the rotation axis to the current configuration in a large-displacement analysis, such as in the case where a prescribed load applied to the reference node of a rotating rigid drum maintains the contact pressure between the tire and drum or the case where a camber angle is applied to the axle of the deformable body.

TRANSPORT VELOCITY
TRANSPORT VELOCITY, USER

The rotating deformable body is also associated with a reference frame. This reference frame can either translate or rotate with respect to the fixed global reference frame. Similarly, each rigid body must be defined in a reference frame that is either fixed, translates, or rotates. For example, to associate straight line travel at ground velocity, $\mathbf{c}$, with a spinning deformable body, the deformable body can be defined in a reference frame translating at velocity $\mathbf{c}$ and the rigid surface can be defined in a fixed reference frame. Alternatively, the deformable body can be defined in a reference frame that does not translate and the rigid body can be defined in a frame translating at velocity $-\mathbf{c}$. Another example is a deformable body precessing along a circular path such as shown in Figure 1. In such a case a rotating frame is associated with the deformable body that defines the precession axis and angular velocity, while the rigid body is defined in a fixed reference frame. All components of the reference frame motion are zero unless otherwise specified; components of the reference frame motion cannot be treated as unknowns to be determined by the simulation.

You can apply a specified motion of the reference frame to all nodes of the deformable body or to the reference node of a rigid body. A translating reference frame is defined by specifying the components of the velocity vector, $\mathbf{c}$. A rotating reference frame is defined by specifying the magnitude of an angular rotation velocity, $\mathrm{\Omega }$, and the position and orientation of the axis of rotation in the current configuration. The position and orientation of the axis are applied at the beginning of the step and remain fixed during the step.

MOTION, TRANSLATION

MOTION, ROTATION 

The rigid surface can be either an analytical surface or made from rigid elements. When the master and slave surfaces move with different velocities, you will normally select to use a Coulomb friction law that assumes that slip occurs if the frictional stress

is equal to the critical stress ${\tau }_{crit}=\mu p$, where ${\tau }_1$ and ${\tau }_2$ are the shear stresses on the contact plane, $\mu$ is the friction coefficient, and p is the contact pressure. No slip occurs when ${\tau }_{eq}<{\tau }_{crit}$. For steady-state transport the condition of no slip is approximated in Abaqus/Standard by stiff “viscous” behavior

where ${\dot{\gamma }}_{\alpha }$ are the tangential slip velocities that depend on deformation along a streamline and

is the “stick viscosity,” R is the radius of the cylinder, and $F_f$ is a user-defined slip tolerance for which the default is 0.005. Using a larger slip tolerance makes convergence of the solution more rapid at the expense of solution accuracy. Using a smaller slip tolerance imposes the “no relative motion” constraint more accurately but may slow convergence. The default value provides a conservative balance between efficiency and accuracy for rolling contact problems.

Since this frictional model used for steady-state rolling is different from the frictional models used with other analysis procedures in Abaqus/Standard, discontinuities may arise in the solutions between a steady-state transport analysis and any other analysis procedure, such as a static footprint analysis. To ensure a smooth transition in the solution, it is recommended that all analysis steps prior to a steady-state rolling analysis use a zero coefficient of friction. You can then modify the friction properties in the steady-state transport analysis step to use the desired friction coefficient (see Changing friction properties during an Abaqus/Standard analysis).

This frictional model is more relevant in a tire analysis since the velocity of the rotating tire strongly depends on the deformation gradients along a streamline on the contact surface. The solution state at a material point depends on the solution of neighboring points, and convective effects must be considered. However, since the deformation gradients along a streamline on the contact surface are small in a disc brake analysis, a simplified frictional model, which ignores the convective effect on the contact surface, can be used. Such a frictional model is discussed in the following section.

When the slave and master surfaces rotate with different velocities, such as contact between a disc and brake assembly, slip will develop between the two deformable surfaces. The transport velocity (Spinning motion) and the motion of a reference frame (Defining a reference frame for translational or rotational motion) can be defined in a steady-state transport analysis procedure to model the steady-state frictional sliding between two deformable bodies that are moving with different velocities. In this case it is assumed that the slip rate simply follows from the difference in velocities specified by the transport velocity and the motion of the reference frame and is independent of the deformation gradient along a streamline or the nodal displacements on the contact surface. No convective effects are considered between the contact surfaces, and the frictional stress does not depend on any history effects. Hence, the frictional stress is given by

where $\mu$ is the friction coefficient, p is the contact pressure, $t_{\alpha }$ are the local tangent directions, and ${\dot{\gamma }}_{\alpha }$ are the slip velocities that are defined by the transport velocity and the motion of the reference frame. If no velocity or the same velocity are defined at contact nodes with friction, sticking conditions are applied automatically. The friction model is described in detail in Coulomb friction.

Such a simplified frictional model is relevant only in a disc brake analysis. It should be used with care in a rolling tire analysis where deformation gradients on the contact surface are significant.

Since this frictional behavior is different from the frictional models used with other analysis procedures in Abaqus/Standard, discontinuities may arise in the solutions between a steady-state transport analysis and any other analysis procedure. An example is the discontinuity that occurs between the initial preloading of the disc pads in a disc brake system and the subsequent braking analysis where the disc spins with a prescribed rotation. To ensure a smooth transition in the solution, it is recommended that all analysis steps prior to a steady-state analysis use a zero coefficient of friction (see Including friction properties in a contact property definition). You can then increase the friction coefficient to the desired value in the steady-state transport analysis (see Changing friction properties during an Abaqus/Standard analysis).

When the slave and master surfaces rotate with the same angular velocity, such as the surface between the bead and rim in a tire analysis, no relative velocity develops between the surfaces. In such a case, frictional stresses develop as a reaction between the bodies. Abaqus/Standard will automatically determine that the slave and master surface rotate with the same speed and apply the standard Coulomb friction model, which is described in detail in Frictional behavior.

When the standard Coulomb friction model is used in a reference frame that implies flow of material through the mesh, convective effects must be considered. However, Abaqus/Standard assumes that no convective effects are present between surfaces during steady-state transport analysis. In other words, Abaqus/Standard assumes that the frictional stress at a point depends on the history of deformation in the Lagrangian reference frame and ignores any history effects that may occur as a result of the deformation that the point experiences during the spinning motion. The assumption that the frictional stress does not depend on history effects during rolling is valid for modeling contact between a tire bead and rim where relative slip occurs only during rim mounting in a static analysis prior to the steady-state transport analysis. When slip occurs during the steady-state transport analysis, the solution obtained is no longer the correct steady-state solution because convective effects are ignored. To ensure that no slip takes place between the surfaces during steady-state rolling, it is recommended that you modify the friction properties in the steady-state transport analysis step to activate rough friction (see Changing friction properties during an Abaqus/Standard analysis).

In most cases the default automatic incrementation scheme is preferred because it will select increment sizes based on computational efficiency.

STEADY STATE TRANSPORT

Direct user control of the increment size is also provided because if you have considerable experience with a particular problem, you may be able to select a more economical approach.

STEADY STATE TRANSPORT, DIRECT

STEADY STATE TRANSPORT, DIRECT=NO STOP

The frictional forces that develop on the contact surface as a result of steady-state rolling are functions of the spinning angular velocity, $\mathit{\omega }$, and the traveling straight line velocity, $\mathbf{c}$, or cornering velocity, $\mathbf{\Omega }$. When these frictional forces are large, convergence of Newton's method becomes difficult. Convergence problems in Abaqus/Standard are usually resolved by taking a smaller load increment. However, contact forces due to steady-state rolling usually do not reduce when the magnitudes of the velocities are reduced. For example, if a spinning object is prevented from moving ($\mathbf{c}=0.0$), full slipping conditions will develop over the entire contact zone for all values of spinning angular velocity $\mathit{\omega }>0.0$. Consequently, the frictional force remains constant for all $\mathit{\omega }>0.0$ (provided that the normal force remains constant), so that smaller increments in the velocities ($\mathit{\omega },\mathbf{\Omega },\mathbf{c}$) do not reduce the magnitude of the frictional forces and, hence, do not overcome convergence difficulties.

To provide for convergence through the use of smaller increments in such cases, the friction coefficient can be increased from zero to the desired value over the analysis step. This is accomplished by setting the initial friction coefficient for the model to zero (see Including friction properties in a contact property definition), then increasing the friction coefficient to its final value in the steady-state transport analysis step (see Changing friction properties during an Abaqus/Standard analysis).

Stiffness terms for Newton iterations associated with steady-state transport rely on derivatives numerically computed along streamlines. These computations can be sensitive to mesh discretization details and whether a surface-to-surface or node-to-surface contact formulation is used. Sensitivity in convergence behavior depending on which contact formulation is used will tend to diminish upon mesh refinement. (See Contact formulations in Abaqus/Standard for further discussion of contact formulations).

If the Mullins effect material model is included in the material definition (see Mullins effect), there could be a strong discontinuity in the response of a structure in transitioning from a static (non-rolling) state to a steady-state rolling state. This discontinuity is due to the damage that occurs during the transient response (such as the damage that occurs as the structure undergoes its first revolution after static preloading). Since the transient response is not modeled during a steady-state transport analysis, the resulting discontinuity in the response can lead to convergence problems. The damage associated with the Mullins effect is independent of the angular speed of rotation: as a result, time increment cutbacks do not resolve the convergence problems. The Mullins effect can be ramped up over the time period of the step in these situations to obtain a converged solution. In such a case the change in response due to damage is applied gradually over the step. The solution at the end of the step corresponds to the fully damaged material; solutions during the step correspond to a partially damaged material and are, therefore, physically meaningless. Thus, it is recommended that in going from a static to a steady-state rolling solution, a do-nothing step at a low angular speed of rotation be first carried out with the Mullins effect ramped on. This facilitates resolution of the discontinuity in a gradual manner. The do-nothing step can then be followed by the regular steady-state transport step with the Mullins effect applied instantaneously at the beginning of the step. This approach is illustrated in Analysis of a solid disc with Mullins effect and permanent set.

STEADY STATE TRANSPORT, MULLINS=RAMP or STEP (default)

Although in principle any material point along a streamline can be used as a starting point for the streamline integration when material convective calculations are performed, Abaqus/Standard always uses the material points in the original sector or the material points in the original cross-section as starting points for the streamline integration in a model with periodic geometry or axisymmetric geometry, respectively.

If the pass-by-pass solution technique is used, after an increment has been performed for all the streamlines, Abaqus/Standard will automatically use the state obtained at the end of the streamline as the starting state for the streamline integration in the subsequent increment. This iterative process is repeated for each increment until a steady-state solution is reached.

If the direct steady-state solution technique is used, several local iterations are usually required for each streamline, with a local iteration corresponding to an integration over a closed loop streamline. After a local iteration has been performed for a streamline, Abaqus/Standard will check to see if the steady-state condition is satisfied for the streamline. This is best measured by ensuring the differences between the stresses/strains at the starting point of the streamline obtained before and after the iteration are sufficiently small. If the steady-state condition is not satisfied for the streamline, Abaqus/Standard will automatically use the state obtained at the end of the previous local iteration as the starting state for the streamline integration in the subsequent local iteration. This iterative process is repeated until a steady-state solution is reached for all the streamlines.

To improve the rate of convergence, it is recommended that you apply loads on elements or nodes away from the starting points of the streamlines.

Unconstrained rigid body modes of the mesh motion will cause convergence problems for a steady-state transport analysis, similar to convergence problems for unconstrained rigid body modes in a static analysis. Friction cannot be relied on to restrict rigid body modes in a steady-state transport analysis, because frictional stresses depend on relative material velocities rather than relative nodal displacements for steady-state transport. Restricting the (steady-state) material velocity does not restrict nodal displacements for steady-state transport analyses. The material velocity includes effects of material flowing through the mesh and is governed by the spinning motion (see Spinning motion), reference frame motions (see Defining a reference frame for translational or rotational motion), and nodal positions relative to the spinning axis.

Consider the examples shown in Figure 2. End-on views are shown in Figure 2, so the axial direction (spinning axis) is horizontal in this figure. The axial component of the reference frame motion is zero for all three of these cases (either by explicit specification or implicitly by default). Since the material velocity in the axial direction at steady state is zero for both bodies (according to the reference frame motion), the frictional force in the axial direction will remain zero for all three of these cases, which may not be intuitive. The first case shown in Figure 2 (a) involves a planar interface and a boundary condition in the axial direction. At the time the rolling body reaches steady state, the axial motion has stopped, the axial friction force is zero, and the reaction force associated with the boundary condition is zero (which also may not be intuitive).

The second case in Figure 2 (b) has a planar interface and an applied force in the axial direction. The axial frictional force for the steady-state solution remains zero, as already discussed, so no axial force arises to counter the applied force. Therefore, Abaqus/Standard will not provide a converged solution in this case, which is an example of unconstrained rigid body mesh motion. The third case shown in Figure 2 (c) is like the second case, except a “curb” has been added to the rigid surface. In this case, a contact force in the normal direction occurs at the location of the “curb,” which counters the applied force, so the analysis is able to converge.

Figure 2. Displacement boundary condition versus concentrated force.

As a real world example, consider a car traveling along a straight planar road with a truck moving parallel to the car, applying a constant concentrated force that pushes the car sideways. With zero toe angle on the car’s front wheels (that is, the wheels are exactly aligned with the longitudinal axis of the car), steady-state motion is impossible, and the car will eventually slip off the road. To resist the push in steady-state motion, the car wheels need to be aligned with the proper toe angle.