ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE Including friction properties in a contact property definitionAbaqus assumes by default that the interaction between contacting bodies is frictionless. You can include a friction model in a contact property definition for both surfacebased contact and elementbased contact. Input File Usage Use both of the following options for surfacebased contact: SURFACE INTERACTION, NAME=interaction_property_name FRICTION Use both of the following options for elementbased contact in Abaqus/Standard: INTERFACE or GAP, ELSET=name FRICTION Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior Elementbased contact is not supported in Abaqus/CAE. Changing friction properties during an analysisThe methods used to change friction properties during an analysis differ between Abaqus/Standard and Abaqus/Explicit. Changing friction properties during an Abaqus/Standard analysisIt is possible to remove, to modify, or to add a friction model that does not involve a user subroutine to a contact property definition in any particular step of an Abaqus/Standard simulation. In some models, such as shrinkfit contact interference problems, friction should not be added until after the first steps have been completed. In other models friction might be removed or lowered to represent the introduction of a lubricant between the bodies. You must identify which contact property definition or contact element set is being changed. Input File Usage Use both of the following options for surfacebased contact: CHANGE FRICTION, INTERACTION=name FRICTION Use both of the following options for elementbased contact: CHANGE FRICTION, ELSET=name FRICTION Abaqus/CAE Usage Define a contact property with a new friction definition. Then change the contact property assigned to an interaction in a particular step. Interaction module: Contact property editor: MechanicalTangential Behavior Interaction editor: Contact interaction property: new_interaction_property_name Elementbased contact is not supported in Abaqus/CAE. Specifying the time variation of the change in friction propertiesYou can specify an amplitude curve (see Amplitude Curves) to define the time variation of changes in friction coefficients and, if applicable, allowable elastic slip (see Stiffness method for imposing frictional constraints in Abaqus/Standard below) throughout the step. If you do not specify an amplitude curve, changes in these friction properties are either applied immediately at the beginning of the step or ramped up linearly over the step, depending on the default amplitude variation assigned to the step (see Defining an analysis), with some exceptions as described below. For many step types the default transition type is a linear ramping from old to new values, which helps avoid convergence problems that can occur upon sudden changes in friction properties. Amplitude curves used to control variations in friction properties are subjected to the following restrictions:
The value of a friction coefficient or allowable elastic slip in effect at a given time is typically equal to the value of the property at the start of the step plus the current amplitude value times the anticipated change in property value over the step. Variations in friction properties must consider the following:
Input File Usage CHANGE FRICTION, AMPLITUDE=name Abaqus/CAE Usage Timedependent changes in friction properties are not supported in Abaqus/CAE. Resetting the frictional properties to their default valuesYou can reset the frictional properties of the specified contact property definition or element set to their original values. Input File Usage Use either of the following options: CHANGE FRICTION, RESET, INTERACTION=name CHANGE FRICTION, RESET, ELSET=name In this case the FRICTION option is not needed. Abaqus/CAE Usage Interaction module: Contact property editor: MechanicalTangential Behavior: Friction formulation: Frictionless Interaction editor: Contact interaction property: default_interaction_property_name Changing friction properties during an Abaqus/Explicit analysisIn Abaqus/Explicit the friction definition is specified as part of the model definition for a general contact analysis and as part of the history definition for a contact pair analysis. See Assigning contact properties for general contact in Abaqus/Explicit and Assigning contact properties for contact pairs in Abaqus/Explicit for information on changing aspects of any contact property definition during an Abaqus/Explicit analysis. Using the basic Coulomb friction modelThe basic concept of the Coulomb friction model is to relate the maximum allowable frictional (shear) stress across an interface to the contact pressure between the contacting bodies. In the basic form of the Coulomb friction model, two contacting surfaces can carry shear stresses up to a certain magnitude across their interface before they start sliding relative to one another; this state is known as sticking. The Coulomb friction model defines this critical shear stress, ${\tau}_{crit}$, at which sliding of the surfaces starts as a fraction of the contact pressure, p, between the surfaces (${\tau}_{crit}=\mu p$). The stick/slip calculations determine when a point transitions from sticking to slipping or from slipping to sticking. The fraction, $\mu $, is known as the coefficient of friction. For the case when the slave surface consists of a nodebased surface, the contact pressure is equal to the normal contact force divided by the crosssectional area at the contact node. In Abaqus/Standard the default crosssectional area is 1.0; you can specify a crosssectional area associated with every node in the nodebased surface when the surface is defined or, alternatively, assign the same area to every node through the contact property definition. In Abaqus/Explicit the crosssectional area is always 1.0, and you cannot change it. The basic friction model assumes that $\mu $ is the same in all directions (isotropic friction). For a threedimensional simulation there are two orthogonal components of shear stress, ${\tau}_{1}$ and ${\tau}_{2}$, along the interface between the two bodies. These components act in the local tangent directions for the contact surfaces or contact elements. The local tangent directions for contact surfaces are defined in Contact formulations in Abaqus/Standard, and those for contact elements are defined in the sections describing contact modeling with those elements. Abaqus combines the two shear stress components into an “equivalent shear stress,” ${\tau}_{eq}$, for the stick/slip calculations, where ${\tau}_{eq}=\sqrt{{\tau}_{1}^{2}+{\tau}_{2}^{2}}$. In addition, Abaqus combines the two slip velocity components into an equivalent slip rate, ${\dot{\gamma}}_{eq}=\sqrt{{\dot{\gamma}}_{1}^{2}+{\dot{\gamma}}_{2}^{2}}$. The stick/slip calculations define a surface (see Figure 1 for a twodimensional representation) in the contact pressure–shear stress space along which a point transitions from sticking to slipping. Figure 1. Slip regions for the basic Coulomb friction model.
There are two ways to define the basic Coulomb friction model in Abaqus. In the default model the friction coefficient is defined as a function of the equivalent slip rate and contact pressure. Alternatively, you can specify the static and kinetic friction coefficients directly. Using the default modelIn the default model you define the coefficient of friction directly as $$\mu =\mu \left({\dot{\gamma}}_{eq},p,\overline{\theta},{\overline{f}}^{\alpha}\right),$$
where ${\dot{\gamma}}_{eq}$ is the equivalent slip rate, p is the contact pressure, $\overline{\theta}=\frac{1}{2}\left({\theta}_{A}+{\theta}_{B}\right)$ is the average temperature at the contact point, and ${\overline{f}}^{\alpha}=\frac{1}{2}\left({f}_{A}^{\alpha}+{f}_{B}^{\alpha}\right)$ is the average predefined field variable $\alpha $ at the contact point. ${\theta}_{A}$, ${\theta}_{B}$, ${f}_{A}^{\alpha}$, and ${f}_{B}^{\alpha}$ are the temperature and predefined field variables at points A and B on the surfaces. Point A is a node on the slave surface, and point B corresponds to the nearest point on the opposing master surface. The temperature and field variables are interpolated along the surface at location B. If the master surface consists of a rigid body, the temperature and field variable at the reference node are used. The friction coefficient can depend on slip rate, contact pressure, temperature, and field variables. By default, it is assumed that the friction coefficients do not depend on field variables. The coefficient of friction can be set to any nonnegative value. A zero friction coefficient means that no shear forces will develop and the contact surfaces are free to slide. You do not need to define a friction model for such a case. Input File Usage FRICTION, DEPENDENCIES=n $\mu $, ${\dot{\gamma}}_{eq}$, p, $\overline{\theta}$, ${\overline{f}}^{\alpha}$ Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Penalty: Friction If necessary, toggle on Use slipratedependent data, Use contactpressuredependent data, and/or Use temperaturedependent data; and/or specify the Number of field variable dependencies in addition to slip rate, contact pressure, and temperature. Specifying static and kinetic friction coefficientsExperimental data show that the friction coefficient that opposes the initiation of slipping from a sticking condition is different from the friction coefficient that opposes established slipping. The former is typically referred to as the “static” friction coefficient, and the latter is referred to as the “kinetic” friction coefficient. Typically, the static friction coefficient is higher than the kinetic friction coefficient. In the default model the static friction coefficient corresponds to the value given at zero slip rate, and the kinetic friction coefficient corresponds to the value given at the highest slip rate. The transition between static and kinetic friction is defined by the values given at intermediate slip rates. In this model the static and kinetic friction coefficients can be functions of contact pressure, temperature, and field variables. Abaqus also provides a model to specify a static and a kinetic friction coefficient directly. In this model it is assumed that the friction coefficient decays exponentially from the static value to the kinetic value according to the formula: $$\mu ={\mu}_{k}+\left({\mu}_{s}{\mu}_{k}\right){e}^{{d}_{c}{\dot{\gamma}}_{eq}},$$
where ${\mu}_{k}$ is the kinetic friction coefficient, ${\mu}_{s}$ is the static friction coefficient, ${d}_{c}$ is a userdefined decay coefficient, and ${\dot{\gamma}}_{eq}$ is the slip rate (see Oden, J. T. and J. A. C. Martins, 1985). This model can be used only with isotropic friction and does not allow dependence on contact pressure, temperature, or field variables. There are two ways of defining this model. Providing the static, kinetic, and decay coefficients directlyYou can provide the static friction coefficient, the kinetic friction coefficient, and the decay coefficient directly (see Figure 2). Figure 2. Exponential decay friction model.
Input File Usage FRICTION, EXPONENTIAL DECAY ${\mu}_{s}$, ${\mu}_{k}$, ${d}_{c}$ Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: StaticKinetic Exponential Decay: Friction, Definition: Coefficients Using test data to fit the exponential modelAlternatively, you can provide test data points to fit the exponential model. At least two data points must be provided. The first point represents the static coefficient of friction specified at ${\dot{\gamma}}_{eq}=0.0$, and the second point, (${\dot{\gamma}}_{2}$, ${\mu}_{2}$) (shown in Figure 3), corresponds to an experimental measurement taken at a reference slip rate ${\dot{\gamma}}_{2}$. An additional data point can be specified to characterize the exponential decay. If this additional data point is omitted, Abaqus will automatically provide a third data point, (${\dot{\gamma}}_{\mathrm{\infty}}$, ${\mu}_{\mathrm{\infty}}$), to model the assumed asymptotic value of the friction coefficient at infinite velocity. In such a case ${\mu}_{\mathrm{\infty}}$ is chosen such that $\left({\mu}_{2}{\mu}_{\mathrm{\infty}}\right)/\left({\mu}_{1}{\mu}_{\mathrm{\infty}}\right)=0.05$. Input File Usage FRICTION, EXPONENTIAL DECAY, TEST DATA ${\mu}_{1}$ ${\mu}_{2}$, ${\dot{\gamma}}_{2}$ ${\mu}_{\mathrm{\infty}}$ Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: StaticKinetic Exponential Decay: Friction, Definition: Test data Figure 3. Exponential decay friction model specified with test data
points.
Using the optional shear stress limitYou can specify an optional equivalent shear stress limit, ${\tau}_{max}$, so that, regardless of the magnitude of the contact pressure stress, sliding will occur if the magnitude of the equivalent shear stress, ${\tau}_{eq}$, reaches this value (see Figure 4). A value of zero is not allowed. Figure 4. Slip regions for the friction model with a limit on the critical shear
stress.
This shear stress limit is typically introduced in cases when the contact pressure stress may become very large (as can happen in some manufacturing processes), causing the Coulomb theory to provide a critical shear stress at the interface that exceeds the yield stress in the material beneath the contact surface. A reasonable upper bound estimate for ${\tau}_{max}$ is ${\sigma}_{y}/\sqrt{3}$, where ${\sigma}_{y}$ is the Mises yield stress of the material adjacent to the surface; however, empirical data are the best source for ${\tau}_{max}$. Input File Usage FRICTION, TAUMAX=${\tau}_{max}$ Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Penalty or Lagrange Multiplier: Shear Stress, Shear stress limit: Specify: ${\tau}_{max}$ Limitations with the shear stress limitIn Abaqus/Explicit a shear stress limit cannot be used when a contact pair uses a nodebased surface as one of the surfaces. Anisotropic friction with directional preference as a surface propertyYou can specify an anisotropic friction model in Abaqus/Explicit for which directional preferences are specified as surface properties, while the nominal, or average, friction coefficient is specified as a contact interaction property in the same manner as for isotropic friction. The resulting critical contact shear stress surface is elliptical in the ${\tau}_{1}$–${\tau}_{2}$ plane, as shown in Figure 5. Points on the critical shear stress surface satisfy the equation: $$\sqrt{{\tau}_{1}^{2}+{\tau}_{2}^{2}}={s}_{combined}{\left(\theta \right)\text{\hspace{0.17em}}\mu}_{nom}P,$$
where ${s}_{combined}$ represents the combined effects of surfacebased directional preferences (and these combined effects evolve as the relative surface orientations change), ${\mu}_{nom}$ is the specified nominal (average) friction coefficient, and $P$ is the contact pressure. Maximum and minimum values of ${s}_{combined}$, corresponding to directions along the major and minor axes of the critical shear stress surface, are ${s}_{combined}^{\mathrm{max}}=1+{\u03f5}_{combined}$ and ${s}_{combined}^{\mathrm{min}}=1{\u03f5}_{combined}$. Figure 5. Critical shear stress surface for anisotropic friction.
$\u03f5$ is the frictional directional preference factor. It is a unitless parameter that can range from –1.0 to 1.0 and is a measure of the eccentricity of the scaling ellipse. The most commonly used eccentricity measure for ellipses is $e=\text{\hspace{0.17em}}\frac{c}{a}$ (see Figure 6). The relationship between $\u03f5$ and $e$ is: $${\left(\frac{b}{a}\right)}^{2}=\frac{{(1\u03f5)}^{2}}{{(1+\u03f5)}^{2}},$$
$$e=\text{\hspace{0.17em}}2*\frac{\sqrt{\u03f5}}{(1+\u03f5)}\mathrm{.}$$
Figure 6. Geometrical quantities for an ellipse.
The critical contact shear stress surface influences the friction algorithm as follows:
${s}_{combined}$ can be thought of as a scaling ellipse calculated as a weighted average of surfacebased scaling ellipses: $${s}_{combined}\left(\theta \right)={w}_{1}{s}_{surf1}\left(\theta \right)+{w}_{2}{s}_{surf2}\left(\theta \right),$$
where the weight factors sum to unity (${w}_{1}+{w}_{2}=1$). ${s}_{surf1}$ and ${s}_{surf2}$ are scaling ellipses representing directional preferences of respective surfaces at a contact location. The maximum and minimum principal values of each scaling ellipse are of the form ${s}_{i}=1+{\u03f5}_{i}$ and ${s}_{i}=1{\u03f5}_{i}$, respectively. A lack of directional preference corresponds to ${\u03f5}_{i}=0$. If both surfaces of a contact interaction contribute directional preference to the frictional behavior, the shape of the ${s}_{combined}$ scaling ellipse evolves as the (relative) orientations of the contacting surfaces change. For example, for contact between like surfaces with equal weighting factors (${w}_{1}={w}_{2}=\frac{1}{2}$): $${\u03f5}_{combined}={\u03f5}_{s}\mathrm{cos}\left(\gamma \right),$$
where ${\u03f5}_{s}{=\u03f5}_{surf1}={\u03f5}_{surf2}$ and $\gamma $ is the angle between major axes of the surface scaling ellipses across the contact interface. Consider the following specific cases for contact between like surfaces:
Figure 9. Examples of contact between like surfaces with directional preferences
aligned (Case 1) and orthogonal (Case 2).
Figure 10. Scaling ellipse combinations when directional preferences of like
surfaces are aligned (Case 1) and orthogonal (Case 2).
Input File Usage Use the following option to specify the nominal friction coefficient for an anisotropic friction model with surfacebased directional preferences: FRICTION, ANISOTROPIC BEHAVIOR=SURFACE PROPERTY Use the following options to specify the surfacebased directional preferences and the frictional directional preference factor: SURFACE PROPERTY ASSIGNMENT, PROPERTY=ORIENTATION FRICTION, DEPENDENCIES=n $\mu $, ${\dot{\gamma}}_{eq}$, p, $\overline{\theta}$, ${\overline{f}}^{\alpha}$ Weighting methods for combining preferential direction effects of surfaces for anisotropic frictionAbaqus/Explicit provides three options for computing weight factors for determination of ${s}_{combined}\left(\theta \right)={w}_{1}{s}_{surf1}\left(\theta \right)+{w}_{2}{s}_{surf2}\left(\theta \right)$. ${w}_{1}={w}_{2}=\frac{1}{2}$ for all cases with ${\u03f5}_{surf1}={\u03f5}_{surf2}$. For cases with ${\u03f5}_{surf1}\ne {\u03f5}_{surf2}$, ${w}_{1}$ is established according to one of the following three weighting methods (and ${w}_{2}=1{w}_{1}$):
Consider a contact interaction in which only one surface introduces directional preference, with ${\u03f5}_{surf1}=\frac{1}{3}$ and ${\u03f5}_{surf2}=0$. In this case balanced weighting leads to ${\u03f5}_{combined}=\frac{1}{6}$, as shown in Figure 11. The other two weighing methods lead to ${w}_{1}=1$ and ${w}_{2}=0$ for this example, in which case the combined scaling ellipse is identical to the scaling ellipse for the surface with directional preference and ${\u03f5}_{combined}=\frac{1}{3}$. Figure 11. Balanced weighting for anisotropic friction with one surface
contributing directional preference.
The effect of balanced weighting for a situation with ${\u03f5}_{surf1}=\frac{1}{3}$ and ${\u03f5}_{surf2}=\frac{1}{5}$ with a $45\xb0$ angle between major axes of the surface scaling ellipses is represented in Figure 12. Weight factors for this combination of surface scaling ellipses according to the different weighting methods are:
Figure 12. Balanced weighting for anisotropic friction with both surfaces
contributing directional preference.
Input File Usage Use the following option to specify the balanced weighting method for combining surfacebased directional preferences for the anisotropic friction model: FRICTION, ANISOTROPIC BEHAVIOR=SURFACE PROPERTY, WEIGHT=BALANCED Use the following option to specify the epsilonproportional weighting method for combining surfacebased directional preferences for the anisotropic friction model: FRICTION, ANISOTROPIC BEHAVIOR=SURFACE PROPERTY, WEIGHT=PROPORTIONAL Use the following option to specify the maximumepsilondominant weighting method for combining surfacebased directional preferences for the anisotropic friction model: FRICTION, ANISOTROPIC BEHAVIOR=SURFACE PROPERTY, WEIGHT=DOMINANT Defining the friction coefficientAs explained, the critical shear stress surface is proportional to the average, or nominal, friction coefficient. For convenience, you can also specify the minimum or maximum friction coefficient rather than the average one. Internally the value will be converted to the average friction coefficient using the following formulas: $${\mu}_{\mathrm{min}}=[1({\omega}_{1}{\u03f5}_{1}+{\omega}_{2}{\u03f5}_{2})]{\mu}_{nom},\text{\hspace{0.17em}}$$
$${\mu}_{\mathrm{max}}=[1+({\omega}_{1}{\u03f5}_{1}+{\omega}_{2}{\u03f5}_{2})]{\mu}_{nom}\mathrm{.}\text{\hspace{0.17em}}$$
Input File Usage Use the following option to specify the average friction coefficient (default): FRICTION, ANISOTROPIC BEHAVIOR=SURFACE PROPERTY, NOMINAL=AVERAGE Use the following option to specify the minimum friction coefficient: FRICTION, ANISOTROPIC BEHAVIOR=SURFACE PROPERTY, NOMINAL=MINIMUM Use the following option to specify the maximum friction coefficient: FRICTION, ANISOTROPIC BEHAVIOR=SURFACE PROPERTY, NOMINAL=MAXIMUM Measure of the eccentricity of the scaling ellipseThe measure of eccentricity of the scaling ellipse for each surface is defined using the frictional directional preference factor $\u03f5$. Sometimes it is useful to specify the scaling ellipse using the ratio of the friction coefficients: $$r=\frac{{\mu}_{\mathrm{max}}}{{\mu}_{\mathrm{min}}}\mathrm{.}$$
The relationship between $\u03f5$ and $r$ is given by the following formula: $$\u03f5=\frac{(r1)}{(r+1)}\mathrm{.}$$
Input File Usage To specify the frictional directional preference factor $\u03f5$ (default): SURFACE PROPERTY ASSIGNMENT, PROPERTY=ORIENTATION, FRICTION ANISOTROPY=EPSILON To specify the ratio of the friction cofficients $r$: SURFACE PROPERTY ASSIGNMENT, PROPERTY=ORIENTATION, FRICTION ANISOTROPY=RATIO Output of the preferred directionsThe preferred local directions for each surface in contact can be output by requesting the generic output variable CORIENT (with the respective vector components CORIENT1 and CORIENT2). Anisotropic friction with directional preference associated with contact orientationDirectional preference for this anisotropic friction model is specified as a contact property and is implicitly associated with one surface of a contact interaction. This friction model is available in Abaqus/Standard and is less general than the anisotropic friction model discussed in Anisotropic friction with directional preference as a surface property, which allows both surfaces of a contact interaction to contribute directional preference characteristics. If you indicate that this anisotropic friction model should be used, you must specify two friction coefficients, where ${\mu}_{1}$ is the coefficient of friction in the first local tangent direction and ${\mu}_{2}$ is the coefficient of friction in the second local tangent direction. The critical contact shear stress surface for this friction model (see Figure 13) is elliptical in the ${\tau}_{1}$–${\tau}_{2}$ plane, like the anisotropic friction model discussed in Anisotropic friction with directional preference as a surface property. The shape of the critical contact shear stress surface remains constant in this case, with the extreme points being ${\tau}_{1}^{crit}={\mu}_{1}p$ and ${\tau}_{2}^{crit}={\mu}_{2}p$. The orientation of the critical contact shear stress for this friction model evolves with the local tangent directions of the contact interaction, which are discussed in Local tangent directions on a surface. For example, local tangent directions for the finitesliding, surfacetosurface contact formulation are established from, and evolve with, the slave surface of the contact interaction, so, in this example, directional preference for this anisotropic friction model would evolve with the orientation of the slave surface (and would be independent of the master surface). The size of the criticalshearstress ellipse will change with the change in contact pressure between the surfaces. The direction of slip, $d{\gamma}_{\alpha}$, is orthogonal to the critical shear stress surface. The optional equivalent shear stress limit, ${\tau}_{max},$ is applied to the scaled equivalent shear stress, ${\overline{\tau}}_{eq}$, for anisotropic friction. See Anisotropic friction for the definition and discussion of ${\overline{\tau}}_{eq}$. Figure 13. Critical shear stress surface for the anisotropic friction
model.
The friction coefficients can depend on slip rate, contact pressure, temperature, and field variables. By default, it is assumed that the friction coefficients do not depend on field variables. Input File Usage FRICTION, ANISOTROPIC BEHAVIOR=LEGACY, DEPENDENCIES=n ${\mu}_{1}$, ${\mu}_{2}$, ${\dot{\gamma}}_{eq}$, p, $\overline{\theta}$, ${\overline{f}}^{\alpha}$ Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Penalty: Friction, Directionality: Anisotropic If necessary, toggle on Use slipratedependent data, Use contactpressuredependent data, and/or Use temperaturedependent data; and/or specify the Number of field variable dependencies in addition to slip rate, contact pressure, and temperature. Preventing slipping regardless of contact pressureAbaqus offers the option of specifying an infinite coefficient of friction ($\mu =\infty $). This type of surface interaction is called “rough” friction, and with it all relative sliding motion between two contacting surfaces is prevented (except for the possibility of “elastic slip” associated with penalty enforcement) as long as the corresponding normaldirection contact constraints are active. In most cases Abaqus/Standard uses a penalty method to enforce these tangential constraints; however, a Lagrange multiplier method is used during general (nonperturbation) analysis steps if the corresponding normaldirection constraints have directly enforced “hard contact” or exponential pressureoverclosure behavior. Abaqus/Explicit uses either a kinematic or penalty method, depending on the contact formulation chosen. Rough friction is intended for nonintermittent contact; once surfaces close and undergo rough friction, they should remain closed. Convergence difficulties may arise in Abaqus/Standard if a closed contact interface with rough friction opens, especially if large shear stresses have developed. The rough friction model is typically used in conjunction with the no separation contact pressureoverclosure relationship for motions normal to the surfaces (see Using the no separation relationship), which prohibits separation of the surfaces once they are closed. When rough friction is used with the no separation relationship for hard contact in Abaqus/Explicit specified with the kinematic contact method, no relative motions of the surfaces will occur. For hard contact in Abaqus/Explicit specified with the penalty contact method, relative motions will be limited to the elastic slip and penetration corresponding to the inexact satisfaction of the contact constraints by the applied penalty forces. When softened tangential behavior is specified in Abaqus/Explicit (see Defining tangential softening in Abaqus/Explicit below), the relative surface motions will be governed by the specified softening behavior. Input File Usage FRICTION, ROUGH Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Rough Shear stress versus elastic slip while stickingIn some cases some incremental slip may occur even though the friction model determines that the current frictional state is “sticking.” In other words, the slope of the shear (frictional) stress versus total slip relationship may be finite while in the “sticking” state, as shown in Figure 14. Figure 14. Elastic slip versus shear traction relationship for sticking and
slipping friction.
The relationship shown in this figure is analogous to elasticplastic material behavior without hardening: $\kappa $ corresponds to Young's modulus, and ${\tau}_{crit}$ corresponds to yield stress; sticking friction corresponds to the elastic regime, and slipping friction corresponds to the plastic regime. A finite value of the sticking stiffness may reflect a userspecified physical behavior or may be characteristic of the constraint enforcement method. Frictional constraints are enforced with a stiffness (penalty method) by default in Abaqus/Standard and for the general contact algorithm in Abaqus/Explicit; in this case the sticking stiffness will have a finite value. An infinite sticking stiffness, in which case the elastic slip is always zero, can be achieved with the optional Lagrange multiplier method for imposing frictional constraints in Abaqus/Standard or with the kinematic constraint method (available only for contact pairs) in Abaqus/Explicit. In Abaqus/Explicit some tangential contact damping acts on the elastic slip rate by default, as discussed in Contact damping. Tangential softening to reflect a physical behavior is available only in Abaqus/Explicit. Defining tangential softening in Abaqus/ExplicitTo activate softened tangential behavior in Abaqus/Explicit, specify the slope of the shear stress versus elastic slip relationship ($\kappa $ in Figure 14). User subroutine VFRIC cannot be used in conjunction with softened tangential behavior. Input File Usage FRICTION, SHEAR TRACTION SLOPE=$\kappa $ Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Penalty or StaticKinetic Exponential Decay: Elastic Slip, Specify: $\kappa $ Stiffness method for imposing frictional constraints in Abaqus/StandardThe stiffness method used for friction in Abaqus/Standard is a penalty method that permits some relative motion of the surfaces (an “elastic slip”) when they should be sticking (similar to the allowable elastic slip defined with softened tangential behavior in Abaqus/Explicit). While the surfaces are sticking (i.e., ${\tau}_{eq}<{\tau}_{crit}$ for the basic isotropic Coulomb friction), the magnitude of sliding is limited to this elastic slip. Abaqus continually adjusts the magnitude of the penalty constraint to enforce this condition. The stiffness method in Abaqus/Standard requires the selection of an allowable elastic slip, ${\gamma}_{crit}$. Using a large ${\gamma}_{crit}$ in the simulation makes convergence of the solution more rapid at the expense of solution accuracy (there is greater relative motion of the surfaces when they should be sticking). Behavior in which no slip is permitted in the sticking state is approximated more accurately by allowing only a small ${\gamma}_{crit}$. If ${\gamma}_{crit}$ is chosen very small, convergence problems may occur; in that case, it may be better to use the Lagrange multiplier method to apply the sticking constraint (see Lagrange multiplier method for imposing frictional constraints in Abaqus/Standard later in this section). The default value of allowable elastic slip used by Abaqus/Standard generally works very well, providing a conservative balance between efficiency and accuracy. Abaqus/Standard calculates ${\gamma}_{crit}$ as a small fraction of the “characteristic contact surface length,” ${\overline{l}}_{char}$, and scans all of the facets of all the slave surfaces when calculating ${\overline{l}}_{char}$. Abaqus/Standard reports the value of ${\overline{l}}_{char}$ used for each contact pair in the data (.dat) file if you request detailed printout of contact constraint information (see Controlling the amount of analysis input file processor information written to the data file). The allowable elastic slip is given as ${\gamma}_{crit}={F}_{f}{\overline{l}}_{char}$, where ${F}_{f}$ is the slip tolerance; the default value of ${F}_{f}$ is 0.005. This method of calculating the allowable elastic slip is used for all analysis procedures in Abaqus/Standard except steadystate transport analysis (Steadystate transport analysis), in which the penalty constraint is based on a maximum allowable slip rate, ${\dot{\gamma}}_{crit}$. The maximum slip rate is calculated as $${\dot{\gamma}}_{crit}={F}_{f}2\omega R,$$
where $\omega $ is the angular spinning rate and R is the radius of the rolling structure. If the stiffness method is used for an anisotropic friction model, ${\gamma}_{crit}$ is a nominal allowable elastic slip (or slip rate). If ${\gamma}_{1}^{e}$ and ${\gamma}_{2}^{e}$ represent components of elastic slip in the ${t}_{1}$ and ${t}_{2}$ tangent directions, respectively, the transition from stick to slip will occur when ${\gamma}_{eff}={\gamma}_{crit}$, where ${\gamma}_{eff}$ is computed as $${\gamma}_{eff}=\sqrt{\frac{2\left[{\left({\mu}_{1}{\gamma}_{1}^{e}\right)}^{2}+{\left({\mu}_{2}{\gamma}_{2}^{e}\right)}^{2}\right]}{\mu _{1}{}^{2}+\mu _{2}{}^{2}}}.$$
For example, if ${\gamma}_{2}^{e}=0$, the stick/slip transition will occur at ${\gamma}_{1}^{e}=\sqrt{\frac{1}{2}\left(1+\frac{{\mu}_{2}^{2}}{{\mu}_{1}^{2}}\right)}{\gamma}_{crit}$. Depending on values of ${\mu}_{1}$ and ${\mu}_{2}$, this ${\gamma}_{1}^{e}$ can be greater or smaller than ${\gamma}_{crit}$. As another example, if the “1” and “2” components of elastic slip are equal, the stick/slip transition will occur at ${\gamma}_{1}={\gamma}_{2}=\frac{{\gamma}_{crit}}{\sqrt{2}}$, such that the magnitude of the elastic slip, ${\gamma}_{mag}=\sqrt{{\gamma}_{1}^{2}+{\gamma}_{2}^{2}}={\gamma}_{crit}$. Cases in which the default elastic slip value may not be suitableIn certain situations the default value for the allowable elastic slip may not be suitable. For example, slave surfaces defined by nodebased surfaces or some contact element types, such as GAPUNI elements, have no physical dimensions and Abaqus/Standard cannot estimate a value of ${\overline{l}}_{char}$. For models containing only nodebased surfaces or these types of contact elements, Abaqus/Standard first tries to use the “characteristic contact surface length” of the other contact pairs in the model. If there are none, it calculates ${\overline{l}}_{char}$ using all of the elements in the model and issues a warning message. If a model contains no elements for which a characteristic length can be determined (for example, if it contains only substructures), Abaqus/Standard has no information with which to calculate ${\overline{l}}_{char}$. As a result, it uses a value of 1.0 and issues a warning message. If the contact surface face dimensions vary greatly, the average value of ${\overline{l}}_{char}$ may be unreasonable for some contact surfaces. The elastic slip should then be specified directly for the surfaces with a much smaller “characteristic face dimension.” There are two methods for modifying the allowable elastic slip. One method is to specify ${\gamma}_{crit}$ directly; the other is to specify the slip tolerance, ${F}_{f}$. Some analyses call for nondefault ${\gamma}_{crit}$ or ${F}_{f}$ only in specific steps (see Changing friction properties during an Abaqus/Standard analysis above). Specifying the allowable elastic slip directlyYou can provide the absolute magnitude of ${\gamma}_{crit}$ directly. Specify a reasonable value for the relative displacement that may occur before surfaces actually begin to slip. Typically, the allowable elastic slip is set to a small fraction (10^{−2}–10^{−4}) of a “characteristic contact surface face dimension.” In a steadystate transport analysis you can define the maximum allowable viscous slip rate, ${\dot{\gamma}}_{crit}$. The specified allowable elastic slip will be used only for the contact pairs referencing the contact property definition that contains the friction definition. For example, three surfaces ASURF, BSURF, and CSURF form two contact pairs that each refer to their own contact property definition, as shown below.
In the DEFAULT contact property definition no value for ${\gamma}_{crit}$ is specified, so the allowable elastic slip used for the friction interaction between ASURF and BSURF would be the default value ${F}_{f}{\overline{l}}_{char}$. In the NONDEF contact property definition a value of 0.1 is specified for ${\gamma}_{crit}$, which will be the allowable elastic slip used for the friction interaction between CSURF and BSURF. Input File Usage FRICTION, ELASTIC SLIP=${\gamma}_{crit}$ Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Penalty or StaticKinetic Exponential Decay: Elastic Slip, Absolute distance: ${\gamma}_{crit}$ Changing the default slip toleranceYou can alter the default value of the slip tolerance, ${F}_{f}$. This method of altering the default elastic slip is convenient if the goal is to increase computational efficiency, in which case a value larger than the default of 0.005 would be given, or if the goal is to increase accuracy, in which case a value smaller than the default would be given. Input File Usage FRICTION, SLIP TOLERANCE=${F}_{f}$ Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Penalty or StaticKinetic Exponential Decay: Elastic Slip, Fraction of characteristic surface dimension: ${F}_{f}$ Stiffness method for imposing frictional constraints in Abaqus/ExplicitThe stiffness method used for friction with the general contact algorithm in Abaqus/Explicit and, optionally, with the contact pair method in Abaqus/Explicit is a penalty method that permits some relative motion of the surfaces (an “elastic slip”) when they should be sticking (similar to the allowable elastic slip defined with softened tangential behavior in Abaqus/Explicit). While the surfaces are sticking (i.e., ${\tau}_{eq}<{\tau}_{crit}$), the magnitude of sliding is limited to this elastic slip. Abaqus continually adjusts the magnitude of the penalty constraint to enforce this condition. In Abaqus/Explicit you can choose to have contact constraints for the contact pair algorithm enforced with the penalty method; the general contact algorithm always uses a penalty method (see Contact constraint enforcement methods in Abaqus/Explicit). The default penalty stiffness for frictional constraints is chosen automatically by Abaqus/Explicit and is the same as would be used for normal hard contact constraints. Softening in the normal direction does not affect the penalty stiffness used to enforce stick conditions. If tangential softening is specified (see Defining tangential softening in Abaqus/Explicit above), the penalty stiffness will be equal to the value specified for the slope of the shear stress versus elastic slip relationship. You can specify a scale factor to adjust the penalty stiffness, as discussed in Contact controls for general contact in Abaqus/Explicit and Contact controls for contact pairs in Abaqus/Explicit. Lagrange multiplier method for imposing frictional constraints in Abaqus/StandardIn Abaqus/Standard the sticking constraints at an interface between two surfaces can be enforced exactly by using the Lagrange multiplier implementation. With this method there is no relative motion between two closed surfaces until ${\tau}_{eq}={\tau}_{crit}$. However, the Lagrange multipliers increase the computational cost of the analysis by adding more degrees of freedom to the model and often by increasing the number of iterations required to obtain a converged solution. The Lagrange multiplier formulation may even prevent convergence of the solution, especially if many points are iterating between sticking and slipping conditions. This effect can occur particularly if locally there is a strong interaction between slipping/sticking conditions and contact stresses. Because of the added cost of using the Lagrange friction formulation, it should be used only in problems where the resolution of the stick/slip behavior is of utmost importance, such as modeling fretting between two bodies. In typical metal forming applications or for contact of rubber components, accurate resolution of the stick/slip behavior is not important enough to justify the added costs of the Lagrange multiplier formulation. Input File Usage FRICTION, LAGRANGE Abaqus/CAE Usage Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Lagrange Multiplier Kinematic method for imposing frictional constraints in Abaqus/ExplicitBy default, the contact pair algorithm in Abaqus/Explicit uses a kinematic method for imposing frictional constraints (see Contact constraint enforcement methods in Abaqus/Explicit). The kinematic method applies sticking constraints in a way similar to the optional Lagrange multiplier method in Abaqus/Standard; however, the algorithm is quite different. The value of the force required to enforce sticking at a node is first calculated using the mass associated with the node; the distance the node has slipped; the time increment; and additionally for softened contact, the current value of the elastic slip and the elastic slip versus shear stress slope. For hard contact this sticking force is that which is required to maintain the node's position on the opposite surface in the predicted configuration. For softened contact this force is consistent with the userspecified value for the slope of the shear stress versus elastic slip relationship. The sticking force for each node is calculated using the mass associated with the node, the distance the node has slipped, the shear tractionelastic slip slope (if softened contact is specified in the tangential direction), and the time increment. If the shear stress at the node calculated using this force is less than ${\tau}_{crit}$, the node is considered to be sticking and this force is applied to each surface in opposing directions. If the shear stress exceeds ${\tau}_{crit}$, the surfaces are slipping and the force corresponding to ${\tau}_{crit}$ is applied. In either case the forces result in acceleration corrections tangential to the surface at the slave node and either the nodes of the master surface facet or the points on the analytical rigid surface that it contacts. Userdefined friction modelYou can define the shear stress between contacting surfaces through a user subroutine when the friction behavior provided by Abaqus is not sufficient. The shear stress can be defined as a function of a number of variables such as slip, slip rate, temperature, and field variables. You can also introduce a number of solutiondependent state variables that you can update and use within the friction user subroutines. You can declare a number of properties or constants associated with your friction model and use these values in the user subroutine. In addition to the friction user subroutines, subroutines are available for defining the complete mechanical interaction between surfaces, including the interaction in the normal direction as well as the frictional behavior in the tangential direction; see Userdefined interfacial constitutive behavior for more information. Defining generic frictional behaviorYou can define a generic frictional behavior between contacting surfaces using user subroutine FRIC in Abaqus/Standard. In Abaqus/Explicit the generic frictional behavior for contact pairs is defined in user subroutine VFRIC, while the generic frictional behavior for general contact is defined in user subroutine VFRICTION. Input File Usage Use the following option to define a frictional behavior with user subroutine FRIC or VFRIC: FRICTION, USER, DEPVAR=n, PROPERTIES=p Use the following option to define a frictional behavior with user subroutine VFRICTION: FRICTION, USER=FRICTION, DEPVAR=n, PROPERTIES=p Abaqus/CAE Usage Use the following options to define a frictional behavior with user subroutine FRIC or VFRIC: Interaction module: contact property editor: MechanicalTangential Behavior: Friction formulation: Userdefined, Number of statedependent variables: n, Friction Properties User subroutine VFRICTION is not supported in Abaqus/CAE. Defining complex isotropic frictionAbaqus provides a simple way to specify complex isotropic frictional behavior when the expression for the friction coefficient can be defined explicitly. You need only to specify the friction coefficient, and Abaqus will compute the resulting frictional forces. Abaqus/Standard provides user subroutine FRIC_COEF and Abaqus/Explicit provides user subroutine VFRIC_COEF for this purpose. VFRIC_COEF can be used only with general contact. Input File Usage FRICTION, USER=COEFFICIENT, PROPERTIES=p Abaqus/CAE Usage User subroutines FRIC_COEF and VFRIC_COEF are not supported in Abaqus/CAE. Consideration of incremental rotation of shell and beam thickness offsets in Abaqus/ExplicitBy default, in Abaqus/Explicit slip increment calculations for friction do not account for the incremental rotation of shell and beam thickness offsets, and frictional constraints do not apply a moment to nodes offset from the contact interface due to shell or beam thicknesses. This behavior can be modified for general contact; for details see Consideration of incremental rotation of shell and beam thickness offsets for frictional contact. Improving Abaqus/Standard simulations that include friction in the surface interactionsSeveral features of the frictional interaction of surfaces can have a strong influence on the rate of convergence in an Abaqus/Standard simulation. Unsymmetric terms in the system of equationsFriction constraints produce unsymmetric terms when the surfaces are sliding relative to each other. These terms have a strong effect on the convergence rate if frictional stresses have a substantial influence on the overall displacement field and the magnitude of the frictional stresses is highly solution dependent. Abaqus/Standard will automatically use the unsymmetric solution scheme if $\mu >0.2$ or if $\mu $ is pressuredependent. If desired, you can turn off the unsymmetric solution scheme; see Matrix storage and solution scheme in Abaqus/Standard. No slip occurs with rough friction; the contribution to the stiffness will be fully symmetric, and Abaqus/Standard will use the symmetric solution scheme by default. Heat generated by frictional interaction of surfacesIn fully coupled temperaturedisplacement analysis and fully coupled thermalelectricalstructural analysis, all dissipated mechanical (frictional) energy is converted to heat and distributed equally between the two surfaces by default. This behavior can be modified; for details about this and other thermal surface interactions, see Thermal contact properties. Temperature and fieldvariable dependence of friction properties for structural elementsTemperature and fieldvariable distributions in beam and shell elements can generally include gradients through the crosssection of the element. Contact between these elements occurs at the reference surface; therefore, temperature and fieldvariable gradients in the element are not considered when determining friction properties that depend on these variables. Surface interaction variables related to frictionAbaqus provides output of the shear stresses at points on the slave surface that use a surface interaction model containing frictional properties. The shear stresses, CSHEAR1 and CSHEAR2, are given in the two orthogonal local tangent directions, which are constructed on the master surface (see Contact formulations in Abaqus/Standard). There is only one local tangent direction in twodimensional problems. Details about how to request contact surface variable output are given in About contact pairs in Abaqus/Standard and About contact pairs in Abaqus/Explicit. Contour plots of these variables can also be plotted in Abaqus/CAE. References
