For the real constants FKN, FTOLN, ICONT, PINB, PZER, CZER, FKOP, FKT, SLTO, TNOP, FDMN, and FDMT, you can specify either a positive or negative value. The program interprets a positive value as a scaling factor and interprets a negative value as the absolute value. The program uses the depth of the underlying element as the reference value for ICONT, FTOLN, PINB, and CZER. For example, a positive value of 0.1 for ICONT indicates an initial closure factor of 0.1 x depth of the underlying element. However, a negative value of 0.1 indicates an actual adjustment band of 0.1 units. Contact related settings (ICONT, FTOLN, PINB, FKN, FKT, SLTO) are always averaged across all contact elements in a contact pair.

Figure 3.12: Depth of the Underlying Element shows the depth of the underlying element for a solid element. If the underlying elements are shell or beam elements, the depth will usually be 4 times the element thickness. The final contact depth may also be adjusted based on the average contact length when the shape of the underlying element is relatively thin.

Figure 3.12: Depth of the Underlying Element

Each contact pair has a pair-based depth which is obtained by averaging the depth of each contact element across all the contact elements in a contact pair. This can avoid the problem of very different element-based depths when there are meshes with large variations in element sizes.

For certain real constants, you can define the real constant as a function of primary variables by using tabular input. Table 3.2: Real Constants and Corresponding Primary Variables for CONTA172, CONTA174, CONTA175, CONTA177 lists real constants that allow tabular input and their associated primary variables.

You should follow the positive and negative convention for the real constant values. Use all positive or all negative values. Do not mix positive and negative values.

Use the *DIM command to dimension the table and identify the variables. The possible primary variables used in tabular input are:

Note that the primary variables X, Y, and Z represent the coordinates of the contact detection points at the beginning of solution (undeformed configuration). Coordinate system applicability is determined by the *DIM command.

When defining the tables, the primary variables must be in ascending order in the table indices (as in any table array).

When defining real constants via the R, RMORE, or RMODIF command, enclose the table name in % signs (that is, %tabname%). For example, given a table named CNREAL3 that contains normal contact stiffness (FKN) values, you would issue a command similar to the following:

RMODIF,NSET,3,%CNREAL3%      ! NSET is the real constant set ID associated with the contact pair

For more information and examples of using table inputs, see Tabular Input via Table Array Parameters in the Ansys Parametric Design Language Guide, Applying Loads Using Tabular Input in the Basic Analysis Guide, and the *DIM command.

You can write a USERCNPROP.F subroutine to define your own real constants. The real constants that can be defined via this user subroutine are noted in the real constant table found in each contact element description.

When defining real constants with the R, RMORE, or RMODIF command, you must use the reserved table name _CNPROP and enclose it in % signs (%_CNPROP%). When a value field on one of these commands is set to %_CNPROP%, the program internally calls the user-defined subroutine USERCNPROP. For example, to specify your own normal contact stiffness, FKN, you would issue a command similar to the following:

RMODIF,NSET,3,%_CNPROP%      ! NSET is the real constant set ID associated with the contact pair

If several real constant values are defined via %_CNPROP% for a given contact pair, the subroutine will be called for each of these real constant entries. Therefore, you can use a single USERCNPROP subroutine to modify multiple real constant values. For details, see Defining Your Own Real Constant (USERCNPROP).

Keep the following points in mind when using the Lagrange multiplier methods.

For the augmented Lagrangian method and penalty method, normal and tangential contact stiffnesses are required. The amount of penetration between contact and target surfaces depends on the normal stiffness. The amount of slip in sticking contact depends on the tangential stiffness.

Higher stiffness values decrease the amount of penetration/slip, but can lead to ill-conditioning of the global stiffness matrix and to convergence difficulties. Lower stiffness values can lead to a certain amount of penetration/slip and produce an inaccurate solution. Ideally, you want a high enough stiffness that the penetration/slip is acceptably small, but a low enough stiffness that the problem will be well-behaved in terms of convergence.

The program provides default values for contact stiffnesses (FKN, FKT), allowable penetration (FTOLN), and allowable slip (SLTO). Material properties of underlying elements can affect the calculation of default values of contact stiffnesses, as follows:

In most cases, you do not need to define the contact stiffness. In addition, Ansys recommends that you use KEYOPT(10) = 0 or 2 to allow the program to update the contact stiffness automatically.

For certain contact problems, you may choose to use the real constant FKN to define a normal contact stiffness factor. The usual factor range is from 0.1 - 10.0, with a default of 1.0. The default value should work in most cases. You can also define an absolute normal contact stiffness by specifying a negative value for FKN.

In addition, FKN can be defined as a function of primary variables by using tabular input (%tabname%). The possible primary variables include time, temperature, initial contact detection point location (at the beginning of solution), contact pressure of the previous iteration (positive PRESSURE index values indicate compression, negative PRESSURE index values indicate tension), and current geometric penetration (positive GAP index values indicate penetration, negative GAP index values indicate an open gap). For more information, see Defining Real Constants in Tabular Format.

The user subroutine USERCNPROP.F is also available for defining FKN. To use this subroutine, you must specify the table name %_CNPROP% as the real constant value. For more information, see Defining Real Constants via a User Subroutine.

If you input an absolute normal contact stiffness by specifying a negative value for FKN, you can control the units by using KEYOPT(3). By default, the units of the user-specified absolute normal contact stiffness is FORCE/LENGTH³. You can change the units to FORCE/LENGTH by setting KEYOPT(3) = 1. This KEYOPT(3) = 1 setting is valid only when a penalty-based algorithm is used (KEYOPT(2) = 0 or 1) and the absolute normal contact stiffness is explicitly specified. Using KEYOPT(3) = 1 is not recommended in conjunction with nodal detection options (KEYOPT(4) = 1 or 2) if any midside nodes exist for the CONTA174 3D contact element. (KEYOPT(3) has different meanings in other situations. For more information, see Using KEYOPT(3) to Control Units of Contact Stiffness and Stress State.)

Use real constant FTOLN in conjunction with the augmented Lagrangian method. FTOLN is a tolerance factor to be applied in the direction of the surface normal. The range for this factor is less than 1.0 (usually less than 0.2), with a default of 0.1, and is based on the depth of the underlying solid, shell, or beam element (see Figure 3.12: Depth of the Underlying Element). This factor is used to determine if penetration compatibility is satisfied.

Contact compatibility is satisfied if penetration is within an allowable tolerance (FTOLN times the depth of underlying elements). The depth is defined by the average depth of each individual contact element in the pair. If the program detects any penetration larger than this tolerance, the global solution is still considered unconverged, even though the residual forces and displacement increments have met convergence criteria. You can also define an absolute allowable penetration by specifying a negative value for FTOLN. In general, the default contact normal stiffness is inversely proportional to the final penetration tolerance. The tighter the tolerance, the higher the contact normal stiffness.

When you use real constant FTOLN in conjunction with KEYOPT(10) = 0 or 2, the normal contact stiffness (used for the penalty method and the augmented Lagrange method) is updated at each iteration based on the current mean stress of the underlying elements and the allowable tolerance (FTOLN times the depth of the underlying elements). See also Using KEYOPT(10).

The program automatically defines a default tangential contact stiffness that is proportional to MU and the normal stiffness FKN. The default tangential stiffness corresponds to a default value of FKT = 1.0. A positive value for FKT is a factor. A negative value indicates an absolute value of tangential stiffness.

For KEYOPT(10) = 0 or 2, or when the Lagrange multiplier on normal and penalty on tangent option is used (KEYOPT(2) = 3), the program updates tangential contact stiffness based on current contact normal pressure, PRES, and maximum allowable elastic slip, SLTO (KT = FKT*MU* PRES/SLTO). In addition, other adjustments may be applied to the tangential contact stiffness.

By default, the allowed tangential contact stiffness variation is intended to enhance stiffness updating (when KEYOPT(13) = 0) by calculating an optimal allowable range in stiffness for use in the updating scheme. To increase the tangential stiffness variational range for the frictional contact, set KEYOPT(13) = 1 to make an aggressive refinement to the allowable stiffness range. Use of KEYOPT(13) = 1 is not recommended when contact convergence is relatively easy as it might produce a large amount of elastic slip for sticking contact.

The real constant SLTO is used to control maximum sliding distance when FKT is updated at each iteration. The program provides default tolerance values which work well in most cases.

The default value for SLTO is 1 percent of the average contact length in a pair. However, for a steady-state rolling analysis, the default value is 0.1(ω*R), where ω is the spin velocity specified by the SSTATE command and R is the distance of the contact detection point from the center of rotation.

You can override the default value for SLTO by defining a scaling factor (positive value when using command input) or an absolute value (negative value when using command input). A larger value will enhance convergence but compromise accuracy. Based on the tolerance, current normal pressure, and friction coefficient, the tangential contact stiffness FKT can be obtained automatically. In certain cases users can override FKT by defining a scaling factor (positive input value) or absolute value (negative input value) (see Positive and Negative Real Constants for more information).

In addition, FKT can be defined as a function of primary variables by using tabular input (that is, %tabname%). The possible primary variables include time, temperature, initial contact detection point location (at the beginning of solution), current contact pressure (positive PRESSURE index values indicate compression, negative PRESSURE index values indicate tension), and current geometric penetration (positive GAP index values indicate penetration, negative GAP index values indicate an open gap). For more information, see Defining Real Constants in Tabular Format.

The user subroutine USERCNPROP.F is also available for defining FKT. To use this subroutine, you must specify the table name %_CNPROP% as the real constant value. For more information, see Defining Real Constants via a User Subroutine.

FKN, FTOLN, FKT, and SLTO can be modified from one load step to another. They can also be adjusted in a restart run.

Determining a good stiffness value may require some experimentation on your part. To arrive at a good stiffness value, you can try the following procedure as a "trial run":

In addition, keep these points in mind when specifying contact stiffness:

The normal and tangential contact stiffness can be updated during the course of an analysis, either automatically (due to large strain effects that change the underlying element's stiffness) or explicitly (by user-specified FKN or FKT values). KEYOPT(10) governs how the normal and tangential contact stiffness is updated when the augmented Lagrangian or penalty method is used. In most cases Ansys, Inc. recommends that you use KEYOPT(10) = 0 to allow the program to update contact stiffnesses automatically. The possible settings for KEYOPT(10) are:

The default method of updating normal contact stiffness (KEYOPT(10) = 0 or 2) is suitable for most applications. However, the variational range of the normal contact stiffness may not be wide enough to handle certain contact situations. For example:

The allowed normal contact stiffness variation is intended to enhance stiffness updating when KEYOPT(10) = 0 or 2 by calculating an optimal allowable range in stiffness for use in the updating scheme. To increase the stiffness variational range, set KEYOPT(6) = 1 to make a nominal refinement to the allowable stiffness range, or KEYOPT(6) = 2 to make an aggressive refinement to the allowable stiffness range.

Use of KEYOPT(6) = 1 or 2 is not recommended when contact convergence is relatively easy as it might produce an unnecessary drop in contact stiffness.

Set KEYOPT(6) = 3 to define the pressure-penetration relationship. The augmented Lagrangian method (KEYOPT(2) = 0) with KEYOPT(6) = 3 behaves the same as the penalty algorithm (KEYOPT(2) = 1): no augmentation and penetration tolerance checks are applied. See Pressure-Penetration Relationship (KEYOPT(6) = 3) for more information.

 

3.9.4.6.1. Pressure-Penetration Relationship (KEYOPT(6) = 3)

 

3.9.4.6.1.1. Exponential Pressure-Penetration Relationship

When KEYOPT(6) = 0, 1, or 2, the program uses a uniform normal contact stiffness for each contact pair. This can cause convergence issues when the mesh size across contact elements within a pair varies greatly.

With the exponential pressure-penetration relationship (KEYOPT(6) = 3), the resulting contact stiffness is no longer uniform within a pair. This is a contact-detection-based law that can make contact behavior smoother in the following situations: self contact, contact involving soft materials like rubber, models having a large initial gap, non-uniform contact surface meshes, and contact interface chattering.

When KEYOPT(6) = 3, the contact pressure-penetration relationship follows an exponential law based on default values of real constants PZER (pressure at zero penetration) and CZER (initial contact clearance). PZER is calculated based on underlying element properties. A small contact pressure starts developing as the initial clearance is detected and increases exponentially as the gap reduces and penetration increases.

A positive value for CZER indicates a scaling factor associated with the depth of the underlying elements. A negative value indicates an absolute initial contact clearance value. CZER defaults to 0.01.

A positive value for PZER indicates a scaling factor, with the typical range being from 0.1 - 10.0. PZER default to 1.0. A negative value for PZER indicates an absolute contact pressure at zero penetration. When PZER is negative (an absolute value) and CZER is positive (a scaling factor), the program computes the actual contact pressure internally based on the penetration tolerance FTOLN and the initial contact clearance CZER.

The default values are adequate for most contact models. However, you can specify PZER and/or CZER to define the contact pressure-penetration exponential relationship.

You can also set a maximum cutoff stiffness by inputting real constant FKN. The computed contact stiffness from the exponential relationship will not exceed the cutoff value. If FKN is not specified, the program uses the default value of penalty contact stiffness to calculate the cutoff value. The actual cutoff stiffness is 1000 times the penalty stiffness input by you or computed by the program. For example, if FKN is not input and the program calculates an initial contact stiffness of 42265, the cutoff contact stiffness used is 0.42265E+08.

The following equation is used to define the contact stiffness vs. gap relationship (FKN as a function of gap, g):

where:

c0 = initial gap

p = p0 when g = 0

Figure 3.13: Pressure-Penetration Relationship

Figure 3.14: Stiffness versus Penetration Relationship

 

3.9.4.6.1.2. Defining the Pressure-Penetration Relationship via Tabular Input or the User Subroutine

Contact pressure can be defined as a function of gap by using tabular input (that is, %tabname%) for real constant PZER with GAP as the primary variable. GAP represents current geometric gap/penetration (positive GAP index values indicate penetration, negative GAP index values indicate an open gap). For more information, see Defining Real Constants in Tabular Format. Pressure will be 0 for gap greater than CZER. Ansys recommends defining the table according to CZER.

Alternatively, you can use the user subroutine USERCNPROP.F to define the pressure-gap relationship. See Defining Your Own Real Constant (USERCNPROP) for details. To properly define the relationship, be sure to return the following two output arguments:

cnprop(1) = user defined contact pressure at the given penetration

cnprop(2) = normal contact stiffness at the given penetration (derivative of the contact stiffness with respect to the penetration)

When defined by tabular input or by the USERCNPROP.F user subroutine, PZER must be a positive value, and it represents an absolute pressure (not a factor). This differs from its typical usage.

 

3.9.4.6.1.3. Limitations for the Pressure-Penetration Relationship

• The pressure-penetration feature (KEYOPT(6) = 3):

  • Cannot be used with bonded and no-separation behaviors (KEYOPT(12) > 1).

  • Does not support the Lagrange methods and MPC contact (KEYOPT(2) > 1).

  If the above settings are used, the program assumes aggressive-variation of contact stiffness (KEYOPT(6) = 2).

• KEYOPT(6) = 3 does not support the Augmented Lagrange method (KEYOPT(2) = 0). If these settings are used together, the program switches to the penalty method (KEYOPT(2) = 1) internally.

• When the automatic stiffness ramp-up option is defined (see 3. Automatically ramp up the contact stiffness under Modeling Interference Fit) the program internally actives the aggressive-variation of contact stiffness (KEYOPT(6) = 2) only for the specified load step or time period.

• KEYOPT(6) = 3 is not recommended with the settings listed below since it may not behave as expected:

  • Impact constraints (KEYOPT(7) = 4)

  • Fluid penetration (SFE,,,PRES and KEYOPT(14))

In general, the Lagrange multiplier methods (KEYOPT(2) = 3, 4) do not require normal contact stiffness, FKN, unless overconstraints are detected. Instead they require chattering control parameters, FTOLN and TNOP, by which the program assumes that the contact status remains unchanged. FTOLN is the maximum allowable penetration and TNOP is the maximum allowable tensile contact pressure.

The behavior can be described as follows:

The program provides reasonable defaults for FTOLN and TNOP. FTOLN defaults to the displacement convergence tolerance. TNOP defaults to 1% of the force convergence tolerance divided by the contact area at contact nodes.

When providing values for FTOLN and TNOP:

The objective of FTOLN and TNOP is to provide stability to models which exhibit contact chattering due to changing contact status. If the values you use for these tolerances are too small, the solution will require more iterations. If the values are too large, however, the accuracy of the solution will be affected as a certain amount of penetration or tensile contact force is allowed.

In the basic Coulomb friction model, two contacting surfaces can carry shear stresses up to a certain magnitude across their interface before they start sliding relative to each other. This state is known as sticking. The Coulomb friction model defines an equivalent shear stress τ, at which sliding on the surface begins as a fraction of the contact pressure p (τ = µp + COHE, where  µ is the friction coefficient and COHE specifies the cohesion sliding resistance). Once the shear stress is exceeded, the two surfaces will slide relative to each other. This state is known as sliding. The sticking/sliding calculations determine when a point transitions from sticking to sliding or vice versa.

As an alternative to the program-supplied friction model, you can define your own friction model with the USERFRIC subroutine (see Writing Your Own Friction Law (USERFRIC)). Furthermore, you can define your own contact interaction behavior with the USERINTER subroutine (see Defining Your Own Contact Interaction (USERINTER)).

For frictionless, rough, and bonded contact, the contact element stiffness matrices are symmetric. Contact problems involving friction produce unsymmetric stiffnesses. Using an unsymmetric solver is more computationally expensive than a symmetric solver for each iteration. For this reason, the program uses a symmetrization algorithm by which most frictional contact problems can be solved using solvers for symmetric systems. If frictional stresses have a substantial influence on the overall displacement field and the magnitude of the frictional stresses is highly solution dependent, the symmetric approximation to the stiffness matrix may provide a low rate of convergence. In such cases, choose the unsymmetric solution option (NROPT,UNSYM) to improve convergence.

The interface coefficient of friction, MU, is used for the Coulomb friction model. Input MU as a material property for the contact elements. The Coulomb friction can be isotropic or orthotropic.

Use MU = 0 for frictionless contact. For rough or bonded contact (KEYOPT(12) = 1, 3, 5, or 6. See Selecting Surface Interaction Models), the program assumes infinite frictional resistance regardless of the specified value of MU.

MU can have dependence on temperature, time, normal pressure, sliding distance, or sliding relative velocity. Suitable combinations of up to two fields can be used to define dependency (for example, temperature only, temperature and sliding distance, or sliding relative velocity and normal pressure). If the underlying element is a superelement (MATRIX50), the material property set must be the same as the one used for the original elements that were assembled into the superelement.

Note that if the coefficient of friction is defined as a function of temperature, the program always uses the contact surface temperature as the primary variable (not the average temperature from the contact and target surfaces).

If you want to change the friction coefficient between load steps, it is recommended you change it in a ramped fashion. This is especially important when changing the surface behavior from frictionless to frictional contact. A sudden change in friction can result in a discontinuous frictional force leading to convergence issues. To avoid this, define friction as a function of time (TB,FRIC and TBFIELD with TIME specified as the field variable) to slowly ramp the change in friction coefficient.

Defining Isotropic Friction

Isotropic Friction (TB,FRIC,,,ISO) is available for 2D and 3D contact elements. The isotropic friction model is based on a single coefficient of friction, MU. Contacting surfaces experience the same friction in all directions. You can use either TB command input (recommended method) or the MP command to specify MU. For more information, see Isotropic Friction in the Material Reference.

Defining Orthotropic Friction

Orthotropic friction is available only for the 3D contact elements (CONTA174, CONTA175, CONTA176, and CONTA177). The orthotropic friction model is based on two coefficients of friction, MU1 and MU2, defined in the two principle directions for the element.

See the individual element descriptions to understand the principle directions for each element type. The two principal directions and the direction normal to these two principal directions constitute the friction coordinate system.

See Orthotropic Friction in the Material Reference for details on how to specify the coefficients of friction. Three different orthotropic friction options are available:

Example 3.1: Using TBOPT = ORTHO versus TBOPT = FORTHO

To illustrate the difference between the ORTHO and FORTHO options, consider the example of a flexible rectangular block meshed with contact elements which is pressed down on a rigid target surface on the global X-Z plane. Orthotropic friction can be defined as:

TB,FRIC,,,ORTHO     ! TBOPT = ORTHO
TBDATA,,0.2,0.001   ! MU1 = 0.2, MU2 = 0.001

or

TB,FRIC,,,FORTHO
TBDATA,,0.2,0.001

The friction coordinate system is parallel to the global coordinate system, with the two principal directions initially parallel to the global X and global Z directions.

First, the block slides in the +X direction and then slides back to the starting position. During this sliding motion, the block experiences a friction coefficient of 0.2 for both the ORTHO and FORTHO options.

Next, the block is rotated 90° and made to slide along the Z direction. For the ORTHO option, the block experiences the same friction coefficient of 0.2 in the Z direction since the friction coordinate system has also rotated with the block and contact elements. However, for the FORTHO option, the block experiences a friction coefficient of 0.001 in the Z direction after the rotation since the friction coordinate system is fixed.

The animations below show contour plots of frictional force experienced by the block when the ORTHO and FORTHO options are used. Note the almost zero frictional force after the rotation in the FORTHO case.

Figure 3.15: Sliding Block with TBOPT = ORTHO Friction Option

Figure 3.16: Sliding Block with TBOPT = FORTHO Friction Option

The program provides one extension of classical Coulomb friction: real constant TAUMAX is maximum contact friction with units of stress. This maximum contact friction stress can be introduced so that, regardless of the magnitude of normal contact pressure, sliding will occur if the friction stress reaches this value. You typically use TAUMAX when the contact pressure becomes very large (such as in bulk metal forming processes). TAUMAX defaults to 1.0e20. Empirical data is often the best source for TAUMAX. Its value may be close to , where σ_y is the yield stress of the material being deformed.

You have an option to define TAUMAX as a function of primary variables by using tabular input (that is, %tabname%). The possible primary variables include time, temperature, initial contact detection point location (at the beginning of solution), current contact pressure (positive PRESSURE index values indicate compression, negative PRESSURE index values indicate tension), and current geometric penetration (positive GAP index values indicate penetration, negative GAP index values indicate an open gap). For more information, see Defining Real Constants in Tabular Format.

The user subroutine USERCNPROP.F is also available for defining TAUMAX. To use this subroutine, you must specify the table name %_CNPROP% as the real constant value. For more information, see Defining Real Constants via a User Subroutine.

Another real constant used for the friction law is the cohesion, COHE (default COHE = 0), which has units of stress. It provides sliding resistance, even with zero normal pressure (see Figure 3.17: Sliding Contact Resistance).

Figure 3.17: Sliding Contact Resistance

Two other real constants, FACT and DC are involved in specifying static and dynamic friction coefficients, as described in the next section.

The coefficient of friction can depend on the relative velocity of the surfaces in contact. Typically, the static coefficient of friction is higher than the dynamic coefficient of friction.

The program provides the following exponential decay friction model:

where:

For the isotropic friction model, MU is input using the MP command or the TB command as explained above. For orthotropic friction, MU is the equivalent coefficient of friction computed from MU1 and MU2 which are specified with TB command input:

Figure 3.18: Friction Decay shows the exponential decay curve where the static coefficient of friction is given by:

Figure 3.18: Friction Decay

You can determine the decay coefficient if you know the static and dynamic coefficients of friction and at least one data point (μ₁ ; V_rel1). The equation for friction decay can be rearranged to give:

If you do not specify a decay coefficient and FACT is greater than 1.0, the coefficient of friction will change suddenly from the static to the dynamic value as soon as contact reaches the sliding state. This behavior is not recommended because the discontinuity may lead to convergence difficulties.

In a static analysis, you can model steady-state frictional sliding between two flexible bodies or between a flexible and a rigid body with different velocities. In this case the sliding velocities no longer follow the nodal displacements, and they are predefined through the CMROTATE command. This command sets the velocities on the nodes of the element component as an initial condition at the start of a load step. The program determines the sliding direction based on the direction of the sliding velocities.

This feature is applicable to 3D contact (CONTA174, CONTA175) and is primarily used for generating sliding contact at frictional contact interfaces in a brake squeal analysis. In this case, the contact pair elements (either the contact elements or the target elements) on the brake rotor need to be included in the rotating element component (CM command) that is specified on the CMROTATE command. Ansys recommends that you include only the contact elements or only the target elements in the element component.

Velocities defined by CMROTATE will be ignored for the following contact definitions:

The amplitude of the sliding velocity defined by CMROTATE will affect the solution when the friction coefficient is specified as a function of sliding velocity via the command TB,FRIC, or when static and dynamic friction is defined via the real constants FACT and DC.

In a complex eigenvalue extraction analysis using the QRDAMP or DAMP methods (see MODOPT), the effects of squeal damping will contribute to the damping matrix. The squeal damping can be identified as two parts: destabilizing damping and stabilizing damping.

You can activate destabilizing squeal damping by one of the following methods:

When the destabilizing squeal damping is included by method (1) or (2), you can study its effects by using FDMD as a scaling factor (KEYOPT(16) = 0). FDMD defaults to 1.0. The program multiplies the internally calculated destabilizing damping by this factor.

You can specify a constant friction-sliding velocity gradient directly via FDMD by setting KEYOPT(16) = 1. The defined gradient has units of TIME/LENGTH and it is negative in general.

You can also specify the destabilizing squeal damping coefficient directly via FDMD by setting KEYOPT(16) = 2. The defined damping coefficient has units of MASS/(AREA*TIME) and it is negative in general. In a linear non-prestressed modal analysis, this is the only way to take the destabilizing squeal damping effects into account.

The stabilizing squeal damping is deactivated by default. To activate it, you must specify the scaling factor via the real constant FDMS. FDMS defaults to 0.0. The program multiplies the internally calculated stabilizing damping by this factor. By setting KEYOPT(16) = 1 or KEYOPT(16) = 2 you can specify the stabilizing squeal damping coefficient directly via FDMS. The defined damping coefficient has units of MASS/(AREA*TIME) and it is positive in general. In a linear non-prestressed modal analysis, this is the only way to take the stabilizing squeal damping effects into account.

If squeal damping is included in a brake squeal modal analysis that uses the QR Damp eigensolver (MODOPT,QRDAMP command), care should be taken not to generate a damping matrix with large values (coefficients) relative to the values of the stiffness matrix. The accuracy of the QRDAMP eigensolver is based on the assumption that the values in the damping matrix are at least an order of magnitude smaller than the stiffness matrix values. If large squeal damping matrix values are generated in conjunction with a QRDAMP modal solution, then the QRDAMP eigensolver could produce spurious zero modes, which can generally be ignored. In this case, the non-zero eigenvalues from the QRDAMP modal solution are still accurate. Ansys recommends that you use the DAMP eigensolver (MODOPT,DAMP) to check the final solution.

As a special case, when contact friction is used in a steady-state rolling analysis, the frictional stress calculation is changed to a viscous formulation. For details, see Contact Algorithm in the Theory Reference.

Contact detection points are located at the integration points of the contact elements which are interior to the element surface. The contact element is constrained against penetration into the target surface at its integration points. However, the target surface can, in principle, penetrate through into the contact surface, see Figure 3.19: Contact Detection Located at Gauss Point.

Figure 3.19: Contact Detection Located at Gauss Point

Surface-to-surface contact elements use Gauss integration points as a default, which generally provide more accurate results than the nodal detection scheme, which uses the nodes themselves as the integration points. The node-to-surface contact element, CONTA175, and the line-to-surface contact element, CONTA177, always use the nodal detection scheme.

The nodal detection algorithms require the smoothing of the contact surface (KEYOPT(4) = 1) or the smoothing of the target surface (KEYOPT(4) = 2), which is quite time consuming. You should use this option only to deal with corner, point-to-surface, or edge-to-surface contact (see Figure 3.20: Contact Detection Point Location at Nodal Point). KEYOPT(4) = 1 specifies that the contact normal be perpendicular to the contact surface. KEYOPT(4) = 2 specifies that the contact normal be perpendicular to the target surface. Use KEYOPT(4) = 2 when the target surface is smoother than the contact surface.

Figure 3.20: Contact Detection Point Location at Nodal Point

Be aware, however, that using nodes as the contact detection points can lead to other convergence difficulties, such as node slippage, where the node slips off the edge of the target surface, see Figure 3.21: Node Slippage Using Nodal Detection KEYOPT(4) = 1 or 2. In order to prevent node slippage, you can use real constant TOLS to extend the target surface when the default setting still cannot avoid the problem. For most point-to-surface contact problems, Ansys recommends using CONTA175. See Node-to-Surface Contact later in this guide.

Figure 3.21: Node Slippage Using Nodal Detection KEYOPT(4) = 1 or 2

Smoothing is required for nodal detection algorithms, and it is performed by averaging surface normals connected to the node. As a result, the variation of the surface normal is continuous over the surface, which leads to a better calculation of friction behavior and a better convergence.

Real constant TOLS is used to add a small tolerance that will internally extend the edge of the target surface when you define the contact detection at the nodal point (KEYOPT(4) = 1 or 2). TOLS is useful for problems where contact nodes are likely to lie on the edge of targets (as at symmetry planes or for models generated in a node-to-node contact pattern). In these situations, the contact node may repeatedly slip off the target surface and go completely out of contact, resulting in convergence difficulties from oscillations. Units for TOLS are percent (1.0 implies a 1.0% increase in the target edge length). A small value of TOLS will usually prevent this situation from occurring. The default value is 2 for both small deflection (NLGEOM,OFF) and large deflection (NLGEOM,ON).

The definition of KEYOPT(4) in node-to-surface contact element CONTA175 is different. KEYOPT(4) = 1 for surface-to-surface contact is equivalent to KEYOPT(4) = 1 for node-to-surface contact. However, KEYOPT(4) = 2 for surface-to-surface contact is equivalent to KEYOPT(4) = 0 for node-to surface contact. See KEYOPT(4).

You can define the surface projection contact method by setting KEYOPT(4) = 3 or 4 for the surface-to-surface contact elements (CONTA172 and CONTA174) and the line-to-surface contact element (CONTA177):

For CONTA172 and CONTA174, a unified contact detection approach is also available:

Standard Surface Projection and Dual Shape Function Projection Options (KEYOPT(4) = 3 or 4)

For the standard surface projection (KEYOPT(4) = 3) and dual shape function projection (KEYOPT(4) = 4) options, the contact detection remains at contact nodal points. These options enforce a contact constraint on an overlapping region of the contact and target surfaces (see Figure 3.22: Surface Projection Based Contact) rather than on individual contact nodes (KEYOPT(4) = 1, 2) or Gauss points (KEYOPT(4) = 0). The contact penetration/gap is computed over the overlapping region in an average sense. Advantages of the surface projection based method are:

Figure 3.22: Surface Projection Based Contact

There are certain disadvantages to using surface projection based contact, as follows:

Comparison of the Standard Projection Option and the Dual Shape Function Option

Compared to the standard surface projection option (KEYOPT(4) = 3), the dual shape function projection option (KEYOPT(4) = 4) uses a special interpolation function for the discretization of contact traction. This option reduces dependent terms for each contact constraint. The resulting gap function and slip increments are closer to the local geometric gap/slip at contact nodes. It is more efficient in terms of solution performance and memory usage and generally remedies potential overconstraint due to MPC equations.

The dual shape function option is recommended for Lagrange multiplier contact (KEYOPT(2) = 3 or 4), MPC bonded contact (KEYOPT(2) = 2), and small sliding behavior (KEYOPT(18) = 1 or 2). For MPC bonded contact, the program internally switches to the dual shape function option if the standard projection option is defined.

Be aware that the dual shape function option is not as accurate as the standard projection option when the contact surface mesh is very coarse.

Unified Contact Detection Approach (KEYOPT(4) = 5)

Selecting the best contact detection is problem dependent and can have a significant impact on the solution. Each detection method has advantages and disadvantages:

Figure 3.23: Corner Contact

No detection method works best for all problems. One detection method may be obviously better for the early stage of the deformation, while another method may work better for the later stages.

To overcome this problem, the unified contact detection option (KEYOPT(4) = 5) combines three individual contact detection methods: Gauss point, nodal point with normal to target, and standard surface projection. This approach generally overcomes drawbacks of each individual method. The main advantages are:

Furthermore, the unified detection approach in conjunction with a symmetric contact definition works robustly for non-smoothing contact. Interference fit, press fit, snap fit, and snap-through are typical applications that can benefit from the unified contact approach.

The figure below shows a contact pair with mixed surfaces, edges, and corners under large deformations and displacements.

Figure 3.24: Non-Smoothing Contact with Varying Contact Conditions

Keep in mind that the unified approach is the most expensive option. Use of additional features such as adaptive small sliding (KEYOPT(18) = 2) and contact pair-splitting logic (CNCHECK,DMP) often improve the performance.

Limitations for Surface Projection Based Contact (KEYOPT(4) = 3, 4, or 5)

The surface projection contact method currently does not support the following:

Three different sliding behavior options are available: finite sliding (default), small sliding, and adaptive small sliding. The sliding behavior you choose will have an influence on solution robustness, performance, and accuracy. Select the appropriate sliding behavior based on the relative motion of the contact interfaces in your model.

The finite-sliding option is used by default (KEYOPT(18) = 0). This option allows for arbitrary separation, sliding, and rotation of the contact interfaces. In general, each contact detection point can interact with different target elements, depending on the contact status (open, closed, or sliding). The program re-forms nodal connectivity of the contact element based on the current configuration at each equilibrium iteration. The finite-sliding logic is computationally expensive, but guarantees solution accuracy.

Activate the small-sliding option (KEYOPT(18) = 1) when the contact interface will have relatively-small sliding motion (less than 20% of the contact length) during the entire analysis. For large deflection analysis, this option still permits arbitrary large rotation.

For small sliding, each contact detection point always interacts with the same target element, which is determined from the initial configuration. The nodal connectivity of the contact element remains unchanged throughout the analysis. Contact searching is performed only once in the beginning of the analysis, which is cost-effective.

The small-sliding logic also improves solution robustness. It can easily solve certain complex contact models for which the finite-sliding logic would have difficulties or find no solution. This is especially true for models having a bad quality geometry or mesh and non-smooth contact interfaces. (See this white paper for more discussion of this behavior.)

The small-sliding logic can cause nonphysical results if the relative sliding motion does not remain small. Therefore, if you choose this option it is your responsibility to ensure that the small-sliding assumption is not violated. Use the NLHIST or NLDIAG command to monitor the number of contact points having too much sliding (that is, the SLID value is greater than 50% of the contact length or 50% of the associated target element length).

Use the finite-sliding option if you are not absolutely sure that the small-sliding logic is appropriate.

Use the small-sliding option with great caution for the following cases:

Activate the adaptive small-sliding option (KEYOPT(18) = 2) when the contact interface will have relatively-small sliding motion (less than 20% of the contact length) during each sub-step of the analysis. The contact interface can undergo either small sliding or finite sliding within each substep based on the contact status at the beginning of the substep. If the contact status is closed at the beginning of a substep, small sliding is used during that substep.

For this option, each contact detection point interacts with the same target element, which is determined from the beginning configuration of each substep. The nodal connectivity of the contact element remains unchanged during the substep.

The adaptive small-sliding logic often improves robustness compared to the finite sliding logic and can also improve solution accuracy compared to the small sliding logic. It can handle situations when contact pairs are initially in far-field and then come into contact.

The adaptive small-sliding logic may cause nonphysical results if the relative sliding motion does not remain small within a substep. To avoid this, activate additional time step control (KEYOPT(7) > 0) so that bisection is performed if a large sliding distance is detected within a substep.

To ensure solution accuracy, use the NLHIST or NLDIAG command to monitor the number of contact points having too much sliding (that is, the SLMX value is greater than 50% of the contact length or 50% of the associated target element length).

Rigid body motion is usually not a problem in dynamic analyses. However, in static analyses, rigid body motion occurs when a body is not sufficiently restrained. "Zero or negative pivot" warning messages and impractical, excessively large displacements indicate unconstrained motion in a static analysis.

In simulations where rigid body motions are constrained only by the presence of contact, you must ensure that the contact pairs are in contact in the initial geometry. In other words, you want to build your model so that the contact pairs are "just touching." However, you can encounter various problems in doing so:

For the same reasons, too much initial penetration between target and contact surfaces can occur. In such cases, the contact elements may overestimate the contact forces, resulting in nonconvergence or in breaking-away of the components in contact.

The definition of initial contact is perhaps the most important aspect of building a contact analysis model. Therefore, you should always issue the CNCHECK command before starting the solution to verify the initial contact status. You may find that you need to adjust the initial contact conditions. The program offers several ways to adjust the initial contact conditions of a contact pair.

The following techniques can be performed independently or in combinations of one or more at the beginning of the analysis. They are intended to eliminate small gaps or penetrations caused by numerical round-off due to mesh generation. They are not intended to correct gross errors in either the mesh or in the geometric data.

You can use the above techniques in conjunction with each other. For example, you may wish to set a very precise initial penetration or gap, but the initial coordinates of the finite element nodes may not be able to provide sufficient precision. To accomplish this, you could:

Figure 3.26: Ignoring Initial Penetration, KEYOPT(9) = 1

Figure 3.27: Components of True Penetration

Figure 3.28: Ramping Initial Interference

The program provides a printout (in the output window or file or via the CNCHECK) of the model's initial contact state for each target surface at the beginning of the analysis. This information is helpful for determining the maximum penetration or minimum gap for each target surface.

If no contact is detected for a specific target surface, the program issues a warning. This occurs when the target surface is far from contact (that is, outside of the pinball region), or when the contact/target elements have been killed.

See Positive and Negative Real Constants for more information on these real constants.

Use the CNCHECK,ADJUST command when the gap or penetration to be adjusted is small enough that the movement of nodes will not cause significant mesh distortions. After the CNCHECK,ADJUST command is issued, the coordinates of the nodes that have been moved are modified as shown in Figure 3.29: Effect of Moving Contact Nodes via the ADJUST Option. You can change other contact related settings in PREP7 (for example, set KEYOPT(4) = 0 to use the Gauss detection option) and save the Jobname.db file. Issuing the SAVE command before issuing the CNCHECK,ADJUST command is recommended in order to resume the Jobname.db file with the original contact configuration.

The initial adjustment resulting from CNCHECK,ADJUST is converted to structural displacement values (UX, UY, UZ) and stored in a results file named Jobname.rcn. You can use this file to plot or list nodal adjustment vectors or create a contour plot of the adjustment magnitudes via the displacements (see Reviewing Results in POST1 for more information).

Figure 3.29: Effect of Moving Contact Nodes via the ADJUST Option

Sometimes, the gap or penetration between the contact and target surfaces is so large that moving the contact nodes to the target surface can result in significant mesh distortions. In this case, CNCHECK,MORPH should be used instead of CNCHECK,ADJUST to close gaps or reduce penetration.

When CNCHECK,MORPH is issued, the contact nodes are first moved toward the target (similar to he ADJUST option), then the underlying solid element mesh is morphed to improve the mesh quality. Figure 3.30: Comparison of the MORPH and ADJUST Options shows a case similar to that shown in Figure 3.29: Effect of Moving Contact Nodes via the ADJUST Option, but with a larger gap. This figure demonstrates that the MORPH option improves the mesh quality while moving the contact nodes to close the gap. CNCHECK,ADJUST (on the right) stretches the first layer of solid elements attached to the contact elements, while CNCHECK,MORPH (middle figure) results in a uniform mesh.

Figure 3.30: Comparison of the MORPH and ADJUST Options

As shown in Figure 3.31: Effect of Boundary Conditions on the Morph Option, the final results can be different depending on whether or not you remove displacement constraints before issuing CNCHECK,MORPH. If CNCHECK,MORPH is issued with all constraints in place, the contact nodes are moved and the mesh is morphed to improve mesh quality. However, if CNCHECK,MORPH is issued after removing all displacement constraints, then the lower block is rigidly moved to touch the target surface.

Figure 3.31: Effect of Boundary Conditions on the Morph Option

By default, all of the contact and target nodes are constrained during the morphing process. Therefore, any of those nodes that did not move to close the gap or penetration will likewise not move during the morphing process. To circumvent this and allow boundary nodes attached to contact elements to move, CNCHECK,MORPH unselects the far-field contact elements (similar to CNCHECK,UNSELECT) before morphing the mesh. You can further adjust the boundary node movements by setting TRlevel = AGGRE on the CNCHECK,MORPH command to automatically unselect additional contact elements, therefore allowing movement of the boundary nodes attached to them during morphing.

You can override the automatic unselect logic by manually unselecting the contact and target elements whose nodes you want to allow to move and applying displacement constraints on the nodes you want to prevent from moving. The manually unselected elements should be reselected after the morphing and before the actual solution.

Assumptions and Restrictions for CNCHECK,MORPH

The position and motion of a contact element relative to its associated target surface determines the contact element status. The program monitors each contact element and assigns a status:

A contact element is considered to be in near-field contact when its integration points (Gauss points or nodal points) are within a code-calculated (or user-defined) distance to the corresponding target surface. This distance is referred to as the pinball region. The pinball region is a circle (in 2D) or a sphere (in 3D) centered about the Gauss point.

Use real constant PINB to specify a scaling factor (positive value for PINB when using command input) or absolute value (negative value for PINB when using command input) for the pinball region. You can specify PINB to have any value.

By default, the program defines the pinball region as a circle for 2D or a sphere for 3D of radius 2*depth (if rigid-to-flexible contact) or 1*depth (if flexible-to-flexible contact) of the underlying element. See the discussion of element depth in Positive and Negative Real Constant Values. For the no-separation (KEYOPT(12) = 4), bonded-always (KEYOPT(12) = 5), and bonded-initial (KEYOPT(12) = 6) options, the PINB default is different than described here. See Selecting Surface Interaction Models for more information.)

If you input a value for real constant CNOF (contact surface offset) and the default PINB value is less than the absolute value of CNOF, the default for PINB will be set to the absolute value of (1.1*CNOF).

The computational cost of searching for contact depends on the size of the pinball region. Far-field contact (open and not near contact) element calculations are simple and add little computational demands. The near-field calculations (for contact elements that are nearly or actually in contact) are slower and more complex. The most complex calculations occur once the elements are in actual contact.

Setting a proper pinball region is useful to overcome spurious contact definitions if the target surface has several convex regions. However, the default setting should be appropriate for most contact problems.

For the purpose of trouble-shooting, note that the program uses a slightly larger pinball radius when reporting initial contact information (via the CNCHECK,DETAIL command or the Mechanical Contact Tool) than is actually used in the solution. This can help you to identify potentially missing or spurious contact.

The program warns you when there is an abrupt change in status (for example, from far-field to closed) during a contact analysis. This may indicate that the substep increment is too large, or possibly (but not likely) that the pinball value (PINB) is too small.

For more information about the PINB real constant, see Positive and Negative Real Constants.

The surface-to-surface contact elements support normal unilateral contact models as well as other mechanical surface interaction models.

As an alternative to the program-supplied contact interactions, you can define your own interfacial model with the USERINTER subroutine (see User-Defined Subroutines for Contact Interfacial Behaviors).

Use KEYOPT(12) to model different contact surface behaviors.

For all types of bonded contact (KEYOPT(12) = 2, 3, 4, 5, and 6), separation of contact can be modeled using the debonding feature. For more information, see Debonding.

For the no-separation option (KEYOPT(12) = 4), the bonded-always option (KEYOPT(12) = 5), and bonded-initial option (KEYOPT(12) = 6 ) a relatively small PINB value (pinball region) may be used to prevent any false contact. For these KEYOPT(12) settings, the default for PINB is 0.25 (25% of the contact depth). (The default PINB value may differ from what is described here if CNOF is input. See Defining the Pinball Region (PINB) for more information.)

When friction is defined for the no-separation options (KEYOPT(12) = 2 and 4), the program computes frictional stress only when the gap is closed. For an open gap or tensile pressure, it is treated as frictionless.

See Positive and Negative Real Constants for more information on the real constants mentioned above.

Real constant FKOP is the stiffness factor applied when contact opens. FKOP is only used for no separation or bonded contact (KEYOPT(12) = 2 through 6). If FKOP is input as a scaling factor (positive value for command input), the true contact opening stiffness equals FKOP times the contact stiffness applied when contact closes. If FKOP is input as an absolute value (negative value for command input), the value is applied as an absolute contact opening stiffness. The default FKOP value is 1.

In addition, FKOP can be defined as a function of primary variables by using tabular input (that is, %tabname%). The possible primary variables include time, temperature, initial contact detection point location (at the beginning of solution), and current geometric gap distance (positive GAP index values indicate penetration, negative GAP index values indicate an open gap). For more information, see Defining Real Constants in Tabular Format.

The user subroutine USERCNPROP.F is also available for defining FKOP. To use this subroutine, you must specify the table name %_CNPROP% as the real constant value. For more information, see Defining Real Constants via a User Subroutine.

No separation and bonded contact generate a "pull-back" force when contact opening occurs, and that force may not completely prevent separation. To reduce separation, define a larger value for FKOP. Also, in some cases separation is expected while connection between the contacting surfaces is required to prevent rigid body motion. In such instances, you can specify a small value for FKOP to maintain the connection between the contact surfaces (this is a "weak spring" effect).

For bonded contact, the default contact opening stiffness is affected by the normal contact stiffness. However, the tangential stiffness remains unchanged when an absolute value of tangential stiffness (a negative value input for FKT) is specified, regardless of the contact status or the value of FKOP.

For bonded and no separation contact, if no other nonlinearities exist in the model (plasticity, large deformation, or unilateral contact), a nonlinear solution is generally not required to obtain an accurate solution. In this case, it is possible for the program to treat the bonded and no separation contact types as linear contact. Linear contact is supported for all contact algorithms (KEYOPT(2)), including Lagrange multiplier surface-based constraints.

To activate linear contact, use the following KEYOPT settings:

or

When the above settings are enabled, the contact searching and the factorized stiffness matrix are performed once in the beginning of the linear analysis, which can result in significant performance improvement for the entire solution.

Linear contact is not supported for the following scenarios:

In most welding processes, after the materials around contacting surfaces exceed a critical temperature, the surfaces start to melt and bond with each other. To model this, you can specify the critical temperature using real constant TBND. As soon as the temperature at the contact surface (T_c) for closed contact exceeds this melting temperature, the contact will change to “bonded.” The contact status will remain bonded for the rest of analysis, even if the temperature subsequently decreases below the critical value.

The contact surface temperature T_c is obtained either from a coupled thermal-structural solution in which the TEMP degree of freedom is present or from a temperature body load applied to a model having structural degrees of freedom only.

In addition, TBND can be defined as a function of primary variables by using tabular input (that is, %tabname%). The possible primary variables include time, temperature, initial contact detection point location (at the beginning of solution), current contact pressure (positive PRESSURE index values indicate compression, negative PRESSURE index values indicate tension), and current geometric penetration (positive GAP index values indicate penetration, negative GAP index values indicate an open gap). For more information, see Defining Real Constants in Tabular Format.

The user subroutine USERCNPROP.F is also available for defining TBND. To use this subroutine, you must specify the table name %_CNPROP% as the real constant value. For more information, see Defining Real Constants via a User Subroutine.

When defining TBND via tabular input or the user subroutine, the TBND real constant should be defined as a bonding state other than the critical temperature: as soon as the value of TBND returned from the table definition or from the user subroutine is equal to or larger than 1.0, the contact is changed to “bonded.” The contact status will remain bonded for the rest of the analysis, even if the TBND value obtained from the table or the user subroutine subsequently falls below 1.0.

The bonded contact options (KEYOPT(12) = 5 or 6) can be used with the MPC approach (KEYOPT(2) = 2) to model various types of assemblies (see Multipoint Constraints and Assemblies). The MPC approach is generally recommended for modeling shell-shell assemblies (see Modeling Solid-Solid and Shell-Shell Assemblies). However, there may be cases where the MPC approach causes the shell-shell assembly model to be overconstrained.

To alleviate this problem, you can use a penalty-based method for shell-shell assemblies. Using the penalty-based method constrains rotational DOFs in addition to translational DOFs. This capability is available for contact elements CONTA174 and CONTA175 in conjunction with TARGE170.

To use this method, first set KEYOPT(2) = 0 or 1 (augmented Lagrangian or penalty function) and KEYOPT(12) = 5 or 6 (bonded always or bonded initial contact) for the contact elements. You must also set KEYOPT(5) = 2 (projected constraint for shell-shell assembly) for the TARGE170 target elements for this penalty-based method to be used.

The penalty stiffness used for rotational DOFs is equal to (contact stiffness used for translational DOFs) * (contact length). The contact stiffness for translational DOFs is input by real constant FKN, or defaults to an internal value. The contact length is always calculated internally and is printed in the output file. The figure below shows the difference in using a conventional penalty-based shell-shell assembly and this method.

Figure 3.38: Penalty-Based Shell-Shell Assembly

The surface-to-surface contact elements can model a rigid body (or one linear elastic body) contacting another linear elastic body undergoing small motions. These elastic bodies can be modeled using superelements, which greatly reduces the number of degrees of freedom involved in the contact iteration. Remember that any contact or target nodes must be either all master nodes of the superelements or all condensed nodes of the superelements. When the contact pair is built in original elements used to generate superelements, the contact status will not change from its initial status.

Because the superelement consists only of a group of retained nodal degrees of freedom, it has no surface geometry on which the program can define a contact and target surface. Therefore, the contact and target surface must be defined on the surface of the original elements before they are assembled into a superelement. Information taken from the superelement includes nodal connection and assembly stiffness, but no material property or stress states (whether axisymmetric, plane stress, or plane strain). One restriction is that the material property set used for the contact elements must be the same as the one used for the original elements before they were assembled into superelements.

In a 2-D analysis with superelements, use KEYOPT(3) to define the stress state for the CONTA172 elements. The default setting (KEYOPT(3) = 0) does not apply to superelements. All other KEYOPT(3) settings are valid only when superelements are present:

In a 3D contact analysis (CONTA174), KEYOPT(3) is not used to specify the stress state when superelements are present. The program automatically detects whether the underlying element is a superelement.

For 2D and 3D analyses without superelements, KEYOPT(3) of the contact elements can be used to control the units of normal contact stiffness in some circumstances. Note that when superelements are present, normal contact stiffness always has the units FORCE/LENGTH³.

Rigid body motion often occurs in the beginning of an analysis due to the fact that the initial contact condition is not well established. Following are possible causes:

For standard contact (KEYOPT(12) = 0) or rough contact (KEYOPT(12) = 1), you can use real constants FDMN and FDMT to define contact damping scaling factors along contact normal and tangential directions. The primary goal of this contact stabilization technique is to damp relative motions between the contact and target surfaces for open contact. It provides a certain amount of resistance to reduce the risk of rigid body motion.

The damping forces are calculated by:

where V_n and V_t are the relative velocities along the normal and tangential directions, and A_c is the area domain of the contact surface. The units of the damping coefficients of FDMN and FDMT are FORCE/(AREA*VELOCITY). For the contact force-based model (used by CONTA175 and CONTA177), the units are FORCE/VELOCITY.

The specified damping coefficients should be large enough to prevent rigid body motion, but small enough to insure a solution. The ideal values are fully dependent on the specific problem, the time of the load step, and the number of substeps.

The program computes the damping coefficients internally based on several factors:

In general, contact stabilization damping should only be used to prevent rigid body motion when other initial contact adjustment techniques are not efficient or not suitable for a particular situation. Therefore, contact stabilization is deactivated by default.

As an exception, however, the automatic contact stabilization technique will be enabled if all the following conditions are encountered:

Without this automatic contact stabilization, rigid body motion may occur under the above conditions. If you wish to deactivate automatic contact stabilization, set KEYOPT(15) = 1.

You can manually activate contact stabilization damping by setting KEYOPT(15) = 2 or 3. You can also activate or deactivate the contact stabilization damping between load steps via the CNKMOD command (see CNKMOD for details).

Use a positive value of FDMN to specify a damping scaling factor in the normal direction. FDMN defaults to 1.0. You can overwrite the internal normal damping coefficient by specifying a negative value.

Use a positive value of FDMT to specify a damping scaling factor in the tangential direction. FDMT defaults to 1.e-3. You can input an absolute tangential damping coefficient by specifying a negative value for FDMT.

Both FDMN and FDMT can be defined as a function of primary variables by using tabular input (that is, %tabname%). The possible primary variables include time, temperature, initial contact detection point location (at the beginning of solution), and current geometric gap distance (positive GAP index values indicate penetration, negative GAP index values indicate an open gap). For more information, see Defining Real Constants in Tabular Format.

The user subroutine USERCNPROP.F is also available for defining FDMN and FDMT. To use this subroutine, you must specify the table name %_CNPROP% as the real constant value. For more information, see Defining Real Constants via a User Subroutine.

The normal contact stabilization damping is activated if all the following conditions are met:

When KEYOPT(15) = 0, 1, or 2, normal stabilization damping will not be applied if any contact detection point has a closed status in the current iteration. However, when KEYOPT(15) = 3, normal stabilization damping is always applied as long as the current contact status is near-field for any contact detection point, regardless of the current contact status of the entire contact pair.

The tangential contact stabilization damping is automatically activated when the normal damping is activated. In the following circumstances, the tangential damping can be applied independent of the normal damping:

When KEYOPT(15) = 2, the program always applies the tangential stabilization damping for frictionless contact. When KEYOPT(15) = 3, the program always applies the tangential stabilization damping for frictionless or frictional contact unless the contact status is sticking. These settings help to prevent rigid body motion due to large amounts of sliding even for no-separation contact definitions.

Note that the internally computed contact damping is a function of the total number of substeps. The internal damping is ramped down to near zero in subsequent substeps within a load step, and very little damping is applied in the last substep. Therefore, the solution convergence pattern is different when solving a contact analysis that has only one substep (or a few substeps) per load step compared to an analysis having multiple substeps per loadstep. Often times, the solution fails to converge if a small number of substeps is used per load step. In this case, you can specify absolute damping coefficients to overwrite internal damping values. To do so, input negative values for FDMN and FDMT.

Stabilization can alleviate convergence problems, but it can also affect solution accuracy if the applied stabilization energy or damping forces are too large. In most cases, the program automatically activates and deactivates contact stabilization damping and estimates reasonable damping forces. However, it is good practice to check the stabilization energy and forces to determine whether or not they are excessive.

The contact stabilization energy (accessed via the AENE label on the ETABLE command) should be compared to element potential energy. The energies can be output in the Jobname.out file (via the OUTPR command). You can also access the energies as follows:

If the contact stabilization energy is much less than the potential energy (for example, within a 1.0 percent tolerance), the results should be acceptable and there should be no need to check the stabilization forces or tractions further.

You can check the contact pair based damping tractions (maximum normal damping pressure and maximum tangential damping stress) and total contact stabilization energy via the NLHIST and NLDIAG commands. If the maximum damping tractions are much smaller than the maximum contact pressures (for example, within a 0.5 percent tolerance), or the total contact stabilization energy is much smaller than the total contact strain energy, the results are still acceptable.

You can account for the thickness of shells (2D and 3D) and beams using KEYOPT(11). (This does not apply to 3D beam-to-beam contact.) For rigid-to-flexible contact, the program automatically shifts the contact surface to the bottom or top of the shell/beam surface. For flexible-to-flexible contact, the program automatically shifts both the contact and target surfaces which are attached to shell/beam elements. By default, the program does not account for the element thickness, and beams and shells are discretized at their mid-surface in which penetration distance is calculated from the mid-surface.

When you set KEYOPT(11) = 1 to account for beam or shell thickness, the contact distance is calculated from either the top or the bottom surface as specified previously in Steps in a Contact Analysis.

When building your model geometry, if you are going to account for thickness, remember the offsets which may come from either the contact surface or target surface or from both. When you specify a contact offset (CNOF) along with setting KEYOPT(11) = 1, it is defined from the top or bottom of the shell/beam, not the mid-surface. When used with SHELL181, SHELL208, SHELL209, SHELL281, or ELBOW290, changes in thickness during deformation are also taken into account.

For line-to-surface contact modeled with CONTA177, KEYOPT(11) is used to account for thickness of beam elements on the contact side and shell elements on the target side. See Accounting for Thickness Effect (KEYOPT(11)) for more information.

When using KEYOPT(11) for shell and beam contact, the penetration and gap distances are always measured from the midsurface of the shell or beam element. Any defined offset of the shell or beam element is ignored by the contact elements.

Time step control is an automatic time stepping feature that predicts when the status of a contact element will change and cuts the current time step back.

Impact constraints are used in a transient dynamic analysis to satisfy the momentum and energy balance at the contact and target interface. See Dynamic Contact and Impact Modeling for more information.

Use KEYOPT(7) = 0, 1, 2, or 3 to control time stepping, where KEYOPT(7) = 0 provides no control (the default), and KEYOPT(7) = 3 provides the most control.

Use KEYOPT(7) = 4 to activate impact constraints.