ANSYS uses several real constants and KEYOPTs to control contact behavior using surface-to-surface contact elements. For more information in addition to what is presented here, refer to the individual contact element descriptions in the Element Reference.
If you decide the real constant and KEYOPT settings you have specified for a particular contact pair are not appropriate, you can use the CNCHECK,RESET command to reset all values back to their default settings. Some real constants and key options are not affected by this command; see CNCHECK for details.
In many cases, certain default settings may not be appropriate for your specific model. You can issue the CNCHECK,AUTO command to obtain optimized KEYOPT and real constant settings in terms of robustness and efficiency. Usually, only the undefined or default KEYOPT settings and real constants are changed. Refer to the CNCHECK command description for details of which settings are typically changed. You should always verify these changes by issuing the CNCHECK,DETAIL command to list current contact pair properties. If necessary, you can overwrite the optimized settings by redefining specific KEYOPTs (KEYOPT command) and real constants (RMODIF command).
Two real constants, R1 and R2, are used to define the geometry of the target surface elements. The remaining are used by the contact surface elements.
R1 and R2 define the target element geometry.
FKN defines a normal contact stiffness factor.
FTOLN is a factor based on the thickness of the element which is used to calculate allowable penetration.
ICONT defines an initial closure factor (or adjustment band).
PINB defines a "pinball" region.
PMIN and PMAX define an allowable penetration range for initial penetration.
TAUMAX specifies the maximum contact friction.
CNOF specifies the positive or negative offset value applied to the contact surface.
FKOP specifies the stiffness factor applied when contact opens.
FKT specifies the tangent contact stiffness factor.
COHE specifies the cohesion sliding resistance.
TCC specifies the thermal contact conductance coefficient.
FHTG specifies the fraction of frictional dissipated energy converted into heat.
SBCT specifies the Stefan-Boltzmann constant.
RDVF specifies the radiation view factor.
ECC specifies the electric contact conductance or capacitance per unit area.
FHEG specifies the fraction of electric dissipated energy converted into heat.
FACT specifies the ratio of static to dynamic coefficients of friction.
DC specifies the decay coefficient for static/dynamic friction.
SLTO controls maximum sliding distance when MU is nonzero and the tangent contact stiffness (FKT) is updated at each iteration (KEYOPT(10) = 2) or when KEYOPT(2) = 3.
TNOP specifies the maximum allowable tensile contact pressure.
TOLS adds a small tolerance that extends the edge of the target surface.
MCC specifies the magnetic contact permeance (3-D only).
PPCN specifies the pressure-penetration criterion (surface contact elements only).
FPAT specifies the fluid penetration acting time (surface contact elements only).
COR specifies the coefficient of restitution for impact between rigid bodies using impact constraints (KEYOPT(7) = 4).
STRM specifies load step number for ramping penetration.
FDMN specifies the stabilization damping factor in the normal direction.
FDMT specifies the stabilization damping factor in the tangential direction.
FDMD specifies the destabilizing squeal damping factor (3-D only).
FDMS specifies the stabilizing squeal damping factor (3-D only).
TBND specifies the critical bonding temperature.
Real constant defaults can vary depending on the environment you are working in. The following table compares the default values between ANSYS and the ANSYS Workbench. See your ANSYS sales representative for more information about ANSYS Workbench.
Table 3.1 Summary of Real Constant Defaults in Different Environments
|Real Constants||Description||ANSYS Default||ANSYS Workbench Default|
|1||R1||Radius associated with target geometry |
Radius associated with target geometry
Superelement thickness 
|3||FKN||Normal penalty stiffness factor||1|||
|4||FTOLN||Penetration tolerance factor||0.1||0.1|
|5||ICONT||Initial contact closure||0||0|
|7||PMAX||Upper limit of initial penetration||0||0|
|8||PMIN||Lower limit of initial penetration||0||0|
|9||TAUMAX||Maximum friction stress||1.00E+20||1.00E+20|
|10||CNOF||Contact surface offset||0||0|
|11||FKOP||Contact opening stiffness||1||1|
|12||FKT||Tangent penalty stiffness factor||1||1|
|14||TCC||Thermal contact conductance||0|||
|15||FHTG||Frictional heating factor||1||1|
|17||RDVF||Radiation view factor||1||n/a|
|18||FWGT||Heat distribution weighing factor||0.5||0.5|
|19||ECC||Electric contact conductance||0|||
|20||FHEG||Joule dissipation weighting factor||1||n/a|
|22||DC||Exponential decay coefficient||0||0|
|23||SLTO||Allowable elastic slip||1%||1%|
|24||TNOP||Maximum allowable tensile contact pressure|||||
|25||TOLS||Target edge extension factor|||||
|26||MCC||Magnetic contact permeance||0||n/a|
|28||FPAT||Fluid penetration acting time||0.01||n/a|
|29||COR||Coefficient of restitution||1||1|
|30||STRM||Load step number for ramping penetration||1||1|
|31||FDMN||Normal stabilization damping factor||1||n/a|
|32||FDMT||Tangential stabilization damping factor||0.001||n/a|
|33||FDMD||Destabilizing squeal damping factor||1||n/a|
|34||FDMS||Stabilizing squeal damping factor||0||n/a|
|35||TBND||Critical bonding temperature||n/a||n/a|
10% of target length for NLGEOM,OFF.
2% of target length for NLGEOM,ON.
R1 and R2 are used to define the target element geometry. See Defining Target Element Geometry and the target element descriptions (TARGE169 and TARGE170) for details on how they are used for different geometries.
|GUI:||Main Menu> Preprocessor> Real Constants|
For the real constants FKN, FTOLN, ICONT, PINB, PMAX, PMIN, FKOP, FKT, SLTO, and TNOP, you can specify either a positive or negative value. ANSYS interprets a positive value as a scaling factor and interprets a negative value as the absolute value. ANSYS uses the depth of the underlying element as the reference value to be used for ICONT, FTOLN, PINB, PMAX, and PMIN. 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, PMAX, PMIN, FKN, FKT, SLTO) are always averaged across all contact elements in a contact pair.
Figure 3.10 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.
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.
When the contact pair depth is too small (for example, 10-5), the machine precision may not guarantee the accuracy of penetration to be calculated. You should scale the length unit in the model.
Each contact element includes several KEYOPTS. We recommend using the default settings, which are suitable for most contact problems. For some specific applications, you can override the defaults. The element KEYOPTS allow you to control several aspects of contact behavior.
Degrees of freedom (KEYOPT(1))
Contact stiffness variation range (KEYOPT(6))
For node-to-surface contact (CONTA175), KEYOPT(3) specifies the contact model. For line-to-line contact (CONTA176), KEYOPT(3) specifies the type of beam-to-beam contact. KEYOPT(3) is not used for line-to-surface contact (CONTA177).
KEYOPT defaults can vary depending on the environment you are working in. The following table compares the default values between ANSYS, the ANSYS Contact Wizard, and the ANSYS Workbench. See your ANSYS sales representative for more information about ANSYS Workbench.
Table 3.2 Summary of KEYOPT Defaults in Different Environments
|KEYOPT||Description||ANSYS||ANSYS Contact Wizard||ANSYS Workbench Default Linear (bonded, no sep)||ANSYS Workbench, Default Nonlinear (standard, rough)|
|2||Contact Algorithm||Aug. Lagr.||Aug. Lagr.||Pure Penalty||Pure Penalty|
|3||Stress state when superelement is present||no super elem||no super elem||n/a||n/a|
|4||Location of contact detection point||gauss||gauss||gauss||gauss|
|5||CNOF/ICONT adjustment||No adjust||No adjust||No adjust||No adjust|
|6||Contact stiffnes variation||Use default range||Use default range||Use default range||Use default range|
|7||Element level time increment control||No control||No control||No control||No control|
|8||Asymmetric contact selection||No action||No action||No action||No action|
|9||Effect of initial penetration or gap||Include all||Include all||Exclude all||Include all|
|10||Contact stiffness update||Between load steps||Between iterations||Between load steps||Between load steps|
|11||Beam/shell thickness effect||Exclude||Exclude||Exclude||Exclude|
|12||Behavior of contact surface||Standard||Standard||Bonded||n/a|
|14||Behavior of fluid penetration load||Iteration-based||Iteration-based||n/a||n/a|
|15||Effect of stabilization damping||Active only in first load step||n/a||n/a||n/a|
|16||Squeal damping controls||Damping scaling factor||n/a||n/a||n/a|
*Manual: Requires user to define.
Auto: Selection is based on DOF of underlying element.
For surface-to-surface contact elements, ANSYS offers several different contact algorithms:
Penalty method (KEYOPT(2) = 1)
Augmented Lagrangian (default) (KEYOPT(2) = 0)
Lagrange multiplier on contact normal and penalty on tangent (KEYOPT(2) = 3)
Pure Lagrange multiplier on contact normal and tangent (KEYOPT(2) = 4)
Internal multipoint constraint (MPC) (KEYOPT(2) = 2)
The penalty method uses a contact "spring" to establish a relationship between the two contact surfaces. The spring stiffness is called the contact stiffness. This method uses the following real constants: FKN and FKT for all values of KEYOPT(10), plus FTOLN and SLTO if KEYOPT(10) = 2.
The augmented Lagrangian method (which is the default) is an iterative series of penalty methods. The contact tractions (pressure and frictional stresses) are augmented during equilibrium iterations so that the final penetration is smaller than the allowable tolerance (FTOLN). Compared to the penalty method, the augmented Lagrangian method usually leads to better conditioning and is less sensitive to the magnitude of the contact stiffness. However, in some analyses, the augmented Lagrangian method may require additional iterations, especially if the deformed mesh becomes too distorted.
The pure Lagrange multiplier method enforces zero penetration when contact is closed and "zero slip" when sticking contact occurs. The pure Lagrange multiplier method does not require contact stiffness, FKN and FKT. Instead it requires chattering control parameters, FTOLN and TNOP. This method adds contact traction to the model as additional degrees of freedom and requires additional iterations to stabilize contact conditions. It often increases the computational cost compared to the augmented Lagrangian method.
An alternative algorithm is the Lagrange multiplier method applied on the contact normal and the penalty method (tangential contact stiffness) on the frictional plane. This method enforces zero penetration and allows a small amount of slip for the sticking contact condition. It requires chattering control parameters, FTOLN and TNOP, as well as the maximum allowable elastic slip parameter SLTO.
Another method, the internal multipoint constraint (MPC) algorithm, is used in conjunction with bonded contact (KEYOPT(12) = 5 or 6) and no separation contact (KEYOPT(12) = 4) to model several types of contact assemblies and kinematic constraints. See Multipoint Constraints and Assemblies for more information on how to use this feature.
The Lagrange multiplier methods (KEYOPT(2) = 3, 4) and MPC approach (KEYOPT(2) = 2) do not support the Gauss point detection option (KEYOPT(4) = 0) for surface-to-surface contact. They support the nodal detection options for surface-to-surface contact and node-to-surface contact. When using these options, be careful not to overconstrain the model. The model is overconstrained when a contact node has prescribed boundary conditions, CE and CP equations. ANSYS usually detects and eliminates the overconstraints. However, there is no guarantee that the program will eliminate all the cases of overconstraint. You should always verify your model carefully to address this issue. The Lagrange multiplier also introduces more degrees of freedom which may result in spurious modes for modal and linear eigenvalue buckling analyses. The augmented Lagrangian method would be a better choice for these analysis types.
The Lagrange multiplier methods (KEYOPT(2) = 3, 4) introduce zero diagonal terms in the stiffness matrix. Any iterative solver (e.g., PCG) will encounter a preconditioning matrix singularity with these methods. Therefore, you should switch to sparse solver.
If overconstraint occurs in bonded shell-shell assemblies when using the MPC algorithm, you can switch to the penalty method or the augmented Lagrangian method. See Bonded Contact for Shell-Shell Assemblies for more information.
For 3-D higher order contact elements (CONTA174), the Lagrange multiplier method is applied at each contact node (including mid-side nodes), but the penalty method is applied on the center of the contact elements, even when KEYOPT(2)=3,4 is set.
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.
ANSYS provides default values for contact stiffnesses (FKN, FKT), allowable penetration (FTOLN), and allowable slip (SLTO). In most cases, you do not need to define the contact stiffness. In addition, we recommend that you use KEYOPT(10) = 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 0.01-1.0, with a default of 1.0. The default value is appropriate for bulk deformation. If bending deformation dominates, we recommend using a smaller value (0.1).
The default contact normal stiffness is affected by defined material properties, element size, and the total number of degrees of freedom in the model. Many factors may be applied to the actual contact normal stiffness during the solution. The default contact stiffness listed in the Contact Manager or by the CNCHECK command may be different from the actual contact stiffness reported by the ETABLE command. You should check the value reported by ETABLE to confirm that the appropriate contact normal stiffness is used.
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 3.10). 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 ANSYS 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.
When the contact stiffness is too large (for example, 1016), the machine precision may not guarantee good conditioning of the global stiffness matrix. In this case, you should scale the force unit in the model if possible.
FTOLN is also used in the Lagrange multiplier methods (KEYOPT(2) = 3, 4) as a chattering control parameter.
ANSYS 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) = 2, or when the Lagrange multiplier on normal and penalty on tangent option is used (KEYOPT(2) = 3), ANSYS updates tangential contact stiffness based on current contact normal pressure, PRES, and maximum allowable elastic slip, SLTO (KT = FKT*MU* PRES/SLTO). The real constant SLTO is used to control maximum sliding distance when FKT is updated at each iteration. ANSYS provides default tolerance values which work well in most cases. You can override the default values for SLTO (1% of average contact length in pair) 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).
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":
For bonded contact and rough contact, ANSYS uses MU = 1.0 to calculate tangential 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 we recommend that you use KEYOPT(10) = 2 to allow the program to update contact stiffnesses automatically. The possible settings for KEYOPT(10) are:
KEYOPT(10) = 0: the contact stiffness will be updated at each load step if FKN or FKT is redefined by the user. Stiffness and other settings (ICONT, FTOLN, SLTO, PINB, PMAX, and PMIN) are averaged across contact elements in a contact pair. The default contact stiffness is determined by underlying element depth and material properties.
KEYOPT(10) = 2: the normal contact stiffness will be updated at each iteration based on the current mean stress of the underlying elements and the allowable penetration, FTOLN, except in the very first iteration. The default normal contact stiffness for the first iteration is the same as described for KEYOPT(10) = 0. If bisections occur in the beginning of the analysis, the normal contact stiffness will be reduced by a factor of 0.2 for each bisection. The tangential contact stiffness will be updated at each iteration based on the current contact pressure, MU, and allowable slip (SLTO).
When a Lagrange multiplier method (KEYOPT(2) = 3, 4) or MPC algorithm (KEYOPT(2) = 2) is used, KEYOPT(10) is ignored.
The default method of updating normal contact stiffness is suitable for most applications. However, the variational range of the contact stiffness may not be wide enough to handle certain contact situations. In the case of a very small penetration tolerance (FTOLN), a larger normal contact stiffness is often needed. Furthermore, to stabilize the initial contact condition and to prevent rigid body motion, a smaller normal contact stiffness is required.
The allowed contact stiffness variation is intended to enhance stiffness updating when KEYOPT(10) = 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.
The Lagrange multiplier methods (KEYOPT(2) = 3, 4) do not require contact stiffness, FKN and FKT. Instead they require chattering control parameters, FTOLN and TNOP, by which ANSYS assumes that the contact status remains unchanged. FTOLN is the maximum allowable penetration and TNOP is the maximum allowable tensile contact pressure.
A negative contact pressure occurs when the contact status is closed. A tensile contact pressure (positive) refers to a separation between the contact surfaces, but not necessarily an open contact status. However, the sign of the contact pressure is switched during postprocessing.
The behavior can be described as follows:
If the contact status from the previous iteration is open and the current calculated penetration is smaller than FTOLN, then contact remains open. Otherwise the contact status switches to closed and another iteration is processed.
If the contact status from the previous iteration is closed and the current calculated contact pressure is positive but smaller than TNOP, then contact remains closed. If the tensile contact pressure is larger than TNOP, then the contact status changes from closed to open and ANSYS continues to the next iteration.
ANSYS will provide reasonable defaults for FTOLN and TNOP. FTOLN defaults to the displacement convergence tolerance. TNOP defaults to the force convergence tolerance divided by contact area at contact nodes.
Keep in mind the following when providing values for FTOLN and TNOP:
A positive value is a scaling factor applied to the default values.
A negative value is used as an absolute value (which overrides the default).
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. However, if the values are too large, the accuracy of the solution will be affected since 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 User-defined Friction).
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, ANSYS 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. You can input MU as a material property for the contact elements. Use MU = 0 for frictionless contact. For rough or bonded contact (KEYOPT(12) = 1, 3, 5, or 6; see Selecting Surface Interaction Models), ANSYS 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.
ANSYS provides two models for Coulomb friction: isotropic friction (2-D and 3-D contact) and orthotropic friction (3-D contact). The isotropic friction model is based on a single coefficient of friction, MU. You can use either TB command input (recommended method) or the MP command to specify MU. The orthotropic friction model is based on two coefficients of friction, MU1 and MU2. Use TB command input to specify MU1 and MU2 in two principal directions (see the element descriptions for CONTA173, CONTA174, CONTA175, CONTA176, and CONTA177 for a description of the principal directions for each individual element). See Contact Friction in the Material Reference for details on how to specify the coefficients of friction.
ANSYS 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 σy is the yield stress of the material being deformed.
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 3.11).
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.
ANSYS provides the following exponential decay friction model:
|μ = coefficient of friction.|
|MU = dynamic coefficient of friction.|
|FACT = ratio of static to dynamic coefficients of friction. It defaults to the minimum value of 1.0|
|DC = decay coefficient, which has units of time/length. Therefore, time has some meaning in a static analysis. DC defaults to zero. When DC is zero, the equation is rewritten to be μ = MU for the case of sliding and μ = FACT*MU for the case of sticking.|
|Vrel = slip rate calculated by ANSYS.|
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 3.12 shows the exponential decay curve where the static coefficient of friction is given by:
You can determine the decay coefficient if you know the static and dynamic coefficients of friction and at least one data point (μ1 ; Vrel1). 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. ANSYS determines the sliding direction based on the direction of the sliding velocities.
This feature is primarily useful 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. We recommend 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:
|Rough contact (KEYOPT(12) = 1)|
|Bonded contact (KEYOPT(12) = 2, 5, 6)|
|MPC contact (KEYOPT(12) = 2)|
You should always verify the sliding direction when the velocities defined by CMROTATE are applied on nodes that are shared by more than one frictional contact pair. In this situation, you can redefine any contact elements that have a potentially incorrect sliding direction as frictionless contact.
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:
Define friction as a function of sliding velocity via the TB,FRIC command.
Define static/dynamic friction via real constants FACT and DC.
Define a constant friction-sliding velocity gradient via real constant FDMD in conjunction with KEYOPT(16) = 1.
Specify the destabilizing squeal damping coefficient directly (either a positive or negative value) in conjunction with KEYOPT(16) = 2.
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. ANSYS will multiply 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. ANSYS will multiply 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. It is recommended that you use the DAMP eigensolver (MODOPT,DAMP) to check the final solution.
You can write a USERFRIC subroutine to program your own friction model for 2-D and 3-D contact elements (CONTA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, CONTA177, and CONTA178). See User-Defined Friction in the Material Reference for more information on how to use this feature. See also the Guide to ANSYS User Programmable Features for a detailed description of the USERFRIC subroutine.
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 3.13.
ANSYS 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, the line-to-line contact element, CONTA176, 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-surface, or edge-surface contact (see Figure 3.14). 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 this option (KEYOPT(4) = 2) when the target surface is smoother than the contact surface.
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 3.15. 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, we recommend using CONTA175; see Node-to-Surface Contact later in this guide.
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 10 for small deflection and 2 for 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). For the 3-D line-to-line contact element CONTA176 and the 3-D line-to-surface contact element CONTA177, KEYOPT(4) is not used to select the location of contact detection, and the contact normal is always perpendicular to both the contact and target surfaces. For CONTA176 and CONTA177, KEYOPT(4) is used to specify a surface-based constraint type.
You can define the surface projection contact method by setting KEYOPT(4) = 3 for surface-to-surface contact elements (CONTA171 through CONTA174). For this method, the contact detection remains at contact nodal points. This option enforces a contact constraint on an overlapping region of the contact and target surfaces (see Figure 3.16) 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. The advantages of using this option are the following:
In general, it provides more accurate contact tractions and stresses of underlying elements compared with other KEYOPT(4) settings.
The results are less sensitive to the designation of the contact and target surface.
It satisfies moment equilibrium when an offset exists between contact and target surfaces with friction.
Contact forces do not jump when contact nodes slide off the edge of target surfaces. The real constant TOLS is not used with this option.
There are certain disadvantages to using surface projection based contact, as follows:
This method is computationally more expensive since more nodes are included in each contact constraint condition, especially if 3-D higher order contact/target elements are used in the model. This effect will be more obvious when a modal has a large percentage of contact/target elements, or when the target elements are much more refined than the contact elements.
This method calculates the penetration/gap over the contacting area in an average sense. When a model has corner or edge contact, the averaged penetration/gap could be quite different than the real geometric penetration observed at contact nodes. In this situation, mesh refinement is usually required in order to achieve an accurate solution.
The surface projection contact method currently does not support the following:
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:
Rigid body profiles are often complicated, making it difficult to determine where the first point of contact might occur.
Small gaps between element meshes on both sides of the element pair can be introduced by numerical round-off, even if the solid model is built in an initially-contacting state.
Small gaps can exist between the integration points of the contact elements and target surface elements.
For surface projection based contact, a numerical gap distance can exist even though geometric penetration is observed at a contact node. This can occur because the numerical distance is obtained over the overlapping area in an average sense.
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. ANSYS 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.
Use real constant CNOF to specify a contact surface offset.
Specify a positive value to offset the entire contact surface towards the target surface. Use a negative value to offset the contact surface away from the target surface.
If user-defined values are input for both CNOF and PINB, you must ensure that PINB is greater than CNOF. Otherwise, CNOF will be ignored. However, if a user-defined CNOF is input and the PINB value is left at its default value, the PINB value will be adjusted so that it is larger than the CNOF value, as described in Using PINB.
For the CONTA177 line-to-surface element, CNOF can be used to model thickness of the underlying beam elements. Input half of the beam thickness for CNOF to properly model the thickness effects. See Accounting for Thickness Effect (CNOF and KEYOPT(11)) for more information.
ANSYS can automatically provide the CNOF value to either just close the gap or reduce initial penetration. Set KEYOPT(5) as follows:
Tabular input can also be used to define CNOF. The tabular input can be defined as a function of time and/or x,y,z location (in global or local coordinates). As an example of when tabular input may be useful, consider the case of a CAD geometry based on nominal values. The geometry may lack a slight curvature variation that is important for analysis purposes. Moving nodes to the actual positions can be a tedious process, yet using the original geometry and neglecting the slight variation in curvature will result in a different contacting area. Consequently, use of CNOF as a function of location allows you to easily include curvature that varies with location without having to modify the original CAD geometry.
Use the real constant ICONT to specify a small initial contact closure. This is the depth of an "adjustment band" around the target surface. A positive value for ICONT indicates a scaling factor relative to the depth of the underlying elements. A negative value indicates an absolute contact closure value. The value of ICONT defaults to zero if KEYOPT(5) = 0, 1, 2, or 3. (The ICONT default is different when KEYOPT(12) = 6 for bonded-initial contact; see Selecting Surface Interaction Models for more information). If KEYOPT(5) = 4, ANSYS provides a small (but meaningful) value for ICONT according to the geometric dimensions, and prints a warning message stating what value was assigned. Any contact detection points that fall within this adjustment band are internally shifted to be on the target surface (see Figure 3.17(a)). Only a very small correction is suggested; otherwise, severe discontinuity may occur (see Figure (b)).
The difference between CNOF and ICONT is that the former shifts the entire contact surface with the distance value CNOF, the latter moves all initially open contact points which are inside of adjustment band ICONT onto the target surface.
Use real constants PMIN and PMAX to specify an initial allowable penetration range. When either PMAX or PMIN is specified, ANSYS brings the target surface into a state of initial contact at the beginning of the analysis (see Figure 3.18). If the initial penetration is larger than PMAX, ANSYS adjusts the target surface to reduce penetration. If the initial penetration is smaller than PMIN (and within the pinball region), ANSYS adjusts the target surface to ensure initial contact. Initial adjustment for contact status is performed only in translational modes.
Such adjustment of initial contact status will be performed for a rigid target surface that has either prescribed loads or displacements. Similarly, a target surface that has no boundary conditions specified may also be adjusted for initial contact.
When all the target surface nodes have a prescribed value of zero, the initial adjustment using PMAX and PMIN will not be performed.
Note that ANSYS treats applicable degrees of freedom for target surface nodes independently. For example, if you specify the UX degree of freedom to be "zero," then no initial adjustment is possible along the X direction. However, the PMAX and PMIN options will still be activated in the Y and Z directions.
The initial status adjustment is an iterative process. ANSYS uses a maximum of 20 iterations. If the target surface cannot be brought into an acceptable penetration range (i.e., in the range of PMIN to PMAX), the analysis proceeds with the original geometry. ANSYS issues a warning message in such circumstances, and you may need to manually adjust your initial geometry.
Figure 3.19 illustrates a problem in which initial contact adjustment iteration will fail. The UY degree of freedom for the target has been restrained. Therefore, the only possible adjustment for initial contact is in the X direction. However, in this problem, any movement of the rigid target surface in the X direction will not establish initial contact.
For flexible-to-flexible contact, this technique not only moves the entire target surface but also moves the whole deformable body which attaches to the target surface. Make sure there is no other contact surface or target surface connecting with the deformable body.
Set KEYOPT(9) to adjust initial penetration or gap; see Figure 3.20.
True initial penetration includes two parts:
Penetration or gap due to geometry
Penetration or gap due to user-defined contact surface offset (CNOF).
See Figure 3.21.
KEYOPT(9) provides the following capabilities:
To include initial penetration from both geometry and contact surface offset, set KEYOPT(9) = 0. This is the default.
To ignore initial penetration from both effects, set KEYOPT(9) = 1. When KEYOPT(12) = 4 or 5, this setting for KEYOPT(9) will also ignore the initial force in open-gap springs, thus creating an initially "perfect" contacting surface having no initial forces acting across the contact interface.
To include the defined contact surface offset (CNOF) but ignore the initial penetration due to geometry, set KEYOPT(9) = 3. This option works if initial penetration is detected for certain contact definitions (KEYOPT(12) = 0, 1, 2, 3, or 6). When KEYOPT(12) = 4 or 5, this setting for KEYOPT(9) will also ignore the initial force in open-gap springs, thus creating an initially "perfect" contacting surface having no initial forces acting across the contact interface.
Set KEYOPT(9) = 5 to include the defined contact surface offset (CNOF) but ignore the initial penetration or gap due to geometry as long as the contact is detected within the pinball region (near-field or closed contact). For a bonded contact definition with KEYOPT(12) = 4, or 5, setting KEYOPT(9) = 3 is equivalent to setting KEYOPT(9) = 5.
For problems such as an interference fit, over-penetration is expected. These problems often have convergence difficulties if the initial penetration is step-applied in the first load step. You may overcome convergence difficulties by ramping the initial penetration over the first load step, see Figure 3.22. The following KEYOPT(9) settings provide ramped capabilities:
To ramp the total initial penetration (CNOF + the offset due to geometry), set KEYOPT(9) = 2.
To ramp the defined contact surface penetration (CNOF), but ignore the penetration due to geometry, set KEYOPT(9) = 4. This option works if initial penetration is detected for certain contact definitions (KEYOPT(12) = 0, 1, 2, 3, or 6).
To ramp the defined contact offset (CNOF) but ignore the penetration or gap due to geometry, set KEYOPT(9) = 6. This option works as long as the contact is detected within the pinball region (near-field or closed contact). For a bonded contact definition with KEYOPT(12) = 4 or 5, setting KEYOPT(9) = 4 is equivalent to setting KEYOPT(9) = 6.
For the above KEYOPT(9) settings, you should also set KBC,0 and not specify any external loads in the first load step. Also, be sure that the pinball region is big enough to capture the initial interference.
By default, the ramping options are active only within the first load step. However, you may have a situation where there are multiple interference fits that you want to model sequentially (that is, the interference present in each contact pair will be resolved in different load steps). You can define the load step number in which the ramping option will take place for a given contact pair by using the real constant STRM. For example, you may want to perform a different loading in load step 1, then resolve an interference fit in load step 2 for one contact pair, and finally resolve an interference fit in load step 3 for another contact pair. To accomplish this, you would set STRM = 2 for the first contact pair and set STRM = 3 for the second contact pair. Note that contact will still be active prior to the load step specified by the STRM real constant.
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:
Use CNOF to specify a penetration (positive value) or gap (negative value).
Use KEYOPT(9) = 5 to resolve the initial penetration in the first substep (or KEYOPT(9) = 6 to gradually resolve the initial penetration).
ANSYS 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, ANSYS issues a warning. This occurs when the target surface is far from contact (i.e., 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.
You can adjust the initial contact status in order to close the gap by doing one of the following:
|(a) Define an initial contact adjustment via real constant ICONT. (ICONT may change the shape of the contact detection surface.)|
|(b) Define a contact offset via real constant CNOF. (CNOF does not change the shape of the contact detection surface.)|
|(c) Ignore the penetration by setting KEYOPT(9) = 1. (KEYOPT(9) = 1 does change the shape of the contact detection surface.)|
However, these adjustment methods do not truly change the physical locations of contact nodes; rather, the contact detection locations are adjusted.
The initial adjustment due to (a) is applied only once in the beginning of the contact analysis, where each contact detection point within the ICONT range is made to be in initial contact with the target surface. The contact adjustments due to (b) and (c) offset the entire contact detection surface to close any gap that is present. In doing so, methods (b) and (c) introduce a "rigid region" between the contact and target surfaces during the entire analysis, which can cause a certain amount of residual force if a large rotation appears at the contact surface. This problem can be alleviated by issuing the CNCHECK,ADJUST command, which physically moves contact nodes towards the target surface under the following circumstances:
After issuing the CNCHECK,ADJUST command, the coordinates of the nodes that have been moved are modified as shown in Figure 3.23. 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.
For those contact pairs whose contact nodes you do not wish to physically move towards target surface, do not define KEYOPT(4) = 1 or 2.
The position and motion of a contact element relative to its associated target surface determines the contact element status. ANSYS monitors each contact element and assigns a status:
STAT = 0 Open far-field contact (open and not near contact)
STAT = 1 Open near-field contact
STAT = 2 Sliding contact
STAT = 3 Sticking contact
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 2-D) or a sphere (in 3-D) 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, and assuming that large deflection effects apply (NLGEOM,ON), ANSYS defines the pinball region as a circle for 2-D or a sphere for 3-D of radius 4*depth (if rigid-to-flexible contact) or 2*depth (if flexible-to-flexible contact) of the underlying element. (See the discussion of element depth in Positive and Negative Real Constant Values.) If you include no large-deflection effects (NLGEOM,OFF), the default pinball region is half that of the large-deflection case. (For the no-separation (KEYOPT(12) = 4) and bonded-always (KEYOPT(12) = 5 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 (as described above) 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.
The program will warn 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.
See Positive and Negative Real Constants for more information on this real constant.
In some cases of self contact, ANSYS may erroneously assume contact between a contact and target surface that are in very close geometrical position as shown below.
ANSYS will alert you when it first detects spurious contact in each load step. If ANSYS encounters such contact on the first load step, you'll see the following error message:
Contact element x has too much penetration related to target element y. We assume it (may be more elements) is spurious contact.
If ANSYS encounters an abrupt change in contact that it classifies as spurious contact, you'll see the following message:
Contact element x status changed abruptly with target element y. We assume it (may be more elements) is spurious contact.
ANSYS issues such messages only once per load step. It does not notify you of additional cases of spurious contact that were ignored during the load step.
The surface-to-surface contact elements support normal unilateral contact models as well as other mechanical surface interaction models.
Use KEYOPT(12) to model different contact surface behaviors.
KEYOPT(12) = 0 models standard unilateral contact; that is, normal pressure equals zero if separation occurs.
KEYOPT(12) = 1 models perfectly rough frictional contact where there is no sliding. This case corresponds to an infinite friction coefficient and ignores the material property MU.
KEYOPT(12) = 2 models no separation contact, in which the target and contact surfaces are tied (although sliding is permitted) for the remainder of the analysis once contact is established.
KEYOPT(12) = 3 models "bonded" contact, in which the target and contact surfaces are bonded in all directions (once contact is established) for the remainder of the analysis.
KEYOPT(12) = 4 models no separation contact, in which contact detection points that are either initially inside the pinball region or that once involve contact always attach to the target surface along the normal direction to the contact surface (sliding is permitted).
KEYOPT(12) = 5 models bonded contact, in which contact detection points that are either initially inside the pinball region or that once involve contact always attach to the target surface along the normal and tangent directions to the contact surface (fully bonded).
KEYOPT(12) = 6 models bonded contact, in which the contact detection points that are initially in a closed state will remain attached to the target surface and the contact detection points that are initially in an open state will remain open throughout the analysis.
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) and the bonded-always option (KEYOPT(12) = 5), 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) for small deformation analysis (NLGEOM,OFF) and 0.5 (50% of the contact depth) for large deformation analysis (NLGEOM,ON). (The default PINB value may differ from what is described here if CNOF is input. See Using PINB for more information.)
For the bonded-initial option (KEYOPT(12) = 6), a relatively large ICONT value (initial contact closure) may be used to capture the contact. For this KEYOPT(12) setting, the default for ICONT is 0.05 (5% of the contact depth) when KEYOPT(5) = 0 or 4.
See Positive and Negative Real Constants for more information on the real constants mentioned above.
For bonded contact definitions (KYEOPT(12) = 5 or 6), if the contact is not in a “just touching” position, you may find that no zero modes appear for free vibration. To avoid this issue, use the MPC approach instead of other contact algorithms.
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.
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).
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 (Tc) 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 Tc 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.
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). When this method is used to model shell-shell assemblies, there may be cases where the MPC approach causes the 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 CONTA173, 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) in the contact elements. Setting KEYOPT(5) = 2 (shell-shell constraint) for the target elements will cause 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 it is printed in the output file. The figure below shows the difference in using a conventional penalty-based shell-shell assembly and this method.
In the case of a penalty-based shell-shell assembly, spurious rotational energy exists if there are gaps or penetrations between the contact and target surfaces. This can affect the accuracy of the solution. In this case it is recommended that you use a shell-solid constraint type by setting KEYOPT(5) = 3, 4, or 5 on the target element, which requires use of the MPC algorithm (KEYOPT(2) = 2 on the contact element).
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 slave 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 ANSYS 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.
No superelement used (KEYOPT(3) = 0)
Axisymmetric, use with superelements only (KEYOPT(3) = 1)
Plane strain or plane stress with unit thickness, use with superelements only (KEYOPT(3) = 2)
Plane stress with thickness input use with superelements only (KEYOPT(3) = 3). Note that for this case, use real constant R2 to specify the thickness.
KEYOPT(3) has different meanings in the node-to surface contact element, CONTA175, and in the line-to-line contact element, CONTA176. KEYOPT(3) is not used for the line-to-surface contact element, CONTA177.
For CONTA175, KEYOPT(3) = 1 defines the contact traction-based model. In this case, all of the real constant inputs and contact result quantities have the same units as the surface-to-surface contact elements. KEYOPT(3) = 0 (default) defines the contact force model. In this model, certain real constants and contact result quantities can have different units (a factor of AREA (Length2) difference). See KEYOPT(3).
Rigid body motion often occurs in the beginning of an analysis due to the fact that the initial contact condition is not well established. The causes may include:
Small gaps between element meshes on both sides of the element pair can be introduced by numerical round-off, even if the solid model is built in an initially-contacting state.
Small gaps can exist between the integration points of the contact elements and target surface elements.
For surface projection based contact, a numerical gap distance can exist even though geometric penetration is observed at a contact node. This can occur because the numerical distance is obtained over the overlapping area in an average sense.
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 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:
Number of substeps
Size of time increment for the current substep
In general, contact stabilization damping should only be used for preventing 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 of the following conditions are encountered:
Gauss point based contact (KEYOPT(4) = 0) or surface projection based contact (KEYOPT(4) = 3) is used.
The entire contact pair is in open status.
A geometric penetration is detected at any contact nodal point, despite condition 2 above.
Without this automatic contact stabilization, rigid body motion may occur. If you wish to deactivate automatic contact stabilization, you can simply set KEYOPT(15) = 1.
You can activate contact stabilization damping manually by specifying real constants FDMN and FDMT.
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. The units of the damping coefficient are PRESSURE/VELOCITY. For the contact force-based model (used by CONTA175, CONTA176, and CONTA177), the units are FORCE/VELOCITY.
Use a positive value of FDMT to specify a damping scaling factor in the tangential direction. The tangential contact damping is activated only when the normal damping is activated. FDMT defaults to 0.001. You can overwrite the internally calculated tangential damping coefficient by specifying a user defined value (use a negative value for command input). The units of the damping coefficient are PRESSURE/VELOCITY. For the contact force-based model (used by CONTA175, CONTA176, and CONTA177), the units are FORCE/VELOCITY.
The contact stabilization damping is activated if all of the following conditions are met:
Standard contact (KEYOPT(12) = 0) or rough contact (KEYOPT(12) = 1)
Contact status is near-field
The first load step, unless KEYOPT(15) = 2 or 3
The entire contact pair has an open contact status in the previous substep, unless KEYOPT(15) = 3
When KEYOPT(15) = 0, 1, or 2, stabilization damping will not be applied in the current substep if any contact detection point had a closed status in the previous substep. However, when KEYOPT(15) = 3, stabilization damping is always applied as long as the current contact status is near-field, regardless of the contact status of the previous substep.
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) 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), the results are still acceptable.
You can account for the thickness of shells (2-D and 3-D) and beams (2-D) using KEYOPT(11). (This does not apply to 3-D beam-to-beam contact.) For rigid-to-flexible contact, ANSYS will automatically shift the contact surface to the bottom or top of the shell/beam surface. For flexible-to-flexible contact, ANSYS will automatically shift both the contact and target surfaces which are attached to shell/beam elements. By default, ANSYS 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.
Only use KEYOPT(11) = 1 to account for thickness when you have shell or beam elements with nodes located at the middle surface.
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 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.
KEYOPT(7) = 0: No control. The time step size is unaffected by the prediction. This setting is appropriate for most analyses when automatic time stepping is activated and a small time step size is allowed.
KEYOPT(7) = 1: Time step size is bisected if too much penetration occurs during an iteration, or if the contact status changes dramatically.
KEYOPT(7) = 2: Predict a reasonable increment for the next substep.
KEYOPT(7) = 3: Predict a minimal time increment for the next substep.
Use KEYOPT(7) = 4 to activate impact constraints.
KEYOPT(7) = 4: Use impact constraints for standard or rough contact (KEYOPT(12) = 0 or 1) in a transient dynamic analysis with automatic adjustment of the time increment.
The surface-to-surface contact and target elements allow birth and death. The elements can be removed for part of an analysis and then reactivated for a later stage. This feature is useful for modeling complex metal forming processes where multiple rigid target surfaces need to interact with the contact surface at different stages of the analysis. Springback modeling often requires removing the rigid tools at the end of the forming processes. This option cannot be used with "no separation" or bonded contact.