CONTA176


3-D Line-to-Line Contact

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

CONTA176 Element Description

CONTA176 is used to represent contact and sliding between 3-D line segments (TARGE170) and a deformable line segment, defined by this element. The element is applicable to 3-D beam-beam structural contact analyses. This element is located on the surfaces of 3-D beam or pipe elements with or without midside nodes (such as BEAM188 or BEAM189). Contact occurs when the element surface penetrates one of the 3-D straight line or parabolic line segment elements (TARGE170) on a specified target surface. Coulomb friction, shear stress friction, user-defined friction with the USERFRIC subroutine, and user-defined contact interaction with the USERINTER subroutine are allowed. This element also allows separation of bonded contact to simulate interface delamination. See CONTA176 in the Mechanical APDL Theory Reference for more details about this element. To model beam-to-surface contact, use the line-to-surface contact element, CONTA177.

Figure 176.1:  CONTA176 Geometry

CONTA176 Geometry

CONTA176 Input Data

The geometry and node locations are shown in Figure 176.1: CONTA176 Geometry. The element is defined by two nodes (if the underlying beam element does not have a midside node) or three nodes (if the underlying beam element has a midside node). The element x-axis is along the I-J line of the element. Correct node ordering of the contact element is critical for proper detection of contact. The nodes must be ordered in a sequence that defines a continuous line. See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.

Three different scenarios can be modeled by CONTA176:

Use KEYOPT(3) = 0 for the first two scenarios (internal contact and parallel beams). In both cases, the contact condition is only checked at contact nodes.

Use KEYOPT(3) = 1 for the third scenario (beams that cross). In this case, the contact condition is checked along the entire length of the beams. The beams with circular cross sections are assumed to come in contact in a point-wise manner. Each contact element can potentially contact no more than one target element.

Figure 176.2:  Beam Sliding Inside a Hollow Beam

Beam Sliding Inside a Hollow Beam

Figure 176.3:  Parallel Beams in Contact

Parallel Beams in Contact

Figure 176.4:  Crossing Beams in Contact

Crossing Beams in Contact

The 3-D line-to-line contact elements are associated with the target line segment elements (LINE or PARA segment types for TARGE170) via a shared real constant set. The contact/target surface is assumed to be the surface of a cylinder. For a general beam cross section, use an equivalent circular beam (see Figure 176.5: Equivalent Circular Cross Section). Use the first real constant, R1, to define the radius on the target side (target radius rt). Use the second real constant, R2, to define the radius on the contact side (contact radius rc). Follow these guidelines to define the equivalent circular cross section:

  • Determine the smallest cross section along the beam axis.

  • Determine the largest circle embedded in that cross section.

Figure 176.5:  Equivalent Circular Cross Section

Equivalent Circular Cross Section

The target radius can be entered as either a negative or positive value. Use a negative value when modeling internal contact (a beam sliding inside a hollow beam, or pipe sliding inside another pipe), with the input value equal to the inner radius of the outer beam (see Figure 176.2: Beam Sliding Inside a Hollow Beam). Use a positive value when modeling contact between the exterior surfaces of two cylindrical beams.

For the case of internal contact, the inner beam should usually be considered the contact surface and the outer beam should be the target surface. The inner beam can be considered as the target surface only when the inner beam is much stiffer than the outer beam.

Contact is detected when two circular beams touch or overlap each other. The non-penetration condition for beams with a circular cross section can be defined as follows.

For internal contact:

and for external contact:

where rc and rt are the radii of the cross sections of the beams on the contact and target sides, respectively; and d is the minimal distance between the two beams which also determines the contact normal direction (see Figure 176.4: Crossing Beams in Contact). Contact occurs for negative values of g.

When the contact radius and/or target radius are not defined, the program automatically calculates the equivalent radius for each individual contact/target element based on the associated geometry of underlying beam elements. In this case, the equivalent radius may vary within a contact pair.

ANSYS looks for contact only between contact and target surfaces with the same real constant set. For either rigid-flexible or flexible-flexible contact, one of the deformable surfaces must be represented by a contact surface. See Designating Contact and Target Surfaces in the Contact Technology Guide for more information. If more than one target surface will make contact with the same boundary of beam elements, you must define several contact elements that share the same geometry but relate to separate targets (targets which have different real constant numbers), or you must combine the two target surfaces into one (targets that share the same real constant numbers).

CONTA176 supports isotropic and orthotropic Coulomb friction. For isotropic friction, specify a single coefficient of friction, MU, using either TB command input (recommended) or the MP command. For orthotropic friction, specify two coefficients of friction, MU1 and MU2, in two principal directions using TB command input. (See Contact Friction in the Material Reference for more information.)

For isotropic friction, local element coordinates based on the nodal connectivity are used to define principal directions. In the case of two crossing beams in contact (KEYPT(3) = 1), the first principal direction is defined by 1/2(t1 + t2). The first vector, t1, points from the first contact node to the second contact node, and the second vector, t2, points from the first target node to the second target node. In the case of two parallel beams in contact (KEYOPT(3) = 0), the first principal direction points from the first contact node to the second contact node. In both cases, the second principal direction is defined by taking a cross product of the first principal direction and the contact normal.

For orthotropic friction, the principal directions are determined as follows. The global coordinate system is used by default, or you may define a local element coordinate system with the ESYS command. The first principal direction is defined by projecting the first direction of the chosen coordinate system onto the contact element. The second principal direction is defined by taking a cross product of the first principal direction and the contact normal. These directions also follow the rigid body rotation of the contact element to correctly model the directional dependence of friction. Be careful to choose the coordinate system (global or local) so that the first direction of that system is within 45° of the tangent to the contact surface.

If you want to set the coordinate directions for isotropic friction (to the global Cartesian system or another system via ESYS), you can define orthotropic friction and set MU1 = MU2.

To define a coefficient of friction for isotropic or orthotropic friction that is dependent on temperature, time, normal pressure, sliding distance, or sliding relative velocity, use the TBFIELD command along with TB,FRIC. See Contact Friction in the Material Reference for more information.

To implement a user-defined friction model, use the TB,FRIC command with TBOPT = USER to specify friction properties and write a USERFRIC subroutine to compute friction forces. See Writing Your Own Friction Law (USERFRIC) in the Mechanical APDL Contact Technology Guide for more information on how to use this feature. See also the Guide to User-Programmable Features for a detailed description of the USERFRIC subroutine.

In addition to the user-defined friction subroutine, the contact interaction subroutine USERINTER is available for user-defined interface interactions, including interactions in the normal and tangential directions. See Defining Your Own Contact Interaction (USERINTER) in the Mechanical APDL Contact Technology Guide for more information on how to use this feature. See also the Guide to User-Programmable Features for a detailed description of the USERINTER subroutine.

To model proper momentum transfer and energy balance between contact and target surfaces, impact constraints should be used in transient dynamic analysis. See the description of KEYOPT(7) below and the contact element discussion in the Mechanical APDL Theory Reference for details.

To model separation of bonded contact with KEYOPT(12) = 2, 3, 4, 5, or 6, use the TB command with the CZM label. See Debonding in the Contact Technology Guide for more information.

In addition to controlling the type of beam contact, KEYOPT(3) allows you to choose between a contact force-based model (KEYOPT(3) = 0 or 1; default = 0) and a contact traction-based model (KEYOPT(3) = 2 or 3). The units for certain real constants (FKN, FKT, TNOP) and postprocessing items (PRES, TAUR, TAUS, SFRIC, and so on) vary by a factor of AREA, depending on which model is specified. (For details, see the real constant table and output definitions table.) For more information on using KEYOPT(3) with CONTA176, see KEYOPT(3) in the Contact Technology Guide.

See the Contact Technology Guide for a detailed discussion on contact and using the contact elements. 3-D Beam-to-Beam Contact discusses CONTA176 specifically, including the use of real constants and KEYOPTs.

The following table summarizes the element input. Element Input gives a general description of element input.

CONTA176 Input Summary

Nodes

I, J, (K)

Degrees of Freedom
UX, UY, UZ
Real Constants
R1, R2, FKN, FTOLN, ICONT, PINB,
PMAX, PMIN, TAUMAX, CNOF, FKOP, FKT,
COHE, (Blank), (Blank), (Blank), (Blank), (Blank),
(Blank), (Blank), FACT, DC, SLTO, TNOP,
TOLS, (Blank), (Blank), (Blank), COR, STRM
FDMN, FDMT, , , TBND
See Table 176.1: CONTA176 Real Constants for descriptions of the real constants.
Material Properties
TB command: See Element Support for Material Models for this element.
MP command: MU
Special Features
Birth and death
Debonding
Isotropic friction
Large deflection
Linear perturbation
Nonlinearity
Orthotropic friction
User-defined contact interaction
User-defined friction
KEYOPTs

Presented below is a list of KEYOPTS available for this element. Included are links to sections in the Contact Technology Guide where more information is available on a particular topic.

KEYOPT(1)

Selects degrees of freedom. Currently, the default (UX, UY, UZ) is the only valid option:

0 -- 

UX, UY, UZ

KEYOPT(2)

Contact algorithm:

0 -- 

Augmented Lagrangian (default)

1 -- 

Penalty function

2 -- 

Multipoint constraint (MPC); see Multipoint Constraints and Assemblies in the Contact Technology Guide for more information

3 -- 

Lagrange multiplier on contact normal and penalty on tangent

4 -- 

Pure Lagrange multiplier on contact normal and tangent

KEYOPT(3)

Beam contact type:

0 -- 

Parallel beams or beam inside beam (contact force-based model)

1 -- 

Crossing beams (contact force-based model)

2 -- 

Parallel beams or beam inside beam (contact traction-based model)

3 -- 

Crossing beams (contact traction-based model)

KEYOPT(4)

Type of surface-based constraint (see Surface-based Constraints for more information):

0 -- 

Rigid surface constraint

1 -- 

Force-distributed constraint

3 -- 

Coupling constraint

KEYOPT(5)

CNOF/ICONT Automated adjustment:

0 -- 

No automated adjustment

1 -- 

Close gap with auto CNOF

2 -- 

Reduce penetration with auto CNOF

3 -- 

Close gap/reduce penetration with auto CNOF

4 -- 

Auto ICONT

KEYOPT(6)

Contact stiffness variation (used to enhance stiffness updating when KEYOPT(10) > 0):

0 -- 

Use default range for stiffness updating

1 -- 

Make a nominal refinement to the allowable stiffness range

2 -- 

Make an aggressive refinement to the allowable stiffness range

KEYOPT(7)

Element level time incrementation control / impact constraints:

0 -- 

No control

1 -- 

Automatic bisection of increment

2 -- 

Change in contact predictions are made to maintain a reasonable time/load increment

3 -- 

Change in contact predictions made to achieve the minimum time/load increment whenever a change in contact status occurs

4 -- 

Use impact constraints for standard or rough contact (KEYOPT(12) = 0 or 1) in a transient dynamic analysis with automatic adjustment of time increment

KEYOPT(8)

Asymmetric contact selection:

0 -- 

No action

2 -- 

ANSYS internally selects which asymmetric contact pair is used at the solution stage (used only when symmetry contact is defined).

KEYOPT(9)

Effect of initial penetration or gap:

0 -- 

Include both initial geometrical penetration or gap and offset

1 -- 

Exclude both initial geometrical penetration or gap and offset

2 -- 

Include both initial geometrical penetration or gap and offset, but with ramped effects

3 -- 

Include offset only (exclude initial geometrical penetration or gap)

4 -- 

Include offset only (exclude initial geometrical penetration or gap), but with ramped effects

5 -- 

Include offset only (exclude initial geometrical penetration or gap) regardless of the initial contact status (near-field or closed)

6 -- 

Include offset only (exclude initial geometrical penetration or gap), but with ramped effects regardless of the initial contact status (near-field or closed)


Note:  The effects of KEYOPT(9) are dependent on settings for other KEYOPTs. The indicated initial gap effect is considered only if KEYOPT(12) = 4 or 5. See the discussion on using KEYOPT(9) in the Contact Technology Guide for more information.


KEYOPT(10)

Contact Stiffness Update:

0 -- 

Each load step if FKN is redefined during load step (pair based).

2 -- 

Each iteration based on current mean stress of underlying elements (pair based).

KEYOPT(12)

Behavior of contact surface:

0 -- 

Standard

1 -- 

Rough

2 -- 

No separation (sliding permitted)

3 -- 

Bonded

4 -- 

No separation (always)

5 -- 

Bonded (always)

6 -- 

Bonded (initial contact)


Note:  When KEYOPT(12) = 5 or 6 is used with the MPC algorithm to model surface-based constraints, the KEYOPT(12) setting will have an impact on the local coordinate system of the contact element nodes. See Specifying a Local Coordinate System in the Contact Technology Guide for more information.


KEYOPT(15)

Effect of contact stabilization damping:

0 -- 

Damping is activated only in the first load step (default).

1 -- 

Deactivate automatic damping.

2 -- 

Damping is activated for all load steps.

3 -- 

Damping is activated at all times regardless of the contact status of previous substeps.


Note:  Normal stabilization damping is only applied to the contact element when the current contact status of the contact detection point is near-field. When KEYOPT(15) = 0, 1, or 2, normal stabilization damping is not applied in the current substep if any contact detection point has a closed status. However, when KEYOPT(15) = 3, normal stabilization damping is always applied as long as the current contact status of the contact detection point is near-field. Tangential stabilization damping is automatically activated when normal damping is activated. Tangential damping can also be applied independent of normal damping for sliding contact. See Applying Contact Stabilization Damping in the Contact Technology Guide for more information.


Table 176.1:  CONTA176 Real Constants

No.NameDescriptionFor more information, see this section in the Contact Technology Guide . . .
1R1

Target radius

Real Constants R1, R2

2R2

Contact radius

Real Constants R1, R2

3FKN[1]

Normal penalty stiffness factor [2] [3]

Determining Contact Stiffness and Penetration

4FTOLN

Penetration tolerance factor

Determining Contact Stiffness and Penetration

5ICONT

Initial contact closure

Adjusting Initial Contact Conditions

6PINB

Pinball region

Determining Contact Status and the Pinball Region

or

Defining Influence Range (PINB)

7PMAX

Upper limit of initial allowable penetration

Adjusting Initial Contact Conditions

8PMIN

Lower limit of initial allowable penetration

Adjusting Initial Contact Conditions

9TAUMAX

Maximum friction stress [2] [3]

Choosing a Friction Model

10CNOF

Contact surface offset [2] [3]

Adjusting Initial Contact Conditions

11FKOP

Contact opening stiffness [2] [3]

Selecting Surface Interaction Models

12FKT[1]

Tangent penalty stiffness factor [2] [3]

Determining Contact Stiffness

13COHE

Contact cohesion

Choosing a Friction Model

21FACT

Static/dynamic ratio

Static and Dynamic Friction Coefficients

22DC

Exponential decay coefficient

Static and Dynamic Friction Coefficients

23SLTO

Allowable elastic slip

Using FKT and SLTO

24TNOP

Maximum allowable tensile contact force/pressure [4]

Chattering Control Parameters

25TOLS

Target edge extension factor

Real Constant TOLS

29COR

Coefficient of restitution

Impact Between Rigid Bodies

30STRM

Load step number for ramping penetration

Adjusting Initial Contact Conditions

31FDMNNormal stabilization damping factor [2] [3]

Applying Contact Stabilization Damping

32FDMTTangential stabilization damping factor [2] [3]

Applying Contact Stabilization Damping

35TBNDCritical bonding temperature [2] [3]

Using TBND


  1. For the contact force-based model (KEYOPT(3) = 0 or 1), the units of real constants FKN and FKT have a factor of AREA with respect to those used in the surface-to-surface contact elements. See Performing a 3-D Beam-to-Beam Contact Analysis for more information.

  2. This real constant can be defined as a function of certain primary variables.

  3. This real constant can be defined by the user subroutine USERCNPROP.F.

  4. For the contact force-based model (KEYOPT(3) = 0 or 1), TNOP is the allowable tensile contact force. For the contact traction-based model (KEYOPT(3) = 2 or 3), TNOP is the allowable tensile contact pressure.

CONTA176 Output Data

The solution output associated with the element is in two forms:

A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ETABLE, ESOL). The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.

In either the O or R columns, “Y” indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 176.2:  CONTA176 Element Output Definitions

NameDefinitionOR
ELElement NumberYY
NODESNodes I, J, KYY
XC, YC, ZCLocation where results are reported (same as nodal location)YY
TEMPTemperature T(I)YY
VOLULengthYY
NPINumber of integration pointsY-
ITRGETTarget surface number (assigned by ANSYS)Y-
ISOLIDUnderlying beam element numberY-
CONT:STATCurrent contact statuses11
OLDSTOld contact statuses11
ISEGCurrent contacting target element numberYY
OLDSEGUnderlying old target numberY-
CONT:PENECurrent penetration (gap = 0; penetration = positive value)YY
CONT:GAPCurrent gap (gap = negative value; penetration = 0)YY
NGAPNew or current gap at current converged substep (gap = negative value; penetration = positive value)Y-
OGAPOld gap at previously converged substep (gap = negative value; penetration = positive value)Y-
IGAPInitial gap at start of current substep (gap = negative value; penetration = positive value)YY
GGAPGeometric gap at current converged substep (gap = negative value; penetration = positive value)-Y
CONT:PRESNormal contact force/pressure22
TAUR/TAUS [7]Tangential contact forces/stresses22
KNCurrent normal contact stiffness (units: FORCE/LENGTH for contact force model, FORCE/LENGTH3 for contact traction model) 55
KTCurrent tangent contact stiffness (same units as KN)55
MU [8]Friction coefficientYY
TASS/TASR [7]Total (algebraic sum) sliding in S and R directions33
AASS/AASR [7]Total (absolute sum) sliding in S and R directions33
TOLNPenetration toleranceYY
CONT:SFRICFrictional force/stress, SQRT (TAUR**2+TAUS**2) 22
CONT:STOTALTotal force/stress, SQRT (PRES**2+TAUR**2+TAUS**2)22
CONT:SLIDEAmplitude of total accumulated sliding, SQRT (TASS**2+TASR**2) 33
FDDISFrictional energy dissipation66
ELSITotal equivalent elastic slip distance-Y
PLSITotal (accumulated) equivalent plastic slip due to frictional sliding-Y
GSLIDAmplitude of total accumulated sliding (including near-field)-9
VRELEquivalent sliding velocity (slip rate)-Y
DBAPenetration variationYY
PINBPinball Region-Y
CONT:CNOSTotal number of contact status changes during substepYY
TNOPMaximum allowable tensile contact force/pressure22
SLTOAllowable elastic slipYY
CAREAContacting area-Y
R1Target radius-Y
R2Contact radius-Y
DTSTARTLoad step time during debondingYY
DPARAMDebonding parameterYY
DENERI [11]Energy released due to separation in normal direction - mode I debondingYY
DENERII [11]Energy released due to separation in tangential direction - mode II debondingYY
DENER [12]Total energy released due to debondingYY
CNFX [10]Contact element force-X component-4
CNFY [10]Contact element force-Y component-Y
CNFZ [10]Contact element force-Z component-Y
SDAMPStabilization damping coefficient-Y

  1. The possible values of STAT and OLDST are:

    0 = Open and not near contact
    1 = Open but near contact
    2 = Closed and sliding
    3 = Closed and sticking
  2. For the force-based model (KEYOPT(3) = 0 or 1), the unit of this quantity is FORCE. For the traction-based model (KEYOPT(3) = 2 or 3), the unit is FORCE/AREA.

  3. Only accumulates the sliding for sliding and closed contact (STAT = 2,3).

  4. Contact element forces are defined in the global Cartesian system

  5. For the force-based model (KEYOPT(3) = 0 or 1), the unit of stiffness is FORCE/LENGTH. For the traction-based model (KEYOPT(3) = 2 or 3), the unit is FORCE/LENGTH3.

  6. FDDIS = (contact friction stress)*(sliding distance of substep)/(time increment of substep)

  7. For the case of orthotropic friction in contact between beams, components are defined in the global Cartesian system.

  8. For orthotropic friction, an equivalent coefficient of friction is output.

  9. Accumulated sliding distance for near-field, sliding, and closed contact (STAT = 1,2,3).

  10. The contact element force values (CNFX, CNFY, CNFZ) are calculated based on the individual contact element plus the surrounding contact elements. Therefore, the contact force values may not equal the contact element area times the contact pressure (CAREA * PRES).

  11. DENERI and DENERII are available only when one of the following material models is used: TB,CZM,,,,CBDD or TB,CZM,,,,CBDE.

  12. DENER is available only when one of the following material models is used: TB,CZM,,,,BILI or TB,CZM,,,,EXPO.


Note:  Contact results (including all element results) are generally not reported for elements that have a status of “open and not near contact” (far-field).


The following table lists output available through the ETABLE command using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information.

Name

output quantity as defined in Table 176.2: CONTA176 Element Output Definitions

Item

predetermined item label for ETABLE command

E

sequence number for single-valued or constant element data

NMISC

I, J, K

sequence number for data at nodes I, J, K

Table 176.3:  CONTA176 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEIJK
PRESSMISC13123
TAURSMISC-567
TAUSSMISC-91011
FDDISSMISC-181920
STAT[1]NMISC41123
OLDSTNMISC-567
PENE[2]NMISC-91011
DBANMISC-131415
TASRNMISC-171819
TASSNMISC-212223
KNNMISC-252627
KTNMISC-293031
TOLNNMISC-333435
IGAPNMISC-373839
PINBNMISC42---
CNFXNMISC43---
CNFYNMISC44---
CNFZNMISC45---
ISEGNMISC-464748
AASRNMISC-505152
AASSNMISC-545556
CAREANMISC58---
MUNMISC-626364
DTSTARTNMISC-666768
DPARAMNMISC-707172
CNOSNMISC-112113114
TNOPNMISC-116117118
SLTONMISC-120121122
ELSINMISC-136137138
DENERI or DENERNMISC-140141142
DENERIINMISC-144145146
GGAPNMISC-152153154
VRELNMISC-156157158
SDAMPNMISC-160161162
PLSINMISC-164165166
GSLIDNMISC-168169170
R1NMISC-172173174
R2NMISC-176177178

  1. Element Status = highest value of status of integration points within the element

  2. Penetration = positive value, gap = negative value

You can display or list contact results through several POST1 postprocessor commands. The contact specific items for the PLNSOL, PLESOL, PRNSOL, and PRESOL commands are listed below:

STATContact status
PENEContact penetration
PRESContact pressure for the traction-based model. Contact normal force for the force-based model.
SFRICContact friction stress for the traction-based model. Friction force for the force-based model.
STOTContact total stress (pressure plus friction) for the traction-based model. Total contact force for the force-based model.
SLIDEContact sliding distance
GAPContact gap distance
CNOSTotal number of contact status changes during substep

CONTA176 Assumptions and Restrictions

  • The main restriction is the assumption of constant circular beam cross section. The contact radius is assumed to be the same for all elements in the contact pair.

  • For KEYOPT(3) = 1 (crossing beams), contact between the beams is pointwise, and each contact element contacts no more than one target element.

  • This element is nonlinear and requires a full Newton iterative solution, regardless of whether large or small deflections are specified. An exception to this is when MPC bonded contact is specified (KEYOPT(2) = 2 and KEYOPT(12) = 5 or 6).

  • The normal contact stiffness factor (FKN) must not be so large as to cause numerical instability.

  • FTOLN, PINB, and FKOP can be changed between load steps or during restart stages.

  • You can use this element in nonlinear static or nonlinear full transient analyses.

  • In addition, you can use it in modal analyses, eigenvalue buckling analyses, and harmonic analyses. For these analysis types, the program assumes that the initial status of the element (i.e., the status at the completion of the static prestress analysis, if any) does not change.

CONTA176 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

ANSYS Mechanical Pro 

  • Birth and death is not available.

  • Debonding is not available.

  • User-defined contact is not available.

  • User-defined friction is not available.

  • Linear perturbation is not available.

ANSYS Mechanical Premium 

  • Birth and death is not available.

  • Debonding is not available.

  • User-defined contact is not available.

  • User-defined friction is not available.


Release 17.0 - © SAS IP, Inc. All rights reserved.