CONTA171


2-D 2-Node Surface-to-Surface Contact

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

CONTA171 Element Description

CONTA171 is used to represent contact and sliding between 2-D target surfaces and a deformable surface, defined by this element. The element is applicable to 2-D structural and coupled-field contact analyses. It can be used for both pair-based contact and general contact.

In the case of pair-based contact, the target surface is defined by the 2-D target element type, TARGE169. In the case of general contact, the target surface can be defined by CONTA171 elements (for deformable surfaces) or TARGE169 elements (for rigid bodies only).

This element is located on the surfaces of 2-D solid, shell, or beam elements without midside nodes (such as PLANE13, PLANE55, PLANE182, INTER192, SHELL208, CPT212, and MATRIX50).

The element has the same geometric characteristics as the solid, shell, or beam element face with which it is connected (see Figure 171.1: CONTA171 Geometry). Contact occurs when the element surface penetrates an associated 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 CONTA171 in the Mechanical APDL Theory Reference for more details about this element. Other surface-to-surface contact elements (CONTA172, CONTA173, CONTA174) are also available.

Figure 171.1:  CONTA171 Geometry

CONTA171 Geometry

CONTA171 Input Data

The geometry and node locations are shown in Figure 171.1: CONTA171 Geometry. The element is defined by two nodes (the underlying solid, shell, or beam element has no midside nodes). If the underlying solid, shell, or beam elements do have midside nodes, use CONTA172.

The element x-axis is along the I-J line of the element. The correct node ordering of the contact element is critical for proper detection of contact. The nodes must be ordered such that the target lies to the right side of the contact element when moving from the first contact element node to the second contact element node as in Figure 171.1: CONTA171 Geometry.

Pair-Based Contact versus General Contact

There are two methods to define a contact interaction: the pair-based contact definition and the general contact definition. Both contact definitions can exist in the same model. CONTA171 can be used in either type of contact definition.

The pair-based contact definition is usually more efficient and more robust than the general contact definition; it supports more options and specific contact features.

Pair-Based Contact

In a pair-based contact definition, the 2-D contact surface elements (CONTA171 and CONTA172) are associated with the 2-D target segment elements (TARGE169) via a shared real constant set. The program looks for contact only between surfaces with the same real constant set ID (which is greater than zero). The material ID associated with the contact element is used to specify interaction properties (such as friction coefficient) defined by MP or TB commands.

If more than one target surface will make contact with the same boundary of solid elements, you must define several contact elements that share the same geometry but relate to separate targets (targets which have different real constant numbers). Alternatively, you can combine several target surfaces into one (that is, multiple targets sharing the same real constant number). See Identifying Contact Pairs in the Contact Technology Guide for more information.

For rigid-flexible and 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.

See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.

General Contact

CONTA171 can be used in a general contact definition, although it is not directly generated by the GCGEN command. In a general contact definition, the general contact surfaces are generated automatically by the GCGEN command based on physical parts and geometric shapes in the model. The program overlays contact surface elements (CONTA172) on 2-D deformable bodies (on both lower- and higher-order elements). The general contact definition may also contain target elements (TARGE169) overlaid on the surfaces of standalone rigid bodies and lower-order contact surface elements (CONTA171) overlaid on 2-D deformable bodies.

The GCGEN command automatically assigns section IDs and element type IDs for each general contact surface. As a result, each general contact surface consists of contact or target elements that are easily identified by a unique section ID number. The real constant ID and material ID are always set to zero for contact and target elements in the general contact definition.

The program looks for contact interaction among all surfaces and within each surface. You can further control contact interactions between specific surfaces that could potentially be in contact by using the GCDEF command. The material ID and real constant ID input on GCDEF identify interface properties (defined by MP or TB commands) and contact control parameters (defined by the R command) for a specific contact interaction. Unlike a pair-based contact definition, the contact and target elements in the general contact definition are not associated with these material and real constant ID numbers.

If both pair-based contact and general contact are defined in a model, the pair-based contact definitions are preserved, and the general contact definition automatically excludes overlapping interactions wherever pair-based contact exists.

Some element key options are not used or are set automatically for general contact. See the individual KEYOPT descriptions in "CONTA171 Input Summary" for details.

Friction

To model isotropic friction, use the TB,FRIC,,,,ISO command. You can define a coefficient of friction that is dependent on temperature, time, normal pressure, sliding distance, or sliding relative velocity by using the TBFIELD command along with TB,FRIC,,,,ISO. 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.

Other Input

The contact interaction subroutine USERINTER is available for user-defined interface interactions, including interactions in the normal and tangential directions as well as coupled-field interactions. 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 fluid penetration loads, use the SFE command to specify the fluid pressure and fluid penetration starting points. For more information, see Applying Fluid Pressure-Penetration Loads in the Contact Technology Guide.

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.

To model wear at the contact surface, use the TB command with the WEAR label. See Contact Surface Wear in the Contact Technology Guide for more information.

This element supports various 2-D stress states, including plane stress, plane strain, and axisymmetric states. The stress state is automatically detected according to the stress state of the underlying element. However, if the underlying element is a superelement, you must use KEYOPT(3) to specify the stress state.

Two types of geometry correction are available for this element: surface smoothing and bolt thread modeling. Surface smoothing is a geometry correction technique that eliminates inaccuracies introduced by linear elements on a curved (circular or nearly circular) contact surface. Bolt thread modeling provides a method for simulating contact between a threaded bolt and bolt hole without having to model the detailed thread geometry. Both of these geometry correction techniques are implemented through section definitions (SECTYPE, SECDATA, and SECNUM commands). For more information, see Geometry Correction for Contact and Target Surfaces in the Contact Technology Guide.

A summary of the element input is given in "CONTA171 Input Summary". A general description of element input is given in Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.

CONTA171 Input Summary

Nodes

I, J

Degrees of Freedom

Set by KEYOPT(1)

Real Constants
R1, R2, FKN, FTOLN, ICONT, PINB,
PMAX, PMIN, TAUMAX, CNOF, FKOP, FKT,
COHE, TCC, FHTG, SBCT, RDVF, FWGT,
ECC, FHEG, FACT, DC, SLTO, TNOP,
TOLS, , PPCN, FPAT, COR, STRM,
FDMN, FDMT, , , TBND, WBID,
PCC, PSEE, ABPP, FPFT, FPWT
See Table 171.1: CONTA171 Real Constants for descriptions of the real constants.
Material Properties
TB command: See Element Support for Material Models for this element.
MP command: MU, EMIS
Surface Loads
Pressure, Face 1 (I-J) (opposite to contact normal direction); used for fluid pressure penetration loading. On the SFE command use LKEY = 1 to specify the pressure values, and use LKEY = 2 to specify starting points and penetrating points.
Convection, Face 1 (I-J)
Heat Flux, Face 1 (I-J)
Special Features
Birth and death
Debonding
Fluid pressure penetration
Isotropic friction
Large deflection
Linear perturbation
Nonlinearity
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:

0 -- 

UX, UY

1 -- 

UX, UY, TEMP

2 -- 

TEMP

3 -- 

UX, UY, TEMP, VOLT

4 -- 

TEMP, VOLT

5 -- 

UX, UY, VOLT

6 -- 

VOLT

7 -- 

AZ

8 -- 

UX, UY, PRES

9 -- 

UX, UY, PRES, TEMP

10 --

PRES


Note:  For general contact, the GCGEN command automatically sets KEYOPT(1) based on the degrees of freedom of the underlying solid or shell elements.


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


Note:  For general contact, the GCGEN command automatically sets KEYOPT(2) = 1 (penalty function).


KEYOPT(3)

Units of normal contact stiffness:

0 -- 

FORCE/LENGTH3 (default)

1 -- 

FORCE/LENGTH


Note:  KEYOPT(3) = 1 is valid only when a penalty-based algorithm is used (KEYOPT(2) = 0 or 1) and the absolute normal contact stiffness value is explicitly specified (that is, a negative value input for real constant FKN).



Note:  KEYOPT(3) is not supported for contact elements used in a general contact definition.


If superelements are present in a 2-D model, KEYOPT(3) does not control units of normal contact stiffness. Instead, KEYOPT(3) specifies the stress state as follows: KEYOPT(3) = 1 for axisymmetric; KEYOPT(3) = 2 for plane stress/plane strain with unit thickness; KEYOPT(3) = 3 for plane stress with thickness input. (KEYOPT(3) = 0 indicates no superelements.)

KEYOPT(4)

Location of contact detection point:

0 -- 

On Gauss point (for general cases)

1 -- 

On nodal point - normal from contact surface

2 -- 

On nodal point - normal to target surface

3 -- 

On nodal point - normal from contact surface (projection-based method)


Note:  When using the multipoint constraint (MPC) approach to define surface-based constraints, use KEYOPT(4) in the following way: set KEYOPT(4) = 1 for a force-distributed constraint; set KEYOPT(4) = 2 for a rigid surface constraint; set KEYOPT(4) = 3 for a coupling constraint. See Surface-based Constraints for more information.



Note:  Certain restrictions apply when the surface projection-based method (KEYOPT(4) = 3) is defined. See Using the Surface Projection Based Contact Method (KEYOPT(4) = 3) for more information.


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 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


Note:  KEYOPT(7) = 4 is not supported for contact elements used in a general contact definition.


KEYOPT(8)

Asymmetric contact selection:

0 -- 

No action

2 -- 

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


Note:  KEYOPT(8) is ignored for contact elements used in a general contact definition. Instead, use the command GCDEF,AUTO to enable auto-asymmetric pairing logic.


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.



Note:  KEYOPT(9) is not supported for contact elements used in a general contact definition. Instead, use the command TBDATA,,C1 in conjunction with TB,INTER to specify the effect of initial penetration or gap. If TBDATA,,C1 is not specified, the default for general contact is to exclude initial penetration/gap and offset. For more information, see Interaction Options for General Contact Definitions in the Material Reference.


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).


Note:  For general contact, the GCGEN command automatically sets KEYOPT(10) = 2.


KEYOPT(11)

Beam/Shell thickness effect:

0 -- 

Exclude

1 -- 

Include


Note:  For general contact, the GCGEN command automatically sets KEYOPT(11) = 1.


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.



Note:  KEYOPT(12) is not supported for contact elements used in a general contact definition. Instead, use the command TB,INTER with the appropriate TBOPT label to specify the behavior at the contact surface. For more information, see Interaction Options for General Contact Definitions in the Material Reference.


KEYOPT(14)

Behavior of fluid pressure penetration load. KEYOPT(14) is valid only if a fluid pressure penetration load (SFE,,,PRES) is applied to the contact element:

0 -- 

Fluid pressure penetration load varies during iterations (default)

1 -- 

Fluid pressure penetration load remains constant over the substep


Note:  KEYOPT(14) is not supported for contact elements used in a general contact definition.


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 171.1:  CONTA171 Real Constants

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

Target circle radius

Defining the Target Surface

2R2

Superelement thickness

Defining the Target Surface

3FKN

Normal penalty stiffness factor [1] [2]

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 [1] [2]

Choosing a Friction Model

10CNOF

Contact surface offset [1] [2]

Adjusting Initial Contact Conditions

11FKOP

Contact opening stiffness [1] [2]

Selecting Surface Interaction Models

12FKT

Tangent penalty stiffness factor [1] [2]

Determining Contact Stiffness

13COHE

Contact cohesion

Choosing a Friction Model

14TCC

Thermal contact conductance [1] [2]

Modeling Conduction

15FHTG

Frictional heating factor

Modeling Heat Generation Due to Friction

16SBCT

Stefan-Boltzmann constant

Modeling Radiation

17RDVF

Radiation view factor [1] [2]

Modeling Radiation

18FWGT

Heat distribution weighing factor

Modeling Heat Generation Due to Friction (thermal)

or

Heat Generation Due to Electric Current (electric)

19ECC

Electric contact conductance [1] [2]

Modeling Surface Interaction

20FHEG

Joule dissipation weight factor

Heat Generation Due to Electric Current

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 pressure

Chattering Control Parameters

25TOLS

Target edge extension factor

Selecting Location of Contact Detection

27PPCN

Pressure penetration criterion [1]

[2]

Specifying a Pressure Penetration Criterion

28FPAT

Fluid penetration acting time

Specifying a Fluid Penetration Acting Time

29COR

Coefficient of restitution

Impact Between Rigid Bodies

30STRM

Load step number for ramping penetration

Adjusting Initial Contact Conditions

31FDMNNormal stabilization damping factor [1] [2]

Applying Contact Stabilization Damping

32FDMTTangential stabilization damping factor [1] [2]

Applying Contact Stabilization Damping

35TBNDCritical bonding temperature [1] [2]

Using TBND

36WBIDInternal contact pair ID (used by ANSYS Workbench)  
37PCCPore fluid contact permeability coefficient [1] [2]

Modeling Pore Fluid Flow at the Contact Interface

38PSEEPore fluid seepage coefficient [1] [2]

Modeling Pore Fluid Flow at the Contact Interface

39ABPPAmbient pore pressure [1] [2]

Modeling Pore Fluid Flow at the Contact Interface

40FPFTGap pore fluid flow participation factor [1] [2]

Modeling Pore Fluid Flow at the Contact Interface

41FPWTGap pore fluid flow distribution weighting factor

Modeling Pore Fluid Flow at the Contact Interface


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

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

CONTA171 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 171.2: CONTA171 Element Output Definitions gives element output. In the results file, the nodal results are obtained from its closest integration point.

Table 171.2:  CONTA171 Element Output Definitions

NameDefinitionOR
ELElement NumberYY
NODESNodes I, JYY
XC, YCLocation where results are reportedY5
TEMPTemperatures T(I), T(J)YY
LENGTHElement lengthY-
VOLUAREAYY
NPINumber of integration pointsY-
ITRGETTarget surface number (assigned by the program)Y-
ISOLIDUnderlying solid, shell, or beam element numberY-
CONT:STATCurrent contact statuses11
OLDSTOld contact statuses11
NX, NYSurface normal vector componentsY-
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 pressureYY
CONT:SFRICTangential contact stressYY
KNCurrent normal contact stiffness (Force/Length3)YY
KTCurrent tangent contact stiffness (Force/Length3)YY
MUFriction coefficientYY
CONT:SLIDETotal accumulated sliding (algebraic sum)33
ASLIDETotal accumulated sliding (absolute sum)33
TOLNPenetration toleranceYY
CONT:STOTALTotal stress, SQRT (PRES**2+SFRIC**2)YY
FDDISFrictional energy dissipation66
ELSITotal elastic slip distance-Y
PLSITotal accumulated plastic slip due to frictional sliding-Y
GSLIDAlgebraic sum sliding-7
VRELSliding velocity (slip rate)-Y
DBAPenetration variationYY
PINBPinball Region-Y
CONT:CNOSTotal number of contact status changes during substepYY
TNOPMaximum allowable tensile contact pressureYY
SLTOAllowable elastic slipYY
CAREAContacting area-Y
CONT:FPRSActual applied fluid penetration pressure-Y
FSTARTFluid penetration starting time-Y
DTSTARTLoad step time during debondingYY
DPARAMDebonding parameterYY
DENERI [9]Energy released due to separation in normal direction - mode I debondingYY
DENERII [9]Energy released due to separation in tangential direction - mode II debondingYY
DENER [10]Total energy released due to debondingYY
CNFX [8]Contact element force-X component-4
CNFY [8]Contact element force-Y component-Y
SDAMPStabilization damping coefficient-Y
CONVConvection coefficientYY
RACRadiation coefficientYY
TCCConductance coefficientYY
TEMPSTemperature at contact pointYY
TEMPTTemperature at target surfaceYY
FXCVHeat flux due to convectionYY
FXRDHeat flux due to radiationYY
FXCDHeat flux due to conductanceYY
CONT:FLUXTotal heat flux at contact surfaceYY
FXNPFlux input-Y
CNFHContact element heat flow-Y
JCONTContact current density (Current/Unit Area)YY
CCONTContact charge density (Charge/Unit Area)YY
HJOUContact power/areaYY
ECURTCurrent per contact element-Y
ECHARCharge per contact element-Y
ECCElectric contact conductance (for electric current DOF), or electric contact capacitance per unit area (for piezoelectric or electrostatic DOFs)YY
VOLTSVoltage on contact nodesYY
VOLTTVoltage on associated targetYY
PCCPore fluid contact permeability coefficientYY
PSEEPore fluid seepage coefficient YY
PRESSPore pressure on contact nodesYY
PRESTPore pressure on associated targetYY
PFLUXPore volume flux density per unit area flow into contact surfaceYY
EPELXPore volume flux per contact element-Y
WEARX, WEARYWear correction - X and Y components-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. The program will evaluate model to detect initial conditions.

  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. Available only at centroid as a *GET item.

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

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

  8. The contact element force values (CNFX, CNFY) 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).

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

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


Note:  If ETABLE is used for the CONT items, the reported data is averaged across the element.



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).


Table 171.3: CONTA171 Item and Sequence Numbers 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. The following notation is used in Table 171.3: CONTA171 Item and Sequence Numbers:

Name

output quantity as defined in the Table 171.2: CONTA171 Element Output Definitions

Item

predetermined Item label for ETABLE command

E

sequence number for single-valued or constant element data

I,J

sequence number for data at nodes I, J

Table 171.3:  CONTA171 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEIJ
PRESSMISC512
SFRICSMISC-34
FLUX [3]SMISC-67
FDDIS [3]SMISC-89
FXCV [3]SMISC-1011
FXRD [3]SMISC-1213
FXCD [3]SMISC-1415
FXNPSMISC-1617
JCONT/CCONT/PFLUX [3]SMISC-1819
HJOUSMISC-2021
STAT [1]NMISC1912
OLDSTNMISC-34
PENE [2]NMISC-56
DBANMISC-78
SLIDENMISC-910
KNNMISC-1112
KTNMISC-1314
TOLNNMISC-1516
IGAPNMISC-1718
PINBNMISC20--
CNFXNMISC21--
CNFYNMISC22--
ISEGNMISC-2324
ASLIDENMISC-2526
CAREANMISC27--
MUNMISC-2930
DTSTARTNMISC-3132
DPARAMNMISC-3334
FPRSNMISC-3536
TEMPSNMISC-3738
TEMPTNMISC-3940
CONVNMISC-4142
RACNMISC-4344
TCCNMISC-4546
CNFHNMISC47--
ECURT/ECHAR/EPELXNMISC48--
ECC/PCC/PSEENMISC-4950
VOLTS/PRESSNMISC-5152
VOLTT/PRESTNMISC-5354
CNOSNMISC-5556
TNOPNMISC-5758
SLTONMISC-5960
ELSINMISC-6768
DENERI or DENERNMISC-6970
DENERIINMISC-7172
FSTARTNMISC-7374
GGAPNMISC-7576
VRELNMISC-7778
SDAMPNMISC-7980
PLSINMISC-8182
GSLIDNMISC-8384
WEARXNMISC-8586
WEARYNMISC-8788

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

  2. Penetration = positive value, gap = negative value

  3. A positive value of flux corresponds to flow into the contact surface.

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
SFRICContact friction stress
STOTContact total stress (pressure plus friction)
SLIDEContact sliding distance
GAPContact gap distance
FLUXTotal heat flux at contact surface
CNOSTotal number of contact status changes during substep
FPRSActual applied fluid penetration pressure

CONTA171 Assumptions and Restrictions

  • The 2-D contact element must be defined in an X-Y plane and the Y-axis must be the axis of symmetry for axisymmetric analyses.

  • An axisymmetric structure should be modeled in the +X quadrants.

  • This 2-D contact element works with any 3-D elements in your model.

  • Do not use this element in any model that contains axisymmetric harmonic elements.

  • Node numbering must coincide with the external surface of the underlying solid, shell, or beam element, or with the original elements comprising the superelement.

  • 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 (that is, the status at the completion of the static prestress analysis, if any) does not change.

  • When nodal detection is used and the contact node is on the axis of symmetry in an axisymmetric analysis, the contact pressure on that node is not accurate since the area of the node is zero. The contact force is accurate in this situation.

  • Certain contact features are not supported when this element is used in a general contact definition. For details, see General Contact in the Contact Technology Guide.

CONTA171 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 

  • The AZ DOF (KEYOPT(1) = 7) is not available.

  • 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 

  • The AZ DOF (KEYOPT(1) = 7) is not available.

  • 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.