CONTA175


2D/3D Node-to-Surface Contact

Valid Products: Pro | Premium | Enterprise | PrepPost | Solver | AS add-on

CONTA175 Element Description

CONTA175 may be used to represent contact and sliding between two surfaces (or between a node and a surface, or between a line and a surface) in 2D or 3D. It can be used for both pair-based contact and general contact.

The element is applicable to 2D or 3D structural and coupled field contact analyses. This element is located on the surfaces of solid, beam, and shell elements. 3D solid and shell elements with midside nodes are supported for bonded and no separation contact. For other contact types, lower order solid and shell elements are recommended.

Contact occurs when the element surface penetrates one of the target elements on a specified target surface. In the case of pair-based contact, the target surface is defined by a 2D or 3D target element type, TARGE169 or TARGE170. In the case of general contact, the target surface can be defined by contact elements CONTA172 or CONTA174 for deformable surfaces, or by target elements TARGE169 or TARGE170 for rigid bodies.

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 CONTA175 in the Mechanical APDL Theory Reference for more details about this element.

Figure 175.1: CONTA175 Geometry

CONTA175 Geometry

CONTA175 Input Data

The geometry is shown in Figure 175.1: CONTA175 Geometry. The element is defined by one node. The underlying elements can be 2D or 3D solid, shell, or beam elements. CONTA175 represents 2D or 3D contact depending on whether the associated 2D or 3D target segments are used. Contact can occur only when the outward normal direction of the 2D or 3D target surface points to the contact surface. See Generating Contact Elements in the Contact Technology Guide for more information on controlling the outward normal directions via the ESURF command.

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. CONTA175 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 node-to-surface contact elements (CONTA175) are associated with target segment elements (TARGE169 or TARGE170) via a shared real constant set. The program looks for contact interaction 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 numbers). 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 information on generating elements automatically using the ESURF command.

General Contact

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 for 2D or CONTA174 for 3D) on deformable bodies (on both lower- and higher-order elements); 3D contact line elements (CONTA177) on 3D beams, on feature edges of 3D deformable bodies, and on perimeter edges of shell structures; and vertex-to-surface elements (CONTA175) on convex corners of 2D or 3D solid bodies and/or shell structures. The general contact definition may also contain target elements (TARGE169 or TARGE170) overlaid on the surfaces of standalone rigid 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.

Some element key options are not used or are set automatically for general contact. See the individual KEYOPT descriptions in "CONTAC175 Input Summary" for details.

Friction

CONTA175 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, the default element coordinate system (based on node connectivity of the underlying elements) is used. For orthotropic friction, the global coordinate system is used by default, or you may define a local element coordinate system with the ESYS command. The principal directions are computed on the target surface and then projected onto the contact element (node). The first principal direction is defined by projecting the first direction of the chosen coordinate system onto the target surface. The second principal direction is defined by taking a cross product of the first principal direction and the target 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 only the z-direction parallels (or is nearly parallel to) the surface normal.

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 Contact Technology Guide for more information on how to use this feature. See also the Guide to User-Programmable Features in the Programmer's Reference 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 coupled-field interactions. See Defining Your Own Contact Interaction (USERINTER) in the Contact Technology Guide for more information on how to use this feature. See also the Guide to User-Programmable Features in the Programmer's Reference 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.

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.

KEYOPT(3) allows you to choose between a contact force-based model (KEYOPT(3) = 0, default) and a contact traction-based model (KEYOPT(3) = 1). The units for certain real constants (FKN, FKT, TNOP, and so on) 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 CONTA175, see KEYOPT(3) in the Contact Technology Guide.

This element supports a bolt thread modeling technique that simulates contact between a threaded bolt and bolt hole without having to model the detailed thread geometry. Bolt thread modeling is available for 3D models and 2D axisymmetric models and is implemented through section definitions (SECTYPE, SECDATA, and SECNUM commands). For more information, see Simplified Bolt Thread Modeling in the Contact Technology Guide.

See the Contact Technology Guide for a detailed discussion about contact and using the contact elements. Node-to-Surface Contact discusses CONTA175 specifically, including the use of real constants and KEYOPTs.

A summary of the element input is given in "CONTAC175 Input Summary". A general description of element input is given in Element Input.

CONTAC175 Input Summary

Nodes

I

Degrees of Freedom

Set by KEYOPT(1)

Real Constants
R1, R2, FKN, FTOLN, ICONT, PINB,
PZER, CZER, TAUMAX, CNOF, FKOP, FKT,
COHE, TCC, FHTG, SBCT, RDVF, FWGT,
ECC, FHEG, FACT, DC, SLTO, TNOP,
TOLS, MCC, (Blank), (Blank), COR, STRM,
FDMN, FDMT, FDMD, FDMS, TBND, WBID,
PCC, PSEE, ABPP, FPFT, FPWT, DCC,
DCON, ABDC, , , TFOR, TEND
See Table 175.1: CONTA175 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, DMPR, DMPS
Special Features
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, UZ

1 -- 

UX, UY, UZ, TEMP

2 -- 

TEMP

3 -- 

UX, UY, UZ, TEMP, VOLT

4 -- 

TEMP, VOLT

5 -- 

UX, UY, UZ, VOLT

6 -- 

VOLT

7 -- 

AZ (2D) or MAG (3D)

8 -- 

UX, UY, UZ, PRES

9 -- 

UX, UY, UZ, PRES, TEMP

10 --

PRES

11 --

UX, UY, CONC, TEMP

12 --

UX, UY, CONC, TEMP, VOLT

13 --

UX, UY, CONC

14 --

CONC


Note:  Only KEYOPT(1) = 0 is supported for CONTA175 elements used in a general contact definition.


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)

Contact model:

0 -- 

Contact force-based model (default)

1 -- 

Contact traction-based model


Note:  The traction-based model (KEYOPT(3) = 1) should not be used if the underlying elements are 3D beam or pipe elements.



Note:  For general contact, the GCGEN command automatically sets KEYOPT(3) = 1 (traction-based model).


KEYOPT(4)

Standard KEYOPT(4) Usage

Contact normal direction:

0 -- 

Normal to target surface (default)

1 -- 

Normal from contact nodes

2 -- 

Normal from contact nodes (used for shell/beam bottom surface contact when shell/beam thickness is accounted for; KEYOPT(11) = 1)

3 -- 

Normal to target surface (used for shell/beam bottom surface contact when shell/beam thickness is accounted for; KEYOPT(11) = 1)

Alternate KEYOPT(4) Usage with Surface-Based Constraints

To define a surface-based constraint, set KEYOPT(4) as follows:

0 -- 

Rigid surface constraint. The rigid surface constraint can be based on either the MPC approach (KEYOPT(2) = 2) or the Lagrange multiplier method (KEYOPT(2) = 3).

1 -- 

Force-distributed constraint. The force-distributed constraint can be based on either the MPC approach (KEYOPT(2) = 2) or the Lagrange multiplier method (KEYOPT(2) = 3).

3 -- 

Coupling constraint

For more information, see Surface-Based Constraints in the Contact Technology Guide.

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)

Normal contact stiffness variation (used to enhance stiffness updating when KEYOPT(10) ≠ 1):

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

3 -- 

Use an exponential pressure-penetration relationship

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


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


KEYOPT(8)

Symmetric contact behavior:

0 -- 

Both symmetric pairs are active. However, each pair has its own contact characteristics.

1 -- 

Both symmetric pairs are active and have the same contact characteristics.

2 -- 

The program internally selects which asymmetric contact pair is used at the solution stage (used only when symmetric contact is defined). However, the contact stiffness of the active contact pair is influenced by the underlying element stiffness of the inactive pair.

3 -- 

The program internally selects which asymmetric contact pair is used at the solution stage (used only when symmetric contact is defined). The contact characteristics of the active contact pair are completely independent of the inactive pair.


Note:  KEYOPT(8) settings are ignored for asymmetric contact pairs and rigid-to-rigid contact pairs.



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 iteration based on the current mean stress of underlying elements. The actual elastic slip never exceeds the maximum allowable limit (SLTO) during the entire solution.

1 -- 

Each load step if FKN is redefined during the load step.

2 -- 

Each iteration based on the current mean stress of underlying elements. The actual elastic slip does not exceed the maximum allowable limit (SLTO) within a substep.


Note:  For general contact, the GCGEN command automatically sets KEYOPT(10) = 0.


KEYOPT(11)

Shell Thickness Effect:

0 -- 

Exclude

1 -- 

Include


Note:  KEYOPT(11) is applicable to shell elements whose thickness is defined through real constant input or section properties. However, KEYOPT(11) = 1 is not valid when the underlying elements are part of a pre-integrated shell section (SECTYPE,,GENS).

KEYOPT(11) is applicable to beam elements whose thickness is defined through real constant input. However, KEYOPT(11) = 1 is not valid if the thickness of 2D/3D beams is defined through section properties.


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 affect 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(13)

Tangential contact stiffness variation only for frictional contact.

0 -- 

Use the default range for stiffness updating.

1 -- 

Make an aggressive refinement to the allowable stiffness range.

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.


KEYOPT(16)

Squeal damping controls for interpretation of real constants FDMD and FDMS:

0 -- 

FDMD and FDMS are scaling factors for destabilizing and stabilizing damping (default).

1 -- 

FDMD is a constant friction-sliding velocity gradient. FDMS is the stabilization damping coefficient.

2 -- 

FDMD and FDMS are the destabilizing and stabilization damping coefficients.


Note:  KEYOPT(16) is not supported for contact elements used in a general contact definition.


KEYOPT(18)

Sliding behavior:

0 -- 

Finite sliding (default). The contacting interface can undergo separation, relative large sliding, and arbitrary rotation.

1 -- 

Small sliding. The contacting interface can undergo only small sliding during the entire solution; arbitrary rotation is permitted.

2 -- 

Adaptive small sliding. The contact interface can undergo either small sliding or finite sliding within each substep based on the contact status at the beginning of the substep. If the contact status is closed, small sliding is used.

Table 175.1: CONTA175 Real Constants

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

Target radius for cylinder, cone, or sphere

Defining the Target Surface

2R2

Target radius at second node of cone

Defining the Target Surface

3FKN[5]

Normal penalty stiffness factor [1] [2] [3] [7]

Determining Contact Stiffness and Penetration

4FTOLN

Penetration tolerance factor [7]

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)

7PZERPressure at zero penetration [1] [2]Pressure-Penetration Relationship (KEYOPT(6) = 3)
8CZERInitial contact clearancePressure-Penetration Relationship (KEYOPT(6) = 3)
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[5]

Tangent penalty stiffness factor [1] [2] [7]

Determining Contact Stiffness

13COHE

Contact cohesion

Choosing a Friction Model

14TCC[5]

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[5]

Electric contact conductance or electric contact capacitance [1] [2] [6]

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 force/pressure [4] [7]

Chattering Control Parameters

25TOLS

Target edge extension factor

Selecting Location of Contact Detection

26MCC[5]

Magnetic contact permeance [1] [2]

Modeling Magnetic Contact

29COR

Coefficient of restitution

Impact Between Rigid Bodies

30STRM

Load step number for ramping penetration

or

Starting time for contact stiffness ramping

Modeling Interference Fit

31FDMNNormal stabilization damping factor [1] [2]

Applying Contact Stabilization Damping

32FDMTTangential stabilization damping factor [1] [2]

Applying Contact Stabilization Damping

33FDMDDestabilization squeal damping factor

Forced Frictional Sliding Using Velocity Input

34FDMSStabilization squeal damping factor

Forced Frictional Sliding Using Velocity Input

35TBNDCritical bonding temperature [1] [2]

Using TBND

36WBIDInternal contact pair ID (used by Ansys Workbench)  
37PCC[5]Pore fluid contact permeability coefficient [1] [2]

Modeling Pore Fluid Flow at the Contact Interface

38PSEE[5]Pore 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

42DCC[5]Contact diffusivity coefficient [1] [2]

Modeling Diffusion Flow at the Contact Interface

43DCON[5]Diffusive convection coefficient [1] [2]

Modeling Diffusion Flow at the Contact Interface

44ABDCAmbient concentration [1] [2]

Modeling Diffusion Flow at the Contact Interface

47TFORPair-based force tolerance

Checking Contact Pair-Based Force Convergence

48TENDEnding time for ramping contact stiffnessModeling Interference Fit

  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.

  3. When CONTA175 is used as part of a forced-distributed constraint and KEYOPT(7) = 2 on the target element (TARGE169 or TARGE170), FKN is used to define weighting factors in tabular format with node number as the primary variable.

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

  5. For the contact force-based model (KEYOPT(3) = 0), the units of this real constant has a factor of AREA with respect to those used in the surface-to-surface contact elements. See Performing a Node-to-Surface Contact Analysis for more information.

  6. ECC is electric contact conductance in a current-based electric analysis, or electric contact capacitance in a charge-based electric analysis (see Modeling Surface Interaction).

  7. When the relaxation option is enabled (KEYOPT(11) = 1 on the TARGE169 or TARGE170 element), FKN and FKT are translational relaxation coefficient and rotational relaxation coefficient, respectively, and tabular input is not supported. In addition, FTOLN and TNOP are translational tolerance and rotational tolerance, respectively.

CONTA175 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 175.2: CONTA175 Element Output Definitions

NameDefinitionOR
ELElement NumberYY
NODESNodes IYY
XC, YC, (ZC)Location where results are reported (same as nodal location)YY
TEMPTemperature T(I)YY
VOLUAREA for 3D, Length for 2DYY
NPINumber of integration pointsY-
ITRGETTarget surface number (assigned by Mechanical APDL)Y-
ISOLID [15]Underlying solid or shell 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 [8]Tangential contact forces/stresses22
KNCurrent normal contact stiffness (units: Force/Length for contact force-based model, Force/Length3 for contract traction-based model)55
KTCurrent tangent contact stiffness (same units as KN)55
MU [9]Friction coefficientYY
TASS/TASR [8]Total (algebraic sum) sliding in S and R directions (3D only)33
AASS/AASR [8]Total (absolute sum) sliding in S and R directions (3D only)33
TOLNPenetration toleranceYY
CONT:SFRICFrictional force/stress, SQRT (TAUR**2+TAUS**2) (3D only)22
CONT:STOTALTotal force/stress, SQRT (PRES**2+TAUR**2+TAUS**2) (3D only)22
CONT:SLIDEAmplitude of total accumulated sliding, SQRT (TASS**2+TASR**2) (3D only)33
NX, NYSurface normal vector components (2D only)Y-
CONT:SFRICTangential contact force/stress (2D only)22
CONT:SLIDETotal accumulated sliding (algebraic sum) (2D only)33
ASLIDETotal accumulated sliding (absolute sum) (2D only)33
FDDISFrictional energy dissipation rate77
ELSITotal equivalent elastic slip distance-Y
PLSITotal (accumulated) equivalent plastic slip due to frictional sliding-Y
GSLIDAmplitude of total accumulated sliding (including near-field)-10
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
DTSTARTLoad step time during debondingYY
DPARAMDebonding parameterYY
DENERI [13]Energy released due to separation in normal direction - mode I debondingYY
DENERII [13]Energy released due to separation in tangential direction - mode II debondingYY
DENER [14]Total energy released due to debondingYY
CNFX [11]Contact element force-X component-4
CNFY [11]Contact element force-Y component-4
CNFZ [11]Contact element force-Z component (3D only)-4
CNTX [12]Contact element force due to tangential stresses - X component-4
CNTY [12]Contact element force due to tangential stresses - Y component-4
CNTZ [12]Contact element force due to tangential stresses - Z component-4
SDAMPSqueal damping coefficient (3D only) / Stabilization damping coefficient (2D and 3D)-Y
WEARX, WEARY, WEARZWear correction - X, Y, and Z components-Y
VWEARVolume lost due to wear-Y
CONVConvection coefficientYY
RACRadiation coefficientYY
TCCConductance coefficient66
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)66
VOLTSVoltage on contact nodesYY
VOLTTVoltage on associated targetYY
MCCMagnetic contact permeance66
MFLUXMagnetic flux densityYY
AZS/MAGS2D/3D Magnetic potential on contact nodeYY
AZT/MAGT2D/3D Magnetic potential on associated targetYY
PCCPore fluid contact permeability coefficient66
PSEEPore fluid seepage coefficient 66
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
DCCContact diffusivity coefficient66
DCONDiffusive convection coefficient66
CONCSConcentration on contact nodesYY
CONCTConcentration on associated targetYY
DFLUXDiffusion flux density per unit area flow into contact surfaceYY
EDELXDiffusion flux per contact element-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), the unit of this quantity is FORCE. For the traction-based model (KEYOPT(3) = 1), 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, the unit of stiffness is FORCE/LENGTH. For the traction-based model, the unit is FORCE/LENGTH3.

  6. For the traction-based model, the units of TCC, ECC, MCC, PCC, PSEE, DCC, and DCON are the units used for the force-based model per area.

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

  8. For the case of orthotropic friction, components are defined in the global Cartesian system (default) or in the local element coordinate system specified by ESYS.

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

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

  11. 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).

  12. CNTX, CNTY, and CNTZ report the total contact element forces due to tangential stresses. Since CNFX, CNFY, and CNFZ report the total contact element forces, the contact element forces due to normal pressure are (CNFX-CNTX), (CNFY-CNTY), and (CNFZ-CNTZ).

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

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

  15. The underlying element (ISOLID) can be obtained by a *GET command following a CNCHECK command. See Designating Contact and Target Surfaces for detail.


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 175.3: CONTA175 (3D) Item and Sequence Numbers and Table 175.4: CONTA175 (2D) Item and Sequence Numbers list outputs 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 the tables below:

Name

output quantity as defined in Table 175.2: CONTA175 Element Output Definitions

Item

predetermined Item label for ETABLE command

E

sequence number for single-valued or constant element data

I

sequence number for data at nodes I

Table 175.3: CONTA175 (3D) Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEI
PRESSMISC131
TAURSMISC-5
TAUSSMISC-9
FLUX [3]SMISC-14
FDDIS [3]SMISC-18
FXCV [3]SMISC 22
FXRD [3]SMISC-26
FXCD [3]SMISC-30
FXNPSMISC-34
JCONT/CCONT/PFLUX [3]SMISC-38
HJOUSMISC-42
MFLUX/DFLUX [3]SMISC-46
STAT[1]NMISC411
OLDSTNMISC-5
PENE[2]NMISC-9
DBANMISC-13
TASRNMISC-17
TASSNMISC-21
KNNMISC-25
KTNMISC-29
TOLNNMISC-33
IGAPNMISC-37
PINBNMISC42-
CNFXNMISC43-
CNFYNMISC44-
CNFZNMISC45-
CNTXNMISC186-
CNTYNMISC187-
CNTZNMISC188-
ISEG [4]NMISC-46
AASRNMISC-50
AASSNMISC-54
CAREANMISC58-
MUNMISC-62
DTSTARTNMISC-66
DPARAMNMISC-70
TEMPSNMISC-78
TEMPTNMISC-82
CONVNMISC-86
RACNMISC-90
TCCNMISC-94
CNFHNMISC98-
ECURT/ECHAR/EPELXNMISC99-
ECC/PCC/PSEENMISC-100
VOLTS/PRESSNMISC-104
VOLTT/PRESTNMISC-108
CNOSNMISC-112
TNOPNMISC-116
SLTONMISC-120
MCC/DCCNMISC-124
MAGS/CONCSNMISC-128
MAGT/CONCTNMISC-132
ELSINMISC-136
DENERI or DENERNMISC-140
DENERIINMISC-144
GGAPNMISC-152
VRELNMISC-156
SDAMPNMISC-160
PLSINMISC-164
GSLIDNMISC-168
WEARXNMISC-172
WEARYNMISC-176
WEARZNMISC-180
VWEARNMISC189-
EDELXNMISC185-

Table 175.4: CONTA175 (2D) Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEI
PRESSMISC51
SFRICSMISC-3
FLUX [3]SMISC-6
FDDIS [3]SMISC-8
FXCV [3]SMISC-10
FXRD [3]SMISC-12
FXCD [3]SMISC-14
FXNPSMISC-16
JCONT/CCONT/PFLUX [3]SMISC-18
HJOUSMISC-20
DFLUX [3]SMISC-22
STAT [1]NMISC191
OLDSTNMISC-3
PENE [2]NMISC-5
DBANMISC-7
SLIDENMISC-9
KNNMISC-11
KTNMISC-13
TOLNNMISC-15
IPENENMISC-17
PINBNMISC20-
CNFXNMISC21-
CNFYNMISC22-
CNTXNMISC91-
CNTYNMISC92-
ISEG [4]NMISC-23
CAREANMISC27-
MUNMISC-29
DTSTARTNMISC-31
DPARAMNMISC-33
TEMPSNMISC-37
TEMPTNMISC-39
CONVNMISC-41
RACNMISC-43
TCCNMISC-45
CNFHNMISC47-
ECURT/ECHAR/EPELXNMISC48-
ECC/PCC/PSEENMISC-49
VOLTS/PRESSNMISC-51
VOLTT/PRESTNMISC-53
CNOSNMISC-55
TNOPNMISC-57
SLTONMISC-59
DCCNMISC-61
CONCSNMISC-63
CONCTNMISC-65
ELSINMISC-67
DENERINMISC-69
DENERIINMISC-71
GGAPNMISC-75
VRELNMISC-77
SDAMPNMISC-79
PLSINMISC-81
GSLIDNMISC-83
WEARXNMISC-85
WEARYNMISC-87
VWEARNMISC93-
EDELXNMISC90-

  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.

  4. The floating point output format for large integers may lead to incorrect ISEG values. You should verify the NMISC values via the *GET command. For example, *GET,Par,ELEM,N,NMISC,46 (for the 3D element) returns the ISEG value for node I of element N.

You can display or list contact results through several POST1 postprocessor commands. The contact specific items for the PLETAB, 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

CONTA175 Assumptions and Restrictions

  • 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 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.

  • Only damping defined via KEYOPT(15) is supported. All other damping specifications (Rayleigh damping, DMPSTR, and so on) are not supported.

  • 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.

CONTA175 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 (2D) and MAG (3D) DOFs (KEYOPT(1) = 7) are not available.

  • Birth and death is not available.

  • Debonding is not available.

  • User-defined contact is not available.

  • User-defined friction is not available.

Ansys Mechanical Premium  —  

  • The AZ (2D) and MAG (3D) DOFs (KEYOPT(1) = 7) are not available.

  • Debonding is not available.

  • User-defined contact is not available.

  • User-defined friction is not available.