CONTA175## CONTA175 Element Description

## CONTA175 Input Data

#### Pair-Based Contact versus General Contact

#### Friction

#### Other Input

### CONTAC175 Input Summary

## CONTA175 Output Data

## CONTA175 Assumptions and Restrictions

## CONTA175 Product Restrictions

**2-D/3-D
Node-to-Surface Contact**

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

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 2-D or 3-D. It can be used for both pair-based contact and general contact.

The element is applicable to 2-D or 3-D structural and coupled field contact analyses. This element is located on the surfaces of solid, beam, and shell elements. 3-D 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 2-D or 3-D target element type, TARGE169 or TARGE170. In the case of general contact, the target surface can be defined by contact elements CONTA171 through 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.

The geometry is shown in Figure 175.1: CONTA175 Geometry. The element
is defined by one node. The underlying elements can be 2-D or 3-D solid, shell, or beam
elements. CONTA175 represents 2-D or 3-D contact depending on
whether the associated 2-D or 3-D target segments are used. Contact can occur only when
the outward normal direction of the 2-D or 3-D 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.

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 2-D or CONTA174 for
3-D) on deformable bodies (on both lower- and higher-order elements); 3-D contact line
elements (CONTA177) on 3-D beams, on feature edges of 3-D
deformable bodies, and on perimeter edges of shell structures; and vertex-to-surface
elements (CONTA175) on convex corners of 2-D or 3-D 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 and lower-order contact surface
elements (CONTA171 or CONTA173)
overlaid on 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.

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.

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 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 in the Mechanical APDL Programmer's Reference for a detailed description
of the `USERFRIC`

subroutine.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 Mechanical APDL Contact Technology Guide for more information on
how to use this feature. See also the Guide to User-Programmable Features in the Mechanical APDL 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 3-D models and 2-D 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.

**Nodes**I

**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, MCC, , , COR, STRM, FDMN, FDMT, FDMD, FDMS, TBND, WBID, PCC, PSEE, ABPP, FPFT, FPWT, DCC, DCON, ABDC 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**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:

**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 (2-D) or MAG (3-D)

**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

**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 3-D beam or pipe elements.**Note:**For general contact, the**GCGEN**command automatically sets KEYOPT(3) = 1 (traction-based model).**KEYOPT(4)**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)

**Note:**When using the multipoint constraint (MPC) approach to define surface-based constraints, use KEYOPT(4) in the following way: set KEYOPT(4) = 0 for a rigid surface constraint; set KEYOPT(4) = 1 for a force-distributed constraint; set KEYOPT(4) = 3 for a coupling constraint. See Surface-based Constraints 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) ≠ 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

**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)**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).

**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**,,in conjunction with`C1`

**TB**,INTER to specify the effect of initial penetration or gap. If**TBDATA**,,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`C1`

*Material Reference*.**KEYOPT(10)**Contact Stiffness Update:

**0 --**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.

**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 never exceeds the maximum allowable limit (SLTO) during the entire solution.

**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. It is also applicable to beam elements whose thickness is defined through real constant input. However, KEYOPT(11) = 1 is not valid if the thickness of 2-D/3-D 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 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 appropriatelabel to specify the behavior at the contact surface. For more information, see Interaction Options for General Contact Definitions in the`TBOPT`

*Material Reference*.**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; arbitrary rotation is permitted.

**Table 175.1: CONTA175 Real Constants**

No. | Name | Description | For more information, see this section in the Contact Technology Guide . .
. |
---|---|---|---|

1 | R1 |
Target radius for cylinder, cone, or sphere | |

2 | R2 |
Target radius at second node of cone | |

3 | FKN[4] | ||

4 | FTOLN |
Penetration tolerance factor | |

5 | ICONT |
Initial contact closure | |

6 | PINB |
Pinball region | or |

7 | PMAX |
Upper limit of initial allowable penetration | |

8 | PMIN |
Lower limit of initial allowable penetration | |

9 | TAUMAX | ||

10 | CNOF | ||

11 | FKOP | ||

12 | FKT[4] | ||

13 | COHE |
Contact cohesion | |

14 | TCC[4] | ||

15 | FHTG |
Frictional heating factor | |

16 | SBCT |
Stefan-Boltzmann constant | |

17 | RDVF | ||

18 | FWGT |
Heat distribution weighing factor | Modeling Heat Generation Due to Friction (thermal) orHeat Generation Due to Electric Current (electric) |

19 | ECC[4] | ||

20 | FHEG |
Joule dissipation weight factor | |

21 | FACT |
Static/dynamic ratio | |

22 | DC |
Exponential decay coefficient | |

23 | SLTO |
Allowable elastic slip | |

24 | TNOP |
Maximum allowable tensile contact force/pressure [3] | |

25 | TOLS |
Target edge extension factor | |

26 | MCC[4] | ||

29 | COR |
Coefficient of restitution | |

30 | STRM |
Load step number for ramping penetration | |

31 | FDMN | Normal stabilization damping factor [1] [2] | |

32 | FDMT | Tangential stabilization damping factor [1] [2] | |

33 | FDMD | Destabilization squeal damping factor | |

34 | FDMS | Stabilization squeal damping factor | |

35 | TBND | Critical bonding temperature [1] [2] | |

36 | WBID | Internal contact pair ID (used by ANSYS Workbench) | |

37 | PCC[4] | Pore fluid contact permeability coefficient [1] [2] | |

38 | PSEE[4] | Pore fluid seepage coefficient [1] [2] | |

39 | ABPP | Ambient pore pressure [1] [2] | |

40 | FPFT | Gap pore fluid flow participation factor [1] [2] | |

41 | FPWT | Gap pore fluid flow distribution weighting factor | |

42 | DCC[4] | Contact diffusivity coefficient [1] [2] | |

43 | DCON[4] | Diffusive convection coefficient [1] [2] | |

44 | ABDC | Ambient concentration [1] [2] |

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

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

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

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.

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

Nodal displacements included in the overall nodal solution

Additional element output as shown in Table 175.2: CONTA175 Element Output Definitions.

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 175.2: CONTA175 Element Output Definitions**

Name | Definition | O | R |
---|---|---|---|

EL | Element Number | Y | Y |

NODES | Nodes I | Y | Y |

XC, YC, (ZC) | Location where results are reported (same as nodal location) | Y | Y |

TEMP | Temperature T(I) | Y | Y |

VOLU | AREA for 3-D, Length for 2-D | Y | Y |

NPI | Number of integration points | Y | - |

ITRGET | Target surface number (assigned by ANSYS) | Y | - |

ISOLID | Underlying solid or shell element number | Y | - |

CONT:STAT | Current contact statuses | 1 | 1 |

OLDST | Old contact statuses | 1 | 1 |

ISEG | Current contacting target element number | Y | Y |

OLDSEG | Underlying old target number | Y | - |

CONT:PENE | Current penetration (gap = 0; penetration = positive value) | Y | Y |

CONT:GAP | Current gap (gap = negative value; penetration = 0) | Y | Y |

NGAP | New or current gap at current converged substep (gap = negative value; penetration = positive value) | Y | - |

OGAP | Old gap at previously converged substep (gap = negative value; penetration = positive value) | Y | - |

IGAP | Initial gap at start of current substep (gap = negative value; penetration = positive value) | Y | Y |

GGAP | Geometric gap at current converged substep (gap = negative value; penetration = positive value) | - | Y |

CONT:PRES | Normal contact force/pressure | 2 | 2 |

TAUR/TAUS [8] | Tangential contact forces/stresses | 2 | 2 |

KN | Current normal contact stiffness (units: Force/Length for contact
force-based model, Force/Length^{3} for contract
traction-based model) | 5 | 5 |

KT | Current tangent contact stiffness (same units as KN) | 5 | 5 |

MU [9] | Friction coefficient | Y | Y |

TASS/TASR [8] | Total (algebraic sum) sliding in S and R directions (3-D only) | 3 | 3 |

AASS/AASR [8] | Total (absolute sum) sliding in S and R directions (3-D only) | 3 | 3 |

TOLN | Penetration tolerance | Y | Y |

CONT:SFRIC | Frictional force/stress, SQRT (TAUR**2+TAUS**2) (3-D only) | 2 | 2 |

CONT:STOTAL | Total force/stress, SQRT (PRES**2+TAUR**2+TAUS**2) (3-D only) | 2 | 2 |

CONT:SLIDE | Amplitude of total accumulated sliding, SQRT (TASS**2+TASR**2) (3-D only) | 3 | 3 |

NX, NY | Surface normal vector components (2-D only) | Y | - |

CONT:SFRIC | Tangential contact force/stress (2-D only) | 2 | 2 |

CONT:SLIDE | Total accumulated sliding (algebraic sum) (2-D only) | 3 | 3 |

ASLIDE | Total accumulated sliding (absolute sum) (2-D only) | 3 | 3 |

FDDIS | Frictional energy dissipation | 7 | 7 |

ELSI | Total equivalent elastic slip distance | - | Y |

PLSI | Total (accumulated) equivalent plastic slip due to frictional sliding | - | Y |

GSLID | Amplitude of total accumulated sliding (including near-field) | - | 10 |

VREL | Equivalent sliding velocity (slip rate) | - | Y |

DBA | Penetration variation | Y | Y |

PINB | Pinball Region | - | Y |

CONT:CNOS | Total number of contact status changes during substep | Y | Y |

TNOP | Maximum allowable tensile contact force/pressure | 2 | 2 |

SLTO | Allowable elastic slip | Y | Y |

CAREA | Contacting area | - | Y |

DTSTART | Load step time during debonding | Y | Y |

DPARAM | Debonding parameter | Y | Y |

DENERI [13] | Energy released due to separation in normal direction - mode I debonding | Y | Y |

DENERII [13] | Energy released due to separation in tangential direction - mode II debonding | Y | Y |

DENER [14] | Total energy released due to debonding | Y | Y |

CNFX [11] | Contact element force-X component | - | 4 |

CNFY [11] | Contact element force-Y component | - | 4 |

CNFZ [11] | Contact element force-Z component (3-D 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 |

SDAMP | Squeal damping coefficient (3-D only) / Stabilization damping coefficient (2-D and 3-D) | - | Y |

WEARX, WEARY, WEARZ | Wear correction - X, Y, and Z components | - | Y |

CONV | Convection coefficient | Y | Y |

RAC | Radiation coefficient | Y | Y |

TCC | Conductance coefficient | 6 | 6 |

TEMPS | Temperature at contact point | Y | Y |

TEMPT | Temperature at target surface | Y | Y |

FXCV | Heat flux due to convection | Y | Y |

FXRD | Heat flux due to radiation | Y | Y |

FXCD | Heat flux due to conductance | Y | Y |

CONT:FLUX | Total heat flux at contact surface | Y | Y |

FXNP | Flux input | - | Y |

CNFH | Contact element heat flow | - | Y |

JCONT | Contact current density (Current/Unit Area) | Y | Y |

CCONT | Contact charge density (Charge/Unit Area) | Y | Y |

HJOU | Contact power/area | Y | Y |

ECURT | Current per contact element | - | Y |

ECHAR | Charge per contact element | - | Y |

ECC | Electric contact conductance (for electric current DOF), or electric contact capacitance per unit area (for piezoelectric or electrostatic DOFs) | 6 | 6 |

VOLTS | Voltage on contact nodes | Y | Y |

VOLTT | Voltage on associated target | Y | Y |

MCC | Magnetic contact permeance | 6 | 6 |

MFLUX | Magnetic flux density | Y | Y |

AZS/MAGS | 2-D/3-D Magnetic potential on contact node | Y | Y |

AZT/MAGT | 2-D/3-D Magnetic potential on associated target | Y | Y |

PCC | Pore fluid contact permeability coefficient | 6 | 6 |

PSEE | Pore fluid seepage coefficient | 6 | 6 |

PRESS | Pore pressure on contact nodes | Y | Y |

PREST | Pore pressure on associated target | Y | Y |

PFLUX | Pore volume flux density per unit area flow into contact surface | Y | Y |

EPELX | Pore volume flux per contact element | - | Y |

DCC | Contact diffusivity coefficient | 6 | 6 |

DCON | Diffusive convection coefficient | 6 | 6 |

CONCS | Concentration on contact nodes | Y | Y |

CONCT | Concentration on associated target | Y | Y |

DFLUX | Diffusion flux density per unit area flow into contact surface | Y | Y |

EDELX | Diffusion flux per contact element | - | Y |

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 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.

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

Contact element forces are defined in the global Cartesian system

For the force-based model, the unit of stiffness is FORCE/LENGTH. For the traction-based model, the unit is FORCE/LENGTH

^{3}.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.

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

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

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

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).

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).

DENERI and DENERII are available only when one of the following material models is used:

**TB**,CZM,,,,CBDD or**TB**,CZM,,,,CBDE.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).

Table 175.3: CONTA175 (3-D) Item and Sequence Numbers and Table 175.4: CONTA175 (2-D) 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 (3-D) Item and Sequence Numbers**

Output Quantity Name | ETABLE and
ESOL Command Input | ||
---|---|---|---|

Item | E | I | |

PRES | SMISC | 13 | 1 |

TAUR | SMISC | - | 5 |

TAUS | SMISC | - | 9 |

FLUX [3] | SMISC | - | 14 |

FDDIS [3] | SMISC | - | 18 |

FXCV [3] | SMISC | 22 | |

FXRD [3] | SMISC | - | 26 |

FXCD [3] | SMISC | - | 30 |

FXNP | SMISC | - | 34 |

JCONT/CCONT/PFLUX [3] | SMISC | - | 38 |

HJOU | SMISC | - | 42 |

MFLUX/DFLUX [3] | SMISC | - | 46 |

STAT[1] | NMISC | 41 | 1 |

OLDST | NMISC | - | 5 |

PENE[2] | NMISC | - | 9 |

DBA | NMISC | - | 13 |

TASR | NMISC | - | 17 |

TASS | NMISC | - | 21 |

KN | NMISC | - | 25 |

KT | NMISC | - | 29 |

TOLN | NMISC | - | 33 |

IGAP | NMISC | - | 37 |

PINB | NMISC | 42 | - |

CNFX | NMISC | 43 | - |

CNFY | NMISC | 44 | - |

CNFZ | NMISC | 45 | - |

CNTX | NMISC | 186 | - |

CNTY | NMISC | 187 | - |

CNTZ | NMISC | 188 | - |

ISEG [4] | NMISC | - | 46 |

AASR | NMISC | - | 50 |

AASS | NMISC | - | 54 |

CAREA | NMISC | 58 | - |

MU | NMISC | - | 62 |

DTSTART | NMISC | - | 66 |

DPARAM | NMISC | - | 70 |

TEMPS | NMISC | - | 78 |

TEMPT | NMISC | - | 82 |

CONV | NMISC | - | 86 |

RAC | NMISC | - | 90 |

TCC | NMISC | - | 94 |

CNFH | NMISC | 98 | - |

ECURT/ECHAR/EPELX | NMISC | 99 | - |

ECC/PCC/PSEE | NMISC | - | 100 |

VOLTS/PRESS | NMISC | - | 104 |

VOLTT/PREST | NMISC | - | 108 |

CNOS | NMISC | - | 112 |

TNOP | NMISC | - | 116 |

SLTO | NMISC | - | 120 |

MCC/DCC | NMISC | - | 124 |

MAGS/CONCS | NMISC | - | 128 |

MAGT/CONCT | NMISC | - | 132 |

ELSI | NMISC | - | 136 |

DENERI or DENER | NMISC | - | 140 |

DENERII | NMISC | - | 144 |

GGAP | NMISC | - | 152 |

VREL | NMISC | - | 156 |

SDAMP | NMISC | - | 160 |

PLSI | NMISC | - | 164 |

GSLID | NMISC | - | 168 |

WEARX | NMISC | - | 172 |

WEARY | NMISC | - | 176 |

WEARZ | NMISC | - | 180 |

EDELX | NMISC | 185 | - |

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

Output Quantity Name | ETABLE and
ESOL Command Input | ||
---|---|---|---|

Item | E | I | |

PRES | SMISC | 5 | 1 |

SFRIC | SMISC | - | 3 |

FLUX [3] | SMISC | - | 6 |

FDDIS [3] | SMISC | - | 8 |

FXCV [3] | SMISC | - | 10 |

FXRD [3] | SMISC | - | 12 |

FXCD [3] | SMISC | - | 14 |

FXNP | SMISC | - | 16 |

JCONT/CCONT/PFLUX [3] | SMISC | - | 18 |

HJOU | SMISC | - | 20 |

DFLUX [3] | SMISC | - | 22 |

STAT [1] | NMISC | 19 | 1 |

OLDST | NMISC | - | 3 |

PENE [2] | NMISC | - | 5 |

DBA | NMISC | - | 7 |

SLIDE | NMISC | - | 9 |

KN | NMISC | - | 11 |

KT | NMISC | - | 13 |

TOLN | NMISC | - | 15 |

IPENE | NMISC | - | 17 |

PINB | NMISC | 20 | - |

CNFX | NMISC | 21 | - |

CNFY | NMISC | 22 | - |

CNTX | NMISC | 91 | - |

CNTY | NMISC | 92 | - |

ISEG [4] | NMISC | - | 23 |

CAREA | NMISC | 27 | - |

MU | NMISC | - | 29 |

DTSTART | NMISC | - | 31 |

DPARAM | NMISC | - | 33 |

TEMPS | NMISC | - | 37 |

TEMPT | NMISC | - | 39 |

CONV | NMISC | - | 41 |

RAC | NMISC | - | 43 |

TCC | NMISC | - | 45 |

CNFH | NMISC | 47 | - |

ECURT/ECHAR/EPELX | NMISC | 48 | - |

ECC/PCC/PSEE | NMISC | - | 49 |

VOLTS/PRESS | NMISC | - | 51 |

VOLTT/PREST | NMISC | - | 53 |

CNOS | NMISC | - | 55 |

TNOP | NMISC | - | 57 |

SLTO | NMISC | - | 59 |

DCC | NMISC | - | 61 |

CONCS | NMISC | - | 63 |

CONCT | NMISC | - | 65 |

ELSI | NMISC | - | 67 |

DENERI | NMISC | - | 69 |

DENERII | NMISC | - | 71 |

GGAP | NMISC | - | 75 |

VREL | NMISC | - | 77 |

SDAMP | NMISC | - | 79 |

PLSI | NMISC | - | 81 |

GSLID | NMISC | - | 83 |

EDELX | NMISC | 90 | - |

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

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

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,,ELEM,`Par`

,NMISC,46 (for the 3-D element) returns the ISEG value for node I of element`N`

.`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:

STAT | Contact status |

PENE | Contact penetration |

PRES | Contact pressure for the traction-based model. Contact normal force for the force-based model. |

SFRIC | Contact friction stress for the traction-based model. Friction force for the force-based model. |

STOT | Contact total stress (pressure plus friction) for the traction-based model. Total contact force for the force-based model. |

SLIDE | Contact sliding distance |

GAP | Contact gap distance |

CNOS | Total number of contact status changes during substep |

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.

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.

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*.

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 (2-D) and MAG (3-D) 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.

Linear perturbation is not available.

**ANSYS Mechanical Premium **

The AZ (2-D) and MAG (3-D) 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.