CONTA174 ## CONTA174 Element Description

## CONTA174 Input Data

#### Pair-Based Contact versus General Contact

#### Friction

#### Other Input

### CONTA174 Input Summary

## CONTA174 Output Data

## CONTA174 Assumptions and Restrictions

## CONTA174 Product Restrictions

**3-D 8-Node
Surface-to-Surface Contact**

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

CONTA174 is used to represent contact and sliding between 3-D target surfaces and a deformable surface defined by this element. The element is applicable to 3-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 3-D target element type, TARGE170. In the case of general contact, the target surface can be defined by CONTA174 elements (for deformable surfaces) or TARGE170 elements (for rigid bodies only).

The element is located on the surfaces of 3-D solid or shell elements with midside nodes (for example, SOLID186, SOLID187, SHELL281, SOLID226, SOLID279, CPT216, MATRIX50).

The element has the same geometric characteristics as the solid or shell element face with which it is connected (see Figure 174.1: CONTA174 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. The element also allows separation of bonded contact
to simulate interface delamination.

See CONTA174 in the *Mechanical APDL Theory Reference* for more details about this element. Other surface-to-surface
contact elements (CONTA171, CONTA172, CONTA173) are also available.

The geometry and node locations are shown in Figure 174.1: CONTA174 Geometry. The element is defined by eight nodes (the
underlying solid or shell element has midside nodes). It can degenerate
to a six node element depending on the shape of the underlying solid
or shell elements. If the underlying solid or shell elements do not
have midside nodes, use CONTA173 (you may
still use CONTA174 but you must drop all
midside nodes). See Quadratic Elements (Midside Nodes) in the *Modeling and Meshing Guide* for more
information on the use of midside nodes.

The node ordering is consistent with the node ordering for the underlying solid or shell element. The positive normal is given by the right-hand rule going around the nodes of the element and is identical to the external normal direction of the underlying solid or shell element surface. For shell elements, the same nodal ordering between shell and contact elements defines upper surface contact; otherwise, it represents bottom surface contact. The contact surface's outward normal should point toward the target surface.

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. CONTA174 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 3-D contact surface elements (CONTA173 and CONTA174) are
associated with 3-D target segment elements (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
(CONTA174) on 3-D 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 3-D solid bodies and/or
shell structures. The general contact definition may also contain target elements
(TARGE170) overlaid on the surfaces of standalone rigid
bodies and lower-order contact surface elements (CONTA173)
overlaid on 3-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 "CONTA174 Input Summary" for details.

CONTA174 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 applicable coordinate system is the default element coordinate system (noted by the R and S axes in the above figure).

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

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

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

To implement a user-defined friction model, use the **TB**,FRIC command with
* TBOPT* = USER to specify friction properties and write a

`USERFRIC`

subroutine to compute friction forces. See Writing Your Own Friction Law (`USERFRIC`

) in the Mechanical APDL Contact Technology Guide for
more information on how to use this feature. See also the Guide to User-Programmable Features 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 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 in the Mechanical APDL Programmer's Reference 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.

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 faceted elements on a curved (spherical or revolute) 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 "CONTA174 Input Summary". A general description of element input is given in Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.

**Nodes**I, J, K, L, M, N, O, P

**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, PPCN, FPAT, COR, STRM, FDMN, FDMT, FDMD, FDMS, TBND, WBID, PCC, PSEE, ABPP, FPFT, FPWT, DCC, DCON, ABDC See Table 174.1: CONTA174 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**Surface Loads**Pressure, Face 1 (I-J-K-L) (opposite to contact normal direction); used for fluid pressure penetration loading. On the **SFE**command use= 1 to specify the pressure values, and use`LKEY`

= 2 to specify starting points and penetrating points.`LKEY`

Convection, Face 1 (I-J-K-L) Heat Flux, Face 1 (I-J-K-L) **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 (or a combination of TBOT, TTOP, and TEMP set by KEYOPT(13))

**3 --**UX, UY, UZ, TEMP, VOLT

**4 --**TEMP, VOLT

**5 --**UX, UY, UZ, VOLT

**6 --**VOLT

**7 --**MAG

**8 --**UX, UY, UZ, PRES

**9 --**UX, UY, UZ, PRES, TEMP

**10 --**PRES

**11 --**UX, UY, UZ, CONC, TEMP

**12 --**UX, UY, UZ, CONC, TEMP, VOLT

**13 --**UX, UY, UZ, CONC

**14 --**CONC

**Note:**For KEYOPT(1) = 8, 9, and 10, the pore pressure (PRES) degree of freedom is ignored at midside nodes if the underlying element is a higher-order 3-D coupled pore-pressure mechanical solid (CPT216, CPT217).**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

**KEYOPT(3)**Units of normal contact stiffness:

**0 --**FORCE/LENGTH

^{3}(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). It is not recommended in conjunction with using nodal detection options (KEYOPT(4) = 1 or 2) if any midside nodes exist for the contact element.**Note:**KEYOPT(3) is not supported for contact elements used in a general contact definition.**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) ≠ 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 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**,,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 to 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

**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(13)**Degree-of-freedom control for contact involving thermal shells:

**0 --**TEMP for contact surface TEMP for target surface **1 --**TBOT for contact surface TBOT for target surface **2 --**TTOP for contact surface TTOP for target surface **3 --**TBOT for contact surface TEMP for target surface **4 --**TEMP for contact surface TBOT for target surface **5 --**TTOP for contact surface TEMP for target surface **6 --**TEMP for contact surface TTOP for target surface **7 --**TBOT for contact surface TTOP for target surface **8 --**TTOP for contact surface TBOT for target surface

**Note:**KEYOPT(13) is only used when the pure thermal contact option is set (KEYOPT(1) = 2) and the element is being used to model thermal transfer between thermal shells (SHELL131, SHELL132) or between thermal shells and thermal solids.**Note:**KEYOPT(13) is not supported for contact elements used in a general contact definition.**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 is applied based on the contact status of the current iteration. Any contact detection point which was previously exposed to the fluid pressure remains in the condition of “penetrating” (default).

**1 --**Fluid pressure penetration load is applied based on the contact status of the last converged substep. Any contact detection point which was previously exposed to the fluid pressure remains in the condition of “penetrating”.

**2 --**Fluid pressure penetration load is applied based on the contact status of the current iteration. At each iteration, the fluid pressure penetration load is newly applied from the initial starting points.

**3 --**Fluid pressure penetration load is applied based on the contact status of the last converged substep. At each iteration, the fluid pressure penetration load is newly applied from the initial starting points.

**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.**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 174.1: CONTA174 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 | 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 | ||

13 | COHE |
Contact cohesion | |

14 | TCC | ||

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 | ||

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 pressure | |

25 | TOLS |
Target edge extension factor | |

26 | MCC | ||

27 | PPCN | ||

28 | FPAT |
Fluid penetration acting time | |

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 | Pore fluid contact permeability coefficient [1] [2] | |

38 | PSEE | 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 | Contact diffusivity coefficient [1] [2] | |

43 | DCON | 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.

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 174.2: CONTA174 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 174.2: CONTA174 Element Output Definitions gives element output. In the results file, the nodal results are obtained from its closest integration point.

**Table 174.2: CONTA174 Element Output Definitions**

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

EL | Element Number | Y | Y |

NODES | Nodes I, J, K, L, M, N, O, P | Y | Y |

XC, YC, ZC | Location where results are reported | Y | 5 |

TEMP | Temperatures T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P) | Y | Y |

VOLU | AREA | Y | Y |

NPI | Number of integration points | Y | - |

ITRGET | Target surface number (assigned by the program) | 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 from 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 pressure | Y | Y |

TAUR/TAUS [7] | Tangential contact stresses | Y | Y |

KN | Current normal contact stiffness
(Force/Length^{3}) | Y | Y |

KT | Current tangent contact stiffness
(Force/Length^{3}) | Y | Y |

MU [8] | Friction coefficient | Y | Y |

TASS/TASR [7] | Total (algebraic sum) sliding in S and R directions | 3 | 3 |

AASS/AASR [7] | Total (absolute sum) sliding in S and R directions | 3 | 3 |

TOLN | Penetration tolerance | Y | Y |

CONT:SFRIC | Frictional stress, SQRT (TAUR**2+TAUS**2) | Y | Y |

CONT:STOTAL | Total stress, SQRT (PRES**2+TAUR**2+TAUS**2) | Y | Y |

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

FDDIS | Frictional energy dissipation | 6 | 6 |

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) | - | 9 |

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 pressure | Y | Y |

SLTO | Allowable elastic slip | Y | Y |

CAREA | Contacting area | - | Y |

CONT:FPRS | Actual applied fluid penetration pressure | - | Y |

FSTART | Fluid penetration starting time | - | Y |

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

DPARAM | Debonding parameter | Y | Y |

DENERI [12] | Energy released due to separation in normal direction - mode I debonding | Y | Y |

DENERII [12] | Energy released due to separation in tangential direction - mode II debonding | Y | Y |

DENER [13] | Total energy released due to debonding | Y | Y |

CNFX [10] | Contact element force-X component | - | 4 |

CNFY [10] | Contact element force-Y component | - | 4 |

CNFZ [10] | Contact element force-Z component | - | 4 |

CNTX [11] | Contact element force due to tangential stresses - X component | - | 4 |

CNTY [11] | Contact element force due to tangential stresses - Y component | - | 4 |

CNTZ [11] | Contact element force due to tangential stresses - Z component | - | 4 |

SDAMP | Squeal damping coefficient / Stabilization damping coefficient | - | 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 | Y | Y |

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) | Y | Y |

VOLTS | Voltage on contact nodes | Y | Y |

VOLTT | Voltage on associated target | Y | Y |

MCC | Magnetic contact permeance | Y | Y |

MFLUX | Magnetic flux density | Y | Y |

MAGS | Magnetic potential on contact node | Y | Y |

MAGT | Magnetic potential on associated target | Y | Y |

PCC | Pore fluid contact permeability coefficient | Y | Y |

PSEE | Pore fluid seepage coefficient | Y | Y |

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 | Y | Y |

DCON | Diffusive convection coefficient | Y | Y |

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 The program will evaluate model to detect initial conditions.

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

Contact element forces are defined in the global Cartesian system.

Available only at centroid as a

***GET**item.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 174.3: CONTA174 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 174.3: CONTA174 Item and Sequence Numbers:

**Name**output quantity as defined in the Table 174.2: CONTA174 Element Output Definitions

**Item**predetermined Item label for

**ETABLE**command**E**sequence number for single-valued or constant element data

**I,J,K,L**sequence number for data at nodes I,J,K,L,

**Table 174.3: CONTA174 Item and Sequence Numbers**

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

Item | E | I | J | K | L | |

PRES | SMISC | 13 | 1 | 2 | 3 | 4 |

TAUR | SMISC | - | 5 | 6 | 7 | 8 |

TAUS | SMISC | - | 9 | 10 | 11 | 12 |

FLUX [3] | SMISC | - | 14 | 15 | 16 | 17 |

FDDIS [3] | SMISC | - | 18 | 19 | 20 | 21 |

FXCV [3] | SMISC | 22 | 23 | 24 | 25 | |

FXRD [3] | SMISC | - | 26 | 27 | 28 | 29 |

FXCD [3] | SMISC | - | 30 | 31 | 32 | 33 |

FXNP | SMISC | - | 34 | 35 | 36 | 37 |

JCONT/CCONT/PFLUX [3] | SMISC | - | 38 | 39 | 40 | 41 |

HJOU | SMISC | - | 42 | 43 | 44 | 45 |

MFLUX/DFLUX [3] | SMISC | - | 46 | 47 | 48 | 49 |

STAT [1] | NMISC | 41 | 1 | 2 | 3 | 4 |

OLDST | NMISC | - | 5 | 6 | 7 | 8 |

PENE [2] | NMISC | - | 9 | 10 | 11 | 12 |

DBA | NMISC | - | 13 | 14 | 15 | 16 |

TASR | NMISC | - | 17 | 18 | 19 | 20 |

TASS | NMISC | - | 21 | 22 | 23 | 24 |

KN | NMISC | - | 25 | 26 | 27 | 28 |

KT | NMISC | - | 29 | 30 | 31 | 32 |

TOLN | NMISC | - | 33 | 34 | 35 | 36 |

IGAP | NMISC | - | 37 | 38 | 39 | 40 |

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 | 47 | 48 | 49 |

AASR | NMISC | - | 50 | 51 | 52 | 53 |

AASS | NMISC | - | 54 | 55 | 56 | 57 |

CAREA | NMISC | 58 | 59 | 60 | 61 | 184 |

MU | NMISC | - | 62 | 63 | 64 | 65 |

DTSTART | NMISC | - | 66 | 67 | 68 | 69 |

DPARAM | NMISC | - | 70 | 71 | 72 | 73 |

FPRS | NMISC | - | 74 | 75 | 76 | 77 |

TEMPS | NMISC | - | 78 | 79 | 80 | 81 |

TEMPT | NMISC | - | 82 | 83 | 84 | 85 |

CONV | NMISC | - | 86 | 87 | 88 | 89 |

RAC | NMISC | - | 90 | 91 | 92 | 93 |

TCC | NMISC | - | 94 | 95 | 96 | 97 |

CNFH | NMISC | 98 | - | - | - | - |

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

ECC/PCC/PSEE | NMISC | - | 100 | 101 | 102 | 103 |

VOLTS/PRESS | NMISC | - | 104 | 105 | 106 | 107 |

VOLTT/PREST | NMISC | - | 108 | 109 | 110 | 111 |

CNOS | NMISC | - | 112 | 113 | 114 | 115 |

TNOP | NMISC | - | 116 | 117 | 118 | 119 |

SLTO | NMISC | - | 120 | 121 | 122 | 123 |

MCC/DCC | NMISC | - | 124 | 125 | 126 | 127 |

MAGS/CONCS | NMISC | - | 128 | 129 | 130 | 131 |

MAGT/CONCT | NMISC | - | 132 | 133 | 134 | 135 |

ELSI | NMISC | - | 136 | 137 | 138 | 139 |

DENERI or DENER | NMISC | - | 140 | 141 | 142 | 143 |

DENERII | NMISC | - | 144 | 145 | 146 | 147 |

FSTART | NMISC | - | 148 | 149 | 150 | 151 |

GGAP | NMISC | - | 152 | 153 | 154 | 155 |

VREL | NMISC | - | 156 | 157 | 158 | 159 |

SDAMP | NMISC | - | 160 | 161 | 162 | 163 |

PLSI | NMISC | - | 164 | 165 | 166 | 167 |

GSLID | NMISC | - | 168 | 169 | 170 | 171 |

WEARX | NMISC | - | 172 | 173 | 174 | 175 |

WEARY | NMISC | - | 176 | 177 | 178 | 179 |

WEARZ | NMISC | - | 180 | 181 | 182 | 183 |

EDELX | NMISC | 185 | - | - | - | - |

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 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 **PLNSOL**, **PLESOL**, **PRNSOL**, and **PRESOL** commands are listed below:

STAT | Contact status |

PENE | Contact penetration |

PRES | Contact pressure |

SFRIC | Contact friction stress |

STOT | Contact total stress (pressure plus friction) |

SLIDE | Contact sliding distance |

GAP | Contact gap distance |

FLUX | Total heat flux at contact surface |

CNOS | Total number of contact status changes during substep |

FPRS | Actual applied fluid penetration pressure |

The 3-D contact element must coincide with the external surface of the underlying solid or shell element.

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

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

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

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

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

It is possible for at least one midside node of the contact element to be in contact while the corner nodes are not in contact. Because the program reports contact results only for the corner nodes, the element may have a closed contact status even though the reported contact pressure is zero. To verify the contact status for contact elements in this situation, list the following

**ETABLE**quantities: SMISC,13 (PRES); NMISC,41 (STAT); NMISC,43 (CNFX); NMISC,44 (CNFY); and NIMSC,45 (CNFZ).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 MAG 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 MAG 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.