CONTA175

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. 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 segment elements (TARGE169, TARGE170) on a specified target surface. Coulomb friction,
shear stress friction, and user defined friction with the USERFRIC
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.
The element is defined by one node. The underlying elements can be
2-D or 3-D solid, shell, or beam elements. The 3-D underlying solid
or shell elements must have no midside nodes. CONTA175 represents 2-D or 3-D contact depending on whether the associated
2-D (TARGE169) or 3-D (TARGE170) segments are used. Remember, 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 generating elements
automatically using the **ESURF** command.

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 User-Defined Friction in the *Material Reference* for more information
on how to use this feature. See also the *Guide to ANSYS User Programmable Features* for a detailed description
of the USERFRIC 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.

The contact surface elements are associated with the target
segment elements (TARGE169, TARGE170) via a shared real constant set. ANSYS looks for contact only between
surfaces with the same real constant set. For either rigid-flexible
or flexible-flexible contact, one of the deformable surfaces must
be represented by a contact surface. See Designating Contact and Target Surfaces in the *Contact Technology Guide* for more information.
If more than one target surface will make contact with the same boundary
of 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), or you must combine the two target
surfaces into one (targets that share the same real constant numbers).

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.

See the *Contact Technology Guide* for a detailed discussion on 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**UX, UY, (UZ) (if KEYOPT(1) = 0 UX, UY, (UZ), TEMP (if KEYOPT(1) = 1) TEMP (if KEYOPT(1) = 2) UX, UY, (UZ), TEMP, VOLT (if KEYOPT(1) = 3) TEMP, VOLT (if KEYOPT(1) = 4) UX, UY, (UZ), VOLT (if KEYOPT(1) = 5) VOLT (if KEYOPT(1) = 6) AZ (2-D), MAG (3-D) (if KEYOPT(1) = 7) **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 See Table 175.1: CONTA175 Real Constants for descriptions of the real constants. **Material Properties**MU, EMIS ( **MP**command)FRIC ( **TB**command; see Contact Friction in the*Material Reference*)CZM ( **TB**command; see Cohesive Zone Materials Used for Debonding in the*Contact Technology Guide*)**Special Features**Birth and death Debonding Isotropic friction Large deflection Linear perturbation Nonlinear Orthotropic friction 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)

**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 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)

**3 --**Normal to target surface (used for shell/beam bottom surface contact when shell/beam thickness is accounted for)

**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. 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) > 0):

**0 --**Use default range for stiffness updating

**1 --**Make a nominal refinement to the allowable stiffness range

**2 --**Make an aggressive refinement to the allowable stiffness range

**KEYOPT(7)**Element level time incrementation control / impact constraints:

**0 --**No control

**1 --**Automatic bisection of increment

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

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

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

**Note:**KEYOPT(7) = 2, 3, and 4 include an automatic adjustment of the time increment. This is activated only if the command

**SOLCONTROL**,ON,ON was issued prior to the solution.**KEYOPT(8)**Asymmetric contact selection:

**0 --**No action

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

**KEYOPT(9)**Effect of initial penetration or gap:

**0 --**Include both initial geometrical penetration or gap and offset

**1 --**Exclude both initial geometrical penetration or gap and offset

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

**3 --**Include offset only (exclude initial geometrical penetration or gap)

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

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

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

**Note:**The effects of KEYOPT(9) are dependent on settings for other KEYOPTs. For KEYOPT(9) = 1, 3, or 4, the indicated initial gap effect is considered only if KEYOPT(12) = 4 or 5. See the discussion on using KEYOPT(9) in the

*Contact Technology Guide*for more information.**KEYOPT(10)**Contact Stiffness Update:

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

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

**KEYOPT(11)**Shell Thickness Effect (only for real constant based thickness input):

**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.**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:**Stabilization damping is only applied to contact pairs in near-field contact. When KEYOPT(15) = 0, 1, or 2, stabilization damping will not be applied in the current substep if any contact detection point had a closed status in the previous substep. However, when KEYOPT(15) = 3, stabilization damping is always applied as long as the current contact status is near-field. 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.

**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 | Normal penalty stiffness factor | |

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 | Maximum friction stress | |

10 | CNOF | Contact surface offset | |

11 | FKOP | Contact opening stiffness | |

12 | FKT | Tangent penalty stiffness factor | |

13 | COHE | Contact cohesion | |

14 | TCC | Thermal contact conductance | |

15 | FHTG | Frictional heating factor | |

16 | SBCT | Stefan-Boltzmann constant | |

17 | RDVF | Radiation view factor | |

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

19 | ECC | Electric contact conductance | |

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 [1] | |

25 | TOLS | Target edge extension factor | |

26 | MCC | Magnetic contact permeance | |

29 | COR | Coefficient of restitution | |

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

31 | FDMN | Normal stabilization damping factor | |

32 | FDMT | Tangential stabilization damping factor | |

33 | FDMD | Destabilization squeal damping factor | |

34 | FDMS | Stabilization squeal damping factor | |

35 | TBND | Critical bonding temperature |

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 pressure | 2 | 2 |

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

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

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

MU[9] | Friction coefficient | 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 stress SQRT (TAUR**2+TAUS**2) (3-D only) | 2 | 2 |

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

CONT:SLIDE | Total sliding SQRT (TASS**2+TASR**2) (3-D only) | Y | Y |

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

CONT:SFRIC | Tangential contact 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 | Elastic slip distance for sticking contact within a substep | - | Y |

VREL | 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 | 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 | Energy released due to separation in normal direction - mode I debonding | Y | Y |

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

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

CNFY | Contact element force-Y component | - | Y |

CNFZ | Contact element force-Z component (3-D only) | - | Y |

SDAMP | Squeal damping coefficient (3-D only) | - | 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 |

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 the quantities is FORCE. For the traction-based model (KEYOPT(3) = 1), the unit is FORCE/AREA.

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-ased model, the unit is FORCE/LENGTH

^{3}.The units of TCC, ECC, and MCC in the traction-based model should be the units of TCC, ECC, and MCC of 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.

| 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 manual
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 | SMISC | - | 14 |

FDDIS | SMISC | - | 18 |

FXCV | SMISC | 22 | |

FXRD | SMISC | - | 26 |

FXCD | SMISC | - | 30 |

FXNP | SMISC | - | 34 |

JCONT | SMISC | - | 38 |

CCONT | SMISC | - | 38 |

HJOU | SMISC | - | 42 |

MFLUX | 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 | - |

ISEG | 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 | NMISC | 99 | - |

ECHAR | NMISC | 99 | - |

ECC | NMISC | - | 100 |

VOLTS | NMISC | - | 104 |

VOLTT | NMISC | - | 108 |

CNOS | NMISC | - | 112 |

TNOP | NMISC | - | 116 |

SLTO | NMISC | - | 120 |

MCC | NMISC | - | 124 |

MAGS | NMISC | - | 128 |

MAGT | NMISC | - | 132 |

ELSI | NMISC | - | 136 |

DENERI | NMISC | - | 140 |

DENERII | NMISC | - | 144 |

GGAP | NMISC | - | 152 |

VREL | NMISC | - | 156 |

SDAMP | NMISC | - | 160 |

**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 | SMISC | - | 6 |

FDDIS | SMISC | - | 8 |

FXCV | SMISC | - | 10 |

FXRD | SMISC | - | 12 |

FXCD | SMISC | - | 14 |

FXNP | SMISC | - | 16 |

JCONT | SMISC | - | 18 |

CCONT | SMISC | - | 18 |

HJOU | SMISC | - | 20 |

MFLUX | 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 | - |

ISEG | 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 | NMISC | 48 | - |

ECHAR | NMISC | 48 | - |

ECC | NMISC | - | 49 |

VOLTS | NMISC | - | 51 |

VOLTT | NMISC | - | 53 |

CNOS | NMISC | - | 55 |

TNOP | NMISC | - | 57 |

SLTO | NMISC | - | 59 |

MCC | NMISC | - | 61 |

AZS | NMISC | - | 63 |

AZT | NMISC | - | 65 |

ELSI | NMISC | - | 67 |

DENERI | NMISC | - | 69 |

DENERII | NMISC | - | 71 |

GGAP | NMISC | - | 75 |

VREL | NMISC | - | 77 |

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 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.

The USERFRIC subroutine (user-defined friction) can only be used with penalty-based tangential contact (i.e., KEYOPT(2) = 0, 1, or 3).

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 Professional. **

The MU material property is not allowed.

The birth and death special feature is not allowed.

**ANSYS Structural. **

The VOLT DOF (KEYOPT(1) = 3 through 6) is not allowed.

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

**ANSYS Mechanical. **

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