CONTA175

2-D/3-D Node-to-Surface Contact
MP ME ST PR PRN DS DSS <> EM <> <> PP <> EME MFS

CONTA175 Element Description

CONTA175 may be used to represent contact and sliding between two surfaces (or between a node and a surface, or between a line and a surface) in 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.

Figure 175.1  CONTA175 Geometry

CONTA175 Geometry

CONTA175 Input Data

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.

CONTAC175 Input Summary

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.NameDescriptionFor more information, see this section in the Contact Technology Guide . . .
1R1

Target radius for cylinder, cone, or sphere

Defining the Target Surface

2R2

Target radius at second node of cone

Defining the Target Surface

3FKN

Normal penalty stiffness factor

Determining Contact Stiffness and Penetration

4FTOLN

Penetration tolerance factor

Determining Contact Stiffness and Penetration

5ICONT

Initial contact closure

Adjusting Initial Contact Conditions

6PINB

Pinball region

Determining Contact Status and the Pinball Region

or

Defining Influence Range (PINB)

7PMAX

Upper limit of initial allowable penetration

Adjusting Initial Contact Conditions

8PMIN

Lower limit of initial allowable penetration

Adjusting Initial Contact Conditions

9TAUMAX

Maximum friction stress

Choosing a Friction Model

10CNOF

Contact surface offset

Adjusting Initial Contact Conditions

11FKOP

Contact opening stiffness

Selecting Surface Interaction Models

12FKT

Tangent penalty stiffness factor

Determining Contact Stiffness

13COHE

Contact cohesion

Choosing a Friction Model

14TCC

Thermal contact conductance

Modeling Conduction

15FHTG

Frictional heating factor

Modeling Heat Generation Due to Friction

16SBCT

Stefan-Boltzmann constant

Modeling Radiation

17RDVF

Radiation view factor

Modeling Radiation

18FWGT

Heat distribution weighing factor

Modeling Heat Generation Due to Friction (thermal)

or

Heat Generation Due to Electric Current (electric)

19ECC 

Electric contact conductance

Modeling Surface Interaction

20FHEG

Joule dissipation weight factor

Heat Generation Due to Electric Current

21FACT

Static/dynamic ratio

Static and Dynamic Friction Coefficients

22DC

Exponential decay coefficient

Static and Dynamic Friction Coefficients

23SLTO

Allowable elastic slip

Using FKT and SLTO

24TNOP

Maximum allowable tensile contact pressure [1]

Chattering Control Parameters

25TOLS 

Target edge extension factor

Selecting Location of Contact Detection

26MCC

Magnetic contact permeance

Modeling Magnetic Contact

29COR

Coefficient of restitution

Impact Between Rigid Bodies

30STRM

Load step number for ramping penetration

Adjusting Initial Contact Conditions

31FDMNNormal stabilization damping factor

Applying Contact Stabilization Damping

32FDMTTangential stabilization damping factor

Applying Contact Stabilization Damping

33FDMDDestabilization squeal damping factor

Forced Frictional Sliding Using Velocity Input

34FDMSStabilization squeal damping factor

Forced Frictional Sliding Using Velocity Input

35TBNDCritical bonding temperature

Using TBND

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

CONTA175 Output Data

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

A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ETABLE, ESOL). The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.

In either the O or R columns, “Y” indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 175.2  CONTA175 Element Output Definitions

NameDefinitionOR
ELElement NumberYY
NODESNodes IYY
XC, YC, (ZC)Location where results are reported (same as nodal location)YY
TEMPTemperature T(I)YY
VOLUAREA for 3-D, Length for 2-DYY
NPINumber of integration pointsY-
ITRGETTarget surface number (assigned by ANSYS)Y-
ISOLIDUnderlying solid or shell element numberY-
CONT:STATCurrent contact statuses11
OLDSTOld contact statuses11
ISEGCurrent contacting target element numberYY
OLDSEGUnderlying old target numberY-
CONT:PENECurrent penetration (gap = 0; penetration = positive value)YY
CONT:GAPCurrent gap (gap = negative value; penetration = 0)YY
NGAPNew or current gap at current converged substep (gap = negative value; penetration = positive value)Y-
OGAPOld gap at previously converged substep (gap = negative value; penetration = positive value)Y-
IGAPInitial gap at start of current substep (gap = negative value; penetration = positive value)YY
GGAPGeometric gap at current converged substep (gap = negative value; penetration = positive value)-Y
CONT:PRESNormal contact pressure22
TAUR/TAUS[8]Tangential contact stresses22
KNCurrent normal contact stiffness (units: Force/Length for contact force model, units: Force/Length3 for contract traction model)55
KTCurrent tangent contact stiffness (same units as KN)55
MU[9]Friction coefficientY-
TASS/TASR[8]Total (algebraic sum) sliding in S and R directions (3-D only)33
AASS/AASR[8]Total (absolute sum) sliding in S and R directions (3-D only)33
TOLNPenetration toleranceYY
CONT:SFRICFrictional stress SQRT (TAUR**2+TAUS**2) (3-D only)22
CONT:STOTALTotal stress SQRT (PRES**2+TAUR**2+TAUS**2) (3-D only)22
CONT:SLIDETotal sliding SQRT (TASS**2+TASR**2) (3-D only)YY
NX, NYSurface normal vector components (2-D only)Y-
CONT:SFRICTangential contact stress (2-D only)22
CONT:SLIDETotal accumulated sliding (algebraic sum) (2-D only)33
ASLIDETotal accumulated sliding (absolute sum) (2-D only)33
FDDISFrictional energy dissipation77
ELSIElastic slip distance for sticking contact within a substep-Y
VRELSlip rate-Y
DBAPenetration variationYY
PINBPinball Region-Y
CONT:CNOSTotal number of contact status changes during substepYY
TNOPMaximum allowable tensile contact pressure22
SLTOAllowable elastic slipYY
CAREAContacting area-Y
DTSTARTLoad step time during debondingYY
DPARAMDebonding parameterYY
DENERIEnergy released due to separation in normal direction - mode I debondingYY
DENERIIEnergy released due to separation in tangential direction - mode II debondingYY
CNFX[4]Contact element force-X component-Y
CNFYContact element force-Y component-Y
CNFZContact element force-Z component (3-D only)-Y
SDAMPSqueal damping coefficient (3-D only)-Y
CONVConvection coefficientYY
RACRadiation coefficientYY
TCCConductance coefficient66
TEMPSTemperature at contact pointYY
TEMPTTemperature at target surfaceYY
FXCVHeat flux due to convectionYY
FXRDHeat flux due to radiationYY
FXCDHeat flux due to conductanceYY
CONT:FLUXTotal heat flux at contact surfaceYY
FXNPFlux input-Y
CNFHContact element heat flow-Y
JCONTContact current density (Current/Unit Area)YY
CCONTContact charge density (Charge/Unit Area)YY
HJOUContact power/areaYY
ECURTCurrent per contact element-Y
ECHARCharge per contact element-Y
ECCElectric contact conductance (for electric current DOF), or electric contact capacitance per unit area (for piezoelectric or electrostatic DOFs)66
VOLTSVoltage on contact nodesYY
VOLTTVoltage on associated targetYY
MCCMagnetic contact permeance66
MFLUXMagnetic flux densityYY
AZS/MAGS2-D/3-D Magnetic potential on contact nodeYY
AZT/MAGT2-D/3-D Magnetic potential on associated targetYY
  1. The possible values of STAT and OLDST are:

    0 = Open and not near contact
    1 = Open but near contact
    2 = Closed and sliding
    3 = Closed and sticking
  2. For the force-based model (KEYOPT(3) = 0), the unit of the quantities is FORCE. For the traction-based model (KEYOPT(3) = 1), the unit is FORCE/AREA.

  3. Only accumulates the sliding when contact occurs.

  4. Contact element forces are defined in the global Cartesian system

  5. For the force-based model, the unit of stiffness is FORCE/LENGTH. For the traction-ased model, the unit is FORCE/LENGTH3.

  6. 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.

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

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

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


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 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 NameETABLE and ESOL Command Input
ItemEI
PRESSMISC131
TAURSMISC-5
TAUSSMISC-9
FLUXSMISC-14
FDDISSMISC-18
FXCVSMISC 22
FXRDSMISC-26
FXCDSMISC-30
FXNPSMISC-34
JCONTSMISC-38
CCONTSMISC-38
HJOUSMISC-42
MFLUXSMISC-46
STAT[1]NMISC411
OLDSTNMISC-5
PENE[2]NMISC-9
DBANMISC-13
TASRNMISC-17
TASSNMISC-21
KNNMISC-25
KTNMISC-29
TOLNNMISC-33
IGAPNMISC-37
PINBNMISC42-
CNFXNMISC43-
CNFYNMISC44-
CNFZNMISC45-
ISEGNMISC-46
AASRNMISC-50
AASSNMISC-54
CAREANMISC58-
MUNMISC-62
DTSTARTNMISC-66
DPARAMNMISC-70
TEMPSNMISC-78
TEMPTNMISC-82
CONVNMISC-86
RACNMISC-90
TCCNMISC-94
CNFHNMISC98-
ECURTNMISC99-
ECHARNMISC99-
ECCNMISC-100
VOLTSNMISC-104
VOLTTNMISC-108
CNOSNMISC-112
TNOPNMISC-116
SLTONMISC-120
MCCNMISC-124
MAGSNMISC-128
MAGTNMISC-132
ELSINMISC-136
DENERINMISC-140
DENERIINMISC-144
GGAPNMISC-152
VRELNMISC-156
SDAMPNMISC-160

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

Output Quantity NameETABLE and ESOL Command Input
ItemEI
PRESSMISC51
SFRICSMISC-3
FLUXSMISC-6
FDDISSMISC-8
FXCVSMISC-10
FXRDSMISC-12
FXCDSMISC-14
FXNPSMISC-16
JCONTSMISC-18
CCONTSMISC-18
HJOUSMISC-20
MFLUXSMISC-22
STAT[1]NMISC191
OLDSTNMISC-3
PENE[2]NMISC-5
DBANMISC-7
SLIDENMISC-9
KNNMISC-11
KTNMISC-13
TOLNNMISC-15
IPENENMISC-17
PINBNMISC20-
CNFXNMISC21-
CNFYNMISC22-
ISEGNMISC-23
CAREANMISC27-
MUNMISC-29
DTSTARTNMISC-31
DPARAMNMISC-33
TEMPSNMISC-37
TEMPTNMISC-39
CONVNMISC-41
RACNMISC-43
TCCNMISC-45
CNFHNMISC47-
ECURTNMISC48-
ECHARNMISC48-
ECCNMISC-49
VOLTSNMISC-51
VOLTTNMISC-53
CNOSNMISC-55
TNOPNMISC-57
SLTONMISC-59
MCCNMISC-61
AZSNMISC-63
AZTNMISC-65
ELSINMISC-67
DENERINMISC-69
DENERIINMISC-71
GGAPNMISC-75
VRELNMISC-77
  1. Element Status = highest value of status of integration points within the element

  2. Penetration = positive value, gap = negative value

You can display or list contact results through several POST1 postprocessor commands. The contact specific items for the PLNSOL, PLESOL, PRNSOL, and PRESOL commands are listed below:

STATContact status
PENEContact penetration
PRESContact pressure for the traction-based model. Contact normal force for the force-based model.
SFRICContact friction stress for the traction-based model. Friction force for the force-based model.
STOTContact total stress (pressure plus friction) for the traction-based model. Total contact force for the force-based model.
SLIDEContact sliding distance
GAPContact gap distance
CNOSTotal number of contact status changes during substep

CONTA175 Assumptions and Restrictions

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

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

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

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

  • In addition, you can use it in modal analyses, eigenvalue buckling analyses, and harmonic analyses. For these analysis types, the program assumes that the initial status of the element (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).

CONTA175 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

ANSYS 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.


Release 14.0 - © 2011 SAS IP, Inc. All rights reserved.