CONTA174

3-D 8-Node Surface-to-Surface Contact
MP ME ST PR PRN DS DSS <> EM <> <> PP <> EME MFS

CONTA174 Element Description

CONTA174 is used to represent contact and sliding between 3-D "target" surfaces (TARGE170) and a deformable surface, defined by this element. The element is applicable to 3-D structural and coupled field contact analyses.

The element is located on the surfaces of 3-D solid or shell elements with midside nodes (SOLID87, SOLID90, SOLID98, SOLID122, SOLID123, SOLID186, SOLID187, SOLID226, SOLID227, SOLID231, SOLID232, SHELL132, SHELL281, and MATRIX50).

The element has the same geometric characteristics as the solid or shell element face with which it is connected (see Figure 174.1 below). Contact occurs when the element surface penetrates one of the target segment elements (TARGE170) on a specified target surface. Coulomb friction, shear stress friction, and user-defined friction with the USERFRIC 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.

Figure 174.1  CONTA174 Geometry

CONTA174 Geometry

R = Element x-axis for isotropic friction

xo = Element axis for orthotropic friction if ESYS is not supplied (parallel to global X-axis)

x = Element axis for orthotropic friction if ESYS is supplied

CONTA174 Input Data

The geometry and node locations are shown in Figure 174.1. 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. Remember the target surfaces must always be on its outward normal direction. See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.

The 3-D contact surface elements (CONTA173 and CONTA174) are associated with the 3-D target segment elements (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 two target surfaces into one (targets that share the same real constant numbers).

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 xo 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 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 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.

In general, curved contact and target surfaces can be well approximated by quadratic order contact and target elements. However, in certain circumstances (for example, when the midside nodes do not lie exactly on the initial curved geometry because a third party mesh generator was used), using a faceted surface in place of the true curved geometry can significantly affect the accuracy of contact stresses. An optional geometric correction can be used for two types of curved surfaces (spherical and revolute) via SECTYPE and SECDATA section commands. The defined geometry correction can be applied to specific contact elements via a section ID (SECNUM command). For details, 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.

CONTA174 Input Summary

Nodes

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

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)
MAG (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, PPCN, FPAT, COR, STRM
FDMN, FDMT, FDMD, FDMS, TBND
See Table 174.1: CONTA174 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)
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 LKEY = 1 to specify the pressure values, and use LKEY = 2 to specify starting points and penetrating points.
Convection, Face 1 (I-J-K-L)
Heat Flux, Face 1 (I-J-K-L)
Special Features
Birth and death
Debonding
Fluid pressure penetration
Isotropic friction
Large deflection
Linear perturbation
Nonlinear
Orthotropic friction
Section definition for geometry correction of spherical and revolute surfaces
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 -- 

MAG

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(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. 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) > 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 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:

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(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 varies during iterations (default)

1 -- 

Fluid pressure penetration load remains constant over the substep

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 174.1  CONTA174 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

Chattering Control Parameters

25TOLS 

Target edge extension factor

Selecting Location of Contact Detection

26MCC

Magnetic contact permeance

Modeling Magnetic Contact

27PPCN

Pressure penetration criterion

Specifying a Pressure Penetration Criterion

28FPAT

Fluid penetration acting time

Specifying a Fluid Penetration Acting Time

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

CONTA174 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 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

NameDefinitionOR
ELElement NumberYY
NODESNodes I, J, K, L, M, N, O, PYY
XC, YC, ZCLocation where results are reportedY5
TEMPTemperatures T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P)YY
VOLUAREAYY
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 from 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 pressureYY
TAUR/TAUS[7]Tangential contact stressesYY
KNCurrent normal contact stiffness (Force/Length3)YY
KTCurrent tangent contact stiffness (Force/Length3)YY
MU[8]Friction coefficientY-
TASS/TASR[7]Total (algebraic sum) sliding in S and R directions33
AASS/AASR[7]Total (absolute sum) sliding in S and R directions33
TOLNPenetration toleranceYY
CONT:SFRICFrictional stress SQRT (TAUR**2+TAUS**2)YY
CONT:STOTALTotal stress SQRT (PRES**2+TAUR**2+TAUS**2)YY
CONT:SLIDETotal sliding SQRT (TASS**2 + TASR**2)YY
FDDISFrictional energy dissipation66
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 pressureYY
SLTOAllowable elastic slipYY
CAREAContacting area-Y
CONT:FPRSActual applied fluid penetration pressure-Y
FSTARTFluid penetration starting time-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
CNFXContact element force-X component-4
CNFYContact element force-Y component-Y
CNFZContact element force-Z component-Y
SDAMPSqueal damping coefficient-Y
CONVConvection coefficientYY
RACRadiation coefficientYY
TCCConductance coefficientYY
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)YY
VOLTSVoltage on contact nodesYY
VOLTTVoltage on associated targetYY
MCCMagnetic contact permeanceYY
MFLUXMagnetic flux densityYY
MAGSMagnetic potential on contact nodeYY
MAGTMagnetic 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. ANSYS will evaluate model to detect initial conditions.

  3. Only accumulates the sliding when contact occurs.

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

  5. Available only at centroid as a *GET item.

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

  7. 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.

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


Note:

If ETABLE is used for the CONT items, the reported data is averaged across the element.


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 manual 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 NameETABLE and ESOL Command Input
ItemEIJKL
PRESSMISC131234
TAURSMISC-5678
TAUSSMISC-9101112
FLUXSMISC-14151617
FDDISSMISC-18192021
FXCVSMISC 22232425
FXRDSMISC-26272829
FXCDSMISC-30313233
FXNPSMISC-34353637
JCONTSMISC-38394041
CCONTSMISC-38394041
HJOUSMISC-42434445
MFLUXSMISC-46474849
STAT[1]NMISC411234
OLDSTNMISC-5678
PENE[2]NMISC-9101112
DBANMISC-13141516
TASRNMISC-17181920
TASSNMISC-21222324
KNNMISC-25262728
KTNMISC-29303132
TOLNNMISC-33343536
IGAPNMISC-37383940
PINBNMISC42----
CNFXNMISC43----
CNFYNMISC44----
CNFZNMISC45----
ISEGNMISC-46474849
AASRNMISC-50515253
AASSNMISC-54555657
CAREANMISC58----
MUNMISC-62636465
DTSTARTNMISC-66676869
DPARAMNMISC-70717273
FPRSNMISC-74757677
TEMPSNMISC-78798081
TEMPTNMISC-82838485
CONVNMISC-86878889
RACNMISC-90919293
TCCNMISC-94959697
CNFHNMISC98----
ECURTNMISC99----
ECHARNMISC99----
ECCNMISC-100101102103
VOLTSNMISC-104105106107
VOLTTNMISC-108109110111
CNOSNMISC-112113114115
TNOPNMISC-116117118119
SLTONMISC-120121122123
MCCNMISC-124125126127
MAGSNMISC-128129130131
MAGTNMISC-132133134135
ELSINMISC-136137138139
DENERINMISC-140141142143
DENERIINMISC-144145146147
FSTARTNMISC-148149150151
GGAPNMISC-152153154155
VRELNMISC-156157158159
SDAMPNMISC-160161162163
  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
SFRICContact friction stress
STOTContact total stress (pressure plus friction)
SLIDEContact sliding distance
GAPContact gap distance
FLUXTotal heat flux at contact surface
CNOSTotal number of contact status changes during substep
FPRSActual applied fluid penetration pressure

CONTA174 Assumptions and Restrictions

  • 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 (i.e., the status at the completion of the static prestress analysis, if any) does not change.

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

CONTA174 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 MAG DOF (KEYOPT(1) = 7) is not allowed.

ANSYS Mechanical. 

  • The MAG DOF (KEYOPT(1) = 7) is not allowed.


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