CONTA172

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

CONTA172 Element Description

CONTA172 represents contact and sliding between 2-D "target" surfaces (TARGE169) and a deformable surface, defined by this element. The element is applicable to 2-D structural and coupled field contact analyses. This element is located on the surfaces of 2-D solid elements with midside nodes (PLANE35, PLANE77, PLANE53, PLANE121, PLANE183, SHELL209, PLANE223, PLANE230, or MATRIX50). It has the same geometric characteristics as the solid element face with which it is connected (see Figure 172.1). Contact occurs when the element surface penetrates one of the target segment elements (TARGE169) 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 CONTA172 in the Mechanical APDL Theory Reference for more details about this element. See Quadratic Elements (Midside Nodes) in the Modeling and Meshing Guide for a discussion concerning midside nodes. Other surface-to-surface contact elements (CONTA171, CONTA173, CONTA174) are also available.

Figure 172.1  CONTA172 Geometry

CONTA172 Geometry

CONTA172 Input Data

The geometry and node locations are shown in Figure 172.1. The element is defined by three nodes (the underlying solid element has midside nodes). If the underlying solid elements do not have midside nodes, use CONTA171 (you may still use CONTA172 but you must drop the midside nodes). The element x-axis is along the I-J line of the element. The correct node ordering of the contact element is critical for proper detection of contact. The nodes must be ordered such that the target must lie to the right side of the contact element when moving from the first contact element node to the second contact element node as in Figure 172.1. See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.

The 2-D contact surface elements are associated with the 2-D target segment elements (TARGE169) 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 with different real constant numbers), or you must combine the two target surfaces into one (both having the same real constant number).

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 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 isotropic friction, use the TB,FRIC,,,,ISO command. You can define a coefficient of friction that is dependent on temperature, time, normal pressure, sliding distance, or sliding relative velocity by using the TBFIELD command along with TB,FRIC,,,,ISO. 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.

This element supports various 2-D stress states, including plane stress, plane strain, and axisymmetric states. The stress state is automatically detected according to the stress state of the underlying element. However, if the underlying element is a superelement, you must use KEYOPT(3) to specify the stress state.

In general, curved contact and target surfaces can be well approximated by quadratic contact and target elements when the mesh is sufficiently refined. However, in certain circumstances (for example, when linear elements are used or when the midside nodes of quadratic elements do not lie exactly on the initial curved geometry because a third party mesh generator was used) using a straight line in place of the true curved geometry can significantly affect the accuracy of contact stresses. An optional geometric correction can be used for a circular (or nearly circular) arc 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 "CONTA172 Input Summary". A general description of element input is given in Element Input.

CONTA172 Input Summary

Nodes

I, J, K

Degrees of Freedom
UX, UY (if KEYOPT(1) = 0)
UX, UY, TEMP (if KEYOPT(1) = 1)
TEMP (if KEYOPT(1) = 2)
UX, UY, TEMP, VOLT (if KEYOPT(1) = 3)
TEMP, VOLT (if KEYOPT(1) = 4)
UX, UY, VOLT (if KEYOPT(1) = 5)
VOLT (if KEYOPT(1) = 6)
AZ (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, , PPCN, FPAT, COR, STRM
FDMN, FDMT, , , TBND
See Table 172.1: CONTA172 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) (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)
Heat Flux, Face 1 (I-J-K)
Special Features
Birth and death
Debonding
Fluid pressure penetration
Isotropic friction
Large deflection
Linear perturbation
Nonlinear
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

1 -- 

UX, UY, TEMP

2 -- 

TEMP

3 -- 

UX, UY, TEMP, VOLT

4 -- 

TEMP, VOLT

5 -- 

UX, UY, VOLT

6 -- 

VOLT

7 -- 

AZ

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)

Stress state when superelements are present:

0 -- 

Use with h-elements (no superelements)

1 -- 

Axisymmetric (use with superelements only)

2 -- 

Plane stress/Plane strain (use with superelements only)

3 -- 

Plane stress with thickness input (use with superelements only)

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)

Beam/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.

Table 172.1  CONTA172 Real Constants

No.NameDescriptionFor more information, see this section in the Contact Technology Guide . . .
1R1

Target circle radius

Defining the Target Surface

2R2

Superelement thickness

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

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

35TBNDCritical bonding temperature

Using TBND

CONTA172 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 172.2: CONTA172 Element Output Definitions gives element output. In the results file, the nodal results are obtained from its closest integration point.

Table 172.2  CONTA172 Element Output Definitions

NameDefinitionOR
ELElement NumberYY
NODESNodes I, JYY
XC, YCLocation where results are reportedY5
TEMPTemperatures T(I), T(J)YY
LENGTHElement lengthY-
VOLUAREAYY
NPINumber of integration pointsY-
ITRGETTarget surface number (assigned by ANSYS)Y-
ISOLIDUnderlying solid, shell, or beam element numberY-
CONT:STATCurrent contact statuses11
OLDSTOld contact statuses11
NX, NYSurface normal vector componentsY-
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 pressureYY
CONT:SFRICTangential contact stressYY
KNCurrent normal contact stiffness (Force/Length3)YY
KTCurrent tangent contact stiffness (Force/Length3)YY
MUFriction coefficientY-
CONT:SLIDETotal accumulated sliding (algebraic sum)33
ASLIDETotal accumulated sliding (absolute sum)33
TOLNPenetration toleranceYY
CONT:STOTALTotal stress SQRT (PRES**2+SFRIC**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
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
  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)


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 172.3: CONTA172 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 172.3: CONTA172 Item and Sequence Numbers:

Name

output quantity as defined in the Table 172.2: CONTA172 Element Output Definitions

Item

predetermined Item label for ETABLE command

E

sequence number for single-valued or constant element data

I,J

sequence number for data at nodes I, J

Table 172.3  CONTA172 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEIJ
PRESSMISC512
SFRICSMISC-34
FLUXSMISC-67
FDDISSMISC-89
FXCVSMISC-1011
FXRDSMISC-1213
FXCDSMISC-1415
FXNPSMISC-1617
JCONTSMISC-1819
CCONTSMISC-1819
HJOUSMISC-2021
STAT[1]NMISC1912
OLDSTNMISC-34
PENE[2]NMISC-56
DBANMISC-78
SLIDENMISC-910
KNNMISC-1112
KTNMISC-1314
TOLNNMISC-1516
IGAPNMISC-1718
PINBNMISC20--
CNFXNMISC21--
CNFYNMISC22--
ISEGNMISC-2324
ASLIDENMISC-2526
CAREANMISC27--
MUNMISC-2930
DTSTARTNMISC-3132
DPARAMNMISC-3334
FPRSNMISC-3536
TEMPSNMISC-3738
TEMPTNMISC-3940
CONVNMISC-4142
RACNMISC-4344
TCCNMISC-4546
CNFHNMISC47--
ECURTNMISC48--
ECHARNMISC48--
ECCNMISC-4950
VOLTSNMISC-5152
VOLTTNMISC-5354
CNOSNMISC-5556
TNOPNMISC-5758
SLTONMISC-5960
ELSINMISC-6768
DENERINMISC-6970
DENERIINMISC-7172
FSTARTNMISC-7374
GGAPNMISC-7576
VRELNMISC-7778
  1. Element Status = highest value of status of integration points within the element

  2. Penetration = positive value, gap = negative value

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

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

CONTA172 Assumptions and Restrictions

  • The 2-D contact element must be defined in an X-Y plane and the Y-axis must be the axis of symmetry for axisymmetric analyses.

  • An axisymmetric structure should be modeled in the +X quadrants.

  • This 2-D contact element works with any 3-D elements in your model.

  • Do not use this element in any model that contains axisymmetric harmonic elements.

  • Node numbering must coincide with the external surface of the underlying solid element or with the original elements comprising the superelement.

  • 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 nodal detection is used and 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).

CONTA172 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 DOF (KEYOPT(1) = 7) is not allowed.

ANSYS Mechanical. 

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


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