CONTA177

3-D Line-to-Surface Contact
MP ME ST PR PRN <> <> <> <> <> <> PP <> EME MFS

CONTA177 Element Description

CONTA177 is used to represent contact and sliding between 3-D surface segments (TARGE170) and a deformable line segment, defined by this element. The element is applicable to 3-D beam-to-solid and 3-D shell edge-to-solid structural contact analyses. This element is located on the surfaces of 3-D beam or pipe elements with or without midside nodes (such as BEAM188, BEAM189, PIPE288, PIPE289, and ELBOW290). It can also be located on the edge of 3-D shell elements with or without midside nodes, such as SHELL181 and SHELL281. 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. This element also allows separation of bonded contact to simulate interface delamination. See CONTA177 in the Mechanical APDL Theory Reference for more details about this element. To model beam-to-beam contact, use the line-to-line contact element, CONTA176.

Figure 177.1  CONTA177 Geometry

CONTA177 Geometry

CONTA177 Input Data

The geometry and node locations are shown in Figure 177.1. The element is defined by two nodes (if the underlying beam or shell element does not have a midside node) or three nodes (if the underlying beam or shell element has a midside node). The element x-axis is along the I-J line of the element. Correct node ordering of the contact element is critical for proper detection of contact. The nodes must be ordered in a sequence that defines a continuous line. See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.

ANSYS looks for contact only between contact and target surfaces with the same real constant set. For either rigid-flexible or flexible-flexible contact, one of the deformable "surfaces" (beam or shell edge) 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 line 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).

CONTA177 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 Mechanical APDL Material Reference for more information.)

For isotropic friction, local element coordinates based on the nodal connectivity are used as principal directions. The first principal direction points from node I to node J. The second principal direction is defined by taking a cross product of the first principal direction and the contact normal.

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. The first principal direction is defined by projecting the first direction of the chosen coordinate system onto the contact element. 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 Mechanical APDL 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 Mechanical APDL 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.

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. "Line-to-Surface Contact" discusses CONTA177 specifically, including the use of real constants and KEYOPTs.

The following table summarizes the element input. Element Input gives a general description of element input.

CONTA177 Input Summary

Nodes

I, J, (K)

Degrees of Freedom
UX, UY, UZ
Real Constants
R1, R2, FKN, FTOLN, ICONT, PINB,
PMAX, PMIN, TAUMAX, CNOF, FKOP, FKT,
COHE, (Blank), (Blank), (Blank), (Blank), (Blank),
(Blank), (Blank), FACT, DC, SLTO, TNOP,
TOLS, (Blank), (Blank), (Blank), COR, STRM
FDMN, FDMT, , , TBND
See Table 177.1: CONTA177 Real Constants for descriptions of the real constants.
Material Properties
MU (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. Currently, the default (UX, UY, UZ) is the only valid option:

0 -- 

UX, UY, UZ

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)

Type of surface-based constraint (see Surface-based Constraints for more information):

0 -- 

Rigid surface constraint

1 -- 

Force-distributed constraint

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(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 (target side only):

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.

Table 177.1  CONTA177 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[1]

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

Accounting for Thickness Effect (CNOF and KEYOPT(11))

11FKOP

Contact opening stiffness

Selecting Surface Interaction Models

12FKT[1]

Tangent penalty stiffness factor

Determining Contact Stiffness

13COHE

Contact cohesion

Choosing a Friction Model

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 force

Chattering Control Parameters

25TOLS 

Target edge extension factor

Real Constant TOLS

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

  1. The units of real constants FKN and FKT have a factor of AREA with respect to those used in the surface-to-surface contact elements. See Real Constants FKN and FKT for more information.

CONTA177 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 177.2  CONTA177 Element Output Definitions

NameDefinitionOR
ELElement NumberYY
NODESNodes I, J, KYY
XC, YC, ZCLocation where results are reported (same as nodal location)YY
TEMPTemperature T(I)YY
VOLULengthYY
NPINumber of integration pointsY-
ITRGETTarget surface number (assigned by ANSYS)Y-
ISOLIDUnderlying beam 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 force22
TAUR/TAUS[7]Tangential contact stresses22
KNCurrent normal contact stiffness (units: Force/Length) 55
KTCurrent tangent contact stiffness (same units as KN)55
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) 22
CONT:STOTALTotal stress SQRT (PRES**2+TAUR**2+TAUS**2)22
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 force22
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-Y
  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. The unit of the quantities is FORCE.

  3. Only accumulates the sliding when contact occurs.

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

  5. The unit of stiffness is FORCE/LENGTH.

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

  7. For the case of orthotropic friction in contact between beams (or shell edges) and a 3-D surface, components are defined in the global Cartesian system.

  8. 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).

The following table 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.

Name

output quantity as defined in Table 177.2: CONTA177 Element Output Definitions

Item

predetermined item label for ETABLE command

E

sequence number for single-valued or constant element data

I, J, K

sequence number for data at nodes I, J, K

Table 177.3  CONTA177 (3-D) Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEIJK
PRESSMISC13123
TAURSMISC-567
TAUSSMISC-91011
FDDISSMISC-181920
STAT[1]NMISC41123
OLDSTNMISC-567
PENE[2]NMISC-91011
DBANMISC-131415
TASRNMISC-171819
TASSNMISC-212223
KNNMISC-252627
KTNMISC-293031
TOLNNMISC-333435
IGAPNMISC-373839
PINBNMISC42---
CNFXNMISC43---
CNFYNMISC44---
CNFZNMISC45---
ISEGNMISC-464748
AASRNMISC-505152
AASSNMISC-545556
CAREANMISC58---
MUNMISC-626364
DTSTARTNMISC-666768
DPARAMNMISC-707172
CNOSNMISC-112113114
TNOPNMISC-116117118
SLTONMISC-120121122
ELSINMISC-136137138
DENERINMISC-140141142
DENERIINMISC-144145146
GGAPNMISC-152153154
VRELNMISC-156157158
  1. Element Status = highest value of status of integration points within the element

  2. Penetration = positive value, gap = negative value

CONTA177 Assumptions and Restrictions

  • The thickness effects of underlying beam elements on the contact side can be taken into account by specifying the contact surface offset CNOF.

  • The thickness effects of underlying shell elements on the target side can be taken into account by setting KEYOPT(11) = 1.

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

CONTA177 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 (input via MP,MU or TB,FRIC) is not allowed.

  • The birth and death special feature is not allowed.


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