CONTA171

www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS

CONTA171

2-D 2-Node Surface-to-Surface Contact

MP ME ST PR PRN DS DSS <> EM <> <> PP <>

CONTA171 Element Description

CONTA171 is used to represent 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, shell, or beam elements without midside nodes (PLANE42, PLANE67, PLANE182, VISCO106, SHELL208, BEAM3, BEAM23, PLANE13, PLANE55, or MATRIX50). It has the same geometric characteristics as the solid, shell, or beam element face with which it is connected (see Figure 171.1: "CONTA171 Geometry"). Contact occurs when the element surface penetrates one of the target segment elements (TARGE169) on a specified target surface. Coulomb and shear stress friction is allowed. This element also allows separation of bonded contact to simulate interface delamination. See CONTA171 in the Theory Reference for ANSYS and ANSYS Workbench for more details about this element. Other surface-to-surface contact elements (CONTA172, CONTA173, CONTA174) are also available.

Figure 171.1 CONTA171 Geometry

CONTA171 Input Data

The geometry and node locations are shown in Figure 171.1: "CONTA171 Geometry". The element is defined by two nodes (the underlying solid, shell, or beam element has no midside nodes). If the underlying solid, shell, or beam elements do have midside nodes, use CONTA172. 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 171.1: "CONTA171 Geometry". 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 modeling 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) = 4, 5, or 6, use the TB command with the CZM label. See " Debonding" in the Contact Technology Guide for more information.

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.

A summary of the element input is given in "CONTA171 Input Summary". A general description of element input is given in Element Input. For axisymmetric applications see Axisymmetric Elements.

CONTA171 Input Summary

Nodes

I, J

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

See Table 171.1: "CONTA171 Real Constants" for descriptions of the real constants.

Material Properties

DAMP, MU, EMIS (MP command)

CZM (TB command; see Cohesive Zone Materials Used for Debonding in the Contact Technology Guide)

Surface Loads

Convection, Face 1 (I-J)

Heat Flux, Face 1 (I-J)

Special Features

Nonlinear

Large deflection

Debonding

Birth and death

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

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.

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:

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

Note

For KEYOPT(7) = 2 or 3, includes automatic bisection of increment. Activated only if SOLCONTROL,ON,ON at the procedure level.

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

Note

For KEYOPT(9) = 1, 3, or 4, the indicated initial gap effect is considered only if KEYOPT(12) = 4 or 5.

KEYOPT(10)

Contact stiffness update:

0 --: Each load step if FKN is redefined during load step (pair based).
1 --: Each substep based on mean stress of underlying elements from the previous substep (pair based).
2 --: Each iteration based on current mean stress of underlying elements (pair based).
3 --: Each load step if FKN is redefined during load step (individual element based).
4 --: Each substep based on mean stress of underlying elements from the previous substep (individual element based).
5 --: Each iteration based on current mean stress of underlying elements (individual element based).

Note

KEYOPT(10) = 0, 1, and 2 are pair based, meaning that the stiffness and settings for ICONT, FTOLN, PINB, PMAX, and PMIN are averaged across all the contact elements in a contact pair. For KEYOPT(10) = 3, 4, and 5, the stiffness and settings are based on each individual contact element (geometry and material behaviors).

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.

Table 171.1 CONTA171 Real Constants

No.	Name	Description	For more information, see this section in the Contact Technology Guide . . .
1	R1	Target circle radius	Defining the Target Surface
2	R2	Superelement thickness	Defining the Target Surface
3	FKN	Normal penalty stiffness factor	Determining Contact Stiffness and Penetration
4	FTOLN	Penetration tolerance factor	Determining Contact Stiffness and Penetration
5	ICONT	Initial contact closure	Adjusting Initial Contact Conditions
6	PINB	Pinball region	Determining Contact Status and the Pinball Region or Defining Influence Range (PINB)
7	PMAX	Upper limit of initial allowable penetration	Adjusting Initial Contact Conditions
8	PMIN	Lower limit of initial allowable penetration	Adjusting Initial Contact Conditions
9	TAUMAX	Maximum friction stress	Choosing a Friction Model
10	CNOF	Contact surface offset	Adjusting Initial Contact Conditions
11	FKOP	Contact opening stiffness or contact damping	Selecting Surface Interaction Models
12	FKT	Tangent penalty stiffness factor	Determining Contact Stiffness
13	COHE	Contact cohesion	Choosing a Friction Model
14	TCC	Thermal contact conductance	Modeling Conduction
15	FHTG	Frictional heating factor	Modeling Heat Generation Due to Friction
16	SBCT	Stefan-Boltzmann constant	Modeling Radiation
17	RDVF	Radiation view factor	Modeling Radiation
18	FWGT	Heat distribution weighing factor	Modeling Heat Generation Due to Friction (thermal) or Heat Generation Due to Electric Current (electric)
19	ECC	Electric contact conductance	Modeling Surface Interaction
20	FHEG	Joule dissipation weight factor	Heat Generation Due to Electric Current
21	FACT	Static/dynamic ratio	Static and Dynamic Friction Coefficients
22	DC	Exponential decay coefficient	Static and Dynamic Friction Coefficients
23	SLTO	Allowable elastic slip	Using FKT and SLTO
24	TNOP	Maximum allowable tensile contact pressure	Chattering Control Parameters
25	TOLS	Target edge extension factor	Selecting Location of Contact Detection

CONTA171 Output Data

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

Nodal displacements included in the overall nodal solution
Additional element output as shown in Table 171.2: "CONTA171 Element Output Definitions"

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

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates 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 a - indicates that the item is not available.

Table 171.2: "CONTA171 Element Output Definitions" gives element output. In the results file, the nodal results are obtained from its closest integration point.

Table 171.2 CONTA171 Element Output Definitions

Name	Definition	O	R
EL	Element Number	Y	Y
NODES	Nodes I, J	Y	Y
XC, YC	Location where results are reported	Y	5
TEMP	Temperatures T(I), T(J)	Y	Y
LENGTH	Element length	Y	-
VOLU	AREA	Y	Y
NPI	Number of integration points	Y	-
ITRGET	Target surface number (assigned by ANSYS)	Y	-
ISOLID	Underlying solid, shell, or beam element number	Y	-
CONT:STAT	Current contact statuses	1	1
OLDST	Old contact statuses	1	1
NX, NY	Surface normal vector components	Y	-
ISEG	Underlying current target number	Y	Y
OLDSEG	Underlying old target number	Y	-
CONT:PENE	Current penetration (gap = 0; penetration = positive value)	Y	Y
CONT:GAP	Current gap (gap = negative value; penetration = 0)	Y	Y
NGAP	New or current gap at current converged substep (gap = negative value; penetration = positive value)	Y	-
OGAP	Old gap at previously converged substep (gap = negative value; penetration = positive value)	Y	-
IGAP	Initial gap at start of current substep (gap = negative value; penetration = positive value)	Y	Y
CONT:PRES	Normal contact pressure	Y	Y
CONT:SFRIC	Tangential contact stress	Y	Y
KN	Current normal contact stiffness (Force/Length³)	Y	Y
KT	Current tangent contact stiffness (Force/Length³)	Y	Y
MU	Friction coefficient	Y	-
CONT:SLIDE	Total accumulated sliding (algebraic sum)	3	3
CONT:ASLIDE	Total accumulated sliding (absolute sum)	3	3
TOLN	Penetration tolerance	Y	Y
CONT:STOTAL	Total stress SQRT (PRES2+SFRIC2)	Y	Y
DBA	Penetration variation	Y	Y
PINB	Pinball Region	-	Y
CNFX	Contact element force-x component	-	4
CNFY	Contact element force-Y component	-	Y
CONV	Convection coefficient	Y	Y
RAC	Radiation coefficient	Y	Y
TCC	Conductance coefficient	Y	Y
TEMPS	Temperature at contact point	Y	Y
TEMPT	Temperature at target surface	Y	Y
FXCV	Heat flux due to convection	Y	Y
FXRD	Heat flux due to radiation	Y	Y
FXCD	Heat flux due to conductance	Y	Y
FDDIS	Frictional energy dissipation	6	6
FLUX	Total heat flux at contact surface	Y	Y
FXNP	Flux input	-	Y
CNFH	Contact element heat flow	-	Y
CAREA	Contacting area	-	Y
JCONT	Contact current density (Current/Unit Area)	Y	Y
CCONT	Contact charge density (Charge/Unit Area)	Y	Y
HJOU	Contact power/area	Y	Y
ECURT	Current per contact element	-	Y
ECHAR	Charge per contact element	-	Y
ECC	Electric contact conductance (for electric current DOF), or electric contact capacitance per unit area (for piezoelectric or electrostatic DOFs)	Y	Y
VOLTS	Voltage on contact nodes	Y	Y
VOLTT	Voltage on associated target	Y	Y
CNOS	Total number of contact status changes during substep	Y	Y
TNOP	Maximum allowable tensile contact pressure	Y	Y
SLTO	Allowable elastic slip	Y	Y
ELSI	Elastic slip distance for sticking contact within a substep	-	Y
DTSTART	Load step time during debonding	Y	Y
DPARAM	Debonding parameter	Y	Y
DENERI	Energy released due to separation in normal direction - mode I debonding	Y	Y
DENERII	Energy released due to separation in tangential direction - mode II debonding	Y	Y

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
ANSYS will evaluate model to detect initial conditions.
Only accumulates the sliding when contact occurs.
Contact element forces are defined in the global Cartesian system.
Available only at centroid as a *GET item.
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.

Table 171.3: "CONTA171 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 171.3: "CONTA171 Item and Sequence Numbers":

Name: output quantity as defined in the Table 171.2: "CONTA171 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 171.3 CONTA171 Item and Sequence Numbers

Output Quantity Name	ETABLE and ESOL Command Input
Output Quantity Name	Item	E	I	J
PRES	SMISC	5	1	2
SFRIC	SMISC	-	3	4
FLUX	SMISC	-	6	7
FDDIS	SMISC	-	8	9
FXCV	SMISC	-	10	11
FXRD	SMISC	-	12	13
FXCD	SMISC	-	14	15
FXNP	SMISC	-	16	17
JCONT	SMISC	-	18	19
CCONT	SMISC	-	18	19
HJOU	SMISC	-	20	21
STAT[1]	NMISC	19	1	2
OLDST	NMISC	-	3	4
PENE[2]	NMISC	-	5	6
DBA	NMISC	-	7	8
SLIDE	NMISC	-	9	10
KN	NMISC	-	11	12
KT	NMISC	-	13	14
TOLN	NMISC	-	15	16
IGAP	NMISC	-	17	18
PINB	NMISC	20	-	-
CNFX	NMISC	21	-	-
CNFY	NMISC	22	-	-
ISEG	NMISC	-	23	24
ASLIDE	NMISC	-	25	26
CAREA	NMISC	-	27	28
MU	NMISC	-	29	30
DTSTART	NMISC	-	31	32
DPARAM	NMISC	-	33	34
TEMPS	NMISC	-	37	38
TEMPT	NMISC	-	39	40
CONV	NMISC	-	41	42
RAC	NMISC	-	43	44
TCC	NMISC	-	45	46
CNFH	NMISC	47	-	-
ECURT	NMISC	48	-	-
ECHAR	NMISC	48	-	-
ECC	NMISC	-	49	50
VOLTS	NMISC	-	51	52
VOLTT	NMISC	-	53	54
CNOS	NMISC	-	55	56
TNOP	NMISC	-	57	58
SLTO	NMISC	-	59	60
ELSI	NMISC	-	67	68
DENERI	NMISC	-	69	70
DENERII	NMISC	-	71	72

Element Status = highest value of status of integration points within the element
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:

STAT	Contact status
PENE	Contact penetration
PRES	Contact pressure
SFRIC	Contact friction stress
STOT	Contact total stress (pressure plus friction)
SLIDE	Contact sliding distance
GAP	Contact gap distance
FLUX	Total heat flux at contact surface
CNOS	Total number of contact status changes during substep

CONTA171 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, shell, or beam 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.
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.
The value of FKN can be smaller when combined with the Lagrangian multiplier method, for which FTOLN must be used.
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.
This element allows birth and death and will follow the birth and death status of the underlying solid, shell, beam, or target elements.

CONTA171 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.
The DAMP material property 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.