CONTA171

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

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 (such as PLANE13, PLANE55, PLANE182, MATRIX50, and SHELL208). It has the same geometric characteristics
as the solid, shell, or beam element face with which it is connected
(see Figure 171.1). 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 CONTA171 in the *Mechanical APDL Theory Reference* for
more details about this element. Other surface-to-surface contact
elements (CONTA172, CONTA173, CONTA174) are also available.

The geometry and node locations are shown in Figure 171.1. 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. 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) = 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 linear contact and target elements when
the mesh is sufficiently refined. However, using a straight line in
place of the true curved geometry can significantly affect the accuracy
of contact stresses in some contact applications. 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 "CONTA171 Input Summary". A general description of element input is given in Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.

**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, , PPCN, FPAT, COR, STRM FDMN, FDMT, , , TBND See Table 171.1: CONTA171 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) Heat Flux, Face 1 (I-J) **Special Features**Birth and death Debonding Fluid pressure penetration Isotropic friction Large deflection Linear perturbation Nonlinear 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)

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.

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 171.1 CONTA171 Real Constants**

No. | Name | Description | For more information, see this section in the Contact Technology Guide . .
. |
---|---|---|---|

1 | R1 | Target circle radius | |

2 | R2 | Superelement thickness | |

3 | FKN | Normal penalty stiffness factor | |

4 | FTOLN | Penetration tolerance factor | |

5 | ICONT | Initial contact closure | |

6 | PINB | Pinball region | or |

7 | PMAX | Upper limit of initial allowable penetration | |

8 | PMIN | Lower limit of initial allowable penetration | |

9 | TAUMAX | Maximum friction stress | |

10 | CNOF | Contact surface offset | |

11 | FKOP | Contact opening stiffness | |

12 | FKT | Tangent penalty stiffness factor | |

13 | COHE | Contact cohesion | |

14 | TCC | Thermal contact conductance | |

15 | FHTG | Frictional heating factor | |

16 | SBCT | Stefan-Boltzmann constant | |

17 | RDVF | Radiation view factor | |

18 | FWGT | Heat distribution weighing factor | Modeling Heat Generation Due to Friction (thermal) orHeat Generation Due to Electric Current (electric) |

19 | ECC | Electric contact conductance | |

20 | FHEG | Joule dissipation weight factor | |

21 | FACT | Static/dynamic ratio | |

22 | DC | Exponential decay coefficient | |

23 | SLTO | Allowable elastic slip | |

24 | TNOP | Maximum allowable tensile contact pressure | |

25 | TOLS | Target edge extension factor | |

27 | PPCN | Pressure penetration criterion | |

28 | FPAT | Fluid penetration acting time | |

29 | COR | Coefficient of restitution | |

30 | STRM | Load step number for ramping penetration | |

31 | FDMN | Normal stabilization damping factor | |

32 | FDMT | Tangential stabilization damping factor | |

35 | TBND | Critical bonding temperature |

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 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 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 | Current contacting target element 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 |

GGAP | Geometric gap at current converged substep (gap = negative value; penetration = positive value) | - | Y |

CONT:PRES | Normal contact pressure | Y | Y |

CONT:SFRIC | Tangential contact stress | Y | Y |

KN | Current normal contact stiffness (Force/Length^{3}) | Y | Y |

KT | Current tangent contact stiffness (Force/Length^{3}) | Y | Y |

MU | Friction coefficient | Y | - |

CONT:SLIDE | Total accumulated sliding (algebraic sum) | 3 | 3 |

ASLIDE | Total accumulated sliding (absolute sum) | 3 | 3 |

TOLN | Penetration tolerance | Y | Y |

CONT:STOTAL | Total stress SQRT (PRES**2+SFRIC**2) | Y | Y |

FDDIS | Frictional energy dissipation | 6 | 6 |

ELSI | Elastic slip distance for sticking contact within a substep | - | Y |

VREL | Slip rate | - | Y |

DBA | Penetration variation | Y | Y |

PINB | Pinball Region | - | Y |

CONT: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 |

CAREA | Contacting area | - | Y |

CONT:FPRS | Actual applied fluid penetration pressure | - | Y |

FSTART | Fluid penetration starting time | - | 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 |

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 |

CONT:FLUX | Total heat flux at contact surface | Y | Y |

FXNP | Flux input | - | Y |

CNFH | Contact element heat flow | - | 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 |

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 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)

| If |

| 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 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 | |||
---|---|---|---|---|

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 | - | - |

MU | NMISC | - | 29 | 30 |

DTSTART | NMISC | - | 31 | 32 |

DPARAM | NMISC | - | 33 | 34 |

FPRS | NMISC | - | 35 | 36 |

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 |

FSTART | NMISC | - | 73 | 74 |

GGAP | NMISC | - | 75 | 76 |

VREL | NMISC | - | 77 | 78 |

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 |

FPRS | Actual applied fluid penetration pressure |

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. 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 (KEYOPT(2) = 0, 1, or 3).

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.