2-D 2-Node Surface-to-Surface Contact
CONTA171 is used to represent contact and sliding between 2-D target surfaces and a deformable surface, defined by this element. The element is applicable to 2-D structural and coupled-field contact analyses. It can be used for both pair-based contact and general contact.
In the case of pair-based contact, the target surface is defined by the 2-D target element type, TARGE169. In the case of general contact, the target surface can be defined by CONTA171 elements (for deformable surfaces) or TARGE169 elements (for rigid bodies only).
The element 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 an associated target surface.
Coulomb friction, shear stress friction, user-defined friction
USERFRIC subroutine, and user-defined
contact interaction with the
are allowed. This element also allows separation of bonded contact
to simulate interface delamination.
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 lies 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.
There are two methods to define a contact interaction: the pair-based contact definition and the general contact definition. Both contact definitions can exist in the same model. CONTA171 can be used in either type of contact definition.
The pair-based contact definition is usually more efficient and more robust than the general contact definition; it supports more options and specific contact features.
In a pair-based contact definition, the 2-D contact surface elements (CONTA171 and CONTA172) are associated with the 2-D target segment elements (TARGE169) via a shared real constant set. The program looks for contact only between surfaces with the same real constant set ID (which is greater than zero). The material ID associated with the contact element is used to specify interaction properties (such as friction coefficient) defined by MP or TB commands.
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). Alternatively, you can combine several target surfaces into one (that is, multiple targets sharing the same real constant number). See Identifying Contact Pairs in the Contact Technology Guide for more information.
For rigid-flexible and 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.
CONTA171 can be used in a general contact definition, although it is not directly generated by the GCGEN command. In a general contact definition, the general contact surfaces are generated automatically by the GCGEN command based on physical parts and geometric shapes in the model. The program overlays contact surface elements (CONTA172) on 2-D deformable bodies (on both lower- and higher-order elements) and vertex-to-surface elements (CONTA175) on convex corners of 2-D solid bodies and/or shell structures. The general contact definition may also contain target elements (TARGE169) overlaid on the surfaces of standalone rigid bodies and lower-order contact surface elements (CONTA171) overlaid on 2-D deformable bodies.
The GCGEN command automatically assigns section IDs and element type IDs for each general contact surface. As a result, each general contact surface consists of contact or target elements that are easily identified by a unique section ID number. The real constant ID and material ID are always set to zero for contact and target elements in the general contact definition.
The program looks for contact interaction among all surfaces and within each surface. You can further control contact interactions between specific surfaces that could potentially be in contact by using the GCDEF command. The material ID and real constant ID input on GCDEF identify interface properties (defined by MP or TB commands) and contact control parameters (defined by the R command) for a specific contact interaction. Unlike a pair-based contact definition, the contact and target elements in the general contact definition are not associated with these material and real constant ID numbers.
If both pair-based contact and general contact are defined in a model, the pair-based contact definitions are preserved, and the general contact definition automatically excludes overlapping interactions wherever pair-based contact exists.
Some element key options are not used or are set automatically for general contact. See the individual KEYOPT descriptions in "CONTA171 Input Summary" 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 Writing Your Own Friction Law (
USERFRIC) in the for
more information on how to use this feature. See also the Guide to User-Programmable Features in the for a detailed description
The contact interaction subroutine
USERINTER is available for
user-defined interface interactions, including interactions in the normal and tangential
directions as well as coupled-field interactions. See Defining Your Own Contact Interaction (
USERINTER) in the for more information on
how to use this feature. See also the Guide to User-Programmable Features in the for a detailed description of the
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.
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.
Two types of geometry correction are available for this element: surface smoothing and bolt thread modeling. Surface smoothing is a geometry correction technique that eliminates inaccuracies introduced by linear elements on a curved (circular or nearly circular) contact surface. Bolt thread modeling provides a method for simulating contact between a threaded bolt and bolt hole without having to model the detailed thread geometry. Both of these geometry correction techniques are implemented through section definitions (SECTYPE, SECDATA, and SECNUM commands). For more information, 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.
Set by KEYOPT(1)
|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, WBID,|
|PCC, PSEE, ABPP, FPFT, FPWT, DCC,|
|See Table 171.1: CONTA171 Real Constants for descriptions of the real constants.|
|TB command: See Element Support for Material Models for this element.|
|MP command: MU, EMIS, DMPR|
|Pressure, Face 1 (I-J) (opposite to contact normal direction);
used for fluid pressure penetration loading. On the SFE command use |
|Convection, Face 1 (I-J)|
|Heat Flux, Face 1 (I-J)|
|Birth and death|
|Fluid pressure penetration|
|User-defined contact interaction|
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.
Selects degrees of freedom:
UX, UY, TEMP
UX, UY, TEMP, VOLT
UX, UY, VOLT
UX, UY, PRES
UX, UY, PRES, TEMP
UX, UY, CONC, TEMP
UX, UY, CONC, TEMP, VOLT
UX, UY, CONC
Note: For general contact, the GCGEN command automatically sets KEYOPT(1) based on the degrees of freedom of the underlying solid or shell elements.
Augmented Lagrangian (default)
Lagrange multiplier on contact normal and penalty on tangent
Pure Lagrange multiplier on contact normal and tangent
Note: For general contact, the GCGEN command automatically sets KEYOPT(2) = 1 (penalty function).
Units of normal contact stiffness:
Note: KEYOPT(3) = 1 is valid only when a penalty-based algorithm is used (KEYOPT(2) = 0 or 1) and the absolute normal contact stiffness value is explicitly specified (that is, a negative value input for real constant FKN).
Note: KEYOPT(3) is not supported for contact elements used in a general contact definition.
If superelements are present in a 2-D model, KEYOPT(3) does not control units of normal contact stiffness. Instead, KEYOPT(3) specifies the stress state as follows: KEYOPT(3) = 1 for axisymmetric; KEYOPT(3) = 2 for plane stress/plane strain with unit thickness; KEYOPT(3) = 3 for plane stress with thickness input. (KEYOPT(3) = 0 indicates no superelements.)
Location of contact detection point:
On Gauss point (for general cases)
On nodal point - normal from contact surface
On nodal point - normal to target surface
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; set KEYOPT(4) = 3 for a coupling 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.
CNOF/ICONT Automated adjustment:
No automated adjustment
Close gap with auto CNOF
Reduce penetration with auto CNOF
Close gap/reduce penetration with auto CNOF
Contact stiffness variation (used to enhance stiffness updating when KEYOPT(10) ≠ 1):
Use default range for stiffness updating
Make a nominal refinement to the allowable stiffness range
Make an aggressive refinement to the allowable stiffness range
Element level time incrementation control / impact constraints:
Automatic bisection of increment
Change in contact predictions made to maintain a reasonable time/load increment
Change in contact predictions made to achieve the minimum time/load increment whenever a change in contact status occurs
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) = 4 is not supported for contact elements used in a general contact definition.
Asymmetric contact selection:
The program internally selects which asymmetric contact pair is used at the solution stage (used only when symmetry contact is defined).
Note: KEYOPT(8) is ignored for contact elements used in a general contact definition. Instead, use the command GCDEF,AUTO to enable auto-asymmetric pairing logic.
Effect of initial penetration or gap:
|Include both initial geometrical penetration or gap and offset|
Exclude both initial geometrical penetration or gap and offset
Include both initial geometrical penetration or gap and offset, but with ramped effects
Include offset only (exclude initial geometrical penetration or gap)
Include offset only (exclude initial geometrical penetration or gap), but with ramped effects
Include offset only (exclude initial geometrical penetration or gap) regardless of the initial contact status (near-field or closed)
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. 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.
Note: KEYOPT(9) is not supported for contact elements used in
a general contact definition. Instead, use the command TBDATA,,
C1 in conjunction with TB,INTER to specify the effect of initial penetration or gap. If TBDATA,,
C1 is not specified,
the default for general contact is to exclude initial penetration/gap
and offset. For more information, see Interaction Options for General Contact Definitions in the Material Reference.
Contact stiffness update:
Each iteration based on the current mean stress of underlying elements. The actual elastic slip does not exceed the maximum allowable limit (SLTO) within a substep.
Each load step if FKN is redefined during the load step.
Each iteration based on the current mean stress of underlying elements. The actual elastic slip never exceeds the maximum allowable limit (SLTO) during the entire solution.
Note: For general contact, the GCGEN command automatically sets KEYOPT(10) = 0.
Beam/Shell thickness effect:
Note: For general contact, the GCGEN command automatically sets KEYOPT(11) = 1.
Behavior of contact surface:
No separation (sliding permitted)
No separation (always)
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.
Note: KEYOPT(12) is not supported for contact elements used
in a general contact definition. Instead, use the command TB,INTER with the appropriate
TBOPT label to specify the behavior at the contact surface. For more information,
see Interaction Options for General Contact Definitions in
the Material Reference.
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:
Fluid pressure penetration load is applied based on the contact status of the current iteration. Any contact detection point which was previously exposed to the fluid pressure remains in the condition of “penetrating” (default).
Fluid pressure penetration load is applied based on the contact status of the last converged substep. Any contact detection point which was previously exposed to the fluid pressure remains in the condition of “penetrating”.
Fluid pressure penetration load is applied based on the contact status of the current iteration. At each iteration, the fluid pressure penetration load is newly applied from the initial starting points.
Fluid pressure penetration load is applied based on the contact status of the last converged substep. At each iteration, the fluid pressure penetration load is newly applied from the initial starting points.
Note: KEYOPT(14) is not supported for contact elements used in a general contact definition.
Effect of contact stabilization damping:
Damping is activated only in the first load step (default).
Deactivate automatic damping.
Damping is activated for all load steps.
Damping is activated at all times regardless of the contact status of previous substeps.
Note: Normal stabilization damping is only applied to the contact element when the current contact status of the contact detection point is near-field. When KEYOPT(15) = 0, 1, or 2, normal stabilization damping is not applied in the current substep if any contact detection point has a closed status. However, when KEYOPT(15) = 3, normal stabilization damping is always applied as long as the current contact status of the contact detection point is near-field. Tangential stabilization damping is automatically activated when normal damping is activated. Tangential damping can also be applied independent of normal damping for sliding contact. See Applying Contact Stabilization Damping in the Contact Technology Guide for more information.
Finite sliding (default). The contacting interface can undergo separation, relative large sliding, and arbitrary rotation.
Small sliding. The contacting interface can undergo only small sliding; arbitrary rotation is permitted.
Table 171.1: CONTA171 Real Constants
|No.||Name||Description||For more information, see this section in the Contact Technology Guide . . .|
Target circle radius
Penetration tolerance factor
Initial contact closure
Upper limit of initial allowable penetration
Lower limit of initial allowable penetration
Frictional heating factor
Heat distribution weighing factor
Modeling Heat Generation Due to Friction (thermal)or
Heat Generation Due to Electric Current (electric)
Joule dissipation weight factor
Exponential decay coefficient
Allowable elastic slip
Maximum allowable tensile contact pressure
Target edge extension factor
Pressure penetration criterion 
Fluid penetration acting time
Coefficient of restitution
Load step number for ramping penetration
|31||FDMN||Normal stabilization damping factor  |
|32||FDMT||Tangential stabilization damping factor  |
|35||TBND||Critical bonding temperature  |
|36||WBID||Internal contact pair ID (used by ANSYS Workbench)|
|37||PCC||Pore fluid contact permeability coefficient  |
|38||PSEE||Pore fluid seepage coefficient  |
|39||ABPP||Ambient pore pressure |
|40||FPFT||Gap pore fluid flow participation factor  |
|41||FPWT||Gap pore fluid flow distribution weighting factor|
|42||DCC||Contact diffusivity coefficient  |
|43||DCON||Diffusive convection coefficient  |
|44||ABDC||Ambient concentration  |
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
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
|NODES||Nodes I, J||Y||Y|
|XC, YC||Location where results are reported||Y||5|
|TEMP||Temperatures T(I), T(J)||Y||Y|
|NPI||Number of integration points||Y||-|
|ITRGET||Target surface number (assigned by the program)||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/Length3)||Y||Y|
|KT||Current tangent contact stiffness (Force/Length3)||Y||Y|
|CONT:SLIDE||Total accumulated sliding (algebraic sum)||3||3|
|ASLIDE||Total accumulated sliding (absolute sum)||3||3|
|CONT:STOTAL||Total stress, SQRT (PRES**2+SFRIC**2)||Y||Y|
|FDDIS||Frictional energy dissipation||6||6|
|ELSI||Total elastic slip distance||-||Y|
|PLSI||Total accumulated plastic slip due to frictional sliding||-||Y|
|GSLID||Algebraic sum sliding||-||7|
|VREL||Sliding velocity (slip rate)||-||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|
|CONT:FPRS||Actual applied fluid penetration pressure||-||Y|
|FSTART||Fluid penetration starting time||-||Y|
|DTSTART||Load step time during debonding||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|
|DENER ||Total energy released due to debonding||Y||Y|
|CNFX ||Contact element force-X component||-||4|
|CNFY ||Contact element force-Y component||-||4|
|CNTX ||Contact element force due to tangential stresses - X component||-||4|
|CNTY ||Contact element force due to tangential stresses - Y component||-||4|
|SDAMP||Stabilization damping coefficient||-||Y|
|WEARX, WEARY||Wear correction - X and Y components||-||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|
|CNFH||Contact element heat flow||-||Y|
|JCONT||Contact current density (Current/Unit Area)||Y||Y|
|CCONT||Contact charge density (Charge/Unit 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|
|PCC||Pore fluid contact permeability coefficient||Y||Y|
|PSEE||Pore fluid seepage coefficient||Y||Y|
|PRESS||Pore pressure on contact nodes||Y||Y|
|PREST||Pore pressure on associated target||Y||Y|
|PFLUX||Pore volume flux density per unit area flow into contact surface||Y||Y|
|EPELX||Pore volume flux per contact element||-||Y|
|DCC||Contact diffusivity coefficient||Y||Y|
|DCON||Diffusive convection coefficient||Y||Y|
|CONCS||Concentration on contact nodes||Y||Y|
|CONCT||Concentration on associated target||Y||Y|
|DFLUX||Diffusion flux density per unit area flow into contact surface||Y||Y|
|EDELX||Diffusion flux per contact element||-||Y|
|0 = Open and not near contact|
|1 = Open but near contact|
|2 = Closed and sliding|
|3 = Closed and sticking|
Available only at centroid as a *GET item.
The contact element force values (CNFX, CNFY) are calculated based on the individual contact element plus the surrounding contact elements. Therefore, the contact force values may not equal the contact element area times the contact pressure (CAREA * PRES).
CNTX and CNTY report the total contact element forces due to tangential stresses. Since CNFX and CNFY report the total contact element forces, the contact element forces due to normal pressure are (CNFX-CNTX) and (CNFY-CNTY).
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 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 reference for more information. The following notation is used in Table 171.3: CONTA171 Item and Sequence Numbers:
Table 171.3: CONTA171 Item and Sequence Numbers
|Output Quantity Name||ETABLE and ESOL Command Input|
|DENERI or DENER||NMISC||-||69||70|
The floating point output format for large integers may lead to incorrect ISEG
values. You should verify the NMISC values via the *GET
command. For example,
returns the ISEG value for node I of element
|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 the global X-Y plane as shown in Figure 171.1: CONTA171 Geometry, 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 (that is, 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.
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 Mechanical Pro
The AZ DOF (KEYOPT(1) = 7) is not available.
Birth and death is not available.
Debonding is not available.
User-defined contact is not available.
User-defined friction is not available.
Linear perturbation is not available.
ANSYS Mechanical Premium
The AZ DOF (KEYOPT(1) = 7) is not available.
Birth and death is not available.
Debonding is not available.
User-defined contact is not available.
User-defined friction is not available.