CONTA175

2D/3D Node-to-Surface Contact

CONTA175 Element Description

CONTA175 may be used to represent contact and sliding between two surfaces (or between a node and a surface, or between a line and a surface) in 2D or 3D. It can be used for both pair-based contact and general contact.

The element is applicable to 2D or 3D structural and coupled field contact analyses. This element is located on the surfaces of solid, beam, and shell elements. 3D solid and shell elements with midside nodes are supported for bonded and no separation contact. For other contact types, lower order solid and shell elements are recommended.

Contact occurs when the element surface penetrates one of the target elements on a specified target surface. In the case of pair-based contact, the target surface is defined by a 2D or 3D target element type, TARGE169 or TARGE170. In the case of general contact, the target surface can be defined by contact elements CONTA172 or CONTA174 for deformable surfaces, or by target elements TARGE169 or TARGE170 for rigid bodies.

Coulomb friction, shear stress friction, user-defined friction with the USERFRIC subroutine, and user-defined contact interaction with the USERINTER subroutine are allowed. This element also allows separation of bonded contact to simulate interface delamination. See CONTA175 in the Mechanical APDL Theory Reference for more details about this element.

Figure 175.1: CONTA175 Geometry

CONTA175 Input Data

The geometry is shown in Figure 175.1: CONTA175 Geometry. The element is defined by one node. The underlying elements can be 2D or 3D solid, shell, or beam elements. CONTA175 represents 2D or 3D contact depending on whether the associated 2D or 3D target segments are used. Contact can occur only when the outward normal direction of the 2D or 3D target surface points to the contact surface. See Generating Contact Elements in the Contact Technology Guide for more information on controlling the outward normal directions via the ESURF command.

Pair-Based Contact versus General Contact

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. CONTA175 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.

Pair-Based Contact

In a pair-based contact definition, the node-to-surface contact elements (CONTA175) are associated with target segment elements (TARGE169 or TARGE170) via a shared real constant set. The program looks for contact interaction 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 numbers). 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.

See Generating Contact Elements in the Contact Technology Guide for information on generating elements automatically using the ESURF command.

General Contact

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 for 2D or CONTA174 for 3D) on deformable bodies (on both lower- and higher-order elements); 3D contact line elements (CONTA177) on 3D beams, on feature edges of 3D deformable bodies, and on perimeter edges of shell structures; and vertex-to-surface elements (CONTA175) on convex corners of 2D or 3D solid bodies and/or shell structures. The general contact definition may also contain target elements (TARGE169 or TARGE170) overlaid on the surfaces of standalone rigid 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.

Some element key options are not used or are set automatically for general contact. See the individual KEYOPT descriptions in "CONTAC175 Input Summary" for details.

Friction

CONTA175 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 Material Reference for more information.)

For isotropic friction, the default element coordinate system (based on node connectivity of the underlying elements) is used. For orthotropic friction, the global coordinate system is used by default, or you may define a local element coordinate system with the ESYS command. The principal directions are computed on the target surface and then projected onto the contact element (node). The first principal direction is defined by projecting the first direction of the chosen coordinate system onto the target surface. The second principal direction is defined by taking a cross product of the first principal direction and the target 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 only the z-direction parallels (or is nearly parallel to) the surface normal.

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 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 Contact Technology Guide for more information on how to use this feature. See also the Guide to User-Programmable Features in the Programmer's Reference for a detailed description of the USERFRIC subroutine.

Other Input

The contact interaction subroutine USERINTER is available for user-defined interface interactions, including interactions in the normal and tangential directions as well coupled-field interactions. See Defining Your Own Contact Interaction (USERINTER) in the Contact Technology Guide for more information on how to use this feature. See also the Guide to User-Programmable Features in the Programmer's Reference for a detailed description of the USERINTER 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.

To model wear at the contact surface, use the TB command with the WEAR label. See Contact Surface Wear in the Contact Technology Guide for more information.

KEYOPT(3) allows you to choose between a contact force-based model (KEYOPT(3) = 0, default) and a contact traction-based model (KEYOPT(3) = 1). The units for certain real constants (FKN, FKT, TNOP, and so on) and postprocessing items (PRES, TAUR, TAUS, SFRIC, and so on) vary by a factor of AREA, depending on which model is specified. (For details, see the real constant table and output definitions table.) For more information on using KEYOPT(3) with CONTA175, see KEYOPT(3) in the Contact Technology Guide.

This element supports a bolt thread modeling technique that simulates contact between a threaded bolt and bolt hole without having to model the detailed thread geometry. Bolt thread modeling is available for 3D models and 2D axisymmetric models and is implemented through section definitions (SECTYPE, SECDATA, and SECNUM commands). For more information, see Simplified Bolt Thread Modeling in the Contact Technology Guide.

See the Contact Technology Guide for a detailed discussion about contact and using the contact elements. Node-to-Surface Contact discusses CONTA175 specifically, including the use of real constants and KEYOPTs.

A summary of the element input is given in "CONTAC175 Input Summary". A general description of element input is given in Element Input.

CONTAC175 Input Summary

Nodes

Degrees of Freedom

Set by KEYOPT(1)

Real Constants

R1, R2, FKN, FTOLN, ICONT, PINB,

PZER, CZER, TAUMAX, CNOF, FKOP, FKT,

COHE, TCC, FHTG, SBCT, RDVF, FWGT,

ECC, FHEG, FACT, DC, SLTO, TNOP,

TOLS, MCC, (Blank), (Blank), COR, STRM,

FDMN, FDMT, FDMD, FDMS, TBND, WBID,

PCC, PSEE, ABPP, FPFT, FPWT, DCC,

DCON, ABDC, , , TFOR, TEND

See Table 175.1: CONTA175 Real Constants for descriptions of the real constants.

Material Properties

TB command: See Element Support for Material Models for this element.

MP command: MU, EMIS, DMPR, DMPS

Special Features

User-defined contact interaction

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, UZ
1 --: UX, UY, UZ, TEMP
2 --: TEMP
3 --: UX, UY, UZ, TEMP, VOLT
4 --: TEMP, VOLT
5 --: UX, UY, UZ, VOLT
6 --: VOLT
7 --: AZ (2D) or MAG (3D)
8 --: UX, UY, UZ, PRES
9 --: UX, UY, UZ, PRES, TEMP
10 --: PRES
11 --: UX, UY, CONC, TEMP
12 --: UX, UY, CONC, TEMP, VOLT
13 --: UX, UY, CONC
14 --: CONC

Note: Only KEYOPT(1) = 0 is supported for CONTA175 elements used in a general contact definition.

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

Note: For general contact, the GCGEN command automatically sets KEYOPT(2) = 1 (penalty function).

KEYOPT(3)

Contact model:

0 --: Contact force-based model (default)
1 --: Contact traction-based model

Note: The traction-based model (KEYOPT(3) = 1) should not be used if the underlying elements are 3D beam or pipe elements.

Note: For general contact, the GCGEN command automatically sets KEYOPT(3) = 1 (traction-based model).

KEYOPT(4)

Standard KEYOPT(4) Usage

Contact normal direction:

0 --: Normal to target surface (default)
1 --: Normal from contact nodes
2 --: Normal from contact nodes (used for shell/beam bottom surface contact when shell/beam thickness is accounted for; KEYOPT(11) = 1)
3 --: Normal to target surface (used for shell/beam bottom surface contact when shell/beam thickness is accounted for; KEYOPT(11) = 1)

Alternate KEYOPT(4) Usage with Surface-Based Constraints

To define a surface-based constraint, set KEYOPT(4) as follows:

0 --: Rigid surface constraint. The rigid surface constraint can be based on either the MPC approach (KEYOPT(2) = 2) or the Lagrange multiplier method (KEYOPT(2) = 3).
1 --: Force-distributed constraint. The force-distributed constraint can be based on either the MPC approach (KEYOPT(2) = 2) or the Lagrange multiplier method (KEYOPT(2) = 3).
3 --: Coupling constraint

For more information, see Surface-Based Constraints in the Contact Technology Guide.

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)

Normal contact stiffness variation (used to enhance stiffness updating when KEYOPT(10) ≠ 1):

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
3 --: Use an exponential pressure-penetration relationship

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) = 4 is not supported for contact elements used in a general contact definition.

KEYOPT(8)

Symmetric contact behavior:

0 --: Both symmetric pairs are active. However, each pair has its own contact characteristics.
1 --: Both symmetric pairs are active and have the same contact characteristics.
2 --: The program internally selects which asymmetric contact pair is used at the solution stage (used only when symmetric contact is defined). However, the contact stiffness of the active contact pair is influenced by the underlying element stiffness of the inactive pair.
3 --: The program internally selects which asymmetric contact pair is used at the solution stage (used only when symmetric contact is defined). The contact characteristics of the active contact pair are completely independent of the inactive pair.

Note: KEYOPT(8) settings are ignored for asymmetric contact pairs and rigid-to-rigid contact pairs.

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.

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. 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.

KEYOPT(10)

Contact Stiffness Update:

0 --: 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.
1 --: Each load step if FKN is redefined during the load step.
2 --: 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.

Note: For general contact, the GCGEN command automatically sets KEYOPT(10) = 0.

KEYOPT(11)

Shell Thickness Effect:

0 --: Exclude
1 --: Include

Note: KEYOPT(11) is applicable to shell elements whose thickness is defined through real constant input or section properties. However, KEYOPT(11) = 1 is not valid when the underlying elements are part of a pre-integrated shell section (SECTYPE,,GENS).

KEYOPT(11) is applicable to beam elements whose thickness is defined through real constant input. However, KEYOPT(11) = 1 is not valid if the thickness of 2D/3D beams is defined through section properties.

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 affect 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.

KEYOPT(13)

Tangential contact stiffness variation only for frictional contact.

0 --: Use the default range for stiffness updating.
1 --: Make an aggressive refinement to the allowable stiffness range.

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: 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.

KEYOPT(16)

Squeal damping controls for interpretation of real constants FDMD and FDMS:

0 --: FDMD and FDMS are scaling factors for destabilizing and stabilizing damping (default).
1 --: FDMD is a constant friction-sliding velocity gradient. FDMS is the stabilization damping coefficient.
2 --: FDMD and FDMS are the destabilizing and stabilization damping coefficients.

Note: KEYOPT(16) is not supported for contact elements used in a general contact definition.

KEYOPT(18)

Sliding behavior:

0 --: Finite sliding (default). The contacting interface can undergo separation, relative large sliding, and arbitrary rotation.
1 --: Small sliding. The contacting interface can undergo only small sliding during the entire solution; arbitrary rotation is permitted.
2 --: Adaptive small sliding. The contact interface can undergo either small sliding or finite sliding within each substep based on the contact status at the beginning of the substep. If the contact status is closed, small sliding is used.

Table 175.1: CONTA175 Real Constants

No.	Name	Description	For more information, see this section in the Contact Technology Guide . . .
1	R1	Target radius for cylinder, cone, or sphere	Defining the Target Surface
2	R2	Target radius at second node of cone	Defining the Target Surface
3	FKN[5]	Normal penalty stiffness factor [1] [2] [3] [7]	Determining Contact Stiffness and Penetration
4	FTOLN	Penetration tolerance factor [7]	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	PZER	Pressure at zero penetration [1] [2]	Pressure-Penetration Relationship (KEYOPT(6) = 3)
8	CZER	Initial contact clearance	Pressure-Penetration Relationship (KEYOPT(6) = 3)
9	TAUMAX	Maximum friction stress [1] [2]	Choosing a Friction Model
10	CNOF	Contact surface offset [1] [2]	Adjusting Initial Contact Conditions
11	FKOP	Contact opening stiffness [1] [2]	Selecting Surface Interaction Models
12	FKT[5]	Tangent penalty stiffness factor [1] [2] [7]	Determining Contact Stiffness
13	COHE	Contact cohesion	Choosing a Friction Model
14	TCC[5]	Thermal contact conductance [1] [2]	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 [1] [2]	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[5]	Electric contact conductance or electric contact capacitance [1] [2] [6]	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 force/pressure [4] [7]	Chattering Control Parameters
25	TOLS	Target edge extension factor	Selecting Location of Contact Detection
26	MCC[5]	Magnetic contact permeance [1] [2]	Modeling Magnetic Contact
29	COR	Coefficient of restitution	Impact Between Rigid Bodies
30	STRM	Load step number for ramping penetration or Starting time for contact stiffness ramping	Modeling Interference Fit
31	FDMN	Normal stabilization damping factor [1] [2]	Applying Contact Stabilization Damping
32	FDMT	Tangential stabilization damping factor [1] [2]	Applying Contact Stabilization Damping
33	FDMD	Destabilization squeal damping factor	Forced Frictional Sliding Using Velocity Input
34	FDMS	Stabilization squeal damping factor	Forced Frictional Sliding Using Velocity Input
35	TBND	Critical bonding temperature [1] [2]	Using TBND
36	WBID	Internal contact pair ID (used by Ansys Workbench)
37	PCC[5]	Pore fluid contact permeability coefficient [1] [2]	Modeling Pore Fluid Flow at the Contact Interface
38	PSEE[5]	Pore fluid seepage coefficient [1] [2]	Modeling Pore Fluid Flow at the Contact Interface
39	ABPP	Ambient pore pressure [1] [2]	Modeling Pore Fluid Flow at the Contact Interface
40	FPFT	Gap pore fluid flow participation factor [1] [2]	Modeling Pore Fluid Flow at the Contact Interface
41	FPWT	Gap pore fluid flow distribution weighting factor	Modeling Pore Fluid Flow at the Contact Interface
42	DCC[5]	Contact diffusivity coefficient [1] [2]	Modeling Diffusion Flow at the Contact Interface
43	DCON[5]	Diffusive convection coefficient [1] [2]	Modeling Diffusion Flow at the Contact Interface
44	ABDC	Ambient concentration [1] [2]	Modeling Diffusion Flow at the Contact Interface
47	TFOR	Pair-based force tolerance	Checking Contact Pair-Based Force Convergence
48	TEND	Ending time for ramping contact stiffness	Modeling Interference Fit

This real constant can be defined as a function of certain primary variables.
This real constant can be defined by the user subroutine USERCNPROP.F.
When CONTA175 is used as part of a forced-distributed constraint and KEYOPT(7) = 2 on the target element (TARGE169 or TARGE170), FKN is used to define weighting factors in tabular format with node number as the primary variable.
For the contact force-based model (KEYOPT(3) = 0), TNOP is the allowable tensile contact force. For the contact traction-based model (KEYOPT(3) = 1), TNOP is the allowable tensile contact pressure.
For the contact force-based model (KEYOPT(3) = 0), the units of this real constant has a factor of AREA with respect to those used in the surface-to-surface contact elements. See Performing a Node-to-Surface Contact Analysis for more information.
ECC is electric contact conductance in a current-based electric analysis, or electric contact capacitance in a charge-based electric analysis (see Modeling Surface Interaction).
When the relaxation option is enabled (KEYOPT(11) = 1 on the TARGE169 or TARGE170 element), FKN and FKT are translational relaxation coefficient and rotational relaxation coefficient, respectively, and tabular input is not supported. In addition, FTOLN and TNOP are translational tolerance and rotational tolerance, respectively.

CONTA175 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 175.2: CONTA175 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 175.2: CONTA175 Element Output Definitions

Name	Definition	O	R
EL	Element Number	Y	Y
NODES	Nodes I	Y	Y
XC, YC, (ZC)	Location where results are reported (same as nodal location)	Y	Y
TEMP	Temperature T(I)	Y	Y
VOLU	AREA for 3D, Length for 2D	Y	Y
NPI	Number of integration points	Y	-
ITRGET	Target surface number (assigned by Mechanical APDL)	Y	-
ISOLID [15]	Underlying solid or shell element number	Y	-
CONT:STAT	Current contact statuses	1	1
OLDST	Old contact statuses	1	1
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 force/pressure	2	2
TAUR/TAUS [8]	Tangential contact forces/stresses	2	2
KN	Current normal contact stiffness (units: Force/Length for contact force-based model, Force/Length³ for contract traction-based model)	5	5
KT	Current tangent contact stiffness (same units as KN)	5	5
MU [9]	Friction coefficient	Y	Y
TASS/TASR [8]	Total (algebraic sum) sliding in S and R directions (3D only)	3	3
AASS/AASR [8]	Total (absolute sum) sliding in S and R directions (3D only)	3	3
TOLN	Penetration tolerance	Y	Y
CONT:SFRIC	Frictional force/stress, SQRT (TAUR2+TAUS2) (3D only)	2	2
CONT:STOTAL	Total force/stress, SQRT (PRES2+TAUR2+TAUS**2) (3D only)	2	2
CONT:SLIDE	Amplitude of total accumulated sliding, SQRT (TASS2+TASR2) (3D only)	3	3
NX, NY	Surface normal vector components (2D only)	Y	-
CONT:SFRIC	Tangential contact force/stress (2D only)	2	2
CONT:SLIDE	Total accumulated sliding (algebraic sum) (2D only)	3	3
ASLIDE	Total accumulated sliding (absolute sum) (2D only)	3	3
FDDIS	Frictional energy dissipation rate	7	7
ELSI	Total equivalent elastic slip distance	-	Y
PLSI	Total (accumulated) equivalent plastic slip due to frictional sliding	-	Y
GSLID	Amplitude of total accumulated sliding (including near-field)	-	10
VREL	Equivalent sliding velocity (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 force/pressure	2	2
SLTO	Allowable elastic slip	Y	Y
CAREA	Contacting area	-	Y
DTSTART	Load step time during debonding	Y	Y
DPARAM	Debonding parameter	Y	Y
DENERI [13]	Energy released due to separation in normal direction - mode I debonding	Y	Y
DENERII [13]	Energy released due to separation in tangential direction - mode II debonding	Y	Y
DENER [14]	Total energy released due to debonding	Y	Y
CNFX [11]	Contact element force-X component	-	4
CNFY [11]	Contact element force-Y component	-	4
CNFZ [11]	Contact element force-Z component (3D only)	-	4
CNTX [12]	Contact element force due to tangential stresses - X component	-	4
CNTY [12]	Contact element force due to tangential stresses - Y component	-	4
CNTZ [12]	Contact element force due to tangential stresses - Z component	-	4
SDAMP	Squeal damping coefficient (3D only) / Stabilization damping coefficient (2D and 3D)	-	Y
WEARX, WEARY, WEARZ	Wear correction - X, Y, and Z components	-	Y
VWEAR	Volume lost due to wear	-	Y
CONV	Convection coefficient	Y	Y
RAC	Radiation coefficient	Y	Y
TCC	Conductance coefficient	6	6
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)	6	6
VOLTS	Voltage on contact nodes	Y	Y
VOLTT	Voltage on associated target	Y	Y
MCC	Magnetic contact permeance	6	6
MFLUX	Magnetic flux density	Y	Y
AZS/MAGS	2D/3D Magnetic potential on contact node	Y	Y
AZT/MAGT	2D/3D Magnetic potential on associated target	Y	Y
PCC	Pore fluid contact permeability coefficient	6	6
PSEE	Pore fluid seepage coefficient	6	6
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	6	6
DCON	Diffusive convection coefficient	6	6
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

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
For the force-based model (KEYOPT(3) = 0), the unit of this quantity is FORCE. For the traction-based model (KEYOPT(3) = 1), the unit is FORCE/AREA.
Only accumulates the sliding for sliding and closed contact (STAT = 2,3).
Contact element forces are defined in the global Cartesian system
For the force-based model, the unit of stiffness is FORCE/LENGTH. For the traction-based model, the unit is FORCE/LENGTH³.
For the traction-based model, the units of TCC, ECC, MCC, PCC, PSEE, DCC, and DCON are the units used for the force-based model per area.
FDDIS = (contact friction stress)*(sliding distance of substep)/(time increment of substep)
For the case of orthotropic friction, components are defined in the global Cartesian system (default) or in the local element coordinate system specified by ESYS.
For orthotropic friction, an equivalent coefficient of friction is output.
Accumulated sliding distance for near-field, sliding, and closed contact (STAT = 1,2,3).
The contact element force values (CNFX, CNFY, CNFZ) 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, CNTY, and CNTZ report the total contact element forces due to tangential stresses. Since CNFX, CNFY, and CNFZ report the total contact element forces, the contact element forces due to normal pressure are (CNFX-CNTX), (CNFY-CNTY), and (CNFZ-CNTZ).
DENERI and DENERII are available only when one of the following material models is used: TB,CZM,,,,CBDD or TB,CZM,,,,CBDE.
DENER is available only when one of the following material models is used: TB,CZM,,,,BILI or TB,CZM,,,,EXPO.
The underlying element (ISOLID) can be obtained by a *GET command following a CNCHECK command. See Designating Contact and Target Surfaces for detail.

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 175.3: CONTA175 (3D) Item and Sequence Numbers and Table 175.4: CONTA175 (2D) Item and Sequence Numbers list outputs 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 the tables below:

Name: output quantity as defined in Table 175.2: CONTA175 Element Output Definitions
Item: predetermined Item label for ETABLE command
E: sequence number for single-valued or constant element data
I: sequence number for data at nodes I

Table 175.3: CONTA175 (3D) Item and Sequence Numbers

Output Quantity Name	ETABLE and ESOL Command Input
Output Quantity Name	Item	E	I
PRES	SMISC	13	1
TAUR	SMISC	-	5
TAUS	SMISC	-	9
FLUX [3]	SMISC	-	14
FDDIS [3]	SMISC	-	18
FXCV [3]	SMISC		22
FXRD [3]	SMISC	-	26
FXCD [3]	SMISC	-	30
FXNP	SMISC	-	34
JCONT/CCONT/PFLUX [3]	SMISC	-	38
HJOU	SMISC	-	42
MFLUX/DFLUX [3]	SMISC	-	46
STAT[1]	NMISC	41	1
OLDST	NMISC	-	5
PENE[2]	NMISC	-	9
DBA	NMISC	-	13
TASR	NMISC	-	17
TASS	NMISC	-	21
KN	NMISC	-	25
KT	NMISC	-	29
TOLN	NMISC	-	33
IGAP	NMISC	-	37
PINB	NMISC	42	-
CNFX	NMISC	43	-
CNFY	NMISC	44	-
CNFZ	NMISC	45	-
CNTX	NMISC	186	-
CNTY	NMISC	187	-
CNTZ	NMISC	188	-
ISEG [4]	NMISC	-	46
AASR	NMISC	-	50
AASS	NMISC	-	54
CAREA	NMISC	58	-
MU	NMISC	-	62
DTSTART	NMISC	-	66
DPARAM	NMISC	-	70
TEMPS	NMISC	-	78
TEMPT	NMISC	-	82
CONV	NMISC	-	86
RAC	NMISC	-	90
TCC	NMISC	-	94
CNFH	NMISC	98	-
ECURT/ECHAR/EPELX	NMISC	99	-
ECC/PCC/PSEE	NMISC	-	100
VOLTS/PRESS	NMISC	-	104
VOLTT/PREST	NMISC	-	108
CNOS	NMISC	-	112
TNOP	NMISC	-	116
SLTO	NMISC	-	120
MCC/DCC	NMISC	-	124
MAGS/CONCS	NMISC	-	128
MAGT/CONCT	NMISC	-	132
ELSI	NMISC	-	136
DENERI or DENER	NMISC	-	140
DENERII	NMISC	-	144
GGAP	NMISC	-	152
VREL	NMISC	-	156
SDAMP	NMISC	-	160
PLSI	NMISC	-	164
GSLID	NMISC	-	168
WEARX	NMISC	-	172
WEARY	NMISC	-	176
WEARZ	NMISC	-	180
VWEAR	NMISC	189	-
EDELX	NMISC	185	-

Table 175.4: CONTA175 (2D) Item and Sequence Numbers

Output Quantity Name	ETABLE and ESOL Command Input
Output Quantity Name	Item	E	I
PRES	SMISC	5	1
SFRIC	SMISC	-	3
FLUX [3]	SMISC	-	6
FDDIS [3]	SMISC	-	8
FXCV [3]	SMISC	-	10
FXRD [3]	SMISC	-	12
FXCD [3]	SMISC	-	14
FXNP	SMISC	-	16
JCONT/CCONT/PFLUX [3]	SMISC	-	18
HJOU	SMISC	-	20
DFLUX [3]	SMISC	-	22
STAT [1]	NMISC	19	1
OLDST	NMISC	-	3
PENE [2]	NMISC	-	5
DBA	NMISC	-	7
SLIDE	NMISC	-	9
KN	NMISC	-	11
KT	NMISC	-	13
TOLN	NMISC	-	15
IPENE	NMISC	-	17
PINB	NMISC	20	-
CNFX	NMISC	21	-
CNFY	NMISC	22	-
CNTX	NMISC	91	-
CNTY	NMISC	92	-
ISEG [4]	NMISC	-	23
CAREA	NMISC	27	-
MU	NMISC	-	29
DTSTART	NMISC	-	31
DPARAM	NMISC	-	33
TEMPS	NMISC	-	37
TEMPT	NMISC	-	39
CONV	NMISC	-	41
RAC	NMISC	-	43
TCC	NMISC	-	45
CNFH	NMISC	47	-
ECURT/ECHAR/EPELX	NMISC	48	-
ECC/PCC/PSEE	NMISC	-	49
VOLTS/PRESS	NMISC	-	51
VOLTT/PREST	NMISC	-	53
CNOS	NMISC	-	55
TNOP	NMISC	-	57
SLTO	NMISC	-	59
DCC	NMISC	-	61
CONCS	NMISC	-	63
CONCT	NMISC	-	65
ELSI	NMISC	-	67
DENERI	NMISC	-	69
DENERII	NMISC	-	71
GGAP	NMISC	-	75
VREL	NMISC	-	77
SDAMP	NMISC	-	79
PLSI	NMISC	-	81
GSLID	NMISC	-	83
WEARX	NMISC	-	85
WEARY	NMISC	-	87
VWEAR	NMISC	93	-
EDELX	NMISC	90	-

Element Status = highest value of status of integration points within the element
Penetration = positive value, gap = negative value
A positive value of flux corresponds to flow into the contact surface.
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, *GET,Par,ELEM,N,NMISC,46 (for the 3D element) returns the ISEG value for node I of element N.

You can display or list contact results through several POST1 postprocessor commands. The contact specific items for the PLETAB, PRNSOL, and PRESOL commands are listed below:

STAT	Contact status
PENE	Contact penetration
PRES	Contact pressure for the traction-based model. Contact normal force for the force-based model.
SFRIC	Contact friction stress for the traction-based model. Friction force for the force-based model.
STOT	Contact total stress (pressure plus friction) for the traction-based model. Total contact force for the force-based model.
SLIDE	Contact sliding distance
GAP	Contact gap distance
CNOS	Total number of contact status changes during substep

CONTA175 Assumptions and Restrictions

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 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.
Only damping defined via KEYOPT(15) is supported. All other damping specifications (Rayleigh damping, DMPSTR, and so on) are not supported.
Certain contact features are not supported when this element is used in a general contact definition. For details, see General Contact in the Contact Technology Guide.

CONTA175 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 Mechanical Pro —

The AZ (2D) and MAG (3D) DOFs (KEYOPT(1) = 7) are not available.
Birth and death is not available.
Debonding is not available.
User-defined contact is not available.
User-defined friction is not available.

Ansys Mechanical Premium —

The AZ (2D) and MAG (3D) DOFs (KEYOPT(1) = 7) are not available.
Debonding is not available.
User-defined contact is not available.
User-defined friction is not available.