CONTA174 is used to represent contact and sliding between 3-D "target" surfaces (TARGE170) and a deformable surface, defined by this element. The element is applicable to 3-D structural and coupled field contact analyses.
The element is located on the surfaces of 3-D solid or shell elements with midside nodes (SOLID87, SOLID90, SOLID98, SOLID122, SOLID123, SOLID186, SOLID187, SOLID226, SOLID227, SOLID231, SOLID232, SHELL132, SHELL281, and MATRIX50).
The element has the same geometric characteristics as the solid or shell element face with which it is connected (see Figure 174.1 below). Contact occurs when the element surface penetrates one of the target segment elements (TARGE170) on a specified target surface. Coulomb friction, shear stress friction, and user-defined friction with the USERFRIC subroutine are allowed. The element also allows separation of bonded contact to simulate interface delamination.
The geometry and node locations are shown in Figure 174.1. The element is defined by eight nodes (the underlying solid or shell element has midside nodes). It can degenerate to a six node element depending on the shape of the underlying solid or shell elements. If the underlying solid or shell elements do not have midside nodes, use CONTA173 (you may still use CONTA174 but you must drop all midside nodes). See Quadratic Elements (Midside Nodes) in the Modeling and Meshing Guide for more information on the use of midside nodes. The node ordering is consistent with the node ordering for the underlying solid or shell element. The positive normal is given by the right-hand rule going around the nodes of the element and is identical to the external normal direction of the underlying solid or shell element surface. For shell elements, the same nodal ordering between shell and contact elements defines upper surface contact; otherwise, it represents bottom surface contact. Remember the target surfaces must always be on its outward normal direction. See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.
The 3-D contact surface elements (CONTA173 and CONTA174) are associated with the 3-D target segment elements (TARGE170) via a shared real constant set. ANSYS looks for contact only between surfaces with the same real constant set. For 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 two target surfaces into one (targets that share the same real constant numbers).
CONTA174 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 applicable coordinate system is the default element coordinate system (noted by the R and S axes in the above figure).
For orthotropic friction, the principal directions are determined as follows. The global coordinate system is used by default, or you may define a local element coordinate system with the ESYS command. (These are depicted by the xo and x axes in the above figure.) The first principal direction is defined by projecting the first direction of the chosen coordinate system onto the contact surface. The second principal direction is defined by taking a cross product of the first principal direction and the contact normal. These directions also follow the rigid body rotation of the contact element to correctly model the directional dependence of friction. Be careful to choose the coordinate system (global or local) so that the first direction of that system is within 45° of the tangent to the contact surface.
If you want to set the coordinate directions for isotropic friction (to the global Cartesian system or another system via ESYS), you can define orthotropic friction and set MU1 = MU2.
To define a coefficient of friction for isotropic or orthotropic friction that is dependent on temperature, time, normal pressure, sliding distance, or sliding relative velocity, use the TBFIELD command along with TB,FRIC. See Contact Friction in the 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.
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.
In general, curved contact and target surfaces can be well approximated by quadratic order contact and target elements. However, in certain circumstances (for example, when the midside nodes do not lie exactly on the initial curved geometry because a third party mesh generator was used), using a faceted surface in place of the true curved geometry can significantly affect the accuracy of contact stresses. An optional geometric correction can be used for two types of curved surfaces (spherical and revolute) 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 "CONTA174 Input Summary". A general description of element input is given in Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.
I, J, K, L, M, N, O, P
|UX, UY, UZ (if KEYOPT(1) = 0)|
|UX, UY, UZ, TEMP (if KEYOPT(1) = 1)|
|TEMP (if KEYOPT(1) = 2)|
|UX, UY, UZ, TEMP, VOLT (if KEYOPT(1) = 3)|
|TEMP, VOLT (if KEYOPT(1) = 4)|
|UX, UY, UZ, VOLT (if KEYOPT(1) = 5)|
|VOLT (if KEYOPT(1) = 6)|
|MAG (if KEYOPT(1) = 7)|
|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, MCC, PPCN, FPAT, COR, STRM|
|FDMN, FDMT, FDMD, FDMS, TBND|
|See Table 174.1: CONTA174 Real Constants for descriptions of the real constants.|
|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)|
|Pressure, Face 1 (I-J-K-L) (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-K-L)|
|Heat Flux, Face 1 (I-J-K-L)|
|Birth and death|
|Fluid pressure penetration|
|Section definition for geometry correction of spherical and revolute surfaces|
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, UZ
UX, UY, UZ, TEMP
UX, UY, UZ, TEMP, VOLT
UX, UY, UZ, VOLT
Augmented Lagrangian (default)
Lagrange multiplier on contact normal and penalty on tangent
Pure Lagrange multiplier on contact normal and tangent
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)
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.
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) > 0):
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
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.
Asymmetric contact selection:
ANSYS internally selects which asymmetric contact pair is used at the solution stage (used only when symmetry contact is defined).
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)
Contact stiffness update:
Each load step if FKN is redefined during load step (pair based).
Each iteration based on current mean stress of underlying elements (pair based).
Shell thickness effect:
Behavior of contact surface:
No separation (sliding permitted)
No separation (always)
Bonded (initial contact)
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 varies during iterations (default)
Fluid pressure penetration load remains constant over the substep
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.
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.
Squeal damping controls for interpretation of real constants FDMD and FDMS:
FDMD and FDMS are scaling factors for destabilizing and stabilizing damping (default).
FDMD is a constant friction-sliding velocity gradient. FDMS is the stabilization damping coefficient.
FDMD and FDMS are the destabilizing and stabilization damping coefficients.
Table 174.1 CONTA174 Real Constants
|No.||Name||Description||For more information, see this section in the Contact Technology Guide . . .|
Target radius for cylinder, cone, or sphere
Target radius at second node of cone
Normal penalty stiffness factor
Penetration tolerance factor
Initial contact closure
Upper limit of initial allowable penetration
Lower limit of initial allowable penetration
Maximum friction stress
Contact surface offset
Contact opening stiffness
Tangent penalty stiffness factor
Thermal contact conductance
Frictional heating factor
Radiation view factor
Heat distribution weighing factor
Modeling Heat Generation Due to Friction (thermal)or
Heat Generation Due to Electric Current (electric)
Electric contact conductance
Joule dissipation weight factor
Exponential decay coefficient
Allowable elastic slip
Maximum allowable tensile contact pressure
Target edge extension factor
Magnetic contact permeance
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|
|33||FDMD||Destabilization squeal damping factor|
|34||FDMS||Stabilization squeal 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 174.2: CONTA174 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 174.2: CONTA174 Element Output Definitions gives element output. In the results file, the nodal results are obtained from its closest integration point.
Table 174.2 CONTA174 Element Output Definitions
|NODES||Nodes I, J, K, L, M, N, O, P||Y||Y|
|XC, YC, ZC||Location where results are reported||Y||5|
|TEMP||Temperatures T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P)||Y||Y|
|NPI||Number of integration points||Y||-|
|ITRGET||Target surface number (assigned by ANSYS)||Y||-|
|ISOLID||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 from 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|
|TAUR/TAUS||Tangential contact stresses||Y||Y|
|KN||Current normal contact stiffness (Force/Length3)||Y||Y|
|KT||Current tangent contact stiffness (Force/Length3)||Y||Y|
|TASS/TASR||Total (algebraic sum) sliding in S and R directions||3||3|
|AASS/AASR||Total (absolute sum) sliding in S and R directions||3||3|
|CONT:SFRIC||Frictional stress SQRT (TAUR**2+TAUS**2)||Y||Y|
|CONT:STOTAL||Total stress SQRT (PRES**2+TAUR**2+TAUS**2)||Y||Y|
|CONT:SLIDE||Total sliding SQRT (TASS**2 + TASR**2)||Y||Y|
|FDDIS||Frictional energy dissipation||6||6|
|ELSI||Elastic slip distance for sticking contact within a substep||-||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|
|CNFX||Contact element force-X component||-||4|
|CNFY||Contact element force-Y component||-||Y|
|CNFZ||Contact element force-Z component||-||Y|
|SDAMP||Squeal damping coefficient||-||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|
|MCC||Magnetic contact permeance||Y||Y|
|MFLUX||Magnetic flux density||Y||Y|
|MAGS||Magnetic potential on contact node||Y||Y|
|MAGT||Magnetic potential on associated target||Y||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.
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.
If ETABLE is used for the CONT items, the reported data is averaged across the element.
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 174.3: CONTA174 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 174.3: CONTA174 Item and Sequence Numbers:
Table 174.3 CONTA174 Item and Sequence Numbers
|Output Quantity Name||ETABLE and ESOL Command Input|
|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 3-D contact element must coincide with the external surface of the underlying solid or shell element.
This element is nonlinear and requires a full Newton iterative solution, regardless of whether large or small deflections are specified. An exception to this is when MPC bonded contact is specified (KEYOPT(2) = 2 and KEYOPT(12) = 5 or 6).
The normal contact stiffness factor (FKN) must not be so large as to cause numerical instability.
FTOLN, PINB, and FKOP can be changed between load steps or during restart stages.
You can use this element in nonlinear static or nonlinear full transient analyses.
In addition, you can use it in modal analyses, eigenvalue buckling analyses, and harmonic analyses. For these analysis types, the program assumes that the initial status of the element (i.e., the status at the completion of the static prestress analysis, if any) does not change.
The USERFRIC subroutine (user-defined friction) can only be used with penalty-based tangential contact (i.e., 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.
The MU material property is not allowed
The birth and death special feature is not allowed.
The VOLT DOF (KEYOPT(1) = 3 through 6) is not allowed.
The MAG DOF (KEYOPT(1) = 7) is not allowed.
The MAG DOF (KEYOPT(1) = 7) is not allowed.