CONTA176 is used to represent contact and sliding between 3-D line segments (TARGE170) and a deformable line segment, defined by this element. The element is applicable to 3-D beam-beam structural contact analyses. This element is located on the surfaces of 3-D beam or pipe elements with or without midside nodes (such as BEAM188 or BEAM189). Contact occurs when the element surface penetrates one of the 3-D straight line or parabolic line segment elements (TARGE170) 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 CONTA176 in the Mechanical APDL Theory Reference for more details about this element. To model beam-to-surface contact, use the line-to-surface contact element, CONTA177.
The geometry and node locations are shown in Figure 176.1. The element is defined by two nodes (if the underlying beam element does not have a midside node) or three nodes (if the underlying beam element has a midside node). The element x-axis is along the I-J line of the element. Correct node ordering of the contact element is critical for proper detection of contact. The nodes must be ordered in a sequence that defines a continuous line. See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.
Three different scenarios can be modeled by CONTA176:
Use KEYOPT(3) = 0 for the first two scenarios (internal contact and parallel beams). In both cases, the contact condition is only checked at contact nodes.
Use KEYOPT(3) = 1 for the third scenario (beams that cross). In this case, the contact condition is checked along the entire length of the beams. The beams with circular cross sections are assumed to come in contact in a point-wise manner. Each contact element can potentially contact no more than one target element.
The 3-D line-to-line contact elements are associated with the target line segment elements (LINE or PARA segment types for TARGE170) via a shared real constant set. The contact/target surface is assumed to be the surface of a cylinder. For a general beam cross section, use an equivalent circular beam (see Figure 176.5). Use the first real constant, R1, to define the radius on the target side (target radius rt). Use the second real constant, R2, to define the radius on the contact side (contact radius rc). Follow these guidelines to define the equivalent circular cross section:
Determine the smallest cross section along the beam axis.
Determine the largest circle embedded in that cross section.
The target radius can be entered as either a negative or positive value. Use a negative value when modeling internal contact (a beam sliding inside a hollow beam, or pipe sliding inside another pipe), with the input value equal to the inner radius of the outer beam (see Figure 176.2). Use a positive value when modeling contact between the exterior surfaces of two cylindrical beams.
For the case of internal contact, the inner beam should usually be considered the contact surface and the outer beam should be the target surface. The inner beam can be considered as the target surface only when the inner beam is much stiffer than the outer beam.
Contact is detected when two circular beams touch or overlap each other. The non-penetration condition for beams with a circular cross section can be defined as follows.
For internal contact:
and for external contact:
where rc and rt are the radii of the cross sections of the beams on the contact and target sides, respectively; and d is the minimal distance between the two beams which also determines the contact normal direction (see Figure 176.4). Contact occurs for negative values of g.
ANSYS looks for contact only between contact and target 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 beam 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).
CONTA176 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, local element coordinates based on the nodal connectivity are used to define principal directions. In the case of two crossing beams in contact (KEYPT(3) = 1), the first principal direction is defined by 1/2(t1 + t2). The first vector, t1, points from the first contact node to the second contact node, and the second vector, t2, points from the first target node to the second target node. In the case of two parallel beams in contact (KEYOPT(3) = 0), the first principal direction points from the first contact node to the second contact node. In both cases, the second principal direction is defined by taking a cross product of the first principal direction and the contact normal.
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. The first principal direction is defined by projecting the first direction of the chosen coordinate system onto the contact element. 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 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.
See the Contact Technology Guide for a detailed discussion on contact and using the contact elements. "3-D Beam-to-Beam Contact" discusses CONTA176 specifically, including the use of real constants and KEYOPTs.
The following table summarizes the element input. Element Input gives a general description of element input.
I, J, (K)
|UX, UY, UZ|
|R1, R2, FKN, FTOLN, ICONT, PINB,|
|PMAX, PMIN, TAUMAX, CNOF, FKOP, FKT,|
|COHE, (Blank), (Blank), (Blank), (Blank), (Blank),|
|(Blank), (Blank), FACT, DC, SLTO, TNOP,|
|TOLS, (Blank), (Blank), (Blank), COR, STRM|
|FDMN, FDMT, , , TBND|
|See Table 176.1: CONTA176 Real Constants for descriptions of the real constants.|
|MU (MP command)|
|FRIC (TB command; see Contact Friction in the )|
|CZM (TB command; see Cohesive Zone Materials Used for Debonding in the Contact Technology Guide)|
|Birth and death|
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. Currently, the default (UX, UY, UZ) is the only valid option:
UX, UY, UZ
Augmented Lagrangian (default)
Lagrange multiplier on contact normal and penalty on tangent
Pure Lagrange multiplier on contact normal and tangent
Beam contact type:
Parallel beams or beam inside beam
Type of surface-based constraint (see Surface-based Constraints for more information):
Rigid surface constraint
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 are 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).
Behavior of contact surface:
No separation (sliding permitted)
No separation (always)
Bonded (initial contact)
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.
Table 176.1 CONTA176 Real Constants
|No.||Name||Description||For more information, see this section in the Contact Technology Guide . . .|
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
Exponential decay coefficient
Allowable elastic slip
Maximum allowable tensile contact force
Target edge extension factor
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|
The units of real constants FKN and FKT have a factor of AREA with respect to those used in the surface-to-surface contact elements. See Performing a 3-D Beam-to-Beam Contact Analysis for more information.
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 176.2: CONTA176 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 176.2 CONTA176 Element Output Definitions
|NODES||Nodes I, J, K||Y||Y|
|XC, YC, ZC||Location where results are reported (same as nodal location)||Y||Y|
|NPI||Number of integration points||Y||-|
|ITRGET||Target surface number (assigned by ANSYS)||Y||-|
|ISOLID||Underlying beam 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||2||2|
|TAUR/TAUS||Tangential contact stresses||2||2|
|KN||Current normal contact stiffness (units: Force/Length)||5||5|
|KT||Current tangent contact stiffness (same units as KN)||5||5|
|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)||2||2|
|CONT:STOTAL||Total stress SQRT (PRES**2+TAUR**2+TAUS**2)||2||2|
|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 force||2||2|
|SLTO||Allowable elastic slip||Y||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||-||Y|
|CNFY||Contact element force-Y component||-||Y|
|CNFZ||Contact element force-Z component||-||Y|
|0 = Open and not near contact|
|1 = Open but near contact|
|2 = Closed and sliding|
|3 = Closed and sticking|
Contact results (including all element results) are generally not reported for elements that have a status of “open and not near contact” (far-field).
The following table 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.
Table 176.3 CONTA176 (3-D) Item and Sequence Numbers
|Output Quantity Name||ETABLE and ESOL Command Input|
The main restriction is the assumption of constant circular beam cross section. The contact radius is assumed to be the same for all elements in the contact pair.
For KEYOPT(3) = 1 (crossing beams), contact between the beams is pointwise, and each contact element contacts no more than one target 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.