3-D Line-to-Surface Contact
CONTA177 is used to represent contact and sliding between 3-D target surfaces and a deformable line segment, defined by this element. The element is applicable to 3-D beam-to-surface, 3-D shell edge-to-surface, and 3-D beam-to-beam (or edge-to-edge) structural contact analyses. It can be used for both pair-based contact and general contact.
This element is located on the surfaces of 3-D beam or pipe elements with or without midside nodes (such as BEAM188, BEAM189, PIPE288, PIPE289, and ELBOW290). It can also be located on feature edges of 3-D solid elements and perimeter edges of 3-D shell elements, with or without midside nodes (such as SHELL181 and SHELL281). Contact occurs when the element surface penetrates an associated target surface.
In the case of pair-based contact, the target surface is defined by the 3-D target element type, TARGE170. In the case of general contact, the target surface can be defined by CONTA173 and/or CONTA174 elements (for deformable surfaces), CONTA177 elements (for 3-D beams and 3-D edges), or TARGE170 elements (for rigid bodies only).
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 177.1: CONTA177 Geometry. The element is defined by two nodes (if the underlying beam or shell element does not have a midside node) or three nodes (if the underlying beam or shell 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.
Four different scenarios can be modelled by CONTA177:
Contact between one beam (or edge) and the surface of a solid or shell
Internal contact where one beam (or pipe) slides inside another hollow beam (or pipe); see Figure 177.2: Beam Sliding Inside a Hollow Beam
External contact between two beams (or edges) that lie next to each other and are roughly parallel; see Figure 177.3: Parallel Beams in Contact
External contact between two beams (or edges) that cross; see Figure 177.4: Crossing Beams in Contact
KEYOPT(3) controls which of the above scenarios are allowed for the element type, and also controls the contact model used (force-based or traction-based):
Use KEYOPT(3) = 0 for the first three scenarios. The contact condition is only checked at contact nodes. The program reports contact force (contact force-based model).
Use KEYOPT(3) = 1 for the first three scenarios. The contact condition is only checked at contact nodes. The program reports contact pressure (contact traction-based model).
Use KEYOPT(3) = 2 for all scenarios. The contact condition is only checked at contact nodes for the first three scenarios, and on an intersection along the beams for the fourth scenario. The program reports contact pressure (contact traction-based model).
Use KEYOPT(3) = 3 for the fourth scenario. The contact condition is only checked on an intersection along the beams. The program reports contact pressure (contact traction-based model).
Use KEYOPT(3) = 4 for the fourth scenario. The contact condition is only checked on an intersection along the beams. The program reports contact force (contact force-based model).
The units for certain real constants (FKN, FKT, TNOP) and postprocessing items (PRES, TAUR, TAUS, SFRIC, and so on) vary by a factor of AREA, depending on whether the contact force-based model (KEYOPT(3) = 0 or 4) or the contact traction-based model (KEYOPT(3) = 1, 2, or 3) is specified. See the real constant table and output definitions table for details. For more information on using KEYOPT(3) with CONTA177, see KEYOPT(3) in the Contact Technology Guide.
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. CONTA177 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 3-D line contact elements (CONTA177) are associated with 3-D target segment elements (TARGE170) via a shared real constant set. The program looks for contact only between contact and target 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 line 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" (beam or shell edge) must be represented by a contact surface. See Designating Contact and Target Surfaces in the Contact Technology Guide for more information.
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 (CONTA174) on 3-D deformable bodies (on both lower- and higher-order elements); 3-D contact line elements (CONTA177) on 3-D beams, on feature edges of 3-D deformable bodies, and on the perimeter edges of shell structures; and vertex-to-surface elements (CONTA175) on convex corners of 3-D solid bodies and/or shell structures. The general contact definition may also contain target elements (TARGE170) overlaid on the surfaces of standalone rigid bodies and lower-order contact surface elements (CONTA173) overlaid on 3-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 surface 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 "CONTA177 Input Summary" for details.
To model beam-to-beam or edge-to-edge contact, the contact/target surface is assumed to be the surface of a cylinder. For a general beam cross section other than the circular section, you need to estimate an equivalent circular radius. Follow these guidelines to define the equivalent radius:
Determine the smallest cross section along the beam axis.
Determine the largest circle embedded in that cross section.
By default, the program models contact between exterior surfaces of two cylindrical beams for both pair-based and general contact. However, defining contact and target radii differs for the two contact methods.
In a pair-based contact definition, the associated TARGE170 target segment elements are either LINE or PARA segment types. Use the first real constant, R1, to define the equivalent radius on the target side, and use the second real constant, R2, to define the equivalent radius on the contact side. To specify internal beam-to-beam contact (a beam sliding inside a hollow beam, or pipe sliding inside another pipe), set KEYOPT(9) = 1 for the associated TARGE170 element type and input R1 as the inner radius of the outer beam (see Figure 177.2: Beam Sliding Inside a Hollow Beam).
SECID,CONTACT,RADIUS ! Set Type = CONTACT and Subtype = RADIUS for user-defined contact radius SECDATA,
VAL1= equivalent outer radius (external beam-to-beam contact) !
VAL2= equivalent inner radius; also set VAL3 = 1 for internal beam-to-beam
To model internal beam-to-beam contact in a general contact definition,
VAL3 = 1 and input
VAL2 equal to
the inner radius of the outer beam.
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 177.4: Crossing Beams in Contact). Contact occurs for negative values of g.
For beam-to-beam contact modeled with either pair-based contact or general contact, if the contact radius and/or target radius are not defined, the program automatically calculates the equivalent radius for each individual contact/target element based on the associated geometry of underlying elements. As a result, the equivalent radius may vary within a contact pair or within a general contact surface.
For rigid targets, the program cannot compute the target radius since underlying elements do not exist. In this case you must explicitly specify the target radius.
CONTA177 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 for more information.)
For isotropic friction, local element coordinates based on the nodal connectivity are used as principal directions. In the case of two crossing beams in contact, 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 all other cases, the first principal direction points from node I to node J, and 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 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 of the
The contact interaction subroutine
USERINTER is available for
user-defined interface interactions, including interactions in the normal and tangential
directions. 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
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 (Pair-Based) and Line-to-Surface Contact (Pair-Based) discuss CONTA177 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 177.1: CONTA177 Real Constants for descriptions of the real constants.|
|TB command: See Element Support for Material Models for this element.|
|MP command: MU, DMPR|
|Birth and death|
|User-defined contact interaction|
|Section definition for the equivalent beam/edge radius.|
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
Note: For general contact, the GCGEN command automatically sets KEYOPT(2) = 1 (penalty function).
Exclude crossing beam-to-beam contact (contact force-based model) (default)
Exclude crossing beam-to-beam contact (contact traction-based model)
Include all scenarios: beam/edge to surface contact, parallel beam-to-beam contact, and crossing beam-to-beam contact (contact traction-based model)
Crossing beam-to-beam contact (contact traction-based model)
Crossing beam-to-beam contact (contact force-based model)
Note: For general contact, the GCGEN command automatically sets KEYOPT(3) = 2.
Type of surface-based constraint (see Surface-based Constraints for more information):
Rigid surface constraint
Note: KEYOPT(4) is not supported for contact elements used in a general contact definition.
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 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
Note: KEYOPT(7) = 4 is not supported for contact elements used in a general contact definition.
Asymmetric contact selection for beam-to-beam (edge-to-edge) contact:
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.
Shell/beam thickness effect (line-to-surface contact only):
Note: In the case of general contact, the GCGEN command automatically sets KEYOPT(11) = 1 for beam-to-surface contact.
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.
Number of target segments interacting with each contact detection point:
Only one target segment
Up to four target segments
Up to eight target segments
Note: In the case of general contact, the GCGEN command automatically sets KEYOPT(14) = 1 for beam-to-beam 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.
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 177.1: CONTA177 Real Constants
|No.||Name||Description||For more information, see this section in the Contact Technology Guide . . .|
Target radius for cylinder, cone, or sphere, used for line-to-surface contact (rigid target)
|Target radius for beam-to-beam contact||Real constants R1, R2|
Target radius at second node of cone, used for line-to-surface contact (rigid target)
|Contact radius for beam-to-beam contact||Real constants R1, R2|
Penetration tolerance factor
Initial contact closure
Upper limit of initial allowable penetration
Lower limit of initial allowable penetration
Exponential decay coefficient
Allowable elastic slip
Maximum allowable tensile contact force/pressure 
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  |
For the contact force-based model (KEYOPT(3) = 0 or 4), 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 Line-to-Surface Contact Analysis for more information.
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.
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 177.2: CONTA177 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 177.2: CONTA177 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 the program)||Y||-|
|ISOLID||Underlying beam 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 ||Tangential contact forces/stresses||2||2|
|KN||Current normal contact stiffness (units: FORCE/LENGTH for contact force model, FORCE/LENGTH3 for contact traction model)||5||5|
|KT||Current tangent contact stiffness (same units as KN)||5||5|
|MU ||Friction coefficient||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 force/stress, SQRT (TAUR**2+TAUS**2)||2||2|
|CONT:STOTAL||Total force/stress, SQRT (PRES**2+TAUR**2+TAUS**2)||2||2|
|CONT:SLIDE||Amplitude of total accumulated sliding, SQRT (TASS**2+TASR**2)||3||3|
|FDDIS||Frictional energy dissipation||6||6|
|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)||-||9|
|VREL||Equivalent sliding velocity (slip rate)||-||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|
|R1||Target radius for beam-to-beam contact||-||Y|
|R2||Contact radius for beam-to-beam contact||-||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|
|CNFZ ||Contact element force - Z component||-||4|
|CNTX ||Contact element force due to tangential stresses - X component||-||4|
|CNTY ||Contact element force due to tangential stresses - Y component||-||4|
|CNTZ ||Contact element force due to tangential stresses - Z component||-||4|
|SDAMP||Stabilization damping coefficient||-||Y|
|0 = Open and not near contact|
|1 = Open but near contact|
|2 = Closed and sliding|
|3 = Closed and sticking|
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).
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).
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 reference for more information.
output quantity as defined in Table 177.2: CONTA177 Element Output Definitions
predetermined item label for ETABLE command
sequence number for single-valued or constant element data
sequence number for data at nodes I, J, K (contact results for line-to-surface and parallel beams in contact)
sequence number for data of crossing beams in contact (contact results at intersection point)
Table 177.3: CONTA177 (3-D) Item and Sequence Numbers
|Output Quantity Name||ETABLE and ESOL Command Input|
|DENERI or DENER||NMISC||-||140||141||142||143|
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,
N,NMISC,46 returns the
ISEG value for node I of element
|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|
Contact results (I, J, K columns in Table 177.3: CONTA177 (3-D) Item and Sequence Numbers) are reported at contact nodes for 3-D beam-to-surface and parallel beam-to-beam contact. Contact results from crossing beam-to-beam contact (IP column in Table 177.3: CONTA177 (3-D) Item and Sequence Numbers) are reported at an intersection point of two crossing beams. When contact from crossing beams is detected, the associated contact pressure (PRES), the contact frictional stress (SFRIC), and the total stress (STOT) are superimposed on each nodes. Maximum values are reported for other contact results (STAT, PENE, SLIDE, GAP, CNOS).
For line-to-surface contact, the thickness effects of underlying beam elements on the contact side and underlying shell elements on the target side can be taken into account by setting KEYOPT(11) = 1.
This element is nonlinear and requires a full Newton iterative solution, regardless of whether large or small deflections are specified. An exception to this is when MPC bonded contact is specified (KEYOPT(2) = 2 and KEYOPT(12) = 5 or 6).
The normal contact stiffness factor (FKN) must not be so large as to cause numerical instability.
FTOLN, PINB, and FKOP can be changed between load steps or during restart stages.
You can use this element in nonlinear static or nonlinear full transient analyses.
In addition, you can use it in modal analyses, eigenvalue buckling analyses, and harmonic analyses. For these analysis types, the program assumes that the initial status of the element (i.e., the status at the completion of the static prestress analysis, if any) does not change.
When 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
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
Birth and death is not available.
Debonding is not available.
User-defined contact is not available.
User-defined friction is not available.