CONTA176
## CONTA176 Element Description

## CONTA176 Input Data

### CONTA176 Input Summary

## CONTA176 Output Data

## CONTA176 Assumptions and Restrictions

## CONTA176 Product Restrictions

**3-D Line-to-Line
Contact**

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

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, 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 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: CONTA176 Geometry. 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:

Internal contact where one beam (or pipe) slides inside another hollow beam (or pipe) (see Figure 176.2: Beam Sliding Inside a Hollow Beam)

External contact between two beams that lie next to each other and are roughly parallel (see Figure 176.3: Parallel Beams in Contact)

External contact between two beams that cross (see Figure 176.4: Crossing Beams in Contact)

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: Equivalent Circular Cross Section). Use the first real constant, R1, to define
the radius on the target side (target radius r_{t}). Use the second real constant, R2, to define the radius on the
contact side (contact radius r_{c}). 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: Beam Sliding Inside a Hollow Beam). 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 r_{c} and r_{t} 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: Crossing Beams in Contact). Contact occurs for negative values of
g.

When 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 beam elements. In this case, the equivalent radius may vary within a contact pair.

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(**t _{1}
** +

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 Writing Your Own Friction Law (`USERFRIC`

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

subroutine.In addition to the user-defined friction subroutine, 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 Mechanical APDL Contact Technology Guide for more information on how to use
this feature. See also the Guide to User-Programmable Features in the Mechanical APDL 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.

In addition to controlling the type of beam contact, KEYOPT(3)
allows you to choose between a contact force-based model (KEYOPT(3)
= 0 or 1; default = 0) and a contact traction-based model (KEYOPT(3)
= 2 or 3). 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 which model is specified. (For details,
see the real constant table and output definitions table.) For more
information on using KEYOPT(3) with CONTA176, see KEYOPT(3) in the *Contact Technology Guide*.

See the *Contact Technology Guide* for a detailed discussion on contact and using
the contact elements. 3-D Beam-to-Beam Contact (Pair-Based) 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.

**Nodes**I, J, (K)

**Degrees of Freedom**UX, UY, UZ **Real Constants**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. **Material Properties****TB**command: See Element Support for Material Models for this element.**MP**command: MU, DMPR**Special Features**Birth and death Debonding Isotropic friction Large deflection Linear perturbation Nonlinearity Orthotropic friction 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. Currently, the default (UX, UY, UZ) is the only valid option:

**0 --**UX, UY, UZ

**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

**KEYOPT(3)**Beam contact type:

**0 --**Parallel beams or beam inside beam (contact force-based model)

**1 --**Crossing beams (contact force-based model)

**2 --**Parallel beams or beam inside beam (contact traction-based model)

**3 --**Crossing beams (contact traction-based model)

**KEYOPT(4)**Type of surface-based constraint (see Surface-based Constraints for more information):

**0 --**Rigid surface constraint

**1 --**Force-distributed constraint

**3 --**Coupling constraint

**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)**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

**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

**KEYOPT(8)**Asymmetric contact selection:

**0 --**No action

**2 --**ANSYS internally selects which asymmetric contact pair is used at the solution stage (used only when symmetry contact is defined).

**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.**KEYOPT(10)**Contact Stiffness Update:

**0 --**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.

**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 never exceeds the maximum allowable limit (SLTO) during the entire solution.

**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 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.**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(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; arbitrary rotation is permitted.

**Table 176.1: CONTA176 Real Constants**

No. | Name | Description | For more information, see this section in the Contact Technology Guide . .
. |
---|---|---|---|

1 | R1 |
Target radius | |

2 | R2 |
Contact radius | |

3 | FKN[1] | ||

4 | FTOLN |
Penetration tolerance factor | |

5 | ICONT |
Initial contact closure | |

6 | PINB |
Pinball region | or |

7 | PMAX |
Upper limit of initial allowable penetration | |

8 | PMIN |
Lower limit of initial allowable penetration | |

9 | TAUMAX | ||

10 | CNOF | ||

11 | FKOP | ||

12 | FKT[1] | ||

13 | COHE |
Contact cohesion | |

21 | FACT |
Static/dynamic ratio | |

22 | DC |
Exponential decay coefficient | |

23 | SLTO |
Allowable elastic slip | |

24 | TNOP |
Maximum allowable tensile contact force/pressure [4] | |

25 | TOLS |
Target edge extension factor | |

29 | COR |
Coefficient of restitution | |

30 | STRM |
Load step number for ramping penetration | |

31 | FDMN | Normal stabilization damping factor [2] [3] | |

32 | FDMT | Tangential stabilization damping factor [2] [3] | |

35 | TBND | Critical bonding temperature [2] [3] |

For the contact force-based model (KEYOPT(3) = 0 or 1), 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.

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.

For the contact force-based model (KEYOPT(3) = 0 or 1), TNOP is the allowable tensile contact force. For the contact traction-based model (KEYOPT(3) = 2 or 3), TNOP is the allowable tensile contact pressure.

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.

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 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**

Name | Definition | O | R |
---|---|---|---|

EL | Element Number | Y | Y |

NODES | Nodes I, J, K | Y | Y |

XC, YC, ZC | Location where results are reported (same as nodal location) | Y | Y |

TEMP | Temperature T(I) | Y | Y |

VOLU | Length | 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/pressure | 2 | 2 |

TAUR/TAUS [7] | Tangential contact forces/stresses | 2 | 2 |

KN | Current normal contact stiffness (units: FORCE/LENGTH for contact force model,
FORCE/LENGTH^{3} for contact traction model) | 5 | 5 |

KT | Current tangent contact stiffness (same units as KN) | 5 | 5 |

MU [8] | Friction coefficient | Y | Y |

TASS/TASR [7] | Total (algebraic sum) sliding in S and R directions | 3 | 3 |

AASS/AASR [7] | Total (absolute sum) sliding in S and R directions | 3 | 3 |

TOLN | Penetration tolerance | Y | Y |

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 |

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 |

R1 | Target radius | - | Y |

R2 | Contact radius | - | Y |

DTSTART | Load step time during debonding | Y | Y |

DPARAM | Debonding parameter | Y | Y |

DENERI [12] | Energy released due to separation in normal direction - mode I debonding | Y | Y |

DENERII [12] | Energy released due to separation in tangential direction - mode II debonding | Y | Y |

DENER [13] | Total energy released due to debonding | Y | Y |

CNFX [10] | Contact element force-X component | - | 4 |

CNFY [10] | Contact element force-Y component | - | 4 |

CNFZ [10] | Contact element force-Z component | - | 4 |

CNTX [11] | Contact element force due to tangential stresses - X component | - | 4 |

CNTY [11] | Contact element force due to tangential stresses - Y component | - | 4 |

CNTZ [11] | Contact element force due to tangential stresses - Z component | - | 4 |

SDAMP | Stabilization damping coefficient | - | 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 or 1), the unit of this quantity is FORCE. For the traction-based model (KEYOPT(3) = 2 or 3), 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 (KEYOPT(3) = 0 or 1), the unit of stiffness is FORCE/LENGTH. For the traction-based model (KEYOPT(3) = 2 or 3), the unit is FORCE/LENGTH

^{3}.FDDIS = (contact friction stress)*(sliding distance of substep)/(time increment of substep)

For the case of orthotropic friction in contact between beams, components are defined in the global Cartesian system.

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.

**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.

**Name**output quantity as defined in Table 176.2: CONTA176 Element Output Definitions

**Item**predetermined item label for

**ETABLE**command**E**sequence number for single-valued or constant element data

NMISC

**I, J, K**sequence number for data at nodes I, J, K

**Table 176.3: CONTA176 Item and Sequence Numbers**

Output Quantity Name |
ETABLE and ESOL Command Input | ||||
---|---|---|---|---|---|

Item | E | I | J | K | |

PRES | SMISC | 13 | 1 | 2 | 3 |

TAUR | SMISC | - | 5 | 6 | 7 |

TAUS | SMISC | - | 9 | 10 | 11 |

FDDIS | SMISC | - | 18 | 19 | 20 |

STAT [1] | NMISC | 41 | 1 | 2 | 3 |

OLDST | NMISC | - | 5 | 6 | 7 |

PENE [2] | NMISC | - | 9 | 10 | 11 |

DBA | NMISC | - | 13 | 14 | 15 |

TASR | NMISC | - | 17 | 18 | 19 |

TASS | NMISC | - | 21 | 22 | 23 |

KN | NMISC | - | 25 | 26 | 27 |

KT | NMISC | - | 29 | 30 | 31 |

TOLN | NMISC | - | 33 | 34 | 35 |

IGAP | NMISC | - | 37 | 38 | 39 |

PINB | NMISC | 42 | - | - | - |

CNFX | NMISC | 43 | - | - | - |

CNFY | NMISC | 44 | - | - | - |

CNFZ | NMISC | 45 | - | - | - |

CNTX | NMISC | 186 | - | - | - |

CNTY | NMISC | 187 | - | - | - |

CNTZ | NMISC | 188 | - | - | - |

ISEG [3] | NMISC | - | 46 | 47 | 48 |

AASR | NMISC | - | 50 | 51 | 52 |

AASS | NMISC | - | 54 | 55 | 56 |

CAREA | NMISC | 58 | - | - | - |

MU | NMISC | - | 62 | 63 | 64 |

DTSTART | NMISC | - | 66 | 67 | 68 |

DPARAM | NMISC | - | 70 | 71 | 72 |

CNOS | NMISC | - | 112 | 113 | 114 |

TNOP | NMISC | - | 116 | 117 | 118 |

SLTO | NMISC | - | 120 | 121 | 122 |

ELSI | NMISC | - | 136 | 137 | 138 |

DENERI or DENER | NMISC | - | 140 | 141 | 142 |

DENERII | NMISC | - | 144 | 145 | 146 |

GGAP | NMISC | - | 152 | 153 | 154 |

VREL | NMISC | - | 156 | 157 | 158 |

SDAMP | NMISC | - | 160 | 161 | 162 |

PLSI | NMISC | - | 164 | 165 | 166 |

GSLID | NMISC | - | 168 | 169 | 170 |

R1 | NMISC | - | 172 | 173 | 174 |

R2 | NMISC | - | 176 | 177 | 178 |

Element Status = highest value of status of integration points within the element.

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,,ELEM,`Par`

,NMISC,46 returns the ISEG value for node I of element`N`

.`N`

You can display or list contact results through several POST1
postprocessor commands. The contact specific items for the **PLNSOL**, **PLESOL**, **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 |

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.

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.