CONTA178

CONTA178 represents contact and sliding
between any two nodes of any types of elements. The element has two
nodes with three degrees of freedom at each node with translations
in the X, Y, and Z directions. It can also be used in 2-D and axisymmetric
models by constraining the UZ degree of freedom. The element is capable
of supporting compression in the contact normal direction and Coulomb
friction in the tangential direction. User-defined friction with the
USERFRIC subroutine is also allowed. The element may be initially
preloaded in the normal direction or it may be given a gap specification.
A longitudinal damper option can also be included. See CONTA178 in the *Mechanical APDL Theory Reference* for
more details about this element. Other contact elements, such as COMBIN40, are also available.

The geometry, node locations, and the coordinate system for
this element are shown in the CONTA178 figure
above. The element is defined by two nodes, an initial gap or interference
(GAP), an initial element status (START), and damping coefficients
CV1 and CV2. The orientation of the interface is defined by the node
locations (I and J) or by a user specified contact normal direction.
The interface is assumed to be perpendicular to the I-J line or to
the specified gap direction. The element coordinate system has its
origin at node I and the x-axis is directed toward node J or in the
user specified gap direction. The interface is parallel to the element
y-z plane. See Generating Contact Elements in the *Contact Technology Guide* for more information on generating elements
automatically using the **EINTF** command.

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) in the Input Summary and the contact element discussion in the *Mechanical APDL Theory Reference* for details.

Four different contact algorithms can be selected:

Pure Lagrange multiplier method (KEYOPT(2) = 4)

Lagrange multiplier on contact normal and penalty on frictional (tangential) direction (KEYOPT(2) = 3)

Augmented Lagrange method (KEYOPT(2) = 0)

Pure Penalty method (KEYOPT(2) = 1)

The following sections outline these four algorithms.

The pure Lagrange multiplier method does not require contact stiffness FKN, FKS. Instead it requires chattering control parameters TOLN, FTOL, by which ANSYS assumes that the contact status remains unchanged. TOLN is the maximum allowable penetration and FTOL is the maximum allowable tensile contact force.

| A negative contact force occurs when the contact status is closed. A tensile contact force (positive) refers to a separation between the contact surfaces, but not necessarily and open contact status. |

The behavior can be described as follows:

If the contact status from the previous iteration is open and the current calculated penetration is smaller than TOLN, then contact remains open. Otherwise the contact status switches to closed and another iteration is processed.

If the contact status from the previous iteration is closed and the current calculated contact force is positive, but smaller than FTOL, then contact remains closed. If the tensile contact force is larger than FTOL, then the contact status changes from closed to open and ANSYS continues to the next iteration.

ANSYS will provide reasonable defaults for TOLN and FTOL. Keep in mind the following when providing values for TOLN and FTOL:

A positive value is a scaling factor applied to the default values.

A negative value is used as an absolute value (which overrides the default).

The objective of TOLN and FTOL is to provide stability to models which exhibit contact chattering due to changing contact status. If the values you use for these tolerances are too small, the solution will require more iterations. However, if the values are too big it will affect the accuracy of the solution, since a certain amount of penetration or tensile contact force are allowed.

Theoretically, the pure Lagrange multiplier method enforces zero penetration when contact is closed and "zero slip" when sticking contact occurs. However the pure Lagrange multiplier method adds additional degrees of freedom to the model and requires additional iterations to stabilize contact conditions. This will increase the computational cost and may even lead to solution divergence if many contact points are oscillating between sticking and sliding conditions during iterations.

An alternative algorithm is the Lagrange multiplier method applied on the contact normal and the penalty method (tangential contact stiffness) on the frictional plane. This method only allows a very small amount of slip for a sticking contact condition. It requires chattering control parameters TOLN, FTOL as well as the maximum allowable elastic slip parameter SLTOL. Again, ANSYS provides default tolerance values which work well in most cases. You can override the default value for SLTOL by defining a scaling factor (positive value) or an absolute value (negative value). Based on the tolerance, current normal contact force, and friction coefficient, the tangential contact stiffness FKS can be obtained automatically. In a few cases, you can override FKS by defining a scaling factor (positive input) or absolute value (negative input). Use care when specifying values for SLTOL and FKS. If the value for SLTOL is too large and the value for FKS too small, too much elastic slip can occur. If the value for SLTOL is too small or the value for FKS too large, the problem may not converge.

The third contact algorithm is the augmented Lagrange method,
which is basically the penalty method with additional penetration
control. This method requires contact normal stiffness FKN, maximum
allowable penetration TOLN, and maximum allowable slip SLTOL. FKS
can be derived based on the maximum allowable slip SLTOL and the current
normal contact force. ANSYS provides a default normal contact stiffness
FKN which is based on the Young's modulus E and the size of the underlying
elements. If Young's modulus E is not found, E = 1x10^{9} will be assumed.

You can override the default normal contact stiffness FKN by defining a scaling factor (positive input) or absolute value (negative input with unit force/length). If you specify a large value for TOLN, the augmented Lagrange method works as the penalty method. Use care when specifying values for FKN and TOLN. If the value for FKN is too small and the value for TOLN too large, too much penetration can occur. If the value for FKN is too large or the value for TOLN too small, the problem may not converge.

The last algorithm is the pure penalty method. This method requires both contact normal and tangential stiffness values FKN, FKS. Real constants TOLN, FTOLN, and SLTOL are not used and penetration is no longer controlled in this method. Default FKN is provided as the one used in the augmented Lagrange method. The default FKS is given by MU x FKN. You can override the default values for FKN and FKS by inputting a scaling factor (positive input) or absolute value (negative input) for these real constants.

The contact normal direction is of primary importance in a contact analysis. By default [KEYOPT(5) = 0 and NX, NY, NZ = 0], ANSYS will calculate the contact normal direction based on the initial positions of the I and J nodes, such that a positive displacement (in the element coordinate system) of node J relative to node I opens the gap. However, you must specify the contact normal direction for any of the following conditions:

If nodes I and J have the same initial coordinates.

If the model has an initial interference condition in which the underlying elements' geometry overlaps.

If the initial open gap distance is very small.

In the above cases, the ordering of nodes I and J is critical. The correct contact normal usually points from node I toward node J unless contact is initially overlapped.

You can specify the contact normal by means of real constants NX, NY, NZ (direction cosines related to the global Cartesian system) or element KEYOPT(5). The following lists the various options for KEYOPT(5):

**KEYOPT(5) = 0**The contact normal is either based on the real constant values of NX, NY, NZ or on node locations when NX, NY, NZ are not defined. For 2-D contact, NZ = 0.

**KEYOPT(5) = 1 (2,3)**The contact normal points in a direction which averages the direction cosines of the X (Y, Z) axis of the nodal coordinates on both nodes I and J. The direction cosines on nodes I and J should be very close. This option may be supported by the

**NORA**and**NORL**commands, which rotate the X axis of the nodal coordinate system to point to the surface normal of solid models.**KEYOPT(5) = 4 (5,6)**The contact normal points to X (Y, Z) of the element coordinate system issued by the

**ESYS**command. If you use this option, make sure that the element coordinate system specified by**ESYS**is the Cartesian system. Otherwise, the global Cartesian system is assumed.

The initial gap defines the gap size (if positive) or the displacement interference (if negative). If KEYOPT(4) = 0, the default, the gap size can be automatically calculated from the GAP real constant and the node locations (projection of vector points from node I to J on the contact normal), that is, the gap size is determined from the additive effect of the geometric gap and the value of GAP.

If KEYOPT(4) = 1, the initial gap size is only based on real constant GAP (node locations are ignored).

By default KEYOPT(9) is set to 0, which means the initial gap
size is applied in the first load step. To ramp the initial gap size
with the first load step (to model initial interference problems,
for example), set KEYOPT(9) = 1. Also, set **KBC**,0
and do not specify any external loads over the first load step.

The force deflection relationships for the contact element can be separated into the normal and tangential (sliding) directions. In the normal direction, when the normal force (FN) is negative, the contact status remains closed (STAT = 3 or 2). In the tangential direction, for FN < 0 and the absolute value of the tangential force (FS) less than μ|FN|, contact "sticks" (STAT = 3). For FN < 0 and FS = μ|FN|, sliding occurs (STAT = 2). As FN becomes positive, contact is broken (STAT = 1) and no force is transmitted (FN = 0, FS = 0).

The contact condition at the beginning of the first substep can be determined from the START parameter. The initial element status (START) is used to define the "previous" condition of the interface at the start of the first substep. This value overrides the condition implied by the interference specification and can be useful in anticipating the final interface configuration and reducing the number of iterations required for convergence. However, specifying unrealistic START values can sometimes degrade the convergence behavior.

If START = 0.0 or blank, the initial status of the element is determined from either the GAP value or the KEYOPT(4) setting. If START = 3.0, contact is initially closed and not sliding (μ ≠ 0), or sliding (if μ = 0.0). If START = 2.0, contact is initially closed and sliding. If START = 1.0, contact is initially open.

The only material property used is the interface coefficient of friction μ (MU). A zero value should be used for frictionless surfaces. Temperatures may be specified at the element nodes (for material property evaluation only). The coefficient of friction μ is evaluated at the average of the two node temperatures. The node I temperature T(I) defaults to TUNIF. The node J temperature defaults to T(I).

For analyses involving friction, using **NROPT**,UNSYM is useful (and, in fact, sometimes required if the coefficient
of friction μ is > 0.2) for problems where the normal and tangential
(sliding) motions are strongly coupled.

To define a coefficient of friction for isotropic 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.

This element also supports user-defined friction. 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.

KEYOPT(3) can be used to specify a "weak spring" across an open
or free sliding interface, which is useful for preventing rigid body
motion that could occur in a static analysis. The weak spring stiffness
is computed by multiplying the normal stiffness KN by a reduction
factor if the real constant REDFACT is positive (which defaults to
1 x 10^{-6}). The weak spring stiffness can
be overridden if REDFACT has a negative value. Set KEYOPT(3) = 1 to
add weak spring stiffness only to the contact normal direction when
contact is open. Set KEYOPT(3) = 2 to add weak spring stiffness to
the contact normal direction for open contact and tangent plane for
frictionless or open contact.

The weak spring only contributes to global stiffness, which prevents a "singularity" condition from occurring during the solution phase if KEYOPT(3) = 1,2. By setting KEYOPT(3) = 3,4, the weak spring will contribute both to the global stiffness and the internal nodal force which holds two separated nodes.

| The weak spring option should |

Use KEYOPT(10) to model the following different contact surface behaviors:

**KEYOPT(10) = 0**Models standard unilateral contact; that is, normal pressure equals zero if separation occurs.

**KEYOPT(10) = 1**Models rough frictional contact where there is no sliding. This case corresponds to an infinite friction coefficient and ignores the material property input MU.

**KEYOPT(10) = 2**Models no separation contact, in which two gap nodes are tied (although sliding is permitted) for the remainder of the analysis once contact is established.

**KEYOPT(10) = 3**Models bonded contact, in which two gap nodes are bonded in all directions (once contact is established) for the remainder of the analysis.

**KEYOPT(10) = 4**Models no separation contact, in which two gap nodes are always tied (sliding is permitted) throughout the analysis.

**KEYOPT(10) = 5**Models bonded contact, in which two gap nodes are bonded in all directions throughout the analysis.

**KEYOPT(10) = 6**Models bonded contact, in which two gap nodes that are initially in a closed state will remain closed and two gap nodes that are initially in an open state will remain open throughout the analysis.

The cylindrical gap option (KEYOPT(1) = 1) is useful where the final contact normal is not fixed during the analysis, such as in the interaction between concentric pipes. With this option, you define the real constants NX, NY, NZ as the direction cosines of the cylindrical axis ( ) in the global Cartesian coordinate system. The contact normal direction lies in a cross section that is perpendicular to the cylindrical axis. The program measures the relative distance |XJ - XI| between the current position of node I and the current position of node J projected onto the cross section. NX, NY, NZ defaults to (0,0,1), which is the case for a 2-D circular gap. With the cylindrical gap option, KEYOPT(4) and KEYOPT(5) are ignored and node ordering can be arbitrary. Real constant GAP is no long referred as the initial gap size and a zero value is not allowed. The following explanation defines the model based on the sign of the GAP value.

A positive GAP value models contact when one smaller cylinder inserted into another parallel larger cylinder. GAP is equal to the difference between the radii of the cylinders (|RJ - RI|) and it represents the maximum allowable distance projected on the cross-section. The contact constraint condition can be written as :

A negative GAP value models external contact between two parallel cylinders. GAP is equal to the sum of the radii of the cylinders (|RJ + RI|) and it represents the minimum allowable distance projected on the cross-section. The contact constraint condition can be written as:

The damping capability is only used for modal and transient
analyses. By default, the damping capability is removed from the element.
Damping is only active in the contact normal direction when contact
is closed. The damping coefficient units are Force (Time/Length).
For a 2-D axisymmetric analysis, the coefficient should be on a full
360° basis. The damping force is computed as , where Cv is the damping coefficient given
by C_{v} = C_{v1} + C_{v2}xV. V is the velocity calculated in the previous substep.
The second damping coefficient (C_{v2}) is available
to produce a nonlinear damping effect.

By default, ANSYS will not print out contact status and contact stiffness for each individual element. Use KEYOPT(12) = 1 to print out such information, which may help in solving problems that are difficult to converge.

A summary of the element input is given in "CONTA178 Input Summary". A general description of element input is given in Element Input.

**Nodes**I, J

**Degrees of Freedom**UX, UY, UZ

**Real Constants**FKN, GAP, START, FKS, REDFACT, NX, NY, NZ, TOLN, FTOL, SLTOL, CV1, CV2, COR See Table 178.1: CONTA178 Real Constants for a description of the real constants **Material Properties**MU ( **MP**command)FRIC ( **TB**command; see Contact Friction in the*Material Reference*)**Surface Loads**None

**Body Loads**Temperatures - T(I), T(J)

**Special Features**Isotropic friction Linear perturbation Nonlinear gap type User-defined friction **KEYOPT(1)**Gap type:

**0 --**Unidirectional gap

**1 --**Cylindrical gap

**KEYOPT(2)**Contact algorithm:

**0 --**Augmented Lagrange method (default)

**1 --**Pure Penalty method

**3 --**Lagrange multiplier on contact normal and penalty on tangent (uses U/P formulation for normal contact, non-U/P formulation for tangential contact)

**4 --**Lagrange multiplier method

**KEYOPT(3)**Weak Spring:

**0 --**Not used

**1 --**Acts across an open contact (only contributes to stiffness)

**2 --**Acts across an open contact or free sliding plane (only contributes to stiffness)

**3 --**Acts across an open contact (contributes to stiffness and internal force)

**4 --**Acts across an open contact or free sliding plane (contributes to stiffness and force)

**KEYOPT(4)**Gap size:

**0 --**Gap size based on real constant GAP + initial node locations

**1 --**Gap size based on real constant GAP (ignore node locations)

**KEYOPT(5)**Basis for contact normal:

**0 --**Node locations or real constants NX, NY, NZ

**1 --**X - component of nodal coordinate system (averaging on two contact nodes)

**2 --**Y - component of nodal coordinate system (averaging on two contact nodes)

**3 --**Z - component of nodal coordinate system (averaging on two contact nodes)

**4 --**X - component of defined element coordinate system (ESYS)

**5 --**Y - component of defined element coordinate system (ESYS)

**6 --**Z - component of defined element coordinate system (ESYS)

**KEYOPT(7)**Element level time incrementation control / impact control:

**0 --**No control.

**1 --**Change in contact predictions are made to maintain a reasonable time/load increment. This option is activated only if the command

**SOLCONTROL**,ON,ON was issued prior to the solution.**2 --**Change in contact predictions are made to achieve the minimum time/load increment whenever a change in contact status occurs. This option is activated only if the command

**SOLCONTROL**,ON,ON was issued prior to the solution.**4 --**Use impact constraints for standard or rough contact (KEYOPT(12) = 0 or 1) in a transient dynamic analysis with automatic adjustment of the time increment. Automatic adjustment of the time increment is performed only if the command

**SOLCONTROL**,ON,ON was issued prior to the solution.

**KEYOPT(9)**Initial gap step size application:

**0 --**Initial gap size is step applied

**1 --**Initial gap size is ramped in the first load step

**KEYOPT(10)**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)

**KEYOPT(12)**Contact Status:

**0 --**Does not print contact status

**1 --**Monitor and print contact status, contact stiffness

**Table 178.1 CONTA178 Real Constants**

No. | Name | Description |
---|---|---|

1 | FKN | Normal stiffness |

2 | GAP | Initial gap size |

3 | START | Initial contact status |

4 | FKS | Sticking stiffness |

5 | REDFACT | KN/KS reduction factor |

6 | NX | Defined gap normal - X component |

7 | NY | Defined gap normal - Y component |

8 | NZ | Defined gap normal - Z component |

9 | TOLN | Penetration tolerance |

10 | FTOL | Maximum tensile contact force |

11 | SLTOL | Maximum elastic slip |

12 | CV1 | Damping coefficient |

13 | CV2 | Nonlinear damping coefficient |

14 | COR | Coefficient of restitution |

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 Element Output Definitions.

The value of USEP is determined from the normal displacement (UN), in the element x-direction, between the contact nodes at the end of a substep. This value is used in determining the normal force, FN. The values represented by UT(Y, Z) are the total translational displacements in the element y and z directions. The maximum value printed for the sliding force, FS, is μ|FN|. Sliding may occur in both the element y and z directions. STAT describes the status of the element at the end of a substep.

If STAT = 3, contact is closed and no sliding occurs

If STAT = 1, contact is open

If STAT = 2, node J slides relative to node I

For a frictionless surface (μ = 0.0), the converged element status is either STAT = 2 or 1.

The element coordinate system orientation angles α and β (shown in Figure 178.1) are computed by the program from the node locations. These values are printed as ALPHA and BETA respectively. α ranges from 0° to 360° and β from -90° to +90°. Elements lying along the Z-axis are assigned values of α = 0°, β = ± 90°, respectively. Elements lying off the Z-axis have their coordinate system oriented as shown for the general α , β position.

| For α
= 90°, β → 90°, the element coordinate
system flips 90° about the Z-axis. The value of ANGLE represents
the principal angle of the friction force in the element y-z plane.
A general description of solution output is given in Element Solution. See the |

**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 178.2 CONTA178 Element Output Definitions**

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

EL | Element Number | Y | Y |

NODES | Nodes - I, J | Y | Y |

XC, YC, ZC | Location where results are reported | Y | 3 |

TEMP | T(I), T(J) | Y | Y |

USEP | Gap size | Y | Y |

FN | Normal force (along I-J line) | Y | Y |

STAT | Element status | 1 | 1 |

OLDST | Old contact status | 1 | 1 |

ALPHA, BETA | Element orientation angles | Y | Y |

MU | Coefficient of friction | 2 | 2 |

UT(Y, Z) | Displacement (node J - node I) in element y and z directions | 2 | 2 |

FS(Y, Z) | Tangential (friction) force in element y and z directions | 2 | 2 |

ANGLE | Principal angle of friction force in element y-z plane | 2 | 2 |

1 - Open contact

2 - Sliding contact

3 - Sticking contact (no sliding)

Available only at centroid as a

***GET**item.

Table 178.3: CONTA178 Item and Sequence Numbers lists output available through
the **ETABLE** command using the Sequence Number method.
See The General Postprocessor
(POST1) in the *Basic Analysis Guide* for more information. The following
notation is used in Table 178.3: CONTA178 Item and Sequence Numbers :

**Name**output quantity as defined in the Element Output Definition

**Item**predetermined Item label for

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

The element operates bilinearly only in static and nonlinear transient dynamic analyses. If used in other analysis types, the element maintains its initial status throughout the analysis.

The element is nonlinear and requires an iterative solution.

Nonconverged substeps are not in equilibrium.

Unless the contact normal direction is specified by (NX, NY, NZ) or KEYOPT(5), nodes I and J must not be coincident or overlapped since the nodal locations define the interface orientation. In this case the node ordering is not an issue. On the other hand, if the contact normal is not defined by nodal locations, the node ordering is critical. Use

**/PSYMB**,**ESYS**to verify the contact normal and use**EINTF**,,,REVE to reverse the normal if wrong ordering is detected. To determine which side of the interface contains the nodes, use**ESEL**,,ENAM,,178 and then**NSLE**,,POS,1.The element maintains its original orientation in either a small or a large deflection analysis unless the cylindrical gap option is used.

For real constants FKN, REDFACT, TOLN, FTOL, SLTOL and FKS, you can specify either a positive or negative value. ANSYS interprets a positive value as a scaling factor and interprets a negative value as the absolute value. These real constants can be changed between load steps or during restart stages.

The Lagrange multiplier methods introduce zero diagonal terms in the stiffness matrix. The PCG solver may encounter precondition matrix singularity. The Lagrange multiplier methods often overconstrain the model if boundary conditions, coupling, and constraint equations applied on the contact nodes overlay the contact constraints. Chattering is most likely to occur due to change of contact status, typically for contact impact problems. The Lagrange multipliers also introduce more degrees of freedom which may result in spurious modes for modal and linear eigenvalue bucking analysis. Therefore, the augmented Lagrange method option is the best choice for: PCG iterative solver, transient analysis for impact problems, modal, and eigenvalue bucking analysis.

The element may not be deactivated with the

**EKILL**command.The USERFRIC subroutine (user-defined friction) can only be used with penalty-based tangential contact (i.e., KEYOPT(2) = 0, 1, or 3).