CONTA176 Element Description

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.

Figure 176.1:  CONTA176 Geometry

CONTA176 Input Data

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:

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.

Figure 176.2:  Beam Sliding Inside a Hollow Beam

Figure 176.3:  Parallel Beams in Contact

Figure 176.4:  Crossing Beams in Contact

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:

Figure 176.5:  Equivalent Circular 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(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 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.

CONTA176 Output Data

The solution output associated with the element is in two forms:

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.

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.

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:

CONTA176 Assumptions and Restrictions

CONTA176 Product Restrictions

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 

ANSYS Mechanical Premium