CONTA177 Element Description

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 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 CONTA177 in the Mechanical APDL Theory Reference for more details about this element. The line-to-line contact element, CONTA176, is also available to model beam-to-beam contact.

Figure 177.1:  CONTA177 Geometry

CONTA177 Input Data

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:

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):

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.

Figure 177.2:  Beam Sliding Inside a Hollow Beam

Figure 177.3:  Parallel Beams in Contact

Figure 177.4:  Crossing Beams in Contact

Pair-Based Contact versus General Contact

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.

Pair-Based Contact

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.

See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.

General Contact

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.

Contact Radius and Target Radius

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:

Figure 177.5:  Equivalent Circular 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).

In a general contact definition, the equivalent beam radius is specified via SECTYPE and SECDATA commands as shown below:

SECTYPE,SECID,CONTACT,RADIUS   ! Set Type = CONTACT and Subtype = RADIUS for user-defined contact radius
SECDATA,VAL1,VAL2,VAL3         ! 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, specify 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 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 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.

Friction

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 Mechanical APDL Material Reference 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 Mechanical APDL 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.

Other Input

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.

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.

CONTA177 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:

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).

CONTA177 Assumptions and Restrictions

CONTA177 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