CONTA171 Element Description

CONTA171 is used to represent contact and sliding between 2-D target surfaces and a deformable surface, defined by this element. The element is applicable to 2-D structural and coupled-field contact analyses. It can be used for both pair-based contact and general contact.

In the case of pair-based contact, the target surface is defined by the 2-D target element type, TARGE169. In the case of general contact, the target surface can be defined by CONTA171 elements (for deformable surfaces) or TARGE169 elements (for rigid bodies only).

This element is located on the surfaces of 2-D solid, shell, or beam elements without midside nodes (for example, PLANE182, INTER192, SHELL208, CPT212, MATRIX50).

The element has the same geometric characteristics as the solid, shell, or beam element face with which it is connected (see Figure 171.1: CONTA171 Geometry). Contact occurs when the element surface penetrates an associated 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 CONTA171 in the Mechanical APDL Theory Reference for more details about this element. Other surface-to-surface contact elements (CONTA172, CONTA173, CONTA174) are also available.

Figure 171.1:  CONTA171 Geometry

CONTA171 Input Data

The geometry and node locations are shown in Figure 171.1: CONTA171 Geometry. The element is defined by two nodes (the underlying solid, shell, or beam element has no midside nodes). If the underlying solid, shell, or beam elements do have midside nodes, use CONTA172.

The element x-axis is along the I-J line of the element. The correct node ordering of the contact element is critical for proper detection of contact. The nodes must be ordered such that the target lies to the right side of the contact element when moving from the first contact element node to the second contact element node as in Figure 171.1: CONTA171 Geometry.

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. CONTA171 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 2-D contact surface elements (CONTA171 and CONTA172) are associated with the 2-D target segment elements (TARGE169) via a shared real constant set. The program looks for contact only between 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 solid 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 number). See Identifying Contact Pairs in the Contact Technology Guide for more information.

For rigid-flexible and 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.

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

General Contact

CONTA171 can be used in a general contact definition, although it is not directly generated by the GCGEN command. 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 (CONTA172) on 2-D deformable bodies (on both lower- and higher-order elements) and vertex-to-surface elements (CONTA175) on convex corners of 2-D solid bodies and/or shell structures. The general contact definition may also contain target elements (TARGE169) overlaid on the surfaces of standalone rigid bodies and lower-order contact surface elements (CONTA171) overlaid on 2-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 surfaces 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 "CONTA171 Input Summary" for details.

Friction

To model isotropic friction, use the TB,FRIC,,,,ISO command. You can define a coefficient of friction that is dependent on temperature, time, normal pressure, sliding distance, or sliding relative velocity by using the TBFIELD command along with TB,FRIC,,,,ISO. 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.

Other Input

The contact interaction subroutine USERINTER is available for user-defined interface interactions, including interactions in the normal and tangential directions as well as coupled-field interactions. 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 fluid penetration loads, use the SFE command to specify the fluid pressure and fluid penetration starting points. For more information, see Applying Fluid Pressure-Penetration Loads in the Contact Technology Guide.

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.

To model wear at the contact surface, use the TB command with the WEAR label. See Contact Surface Wear in the Contact Technology Guide for more information.

This element supports various 2-D stress states, including plane stress, plane strain, and axisymmetric states. The stress state is automatically detected according to the stress state of the underlying element. However, if the underlying element is a superelement, you must use KEYOPT(3) to specify the stress state.

Two types of geometry correction are available for this element: surface smoothing and bolt thread modeling. Surface smoothing is a geometry correction technique that eliminates inaccuracies introduced by linear elements on a curved (circular or nearly circular) contact surface. Bolt thread modeling provides a method for simulating contact between a threaded bolt and bolt hole without having to model the detailed thread geometry. Both of these geometry correction techniques are implemented through section definitions (SECTYPE, SECDATA, and SECNUM commands). For more information, see Geometry Correction for Contact and Target Surfaces in the Contact Technology Guide.

A summary of the element input is given in "CONTA171 Input Summary". A general description of element input is given in Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.

CONTA171 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.

Table 171.2: CONTA171 Element Output Definitions gives element output. In the results file, the nodal results are obtained from its closest integration point.

Table 171.3: CONTA171 Item and Sequence Numbers 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. The following notation is used in Table 171.3: CONTA171 Item and Sequence Numbers:

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:

CONTA171 Assumptions and Restrictions

CONTA171 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