CONTA173 Element Description

CONTA173 is used to represent contact and sliding between 3D target surfaces and a deformable surface defined by this element. The element is applicable to 3D structural and coupled-field contact analyses. It can be use for both pair-based contact and general contact.

In the case of pair-based contact, the target surface is defined by the 3D target element type, TARGE170. In the case of general contact, the target surface can be defined by CONTA173 elements (for deformable surfaces) or TARGE170 elements (for rigid bodies only).

This element is located on the surfaces of 3D solid or shell elements without midside nodes (for example, SOLID185, SOLSH190, SOLID285, SHELL181, INTER205, CPT215, MATRIX50).

The element has the same geometric characteristics as the solid or shell element face with which it is connected (see Figure 173.1: CONTA173 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.

Figure 173.1: CONTA173 Geometry

R = Element x-axis for isotropic friction

x_o = Element axis for orthotropic friction if ESYS is not supplied (parallel to global X-axis)

x = Element axis for orthotropic friction if ESYS is supplied

CONTA173 Input Data

The geometry and node locations are shown in Figure 173.1: CONTA173 Geometry. The element is defined by four nodes (the underlying solid or shell element has no midside nodes). It can degenerate to a three node element depending on the shape of the underlying solid or shell elements. If the underlying solid or shell elements do have midside nodes, use CONTA174.

The node ordering is consistent with the node ordering for the underlying solid or shell element. The positive normal is given by the right-hand rule going around the nodes of the element and is identical to the external normal direction of the underlying solid or shell element surface. For shell elements, the same nodal ordering between shell and contact elements defines upper surface contact; otherwise, it represents bottom surface contact. The contact surface's outward normal should point toward the target surface.

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. CONTA173 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 3D contact surface elements (CONTA173, CONTA174) are associated with the 3D target segment elements (TARGE170) 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 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 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 information on generating elements automatically using the ESURF command.

General Contact

CONTA173 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 (CONTA174) on 3D deformable bodies (on both lower- and higher-order elements); 3D contact line elements (CONTA177) on 3D beams, on feature edges of 3D deformable bodies, and on perimeter edges of shell structures; and vertex-to-surface elements (CONTA175) on convex corners of 3D 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 3D 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 "CONTA173 Input Summary" for details.

Friction

CONTA173 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, the applicable coordinate system is the default element coordinate system (noted by the R and S axes in the above figure).

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. (These are depicted by the x_oand x axes in the above figure.) The first principal direction is defined by projecting the first direction of the chosen coordinate system onto the contact surface. 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 Contact Technology Guide for more information on how to use this feature. See also the Guide to User-Programmable Features in the 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 Contact Technology Guide for more information on how to use this feature. See also the Guide to User-Programmable Features in the 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.

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 faceted elements on a curved (spherical or revolute) 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 "CONTA173 Input Summary". A general description of element input is given in Element Input.

CONTA173 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 173.2: CONTA173 Element Output Definitions gives element output at the element level. In the results file, the nodal results are obtained from its closest integration point.

Table 173.3: CONTA173 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 the Element Reference for more information. The following notation is used in Table 173.3: CONTA173 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:

CONTA173 Assumptions and Restrictions

CONTA173 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  —