CONTA173 Element Description

CONTA173 is used to represent contact and sliding between 3-D "target" surfaces (TARGE170) and a deformable surface, defined by this element. The element is applicable to 3-D structural and coupled field contact analyses. This element is located on the surfaces of 3-D solid or shell elements without midside nodes (SOLID5, SOLID45, SOLID46, SOLID65, SOLID69, SOLID70, SOLID96, SOLID185, SOLSH190, VISCO107, SHELL28, SHELL41, SHELL43, SHELL57, SHELL63, SHELL131, SHELL157, SHELL181, and MATRIX50). It 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 one of the target segment elements (TARGE170) on a specified target surface. Coulomb and shear stress friction is allowed. This element also allows separation of bonded contact to simulate interface delamination. See CONTA173 in the Theory Reference for ANSYS and ANSYS Workbench for more details about this element. Other surface-to-surface contact elements (CONTA171, CONTA172, CONTA174) are also available.

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). 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. Remember the target surfaces must always be on its outward normal direction. See Generating Contact Elements in the Contact Technology Guide for more information on generating elements automatically using the ESURF command.

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 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.

The 3-D contact surface elements are associated with the 3-D target segment elements (TARGE170) via a shared real constant set. ANSYS looks for contact only between 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 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), or you must combine the two target surfaces into one (targets that share the same real constant numbers).

To model separation of bonded contact with KEYOPT(12) = 4, 5, or 6, use the TB command with the CZM label. See " Debonding" in the Contact Technology Guide for more information.

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 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 a - 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 this manual 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 Professional. 

ANSYS Structural. 

ANSYS Mechanical.