6.2. Contact Options

In order to adequately characterize the complex interaction between surfaces in an explicit dynamic analysis, twenty-four different contact types have been incorporated in the ANSYS LS-DYNA program (see the table below). With such a large number of contact options, it is extremely important for a user to have an understanding of each contact type so that the proper contact option can be used to realistically model a physical phenomenon. Therefore, in this section, each of the contact options available in the ANSYS LS-DYNA program will be discussed.

Table 6-1 Contact Types

 Single surfaceNodes to surfaceSurface to surface
General (Normal) SSNTSSTS, OSTS
Automatic ASSC, AG, ASS2DANTSASTS
Rigid  RNTRROTR
Tied  TDNSTDSS, TSES
Tied with failure  TNTSTSTS
Eroding ESSENTSESTS
Edge SE  
Drawbead  DRAWBEAD 
Forming  FNTSFSTS, FOSS

6.2.1. Definition of Contact Types

As shown in the columns of Table 6-1, you can choose from three basic contact types in the ANSYS LS-DYNA program: single surface contact, nodes-to-surface contact, and surface-to-surface contact.

  1. Single Surface Contact (SS, ASSC, AG, ASS2D, ESS, SE)

    Single surface contact is established when a surface of one body contacts itself or the surface of another body. In single surface contact, the ANSYS LS-DYNA program automatically determines which surfaces within a model may come into contact. Therefore, single surface contact is the simplest type to define because no contact or target surface definitions are required. When it is defined, single surface contact allows all external surfaces within a model to come into contact. This option can be very powerful for self-contact or large deformation problems when general areas of contact are not known beforehand. Unlike implicit modeling, where over-defining contact will significantly increase computation time, using single surface contact in an explicit analysis will cause only minor increases in CPU time. Most impact and crash-dynamic applications will require single surface contact to be defined. Since automatic general (AG) contact is very robust and includes shell edge (SE) contact as well as improved beam contact, it is recommended as the first choice for self contact and large deformation problems when the contact conditions are not easy to predict.

  2. Node-to-Surface Contact (NTS, ANTS, RNTR, TDNS, TNTS, ENTS, DRAWBEAD, FNTS)

    Node-to-surface contact is a contact type which is established when a contacting node penetrates a target surface. This type of contact is commonly used for general contact between two surfaces. Use the same rules as in ANSYS implicit to determine which surfaces are target or contact:

    • The flat or concave surface is the target. The convex surface is the contact surface.

    • The coarser mesh is the target surface. The finer mesh is the contact surface.

    In the case of Drawbead contact, the bead is always the nodal contact surface and the blank is always the target surface.

  3. Surface-to-Surface Contact (STS, OSTS, ASTS, ROTR, TDSS, TSTS, ESTS, FSTS, FOSS, TSES)

    Surface-to-surface contact is established when a surface of one body penetrates the surface of another body. Surface-to-surface contact is the most general type of contact as it is commonly used for bodies that have arbitrary shapes with relatively large contact areas. This type of contact is most efficient for bodies that experience large amounts of relative sliding, such as a block sliding on a plane or a sphere sliding within a groove.

6.2.2. Definition of Contact Options

For each of the three contact types, there are often several contact options available. In the ANSYS LS-DYNA program, the following options may be used:

  1. General (Normal) Contact (SS, NTS, STS, OSTS)

    Although the general contact options use the simplest contact algorithms, they still are used for a wide range of applications. In fact, the NTS and STS options are two of the three recommended options for ANSYS LS-DYNA. The primary advantage of using the general contact algorithms is that they are extremely fast and robust. The only concern when working with the general contact options deals with contact surface orientation. The contact surface orientation defines which side of a surface is solid and which side is ‘air'. When using solid elements, ANSYS LS-DYNA automatically sets the contact orientation correctly for the general contact options. For shell elements, however, you must set the contact surface orientation when using general contact. To do this, set the ORIE field of the EDCONTACT command to 2 to activate automatic reorientation of the contact surfaces. It is important to note, the reorientation will occur only if there is no initial penetration of the shell surface.

  2. Automatic Contact (ASSC, AG, ASS2D, ANTS, ASTS)

    Along with the general contact family, the automatic contact options are the most commonly used contact algorithms. The main difference between the automatic and general options is that the contact surface orientation for shell elements is automatically determined by the automatic contact algorithms. In automatic contact, checks are made for contact on both sides of shell elements. Therefore, the contact search depth is always limited. If this is considered to be the reason for breaking through a contact surface, try using general contact with an infinite or a large search depth. See Controlling Contact Depth later in this chapter.

  3. Eroding Contact (ESS, ENTS, ESTS)

    The eroding contact options are needed when the elements forming one or both exterior surfaces experience material failure during contact. Contact is allowed to continue with the remaining interior elements. Eroding contact should be used with solid elements in penetration problems and other applications which experience surface failure. When using eroding contact, a symmetry plane option (V1), an interior/exterior node erosion option (V2), and an adjacent material treatment option (V3) must be specified on the EDCGEN command.

  4. Rigid Contact (RNTR, ROTR)

    The rigid body contact options are similar to the general contact options NTS and OSTS except that, rather than using a linear stiffness to resist penetration, a user-defined force-deflection curve is used. These contacts are typically used for multi-body dynamics where all of the bodies are rigid. Rigid body contacts are beneficial because they can allow inclusion of energy absorption without the need for modeling deformable elements. However, rigid body contact (RNTR, ROTR) cannot be used with deformable bodies. The contact of a rigid body to a deformable body must be defined with general, automatic, or eroding options. For the rigid options, the data curve ID (V1), force calculation method (V2), and unloading option (V3) must be specified on the EDCGEN command.

  5. Tied Contact (TDNS, TDSS, TSES)

    The tied contact options actually 'glue' the contact nodes (surfaces) to the target surfaces. The contact and target surfaces must be initially coplanar so that during initialization, an isoparametric position of the contact node (surface) within the target segment is calculated. Thereafter, upon application of loads or initial velocities, the contact nodes (surfaces) are forced to maintain their isoparametric position within the target surface. The effect of tied contact is that the target surfaces can deform and the slave nodes are forced to follow that deformation. When defining tied contact, the body with the coarser mesh should always be defined as the target surface. Only translational degrees of freedom (UX, UY, and UZ) are affected by tied contact.

  6. Tiebreak (Tied with Failure) Contact (TNTS, TSTS)

    Tiebreak contact is identical to tied contact except that the contact nodes (surfaces) are tied to the target surfaces only until a failure criterion is reached. This is done by 'pinning' the contact nodes (surfaces) to the target using a penalty stiffness; after the failure criterion is exceeded, the contact nodes (surfaces) are allowed to slide relative to, or separate from, the target surface. The tiebreak contact options are typically used to represent spot-welded or bolted connections. The main difference between TNTS and TSTS is that the TSTS failure is based on a failure stress and the TNTS is based on a failure force. When using TSTS, the normal (V1) and shear (V2) failure stresses must be specified using the EDCGEN command. For the TNTS option, the normal (V1) and shear (V2) failure forces and normal (V3) and shear (V4) force exponents must be supplied using the EDCGEN command. Failure of the connection will occur when:

  7. Edge Contact (SE)

    The single edge contact option should be used when contact occurs orthogonal to the shell surface normal direction. This contact option does not require contact or target surface definitions. Single edge contact is often used in sheet metal applications which have their surface normals orthogonal to the impact direction.

  8. Drawbead Contact (DRAWBEAD)

    Drawbead Contact is typically used in metal forming operations in which special care must be taken to restrain the blank. During drawing and stamping simulations, it is common for the blank to lose contact with the forming surfaces. Drawbead contact, which allows implementation of bending and frictional restraining forces, helps to ensure that the blank will remain in contact the entire length of the drawbead depth.

    Figure 6.1:  LS-DYNA Drawbead Representation

    LS-DYNA Drawbead Representation

  9. Forming Contact (FNTS, FSTS, FOSS)

    The forming contact options are primarily used in metal forming applications. For these contact types, the tools and dies are typically defined as the target (master), while the workpiece is defined as the contact (slave) surface. Mesh connectivity is not required for the forming contact option, but the orientation of the tooling meshes must be in the same direction. The forming contact options are based on the Automatic contact types and are therefore very robust in metal forming applications.


Release 18.2 - © ANSYS, Inc. All rights reserved.