Our website uses cookies. By using the website you agree ot its use. More information can be found in our privacy policy.

Contact types

In crash analysis, the deformations can be very large and predetermination of where and how contact will take place may be difficult or impossible. For this reason, the automatic contact options are recommended as these contacts are non-oriented, meaning they can detect penetration coming from either side of a shell element.

Automatic contact types in LS-DYNA are identifiable by the occurrence of the word AUTOMATIC in the *CONTACT command. The contact search algorithms employed by automatic contacts make them better-suited than older contact types to handling disjoint meshes. In the case of shell elements, automatic contact types determine the contact surfaces by projecting normally from the shell mid-plane a distance equal to one-half the ‘contact thickness’. Further, at the exterior edge of a shell surface, the contact surface wraps around the shell edge with a radius equal to one-half the contact thickness thus forming a continuous contact surface. We sometimes refer to this offsetting of the contact surfaces from shell mid-planes as considering shell thickness offsets. The contact 9 thickness can be specified directly or scaled by the user using optional parameters in the contact definition. If the contact thickness is not specified by the user, the contact thickness is equal to the shell thickness (or, in the case of single surface contacts, the minimum of the shell thickness and element edge length). In like fashion, the contact surface for beam elements (where beam contact is considered) is offset from the beam centerline by the equivalent radius of the beam cross-section. Because contact surfaces are offset from shell mid-planes and from beam centerlines, it is extremely important that appropriate gaps between shell and beam parts be modeled in the finite element geometry in order to account for shell thickness and beam cross-section dimensions. Not doing so will result in initial penetrations in the contact surfaces. LS-DYNA will make one pass to eliminate any detected initial penetrations by moving the penetrating slave nodes to the master surface. Not all initial penetrations will necessarily be removed and this can lead to nonphysical contact behavior. Time taken in setting up an accurate initial geometry is always time well spent. Most contact types in LS-DYNA place a limit on the maximum penetration depth that is allowed before the slave node is released and its contact forces are set to zero. This is done mainly in automatic contact types to prevent large contact forces from developing in the opposite sense should the slave node pass through a shell mid-plane. This maximum penetration depth is tabulated for various contact types in Table 6.1 of the Version 960 User’s Manual. Sometimes automatic contact interfaces appear not to work because this contact threshold is reached early in the simulation. This often occurs if extremely thin shell elements are included in the contact surface. In these cases, contact failure can usually be prevented by scaling up the default contact thickness or setting the contact thickness to a value larger than the shell thickness. Alternately, setting SOFT=1 (discussed later) will often correct the problem.

One-way treatment of contact

One-way contact types allow for compression loads to be transferred between the slave nodes and the master segments. Tangential loads are also transmitted if relative sliding occurs when contact friction is active. A Coulomb friction formulation is used with an exponential interpolation function to transition from static to dynamic friction. This transition requires that a decay coefficient be defined and that the static friction coefficient be larger than the dynamic friction coefficient. The one-way term in oneway contact is used to indicate that only the user-specified slave nodes are checked for penetration of the master segments. One-way contacts may be appropriate when the master side is a rigid body, e.g., a punch or die in a metal stamping simulation. A situation where one-way contact may be appropriate for deformable bodies is where a relatively fine mesh (slave) encounters a relatively smooth, coarse mesh (master). Other common applications are beam-to-surface or shell-edge-to-surface scenarios where the beam nodes or the shell edge nodes, respectively, are given as the slave node set. There are a number of keyword options that activate one-way contact.

For contact between an airbag (slave) and segmented rigid dummy model (master), one of the following two contact types are often employed:


For metal stamping, special one-way forming contacts are recommended with the workpiece defined on the slave side:


Orientation is automatic with forming contacts. The rigid tooling surface can be constructed from disjoint element patches where contiguous nodal points are sometimes merged out, but not always. These patches are not assumed to be consistently oriented; consequently, during initialization, the reorientation of these disjoint element patches is performed. Forming contact tracks the nodal points of the blank as they move between the disjoint element patches of the tooling surface. Penalty forces are used to limit penetrations. Generally the ONE_WAY_SURFACE_TO_SURFACE option is recommended since the penetration of master nodes through the slave surface is considered in adaptive remeshing. Without this feature, adaptive remeshing may fail to adequately refine the mesh of the blank to capture sharp details in the master surface, and the master surface will protrude through the blank.

When the surface orientations are known throughout the analysis, the following non-automatic contact types may be effective:


If there is a possibility that the nodes of the slave surface can physically end up behind the master surface, these contact types should be avoided. Shell thickness offsets may or may not be considered with these non-automatic contact types (see SHLTHK in *CONTROL_CONTACT). If shell thickness offsets are inactive (default), then the old node-to-surface contact treatment from public domain DYNA3D is used for contact types 5 and 10 above where incremental searching is used to locate potential master segments for any given slave node. This searching technique uses segment connectivity; therefore, the master surface must not be disjoint. If the geometry of the surfaces have sharp angles or if the segments are very badly shaped, the searching algorithm can fail to find the proper master segment. If the shell thickness offsets are active, SHLTHK>0, the master surface is projected based on nodal normal vectors, and the location of the slave node on a master segment is determined by using global segment-based bucket sorting; therefore, the master surface can be disjoint and sharp edges and bad element shapes do not create significant problems in the searching. The use of nodal normal vectors to project the master surface is quite expensive in CPU costs, but has an advantage that the projected master surface is continuous even for convex surfaces. Until the FORMING contact types were developed, types 5 and 10 contacts with shell thickness offsets were often the contact of choice for sheet metal stamping.

The contact type:


is similar in treatment to *CONTACT_ NODES_TO_SURFACE with shell thickness offsets. Being constraint-based rather than penalty-based, type 18 contact cannot be used with rigid bodies. The forces are computed to keep the slave nodes exactly on the master surface (zero penetration). In general, this contact has never been as stable as the penalty-based contacts and is, therefore, not recommended. Eroding contact types are recommended whenever solid elements involved in the contact definition are subject to erosion (element deletion) due to material failure criteria. These eroding contacts contain logic which allow the contact surface to be updated as exterior elements are deleted. In *CONTACT_ERODING_NODES_TO_SURFACE, the slave side of the contact should be defined using a node set containing all the nodes (not just nodes on the outer suface) of the slave side part(s).

Two-way treatment of contact

This contact works essentially the same way as the corresponding one-way treatments described above, except that the subroutines which check the slaves nodes for penetration, are called a second time to check the master nodes for penetration through the slave segments. In other words, the treatment is symmetric and the definition of the slave surface and master surface is arbitrary since the results will be the same. There is an increased cost of approximately a factor of two due to the extra subroutine calls.

In crash analysis, the contact type …


is a recommended contact type since, in crash simulations, the orientation of parts relative to each other cannot always be anticipated as the model undergoes large deformations. As mentioned before, automatic contacts check for penetration on either side of a shell element.

For metal forming simulations, the contact type …


is available but is generally not used in favor of the one-way forming contacts.

The two-way (symmetric) counterparts to the previously discussed contact types 5, 18, and 16 are:


Tied contact (Translational DOF only, No Failure, No Offset)

In tied contact types, the slave nodes are constrained to move with the master surface. At the beginning of the simulation, the nearest master segment for each slave node is located based on an orthogonal projection of the slave node to the master segment. If the slave node is deemed close to the master segment based on established criteria, the slave node is moved to the master surface. In this way, the initial geometry may be slightly altered without invoking any stresses. It is always recommended that tied contacts NOT be defined by part Ids but rather by node/segment sets. In this way, the user has more direct control over what gets tied to what and thus can prevent unintended constraints. As the simulation progresses, the isoparametric position of the slave node with respect to its master segment is held fixed using kinematic constraint equations. Examples of this contact type are:


These contact types should generally only be used with solid elements since rotational degrees-offreedom of the slave node are not constrained. The use of this contact type for shell elements may produce unrealistically soft behavior. Contact types 2 and 6 differ only in the input format (slave segments vs. slave nodes); the numerical treatment is the same.

In general, when using tied interfaces between similar materials, the master surface should be the more coarsely meshed side since these constraints are not applied symmetrically. However, if one material is significantly softer, the master side should be the stiffest material. Constraint-based tied contacts such as types 2 and 6 cannot be used to tie a rigid body to a deformable body or to another rigid body. Nodes of deformable bodies that the user wishes to be tied to a rigid body can be included as extra nodes for the rigid body using the *CONSTRAINED_EXTRA_NODES command. Alternately, the OFFSET option can be used for tied contacts involving rigid bodies (seebelow).

Tied contact (Translational DOF only, No Failure, With Offset)

This contact types works the same as above but an offset distance between the master segment and the slave node is permitted. Offset tied contacts use a penalty-based formulation and thus can be used to tie rigid bodies. Examples of this contact type are:


This contact type works best if the surfaces are very close, since moments that develop due to the offset are not taken into account.

However, since rotational degrees-of-freedom are not affected, the offset contacts above should not be used with structural elements like beams and shells.

Tied contact (Translational DOF and Rotational DOF, With Failure, No Offset)

This contact interface uses a kinematic type constraint method to tie the slave nodes to the master segments and treats both translational and the rotational degrees-of-freedom. Additionally, failure can be specified when combined with beam elements of material type, *MAT_SPOTWELD, when modeling spot welds. Examples of this contact type are:


With the above types the nodes are projected to lie on the master segment. This is quite important for *CONTACT_SPOTWELD, since the beams that model the spot welds need to be as long as possible to minimize the mass scaling that is necessary to allow the calculation to have a reasonable time step size. With the TORSION option, the torsional forces in the beam, which models the spot weld, are transmitted as equivalent forces to the surrounding nodes of the master surface. The rotational constraint about the axis of the beam is then enforced. The nonlinear shell elements in LS-DYNA have a zero stiffness drilling degree-of-freedom at each node, so it is necessary to carry the torsional forces through the membrane behavior of the shell.

Tied contact (Translational DOF and Rotational DOF, With Failure, With Offset)

These contact interface options uses either a kinematic or penalty type constraint method to tie offset slave nodes to the master segments:


With the BEAM and CONSTRAINT option, the moments that develop from the offsets are computed and used in the update of the master surface. The nodes involved should belong to deformable elements. The CONSTRAINT option cannot be used with rigid bodies. The difficulty with using even the penalty option with rigid bodies is related to the nodal masses of the rigid body. If the nodal masses are accurate then the penalty method is okay. If the masses are nonsense, as is often the case if the rigid body geometry is accurate but the inertial properties are defined independently of the mesh, then the penalty method may break down since the nodal masses of the rigid body are used to set the penalties that are used in the rotational constraints.

Tied contact (Translational DOF, With Failure, With Offset)

The following penalty based contact types allow for the definition of failure parameters. It is extremely important to have the contact segment orientation aligned appropriately as it determines the tensile and compression direction. Failure can be based on the forces or stress along the normal (tensile) and shear directions. Examples of this contact type are:


When offsets are used, there is no option to distribute the moments created by the offsets to the master surface. Originally, this contact was developed to work without offsets. Effort is under way to provide alternatives to these options in the next release of LS-DYNA.

Single surface

These contact types are the most widely used contact options in LS-DYNA, especially for crashworthiness applications. With these types, the slave surface is typically defined as a list of part ID’s. No master surface is defined. Contact is considered between all the parts in the slave list, including self-contact of each part. If the model is accurately defined, these contact types are very reliable and accurate. However, if there is a lot of interpenetrations in the initial configuration, energy balances may show either a growth or decay of energy as the calculation proceeds.

For crash analysis, the contact type…


is recommended. This contact has improved from version to version of LS-DYNA and is the most popular contact option.

The older single surface contact type…


should be avoided since it has not undergone improvement. It eventually will be removed or recoded. The differences between *CONTACT_SINGLE_SURFACE and *CONTACT_AUTOMATIC_SINGLE_SURFACE are twofold. First, the older method uses nodal based bucket sorting where closest nodes are found that do not share common segments. This nodal based searching can break down if the segments vary appreciably in size and shape, especially, if aspect ratios are large. Secondly, the older method uses segment projection to determine the contact surface. This requires the calculation of nodal normal vectors that are area weighted by the segments that share the node, which in turns creates further difficulties for T-intersections and other geometric complications. The calculation of the vectors can require 25% of the total CPU required.

For modeling the deployment of airbags the following contact option is recommended:


With *AIRBAG_SINGLE_SURFACE, contact between nodes and multiple segments is considered. Much more searching is done than in the normal contact option and, consequently, this contact option is much more expensive. During the past several years, the soft constraint option, on optional card A, in the contact definition, set to 2 has proved to deploy airbags very accurately. We current recommend this option for airbag deployment. The latter option is currently being implemented for MPP usage.

The final contact is:


The contact treatment with this option was similar to type 13 through the 950c release of LS-DYNA. The main difference was that three possible contact segments, rather than just two, were stored for each slave node. With 950d and later versions, type 13 was substantially improved and now type 13 is frequently more accurate. The main feature of the GENERAL option is that shell edge-to-edge and beam-to-beam contact is treated automatically. All free edges of the shells and all beam elements are checked for contact with other free edges and beams. Unlike type 13 contact, type 26 contact checks for contact along the entire length of beams and exterior shell edges, not just at the nodes. There is a new option in 960 to also check internal shell edges (INTERIOR option). This is quite expensive, however, and is not usually needed. We plan to update this contact type in version 970 of LS-DYNA to include all the recent improvement in the *AUTOMATIC_SINGLE_SURFACE contact.

Contact entity

This contact type is used for treating deformable nodes against rigid geometric surfaces. The analytical equations defining the geometry of the surface are used in the contact calculations. This is an improvement over the usual segmented surface as represented by a mesh. A penalty-based approach is used in calculating the forces that resist penetration. This contact type is widely used to couple LS-DYNA with rigid body dummies, which have surfaces approximated by nice geometric shapes such as ellipsoids. An automatic mesh generator is used to mesh the rigid surfaces to aid visualizing the results. The mesh is not used in the contact calculations. The analytical rigid surfaces can be of the following types

  • Flat
  • Sphere
  • Cylinder
  • Hyper-ellipsoid
  • Torus
  • Load curve defining the line
  • CAL3D/MADYMO plane
  • CAL3D/MADYMO ellipsoid
  • VDA surface (read from a file)
  • IGES surface (read from a file)

sb 2001