The default settings for these parameters should be used as a starting point, but often non-default values are appropriate depending on the behavior of the contact. The following sections describe the most common contact parameters and make general recommendations regarding their use. Contact parameters may be set using the commands *CONTROL_CONTACT, *CONTACT, and *PART_CONTACT. Certain parameters may be set using more than one command and so a command hierarchy must exist. Parameters set with *CONTROL_CONTACT redefine default settings for all contacts in the model. Contact parameters set in *CONTACT_ will override default settings for individual contacts. Contact parameters set in *PART_CONTACT supercede settings in *CONTACT for contact involving a specific part.

Thickness offsets, SLTHK (card 1, *CONTROL_CONTACT and Optional Card A in *CONTACT_option) AUTOMATIC (*CONTACT_option)

In crashworthiness analysis, sheet metal components are represented using shell elements with the nodal points at the mid-plane surface. Each shell has a thickness, ts, that by default is equal to the thickness of the sheet metal. When these components are included in the contact treatment, shell thickness offsets are used to project the mid-surface of the shell to create the surface for contact. The choice of the contact type determines whether shell thickness offsets are considered.

In LS-DYNA the non-automatic contact types:

• *CONTACT_SURFACE_TO_SURFACE
• *CONTACT_NODES_TO_SURFACE
• *CONTACT_ONE_WAY_SURFACE_TO_SURFACE

use two different treatments depending on the parameter SHLTHK. This parameter can be specified globally on the *CONTROL_CONTACT card and locally for a given contact definition on optional card B of the *CONTACT input. If SHLTHK=0, an incremental search technique is used to determine the closest master segment and shell thickness offsets are not included. If SHLTHK=1, LS-DYNA considers the shell thickness offsets for deformable nodes but ignores the offsets for the nodes of rigid bodies. If SHLTHK=2, then LS-DYNA considers the thickness for both deformable and rigid nodes. For SHLTHK set to 1 or 2 a global bucket search is used to identify contact pairs. After contact is established, incremental searching is used to track the position of the slave nodes on the master surface. An advantage of global bucket searching is that the master and slave surfaces can be disjoint. This is impossible if incremental searching is used since incremental searching assumes that the contact surfaces are fully connected. In these contact types, it is important to orient the contact segment normals, based on the right-hand-rule, towards the contacting surface before the calculation begins. This is called oriented contact. An optional automatic orientation feature may be invoked using the parameter ORIEN on the *CONTROL_CONTACT card; however, for this option to work a gap must exist between opposing shell mid-plane surfaces. AUTOMATIC and single surface contact types always consider shell thickness offsets as shown in Figure 6.1. These contact types use both global bucket sorting and local incremental searching in determining the contact pairs. AUTOMATIC contacts are generally more robust than their nonautomatic counterparts since this contact type has no orientation requirement, i.e., contiguous segments do not obey the right-hand-rule. This is important in crash analysis since metal part can fold over and change the orientation. The contact search algorithm checks for penetration from either side of the shell mid-plane.

Shell Thickness Offset Recommendations

The AUTOMATIC contact types, which consider shell thickness offsets, are recommended for impact and crash analysis. If it is desired that shell thickness offsets of rigid components be disregarded, a non-automatic contact type may be used with the parameter SHLTHK set to 1 in either *CONTROL_CONTACT or on Optional Card B of *CONTACT. Additionally, it is important to ensure that the finite element mesh is constructed so that the shell mid-plane surfaces of the opposing parts are set apart by at least (ts+tm)/2 with meshes of similar density around sharp changes in curvature. If this condition is not satisfied, LS-DYNA will issue warning messages to indicate that penetrations were detected and that the penetrating nodes were moved to eliminate the penetrations. Sometimes the modification of the geometry can change the results. In version 960 of LS-DYNA, an option exists whereby penetrating nodes are not moved but rather the initial penetrations become the baseline from which additional penetration is measured. This option of tracking initial penetrations is invoked by setting the parameter IGNORE equal to 1 on Card 4 of *CONTROL_CONTACT or on optional card C of *CONTACT. We recommend that this option be used in most calculations. See Sections 6.4 and 6.5 for more on shell thickness offsets. In those sections, the term “contact thickness” refers to the magnitude of the shell thickness offsets.

Contact Sliding Friction, FS and FD (card 2, *CONTACT_option)

Contact sliding friction in LSDYNA is based on a Coulomb formulation and uses the equivalent of an elastic-plastic spring. Friction is invoked by giving non-zero values for the static and dynamic friction coefficients, FS and FD, respectively, in the *CONTACT or *PART_CONTACT input. For a detailed description of the frictional contact algorithm, please refer to Section 23.8.6 in the LS-DYNA Theory Manual.

Contact Sliding Friction Recommendations

Figure 6.1 Automatic Contact Segment Based Projection

When setting the frictional coefficients, physical values taken from a handbook such as Marks, provide a starting point. Note that to differentiate static and dynamic friction, FD should be less than FS and the decay coefficient DC must be nonzero. For numerically noisy problems such as crash, the static and dynamic coefficients are frequently set equal to avoid the creation of additional noise. The decay coefficient determines the manner in which the instantaneous net friction coefficient is ransitioned from FS to FD. The parameter, VC, provides a means to limit the frictional contact stress based on the strength of the material. The suggested value for VC is SIGY/sqrt(3) where SIGY is the minimum yield stress of the materials in contact. In LS-DYNA, version 960, the optional parameter FRCENG on card 4 of *CONTROL_CONTACT may be set to write the frictional contact energy to the binary interface database (*DATABASE_BINARY_INTFOR). Routinely, one automatic, single-surface contact with numerous dissimilar materials, are used in full vehicle simulations. In these cases, using a uniform value for FS and FD may be inappropriate. In such instances, it is recommended that the frictional parameters be specified part by part using the contact option in the part definition, *PART_CONTACT. It is helpful in understanding the sensitivity contact friction in a calculation by making two runs utilizing lower-bound and upper-bound friction coefficients.

6.3 Penalty Scale Factors, SFS and SFM (card 3, *CONTACT_option)

So-called penalty scale factors provide a means of increasing or decreasing the contact stiffness. SLSFAC in *CONTROL_CONTACT scales the stiffness of all penalty-based contacts, which have the parameter SOFT set equal to 0 or 2. SLSFAC is applied cumulatively with SFS, i.e., the actual scale factor is the product of SFS and SLSFAC, the slave penalty scale factor, or SFM, the master penalty scale factor, defined on card 3 of the *CONTACT input. SSF, when defined in *PART_CONTACT, is cumulative with the aforementioned penalty scale factors. For contacts with SOFT=1, the aforementioned penalty scale factors have no affect; rather SOFSCL on optional card A is used to scale the contact stiffness when SOFT=1. (SOFT is the first parameter specified on optional card A of *CONTACT.)

Penalty Scale Factors Recommendations

The default values (SFS=SFM=1.0; SLSFAC=0.1) generally work well for contact between similarly refined meshes of comparably stiff materials. For contacts involving dissimilar mesh sizes and dissimilar material constants, non-default values penalty scale factors may be necessary to avoid the breakdown of contact if SOFT=0. Generally, a better alternative than setting scale factors is to set SOFT=1 and leave all penalty scale factors at their default values.

Contact Thickness SST and MST (card 3, *CONTACT_option)

SST and MST on card 3 of *CONTACT allow users to directly specify the desired contact thickness. When the default value of SST=MST=0, is used, the contact thickness is equal to the element thickness specified in the *SECTION_SHELL card.

Contact Thickness Recommendations

Nonzero values of SST and MST are sometimes used to decrease the contact thickness and thus eliminate initial penetrations. This is a poor substitute for accurate mesh generation. When using nonzero values of SST and MST, it is highly recommended to use reasonable values. Specifying a very small thickness value, such as 0.1 mm, will result in contact breakdown owing to the fact that contact thickness goes into determining the maximum penetration allowed before the contact releases a penetrating node. Often, by increasing the contact thickness, breakdown of contact involving very thin materials can be averted. Based on experience, SST and MST should not be less than 0.6-0.7 millimeters. Since nonzero values of SST and MST are applied to all the parts defined in the contact, it may be more prudent to use the OPTT or SFT parameter in *PART_CONTACT to control the contact thickness for individual parts in cases where many parts of widely ranging thickness are included in a single contact.

Contact Thickness Scaling , SFST and SFMT, (card 3, *CONTACT_option)

As an alternative to directly specifying the contact thickness as described above, SFST and/or SFMT may be defined to serve as contact thickness scale factors. These factors are applied to the shell thickness specified in *SECTION_SHELL in order to obtain a contact thickness. The default values of SFST and SFMT are 1.0.

Contact Thickness Scaling Recommendations

The same concepts discussed in Contact Thickness Recommendations apply here. Care must be taken though not to assign contact thickness scale factors so small as to result in a contact thickness that is less than 0.6-0.7 mm.

Viscous Damping, VDC (Card 2, *CONTACT_option)

The viscous contact damping parameter, VDC, on card 2 of *CONTACT is zero by default. Originally, contact damping was implemented to damp out the oscillations that existed normal to the contact surfaces in sheet metal forming simulations. It has been found that contact damping is often beneficial in reducing high-frequency oscillation of contact forces in crash or impact simulations.

Viscous Damping Recommendations

In contacts involving soft materials such as foams and honeycombs, frequent instabilities exist due to contact oscillations. Using a value of VDC between 40-60 (corresponding to 40 to 60% of critical damping), it is found that the model stability improves; however, it may be necessary to reduce the scale factor for the time step size. Generally, a smaller value of 20 is recommended when metals, which have similar material constants, interact.

Contact Segment Extension, MAXPAR (Optional Card A, *CONTACT_option)

MAXPAR on Optional Card A of *CONTACT controls the enlargement of each contact segment that is needed to combat an inherent flaw in segment-based projection. This parameter is no longer used in the AUTOMATIC contact options, except for *AUTOMATIC_GENERAL, starting with version 950d of LS-DYNA. Figure 6.2 shows the contact surface that is projected from the shell mid-plane when using the segment-based projection scheme. It can be seen that at corners of convex surfaces, an open space or gap is present in the contact surface through which a slave node could freely enter without any contact detection. This can result in contact instability, negative contact energy, etc. due to a sudden, large penetration of a node that has entered through a gap. To combat this problem, the contact surface is automatically extended a slight distance parallel to the plane of the contact segment (as well as projected normally from the segment). This slight extention serves to close the gap in the contact surface. In versions starting with 950d, a cylindrical surface is created in the valley which is used as the contact surface with the forces acting normal to the surface.

Segment Extension Recommendations

The default value of MAXPAR (1.025) works well for most analyses, as most sheet metal components are not much greater than 3-4 mm. However, contact instabilities may develop when a part with a very large thickness (> 5-10mm) or having an angular surface is present in the contact definition. Such an instability may be corrected by reducing the contact thickness (discussed in earlier sections) or by increasing the segment enlargement parameter MAXPAR (to as high as, but no greater than, a value of 1.2). Refining the mesh to reduce sharp angles in the contact surface will also help. A certain cost penalty is paid for MAXPAR values greater than default.

Bucket-Sort Frequency, BSORT (Optional Card A, *CONTACT_), NSBCS, (Card 2, *CONTROL_CONTACT)

Bucket sorting refers to a very effective method of contact searching to identify potential master contact segments for any given slave node. This sorting is an expensive part of the contact algorithm so the number of bucket sorts should be kept to a minimum to reduce runtime. If thickness offsets are considered, then all contact types use the bucket sort approach to track the most probable contacting segments. BSORT specifies the number of time steps between bucket sorts. Depending on the contact type, the default bucket sort interval is between 10 and 100 cycles. Except for high speed impact, this interval is almost always adequate. The contact bucket searching frequency should increase, i.e., BSORT should be reduced, if nodes move from one disconnected surface to another in short time intervals or if the surface is folding onto itself. If two relatively smooth simply-connected surfaces are moving across each other without folds, the bucket sorting can be done at larger intervals. Note that if the surfaces are more than several segment widths away from each other, no information is stored related to future contact, and later bucket searching is required to pick up future contacts. Once a slave node is in contact, local searching tracks the motion, and bucket sorting for the nodes, which are in contact, is not necessary.

Bucket-Sort Frequency Recommendations

In certain contact scenarios where contacting parts are moving relative to each other in a rapid fashion, such as airbag deployment, more frequent (than default) bucket sorting intervals may improve the contact behavior. A tell-tale sign inadequate bucket sorting is the appearance of certain penetrating nodes inexplicably being bypassed in the contact treatment. In such cases, using the BSORT parameter

a) MAXPAR = 1.0 b) MAXPAR = 1.2

Figure 6.2 Segment extension using MAXPAR. This option is now obsolete in the AUTOMATIC contact types.

in *CONTACT or NSBCS in *CONTROL_CONTACT, the user can decrease the cycle interval between bucket sorts. Rarely will a value of less than 10 be required.

6.9 Maximum Penetration, PENMAX (Optional card B, *CONTROL_CONTACT), XPENE (Card 2, *CONTROL_CONTACT)

To avoid instability in models, slave nodes that penetrate too far are eliminated from the contact algorithm; however, they remain in other calculations. This is done so that very high forces, which are proportional to large penetration values, are not applied to the penetrating nodes that might lead to instabilities. It’s also necessary for contacts that consider shell thickness offsets to prevent a sudden reversal in direction of contact force as a penetrating node passes through the shell midplane. In non-automatic types and SHLTHK=0, the default maximum penetration is set to 1e+20. In other words, no nodes are released at all. When SHLTHK=1 or 2, the XPENE parameter determines the nodal release criteria and is given as follows:

• Max Distance (Solids) = XPENE (default=4.0) * (thickness of the solid element), SHLTHK=1
• Max Distance (Solids) = 0.05 * (thickness of the solid element), SHLTHK=2
• Max Distance (Shells) = XPENE (default=4.0) * (thickness of shell element), SHLTHK=1
• Max Distance (Shells) = 0.05 * (minimum diagonal length), SHLTHK=2

In AUTOMATIC types and single surface, excluding AUTOMATIC_GENERAL, the maximum allowable penetration is a function of PENMAX that is set to a default value of 0.4 (40%). The maximum allowable penetration in these cases are shown below:

• Max Distance = PENMAX * (thickness of the solid)
• Max Distance = PENMAX * (slave thickness + master thickness)

For *AUTOMATIC_GENERAL only, the default value of PENMAX is set to 200 and provides an almost no nodal release criteria.

6.9.1 Maximum Penetration Recommendations

It is generally recommended that parameters affecting maximum penetration not be changed from the default values. If nodes penetrate too far and are released, the preferred solution is to increase the contact stiffness, change the penalty formulation (SOFT), or increase the contact thickness.

One of the challenging aspects of contact modeling in crash analysis is the handling of interactions between structural metallic parts and non-structural components typically made from foam and plastic. This is especially important when occupants are included in the model. Another challenge is handling contact at corners or edges of geometrically complex parts. Guidelines should be followed to achieve stability in contact as well as reasonable contact behavior. Some of the modeling practices based on experience are discussed below.

Global or local contact

Historically, many individual contact definitions were used for the treatment of contact. The development and implementation of a robust single surface type of contact has changed the way engineers model the contact today. From the standpoints of simplicity in preprocessing, numerical robustness, and computational efficiency, it is now usually advantageous to forsake the use of numerous contact definitions in favor of ONE single-surface-type contact that includes all parts which may interact during the crash event. We often casually refer to this single contact approach as a global contact approach.

This, however, does not mean that one should always avoid local contact definitions. Frequently, there exist certain areas of the vehicle that require special contact considerations where the global contact definition is observed to fail. In such instances the user is encouraged to define local contact interfaces with non-default parameters that would best suit the contact condition.

AUTOMATIC_SINGLE_SURFACE or AUTOMATIC_GENERAL

Though both contact algorithms belong to the single surface contact type, several key parameters distinguish these two contact types. Table 7.1 highlights the important differences.

Table 7.1 Difference between *AUTOMATIC_SINGLE_SURFACE (13) and *AUTOMATIC_GENERAL (26)

Of the two single surface contact types listed in Table 7.1, *AUTOMATIC_GENERAL is computationally more expensive owing to its additional capabilities and its more frequent and thorough contact search.

The *AUTOMATIC_SINGLE_SURFACE contact option is recommended for global contact. To treat special contact conditions where shell edge-to-edge or beam-to-beam contact is anticipated, the additional use of the *AUTOMATIC_GENERAL contact in localized regions is recommended. *AUTOMATIC_GENERAL contact should be used sparingly and only where conditions dictate its use. One advantage of the *AUTOMATIC_SINGLE_SURFACE contact starting with LS-DYNA version 950d is in its more rigorous treatment of interior sharp corners within the finite element mesh and in the handling of triangular contact segments; consequently, the *AUTOMATIC_SINGLE_SURFACE contact is usually superior for parts meshed from triangular and tetrahedron elements. In future version of LS-DYNA, the *AUTOMATIC_GENERAL option will also include these improvements.

Standard penalty-based or soft constraint stiffness method

When several parts of dissimilar mesh sizes and/or dissimilar material properties are included into one global slave set for *AUTOMATIC_SINGLE_SURFACE, the soft constraint stiffness method (SOFT =1) is recommended. The soft constraint method seeks to maximize contact stiffness while also maintaining stable contact behavior. The interacting nodal masses and the global time step are used in formulating the contact stiffness. The segment-based contact method, invoked by setting SOFT=2, calculates contact stiffness much like the soft constraint method but otherwise is quite different. Segment-based contact can often be quite effective where other methods fail at treating contact at sharp corners of parts.

In contrast to a soft constraint approach, the standard penalty-based contact stiffness (SOFT=0) is based on material elastic constants and element dimensions. In foam and plastic materials, the contact stiffness given by the two methods can differ by one or more orders of magnitude. The primary disadvantage of choosing the soft constraint method is its dependence on the global time step. Occasionally, the global time step must be scaled down using the TSSFAC parameter in *CONTROL_TIMESTEP to avoid numerical instabilities in the contact behavior. This results in an increased run time for the entire simulation. As an alternative to reducing the global time step the soft constraint scale factor, SOFSCL, in the *CONTACT definition can be reduced from the default value of 0.1 to 0.04-0.07.

If the standard penalty-based approach in used in a global contact definition, the soft constraint approach can be used locally to handle dissimilar materials in contact. The following are examples where contact behavior may benefit from use of the soft constraint method:

• Airbag to Steering Wheel
• Airbag to Occupant
• Front Tire to SIL
• Spare tire to neighboring components
• Foam to structural components

Using a combination of both contact stiffness methods may promote good contact behavior without having to reduce the global time step.

Definition of slave set

There are several ways to define the slave set for the global contact definition. These include: all parts (this is the default), a set of included parts, a set of excluded parts, or a set of segments. The default, which includes all parts, can sometimes result in obvious instabilities at the beginning of a simulation unless great care is taken in setting up the model to avoid such things as initial penetrations and nonphysical intersections of parts. The option to ignore penetrations on the *CONTROL_ CONTACT keyword (set IGNORE equal to 1) is recommended if care is not taken to eliminate initial penetrations. Many models run perfectly with just one interface definition; others, however, will not run until changes are made to the input, usually by excluding parts or by modifying the finite element mesh to more accurately reflect the physical model. To reiterate, the following methods can be used for defining the global contact definition:

• All parts (default)
• Included parts by *SET_PART
• Excluded parts by *SET_PART. Non-Excluded parts will be considered for contact
• Segments by *SET_SEGMENT

In addition to the above slave sets, a three-dimensional box, defined using *DEFINE_BOX, may be used to restrict the contact to the parts or segments that lie within the box at the start of the calculation. This will reduce the extent of the contact definition leading to a reduction in contact-associated cpu time.

Friction

When using one global contact that includes several components of the vehicle, a uniform friction coefficient (possibly zero) may be acceptable for initial analyses. However, the use of *PART_CONTACT keyword to specify friction coefficients on a part-by-part basis is recommended when friction is expected to play a significant role. Friction coefficients specified in *PART_CONTACT will override friction coefficients specifed elsewhere if and only if FS in *CONTACT is set to -1.0. Please note that the dynamic friction coefficient FD will have no effect unless a nonzero decay coefficient DC is provided.

Contact

Thickness To reduce the number of initial penetrations, the contact thickness can changed from the default element thickness by using the global SST and MST parameters in *CONTACT. The OPTT parameter in *PART_CONTACT can be used to override SST and MST on a part-by-part basis. The user is cautioned against setting the contact thickness to an extremely small value as this practice will often cause contact failure. In fact, for treating contact of very thin shells, e.g., less than 1 mm, it may be necessary to increase the contact thickness to prevent contact failure.

If a contact surface is comprised of tapered shell elements, then a uniform contact thickness should always be specified. The contact assumes that the segment thickness is constant, which can result in thickness discontinuities between adjacent segments. As a node moves between segments of differing thickness, the interface force will either suddenly drop or increase as a result of the discontinuous change in the penetration distance. This can result in negative contact interface energies.