Tied contacts fall into 2 major categories: constraint-based and penalty-based. Those with TIEBREAK, OFFSET, or BEAM_OFFSETin the name are penalty-based.  All others are constraint-based. A node, whether it be on the slave or master side, cannot be involved in more than one constraint-based contact.  Also, rigid bodies cannot be included in a constraint-based contact.

For tied contacts without the offset option, any slave nodes that meet the criteria to be tied will be moved to the master surface during initialization thus eliminating gaps between slave nodes and master segments.  If you see such a gap when viewing the model, the node is not tied. A warning message is written to the d3hsp/messag files whenever a slave node is not tied.

The criteria that must be met for a successful tie are:

• Slave node must be within the normal projection of a master segment

• The offset of the slave node from the master segment in the normal direction cannot exceed a certain tolerance.You can change this tolerance by using negative values for the contact thickness. 

(See Remark 2 on p. 7.42 of the 971 User's Manual.)

There are various tied contacts in LS-DYNA. Which you choose will depend on the application. If the surfaces to be tied are not rigid or otherwise constrained, then a constraint-based tied contact can be used, e.g.,

*CONTACT_TIED_NODES_TO_SURFACE

(if nodes do NOT have rotational DOF, e.g., as in solids or thick shells)

*CONTACT_TIED_SHELL_EDGE_TO_SURFACE  (if any nodes being tied do have rotational DOF, e.g., as in thin shells)
*CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET  (if any nodes being tied do have rotational DOF, e.g., as in thin shells AND a physical gap between the tied surfaces is to be retained)

Rigid Parts

If a rigid part is being tied, then a penalty-based tied contact could be used but not a constraint-based tied contqact. This can be accomplished by adding the word "OFFSET" to the contact name, e.g., *CONTACT_TIED_NODES_TO_SURFACE_OFFSET.  (The exception is when "CONSTRAINED_OFFSET" is used.)
See the notes on p. 7.4 of the 971 User's Manual regarding OFFSET, BEAM_OFFSET, and CONSTRAINED_OFFSET tied contacts.

As an alternative to using tied contact for permanently bonding a deformable body to a rigid body, one could use *CONSTRAINED_EXTRA_NODES.

Tiebreak Contact

"TIEBREAK" contacts have the added feature of including a failure criterion.  These contact types are usually penalty-based.  A constraint-based tied contact with a failure criterion is *CONTACT_TIED_SURFACE_TO_SURFACE_FAILURE.

Automatic tiebreak contacts have some special features (see OPTION parameter) and behave as automatic contacts after failure. 
       tiebreak option for automatic contact
            eq.-3:see 3, moments are transferred
            eq.-2:see 2, moments are transferred
            eq.-1:see 1, moments are transferred
            eq. 1:stick
            eq. 2:tiebreak for nodes initially in contact
            eq. 3:tiebreak after sticking
            eq. 4:sliding only with friction and failure
            eq. 5:elastoplastic interface with damage
            eq. 6:rigid-plastic interface with damage
            eq. 7:DYCOS Discrete Crack Model
            eq. 8:see 6, with thickness offset (Delam model)  (v. 971 only)

Offset Tied Contacts

 
Regular tied offset contacts use a penalty method and do not transmit forces/moments in a beam-like manner. This can lead to nonphysical rotational constraints.  Preferred to these regular offset contacts are BEAM_OFFSET and CONSTRAINED_OFFSET tied contacts which DO transmit forces/moments between the slave node and master segment in a beam-like manner.  The BEAM_OFFSET option is penalty-based and applies only to TIED_SHELL_EDGE_TO_SUFACE contact whereas the CONSTRAINED_OFFSET option is constraint-based and is available for TIED_NODES_TO_SURFACE,  TIED_SURFACE_TO_SURFACE,  and TIED_SHELL_EDGE_TO_SURFACE contacts. 
Be aware that *CONTACT...CONSTRAINED_OFFSET redistributes the mass of the slave nodes to the master surface but (at least) in doing so the rotary inertia of the slave nodes is transformed. In *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET, mass of the slave nodes stays put.  

 
 

Trouble-shooting: Tied contact doesn't appear to work

Look for the word "Warning" in your message file to see if there are any messages about slave nodes not being tied. If slave nodes are too far away from the master surface, the slaves will not be tied.    This threshold distance is defined in Remark 2 on p. 7.42 of the 971 User's Manual.  Note that by setting the slave and/or master contact thickness to a negative value, the threshold distance can be manually controlled.
 
Unfortunately, there's no convenient way to display unconstrained nodes.  A suggestion -- use the unix command grep to get a listing of unconstrained nodes, e.g.,
grep "slave node ID" d3hsp >list

Then edit this listing to make a node set via *SET_NODE_COLUMN. Insert this node set into your input deck and read the deck into LS-PrePost in order to view the node set.

The contact formulation invoked by setting Soft=1 on optional card A of *CONTACT is not so radical a departure from the default penalty contact formulation (Soft=0) as the Soft=2 contact formulation. Soft=1 is more or less the same as Soft=0 EXCEPT in the way the contact stiffness is determined. Soft=1 calculates contact stiffness based on stability considerations taking into account the timestep. In other words, you can liken Soft=1 contact to a group of simple spring-mass systems, each with a Courant timestep matched to the actual timestep used in the simulation. Soft=1 will generally be more effective than Soft=0 for soft materials contacting stiff materials or where the mesh densities of the two contacting surfaces are dissimilar.

When SOFT=1, we use the max of the stiffness as calculated by soft=0 and soft=1. Therefore reducing SOFSCL has no effect if the soft=0 stiffness is larger.

k = max(SLSFAC * SFS * k0, SOFSCL * k1)

where

• k is the penalty stiffness
• SLSFAC is user input on *CONTROL_CONTACT
• SFS is user input on *CONTACT card 3
• SOFSCL is user input on *CONTACT optional card A
• k0 is the stiffness calculated from material bulk modulus and element dimensions
• k1 is the stiffness calculated from nodal masses and the solution time step.

  Note: For two way contact like *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE, replace SFS with SFM (user input on *CONTACT card 3) in the above equation.

  lpb, jpd 12/2002

SOFT = 2 option

When using SOFT=2, the contact stiffness is calculated based on the actual timestep. The contact timestep reported in the d3hsp is not meaningful for SOFT = 2 contact.

The initial penetrations are not eliminated when SOFT=2 is used, rather the initially penetrated location becomes the baseline from which additional penetration is measured. It's this additional penetration that produces contact forces. The initial penetration produces no force. If, during the simulation, the segments in contact move apart to where the current penetration is less than the baseline penetration, the current penetration becomes the new baseline.

The following FAQs provide additional information for SOFT=2 contact. Subject: Segment based contact (called alternate penalty in manual, also pinball)

What is it and how is it used?

Segment based contact is a general purpose shell and solid element penalty type contact algorithm. It does not work with beams. It is activated by setting soft=2 on optional card A (keyword) or put a 2 in columns 1-5 of optional control card 3 (structured). This option is available for contact types 3, a3, 10, a10, 4, 13, a13, 14, 15

Many parameters available for standard penalty contact are also available for segment based contact. Defaults are the same as for the standard penalty contacts except that all segment based contacts use the true shell thickness by default.

• static, dynamic, exponential decay parameters
• forces printed to ncforc and binary interface for files
• Scale factor on default slave and master penalty stiffness
• Viscous damping coefficient
• Optional slave and master thickness and thickness scale factor for shells
• Birth time and death time
• Airbag thickness as a function of time
• Number of cycles between bucket sorts
• Number of cycles between contact force updates
• Symmetry plane option

Others are not.

• small penetration contact search option (not needed)
• PENMAX (not needed)
• coefficient of viscous friction (not available)
• max parametric coordinate in segment search (not needed)
• search depth for automatic contact (not needed)
• Coulomb friction scale factor (not available)
• viscous friction scale factor (not available)
• thickness option flag for 3, 5, and 10 (not needed)
• shooting node logic (not needed)

How do the different segment based contacts differ from each other?

Internally, there is only one segment based contact algorithm with options that are chosen by keyword.

• automatic vs. non automatic contacts

The automatic contacts do shell segment orientation judgments on the fly, but the non automatic do no shell orientation at all, not even during initialization! The motivation for the no orientation option was to allow the user to overcome problems when automatic orientation gets it wrong and penetration occurs. Certain geometries can confuse the automatic orientation logic which determines shell segment orientations during each bucket sort for pairs of segments that are close but not yet in contact. The front of each segment is determined such that each segment faces the center of the other segment.

• one_way_surface_to_surface vs. surface_to_surface

Because segment based contact checks pairs of segments for penetration, a judgment must be made prior to calculating penalty forces about which segment is the master and which is the slave. As it turns out, it is almost always correct to judge the least penetrated element to be the master and the most penetrated to be the slave. This judgment may be reversed by a warped element check since warped elements may be the slave even if least penetrated. That is the logic used by the single_surface and surface_to_surface contacts. The one_way_surface_to_surface overrides this judgment and simply uses the master and slave segments as input by the user.

• airbag_single_surface vs. single_surface

When airbags are initially folded, many thin layers may be piled on top of each other which causes long bucket sort lists and slow contact. To speed up contact and to try to avoid inappropriate contact forces, the airbag contact option removes segment pairs from the bucket sort list if both segments belong to an airbag, and if the inside of one segment is facing the outside of a segment implying that the inside of the bag would contact the outside which is generally not possible.

How does segment based contact differ from the standard penalty contacts?

Because contact is detected between segments, it is nearly impossible for nodes to penetrate undetected as can happen with the standard penalty contact when nodes slip between segments at corners.

Please explain the detail of penetration of one segment into another segment. If segment based contact does not check penetration of nodes of the segment, what is checked for penetration?

It's a complicated thing to explain and to comprehend. A segment A is deemed to have penetrated another segment B when at least one node of segment A has penetrated each of the five planes associated with segment B. It is not necessary that the same node of segment A penetrate each of the five planes. The five planes consist of the plane containing the segment plus the four edge planes of the segment. An edge plane is defined as being perpendicular to the segment and containing one edge of the segment. The attached gif file (soft2.gif) shows three examples of situations where segments are contacted by other segments, but not at nodes. In these cases, a node to segment penetration check will fail to detect contact. The segment-based contact uses logic described above to check not for penetrating nodes, but rather for penetrated segments. To check if a segment is penetrated, I need to check if its surface is penetrated and if each of its edges is penetrated. In the surface to surface example in the attached figure, each of the edges of both segments are clearly penetrated by at least one node of the other segment so contact is detected.

There is no nodal release logic needed with automatic contacts because the initially penetrated side is stored as long as a segment pair remains in contact.

Erosion of shells and solids is handled automatically but unless an eroding contact is used (type 14,15) the memory allocated for contact segments may be insufficient when segments are added due to erosion.

Scaling of penalty forces is very similar to the soft constraint method, which is based on the stability of the local system, 2 masses (segments) separated by a spring (penalty stiffness). The attempt of this method is to scale the stiffness of each interacting pair to an optimum level so that the system remains stable, and penetration small. In reality, penalty stiffness is added without any added mass so we are adding massless springs that depend on segment mass for stability. However, since the segment mass is already accounted for in element time step calculation, there is no way to guarantee stability with any added penalty stiffness. For this reason and because multiple impacts with the same segment are possible, the stiffness is scaled back to a small percentage of the calculated stability limit. For shells, the segment mass is equal to the element mass. For solids, it is equal to 1/2 the element mass. The penalty stiffness is

k = 0.5*slsfac*sfs*(m1*m2/(m1+m2)/(dtc)**2

where slsfac is the default penalty stiffness, sfs is the slave penalty stiffness factor (similar equation for master) m1 and m2 are the segment masses, and dtc is the time step for contact which is set to 1.05*dt2 where dt2 is the initial solution time step. If during the calculation, dt2 rises above dtc, then dtc is reset as 1.05 times the current solution time step, and the penalty stiffness reduced as a result.

Please note, that the solution time step includes the users supplied time step scale factor, tssfac so the contact stiffness becomes greater when tssfac is reduced. This stiffening effect can be quite significant since the square of the time step appears in the denominator it may be desirable to reduce the penalty stiffness when tssfac is reduced.

Initially penetrated nodes are not moved during initialization. Instead, the initial penetration for each segment pair is stored and subtracted from the current penetration before calculating penalty forces. This same logic is used throughout the calculation so that if a node happens to go undetected, it will not be shot out by large penalty forces. The disadvantage of this method is that parts may penetrate too much, but in most applications it is not noticeable. It could be a problem if there is a lot of sliding (such as deep drawing). As one segment slides along a sheet of segments, it will penetrate a little deeper each time it passes from one segment to another because it will enter the new segment from the side. This initial penetration will be ignored and additional penetration must occur to generate sufficient contact forces.

Although the airbag thickness vs. time load curve may be used with segment based contact, it may not be desirable as the growing thickness of the bag tends to add artificial energy to the system and cause the sliding interface energy to become negative. Because segment based contact ignores initial penetrations, airbag simulations can be run without this option.

Segment based contact tends to me more robust at corners in a mesh than standard penalty contact for two reasons. First, as mentioned above, nodes cannot slip between segments at shell corners. Second, more information is available so it is not hard to apply penalty forces in the correct direction at corners in solid element meshes. As a result, the symmetry plane option is not generally needed, but it is still available.

The pinball edge to edge contact option:

Segment based contact uses a parameter called EDGE that activates an edge to edge contact check that works for both shell edges and solid element edges. This method inaccurate and unreliable, and not recommended for general use. Edge to edge contact is probably better treated by type 26 contact. However if the EDGE option is used, it's usually better to isolate the problem edge penetration area and treat it with a separate contact definition than to use the EDGE option in a complex simulation. That said, here is how it works.

Edge-edge penetration is judged to occur when a segment pair is first found to be in contact, and both segments are penetrated by a large distance where

large distance = (1-EDGE/2)*(t1+t2) for 0 < EDGE <= 2

and t1 and t2 are the segment thicknesses. When EDGE=0, the edge contact algorithm is not used. For small values of EDGE, the penetration must be large for the edge-edge contact to be detected, t1+t2 in the limit. For EDGE=2, only edge-edge contact will be detected for any finite depth of penetration, which means that all contacts will be treated as edge-edge contact. Therefore, EDGE>1 is discouraged as it is too likely to misjudge surface penetrations as edge penetrations.

The edge-edge penetration is detected, a force calculation is done by the pinball method in which segments are represented by spheres that bounce off of each other. The force is along the line between segment centers. The spheres are large enough to contain the entire segment (assuming zero thickness) so they extend beyond the edges, possibly by a long distance for segments with large aspect ratio. To avoid flying nodes, the initial penetration of spheres is subtracted from the current depth of penetration prior to calculating penalty forces.

The thickness of solid element segments is zero - oops, a bug was just found. It looks like the EDGE parameter should be left at zero for contact with solids until this is corrected. Solid element thickness will soon be half of the solid element thickness where the thickness is evaluated by element volume divided by segment area.

More on edge-edge contact (5/2002):

The pinball edge option is an attempt to deal with the edge to edge contact case. It simply represents each segment by a sphere that encompasses the nodes of the segment, and the forces are calculated to make the pinballs bounce off of each other. The pinball has a radius equal to the distance from the segment center to the most distant node. The pinball will extend beyond the segment edges and surface and therefore does not accurately represent the segment shape. I recommend that you do not use this option as it does not handle edge to edge contact as well as the automatic general contact. Please use the default parameter value, EDGE=0.

In version 970, I have added an accurate edge to edge option that does not use the pinball idea. Instead, when edge to edge contact is detected, it identifies the edges that are in contact and calculates a penalty force that is normal to those edges. This new option makes the old pinball approach obsolete although it will still remain as an option for backward compatibility between versions.

Addendum:

SOFT=2 is generally good at handling dissimilar mesh refinements or dissimilar material stiffnesses.

Version 970 options:

Optional Card A, 5th field SBOPT (previously EDGE): segment based contact options ............... .10000E+01

• eq.0: default is 2
• gt.0 and lt.2: pinball edge-edge contact
• eq.2: default, assume planer segments
• eq.3: warped segment option
• eq 4: sliding option
• eq 5: do options 3 and 4

Optional Card A, 6th field DEPTH: search depth options for segment based contact 2 * eq.0:default is 2

• eq.2:check surface penetration only
• eq.3:check surface penetration but measure depth of penetration at segment edges as well as nodes
• eq.5:check surface penetration and also edge to edge penetration

For contact which includes edge-edge treatment in non-airbag contact problems, SBOPT=3, DEPTH=5 is recommended by Lee Bindeman.

For folded airbag contact (fabric-fabric contact) with SOFT=2, refer to contact.airbag.

Segment based contact (SOFT=2) does not use the shooting node logic parameter. There is no need for shooting node logic because the segment based contact ignores initial penetrations. Penalty forces are proportional to penetration in excess of the initial penetration. In equation form, this is

f = k*(d-di)

where f is a force, k is penalty stiffness, d the current penetration depth, and di the initial penetration depth.

I should mention that the ignore option (optional card C, or 4th card of *CONTROL_CONTACT) causes the default contact to ignore initial penetrations which also makes shooting node logic unnecessary.

Release threshold:

Segment based contact does not use PENMAX. There is no need to release segments when penetration is large because the side of impact is recorded for each shell segment in contact. As long as a pair of segments remains in contact, penalty forces push back to the side of impact.

User's manual states that only ISYM, I2D3D, SLDTHK, and SLDSTF are active on Optional Card B.

lpb, jpd 12/2002 revised 5/16/2003

For both the SMP and MPP LS-DYNA version, there are some restrictions concerning this option:

• it isn't supported for SOFT=2
• it isn't available for solid elements

For the SMP LS-DYNA version, there are some further restrictions concerning the SMOOTH option:

• it must be put before the other contacts
• it works only for ONE_WAY_ type of contact
• the rigid part must be defined on the master side
• element normals have to be consistent
• no sharp angle
• rigid bodies must be connected and only part IDs are accepted

Any edge with an angle between two contact segments bigger than an angle defined by FLANGL (*CONTACT optional Card C) will be treated as feature line during surface fitting in smooth contact.

"Shooting node logic" puts a penetrating node back to the master surface without applying any contact force. This occurs on the first cycle that a penetration is sensed. In subsequent cycles, penetration produces contact forces.  After the penetrating node is pushed back so that it is no longer penetrating a master surface, "shooting node logic" can  again be invoked the next time penetration occurs.

"Shooting node logic" can be beneficial in the case where a slave node suddenly finds itself well behind it's master segment (whereas there was no penetration in the preceding cycle). In such a case, the logic prevents a huge contact force that might  otherwise cause an instability. The penetrating node is simply placed back on the master surface.   

If the "shooting node logic" doesn't prevent shooting nodes, then consider the following potential root causes:

• inappropriate use of fully integrated element formulations in areas of large deformation

• a stability issue that may be rectified simply by reducing the timestep scale factor

• out-of-control hourglassing that may be brought under control by an alternate hourglass control or refinement of the mesh

• poor choice of contact type possibly aggravated by detected and/or undetected initial penetrations.

NOTE:

Setting IGNORE=1 supersedes use of "shooting node logic".

1. Introduction

Contact definitions allow the modeling of interaction between one or more parts in a simulation model and have become a necessity in any small or large deformation problem. The main objective of the contact interfaces is to eliminate any `overlap` or `penetration` between the interacting surfaces and they accomplish this by first detecting the amount of penetration and then applying a force to remove them. Depending on the type of algorithm used to remove the penetration, both energy and momentum is conserved. This article discusses the presence of penetration in non-tied penalty-based contact interfaces during the initialization of the problem, usually termed as `cinitial penetration`, its effects on the accuracy, robustness of the model and how LS-DYNA has features that can minimize its adverse effects.

2. Detecting Penetrations

In order to detect the penetration due to contact, LS-DYNA first performs a global search using the Bucket-Sort approach and then a local search using the incremental search technique, to find the closest master segment for any given slave node or a segment. Once a closest segment is found, it projects the slave nodal coordinates onto the closest master segment to compute its orthogonal distance. This is shown in Figure [1]. The projected normal distance is computed using a local coordinate system that is embedded in the master segment and is updated every cycle. Based on the sign of the projected distance, LS-DYNA determines if the node is inside (penetration) or outside (no-penetration) the master segment. Projected distance that is less than 0 indicates that a penetration has occurred while a positive projected distance indicates a no penetration condition.

3. Initial Penetration

Initial penetration is a term used frequently to describe the amount of penetration that exists between a node and its closest master segment (in the case of classic node/ segment treatment) or between two interacting segments (in the case of `segment-based` treatment) during the initialization of the problem. This is shown in Figure [2] by considering only the thickness on the master segment for simplicity.

4. Need for Penetration-Free Simulation Model at First Cycle

Existence of penetration at the first cycle in non-interference contact definitions, which is after the initialization of the problem, has several adverse effects on the quality of the simulation. LS-DYNA attempts to remove any penetration that may exist at the first cycle by applying forces to the nodes involved. This initial force can in some instances be very large which may have adverse effects on the stability of the model. These forces could also lead to localized initial stresses and strains that may be non-physical. Additionally, if the penetrations were unable to be removed completely at the first cycle, they tend to be carried over to the subsequent cycles leading to a `negative energy` condition altering the numerical accuracy of the simulations. Experience with large and complicated models show that any existence of penetration at the first cycle effects repeatability and robustness when the model is run using multiple combinations of software and hardware. These shortcomings of initial penetrations motivate both the developers and the users to find a method that not only eliminate the issues but they do that in a way that requires minimum user effort.

5. Default Treatment to the Handle Initial Penetrations in Node/ Segment Contact

In the default treatment, when a slave node is found to penetrate its closest master segment, LS-DYNA updates the nodal coordinates to remove the penetration. Who gets updated depends on the contact definition itself. When the contact definition belongs to the family of `Single Surface` such as *CONTACT_AUTOMATIC_SINGLE_SURFACE or *CONTACT_AUTMOATIC_GENERAL or *CONTACT_AIRBAG_SINGLE_SURFACE to list a few, then both the slave node AND the master segment is moved by the amount. When the contact definition belongs to the family of `ONE-WAY` or `TWOWAY`, then only the slave nodal coordinates are updated to remove the penetration.

In both cases, the removal of penetration is performed using three iterations. At the end of these three iterations, it is possible for penetrations to exist and is entirely based on the model content and the sequence of the contact definitions. For example, we can have two contact definitions C1 and C2 in that order. During the first iterative pass, if we detect penetration of slave node SN1 with master segment MS1, we update the nodal coordinate of SN1 such that it lies exactly on the surface of MS1. Within the same iterative pass, we now check for penetrations due to C2. I f SN1 belongs to C2 and is found to penetrate another master segment MS2 in the opposite direction, then we again update the nodal coordinates of SN1 which could void the step performed earlier while handling C1. This type of situation could result in the existence of penetration of SN1 even after 3 iterative pass.

6. Advantages and Disadvantages of the Default Initial Penetration Removal Process

7. Treatment of Initial Penetrations when IGNORE=1 for Node/ Segment Contact

IGNORE parameter available in both *CONTROL_CONTACT and *CONTACT_{ OPTION} (Optional Card `C`) keywords allows a new method of handling the presence of initial penetrations. When IGNORE=0, LS-DYNA uses the old default method by updating the nodal coordinates of the offending nodes/ segments. This is illustrated in Figure [3]. When IGNORE=2, LS-DYNA does exactly the same steps as described above with the exception that a list of offending nodes and their initial penetration values are written into D3HSP file.

8. Recommendations

The most obvious recommendation would be to have no initial penetrations at all. However, this is rather difficult due to the nature of the model building process and the number of design changes that usually occur during the course of the product lifecycle. Accepting this, there are several methods to treat initial penetrations and they are briefly discussed here:

• Use of external pre-processors.
  • Instead of a fixed number of iterations to remove penetration by LS-DYNA, external preprocessors allow a user-defined number of iterations until a certain level of acceptable penetrations are reached. This approach may assure zero or minimal penetration levels but comes at the cost of geometry update which may be undesirable from the design perspective. Additionally, they still may not resolve issues such as dependent nodal penetrations where one contact interferes with another as discussed above. Lastly, depending on the penetration condition, it is extremely difficult to match the penetration-check algorithms between the preprocessors and LS-DYNA as the checks are refined in newer releases in LS-DYNA. Using external pre-processor is recommended for simple models as long as the updated coordinates do not deviate significantly from the original geometry which in complicated models could be extremely difficult to verify. LS-PrePost (version 2) provides a feature to detect and remove initial penetrations. More information on this new feature can be viewed at http://www.lstc.com/lspp.
• Contact thickness scaling
  • LS-DYNA allows scaling of contact thickness in several ways which has no effect on the structural thickness specified in the section definitions. The first method involves scaling of contact thickness that affects ALL segments for a particular contact definition.

    The first method involves using any of the parameters such as SST, MST, SFST, SFMT in individual contact keyword *CONTACT_{ OPTION}. SST and MST values override values specified in the section definitions while SFST and SFMT SCALE them. Using this method, one can quickly replace or scale-down the contact thickness for the entire contact but comes with certain drawbacks. If the penetration levels are located in a localized region, using this approach we are scaling down all the segments that has no penetration levels associated which could create additional clearances between components that originally did not have any initial penetrations.

    The second method involves replacing or scaling the contact thickness at a PART level using the _CONTACT opt ion in the *PART keyword. Parameter OPTT can be used to override the thickness or parameters SFST can be used to scale the contact thickness. This method is highly recommended if the penetration level exists in a localized region since it only affects the scaling or overriding of values for the part that uses the _CONTACT option.

• IGNORE parameter in CONTACT and CONTROL CONTACT keyword
  • Considering the difficulties in using any external pre-processor to remove initial penetrations, the option of using the IGNORE parameter to remember the penetration history without modifying the nodal coordinates is very attractive considering it involves the minimum of users time and effort. During the course of a product lifecycle, several design changes related size and shape will be incorporated. Size changes, involving shell component thicknesses, will alter the initial penetration conditions if IGNORE parameter is not considered which may lead to geometry updates that may alter the solution. Using IGNORE=1 causes LS-DYNA to skip the geometry update step thereby preserving the geometry while considering size changes.

9. Acknowledgements

It is with extreme pleasure that I acknowledge Dr. Lee Bindeman, for sharing information related to segment -based contacts, Dr. Jason Wang for sharing information related to the MPP version of LS-DYNA, and Dr. Morten Jenson for reviewing this article.

10. References

• Sliding Interfaces With Contact - impact In Large Scale Lagrangian Computations, Dr. John Hallquist.
• A Procedure for the Solution of Finite-Deformation Contact - Impact Problems, Dr. John Hallquist.
• Contact - Impact Algorithm, LS-DYNA Theory Manual, 2006, Livermore Software Technology Corporation.
• LS-DYNA Keyword Users Manual, 2006, Livermore Software Technology Corporation.

Figure [1] SLAVE NODE PROJECTION

Figure [2] INITIAL PENETRATION

Figure [3] PENETRATION TREATMENT FOR IGNORE > 0

Original from: Suri Bala, 2006

Transducers are NOT implemented for 2D contact and should not be defined in a 2D model.

Update in LS-DYNA 971:

Added master surface to force transducer penalty option to gather force interactions between surfaces in single surface contact.

Edge-to-edge contact can be treated in LS-DYNA via the following three contact types:

*CONTACT_SINGLE_EDGE

*CONTACT_AUTOMATIC_GENERAL

*CONTACT_AUTOMATIC_SINGLE_SURFACE with SOFT=2 and DEPTH=5

You can ignore the "The LS-DYNA time step size should not exceed ..." message if all your contacts use SOFT=1 or SOFT=2. The "surface timestep" need only be considered for penalty-based contacts that use SOFT=0. If your timestep exceeds the minimum "surface timestep" of a SOFT=0 contact, this does not necessarily invalidate the results. It's just a flag to let you know an instability COULD occur and keep an eye on the behavior of that contact (via animations, SLEOUT, internal energies in the area of the suspect contact).

Options for controlling the thickness of shell elements within the contact routines:

• OPTT: the thickness per material, specified in *PART_CONTACT
• SFT: thickness scaling per material, from *PART_CONTACT

• SST/MST: slave/master thickness given on *CONTACT card

• SFST/SFMT: slave/master thickness scaling on *CONTACT card
• THKCHG: flag to update thickness for single surface contacts, on the *CONTROL_CONTACT card
• SSTHK: "use actual thickness" flag for single surface contacts, on the *CONTROL_CONTACT card
• SPOTHIN: spotweld thinning parameter, on *CONTROL_CONTACT
• ISTUPD: flag to update shell thicknesses, on *CONTROL_SHELL

How thicknesses are initially determined:

1. For each contact node, the contact thickness is set to the thickness of the shell element that contains it. If SFST/SFMT or SFT are set, scale the thickness (with SFT overriding SFST/SFMT). If SSTHK is 0 and the contact is single surface, limit thickness to 40% of the minimum edge length of the element.
2. If SST/MST or OPTT are set, overwrite the above with this value, with OPTT taking precedence.

How thicknesses are updated for nodes of deformable bodies*:

*Nodes of rigid bodies are not updated.

When SOFT=1, contact stiffness is calculated as follows:                                                                                                     

k = max[SLSFAC*SFS*k0, SOFSCL*k1] where

• k is the penalty stiffness

• SLSFAC is user input on *CONTROL_CONTACT
• SFS is user input on *CONTACT (Card 3)
• SOFSCL is user input on *CONTACT (Optional Card A)
• k0 is the stiffness calculated from material bulk modulus and element dimensions. This is the stiffness used when SOFT=0 (see Section 23.7 in the LS-DYNA Theory Manual).
• k1 is the stiffness calculated from nodal masses and the solution time step (analogous to how Courant time step is determined based on mass and stiffness).
• k1 is proportional to 1/(time step)^2. Thus, if the time step is cut in half, the contact stiffness increases by a factor of 4.

When SOFT=2, contact stiffness is calculated in similar fashion to k1 above and can be scaled by SLSFAC and by SFS. So again, the contact stiffness is proportional to 1/(time step)^2.

Time step can affect contact behavior aside from contact stiffness. The bucket sorting interval is based on a number of time steps. Thus, if the time step is reduced, there will be less time between bucket sorts. Also, the incremental penetrations will likely be smaller if the time step is reduced.

Automatic vs. Non-automatic:

Automatic contacts are recommended for most explicit simulations. Non-automatic contacts (in which contact orientation is important) are sometimes used for metal forming simulations where the geometries are very straightforward and contact surface orientation can be reliably established before the simulation is conducted. Non-automatic contacts are generally recommended for implicit simulations.

Contact types:

Type 13 contact *CONTACT_AUTOMATIC_SINGLE_SURFACE is a single surface contact (no master surface is defined) that always considers shell thickness and has no orientation. Thus it's necessary that shell surfaces be modeled with at least a small gap between them. To avoid initial penetrations, the gap should be no less than the average thickness of the two shells potentially in contact. No gap is necessary between solid elements. The contact searching algorithm for type 13 contact is more complex than for type 3 *CONTACT_SURFACE_TO_SURFACE or a3 *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE, i.e., type 13 can handle situations such as shell edge to surface, and to some extent, beam to shell surface. As with any single surface contact type, resultant forces are not directly retrievable in the RCFORC file; one must define a *CONTACT_FORCE_TRANSDUCER_PENALTY in order to retrieve the contact forces. The article What is the difference between CONTACT_AUTOMATIC_SINGLE_SURFACE and CONTACT_AUTOMATIC_GENERAL ? provides additional information on *CONTACT_AUTOMATIC_SINGLE_SURFACE and contrasts it to *CONTACT_AUTOMATIC_GENERAL.

Type 3 contact *CONTACT_SURFACE_TO_SURFACE is a surface-to-surface (two-way) contact where shell thickness consideration can either be turned on or off either in *CONTACT or *CONTROL_CONTACT (*CONTACT_ has priority). The orientation of the contact segments is important with this contact type as the shell only looks in one direction for potential contact. In a two-way contact such *CONTACT_SURFACE_TO_SURFACE, nodes on the slave side are first checked for penetration thru the master surface and then master nodes are checked for penetration thru the slave surface. The exception is this approach is when segment-based contact is invoked by setting SOFT=2. Type a3 Contact type a3 has no orientation (a shell looks for potential contact from either side of the shell midplane) and always considers shell thickness, so in this regard, it's quite similar to a type 13 contact. Table 6.1 in the 950 Keyword User's Manual lists the maximum penetration d that defines when a penetrating node is released from contact consideration. This distance d is different for a type 3 contact than for a type 13 contact.

Some notes on contact parameters:

SOFT

SOFT is the first parameter on Optional Card A of *CONTACT_ The default value of SOFT is 0. SOFT=1 is more or less the same as SOFT=0 EXCEPT in the way the contact stiffness is determined. SOFT=2 is a radical departure from SOFT=0, both in the way contact stiffness is determined but also in the manner that the search for penetration is conducted. SOFT=2 invokes what is called "segment-based contact". For notes regarding contact with SOFT= 1 and 2, see the article SOFT option .

IGNORE

At any point during the simulation, if a node is suddenly found to be below the surface (say, it was moving very fast and wasn't detected before penetration), the old style (IGNORE=0) algorithm just moves the node to the master surface without applying any forces (we term this "shooting node logic"). If the shooting node logic is turned off (SNLOG=1), then you get large forces suddenly appearing, and negative contact energy. If IGNORE is set to 1 then the shooting node logic flag SNLOG has no affect. Rather the amount of sudden penetration is noted and compensated for by adjusting the contact thickness locally. So at any time during the simulation, if a sudden penetration is detected, the program doesn't apply any large forces nor are any nodes moved. Contact forces, however, will resist FURTHER penetration.

jpd 12/2002 revised 4/2003 revised 9/2003 auto vs. non-auto

If the contact situation is beam-to-shell-EDGE, one might have a problem. In that case, one have to stick with  *CONTACT_AUTOMATIC_GENERAL AND add null beams (low density beams utilizing *MAT_NULL) along (merged to) the outer edges of the shells. The null beam part should be added to the slave side of the contact.