1. Chapter 6
Contact Surfaces

2. Chapter Objectives
Upon completion of this chapter, students will be able to define and utilize Contact Surfaces within the ANSYS/LS-DYNA Program
1. Give an overview of contact within ANSYS/LS-DYNA
2. Describe the three different contact algorithms in ANSYS/LS-DYNA
3. Describe the ten different contact families available
4. Define how contact surfaces are created
5. Describe advanced contact control options in ANSYS/LS-DYNA
6. Provide guidelines for using contact in ANSYS/LS-DYNA
7. Given step-by-step guidance, a contact exercise will be performed.
March 15, 2001
Inventory #001458
6-2

3. Contact Surfaces - Overview
Unlike ANSYS implicit, elements are not used to define contact within the ANSYS/LS-DYNA program.
Contact in ANSYS/LS-DYNA is defined using contact surfaces. Contact occurs when one segment of a model’s outer surface penetrates another segment.
Since contact elements are not used, determining regions (i.e. nodal components) where contact may occur beforehand is not necessary. In addition, real constants, such as the normal contact stiffness, kn , do not need to be specified.
With 24 different contact types available, contact surfaces within ANSYS/LS-DYNA allow the user to represent a wide range of interactions between surfaces.
To define contact in ANSYS/LS-DYNA, a user simply indicates the contact surfaces (not always required), the type of contact between them, and any specific parameters related to a given contact type.
It is not only much easier to define contact in ANSYS/LS-DYNA, but the overall range of contact capabilities exceeds that available in ANSYS implicit.
March 15, 2001
Inventory #001458
6-3

4. (continued) Contact Surfaces - Overview
With 24 different contact types available, it is often difficult to determine which contact type best defines the physical system being modeled.
To properly select a contact surface for a given model, it is important to understand the different contact algorithms and contact families available within ANSYS/LS-DYNA.
A contact algorithm is a method by which the program processes contact surfaces. There are three different contact algorithms available in ANSYS/LS-DYNA:
1. Single Surface Contact
2. Nodes to Surface Contact
3. Surface to Surface Contact
A contact family is a set of contact types that have specialized similar properties. There are ten different contact families available in ANSYS/LS-DYNA:
1. General 5. Tied with Failure Forming
2. Automatic 6. Eroding Two-dimensional
3. Rigid 7. Edge
4. Tied 8. Drawbead
March 15, 2001
Inventory #001458
6-4

5. (continued) Contact Surfaces - Overview
In the following pages, each of the contact algorithms and contact families will be described in detail so that the proper contact type may be used to accurately represent the physical phenomenon being modeled.
March 15, 2001
Inventory #001458
6-5

6. Single Surface Contact - Description
The single surface contact algorithm establishes contact when an external surface of one body contacts itself or the external surface of another body.
Single surface contact is the most general type of contact because the ANSYS/LS-DYNA program automatically searches all of the external surfaces within a model to determine if penetration has occurred.
Since all of the external surfaces are included, no contact or target surface definitions are required.
Single surface contact can be very powerful for self-contact or large deformation problems where areas of contact are not known beforehand.
March 15, 2001
Inventory #001458
6-6

7. (continued) Single Surface Contact - Description
Unlike implicit modeling, where over-defining contact will dramatically increase CPU time , single surface contact in ANSYS/LS-DYNA will cause minor CPU time increases.
Most impact and crash applications require single surface contact to be defined
The single surface contact algorithm automatically releases the contact if the penetration exceeds 40 % of the thickness of the contacted element. This can cause potential problems for the following conditions:
1. Excessively thin parts
2. Soft materials that have low stiffness values
3. Contact between bodies with extremely high velocities
The single surface contact algorithm does not record the overall resultant contact forces in the ASCII rcforc file. If contact forces are desired, node to surface or surface to surface algorithms should be used.
The valid types are Single Surface, Automatic Single Surface, Automatic General, Eroding Single Surface, 2-D Single Surface, and Single Edge
March 15, 2001
Inventory #001458
6-7

8. Nodes to Surface Contact - Description
The nodes to surface contact algorithm establishes contact when a contacting node penetrates a target surface. It is the fastest algorithm because it is asymmetric. Only the treatment of contact nodes impacting the target surface is considered.
For node to surface contact, nodal components or part numbers for the contact and target surfaces must be specified, similar to the ANSYS implicit method.
Node to surface contact is very robust for problems where the contact area is relatively small and the contact area is known beforehand. It is also efficient for modeling nodes contacting rigid bodies.
The following guidelines should be used with nodes to surface contact:
The nodes to surface contact algorithm records the overall resultant contact forces in the ASCII rcforc file.
The valid contact types are NTS, ANTS, RNTR, TDNS, TNTS, ENTS, DRAW, FNTS
1. Flat or convex surfaces should be targets while concave surfaces should be contacts.
2. Coarser meshes should be targets and finer meshes should be contact surfaces.
3. For Drawbead contact, the bead is always the nodal contact surface and the blank is the target.
CONTACT NODES
TARGET SURFACE
March 15, 2001
Inventory #001458
6-8

9. Surface to Surface Contact - Description
The surface to surface contact algorithm establishes contact when the surface of one body penetrates the surface of another.
Surface to surface contact is fully symmetric so that the choice of contact and target surfaces are arbitrary.
For surface to surface contact, nodal components or part numbers are required for the contact & target surfaces. Nodes may belong to multiple contact surfaces.
Surface to surface contact is a general algorithm and is commonly used for bodies that have large contact areas and the contact surfaces are known.
The surface to surface contact algorithm records the overall resultant contact forces in the ASCII rcforc file.
The valid contact types are STS, OSTS, ASTS, ROTR, TDSS, TSTS, ESTS, FSTS, FOSS, TSES
CONTACT AND TARGET DEFINITIONS ARBITRARY V
Surface to surface contact is most efficient for bodies that experience large amounts of relative sliding, such as a block sliding on a plane.
March 15, 2001
Inventory #001458
6-9

10. Automatic and General Contact
The automatic and general contact families differ with their treatment of shell contact forces
General contact does not consider shell thickness on contact force calculations.
Automatic contact allows contact to occur on both sides of shell elements
The contact forces for shell elements in automatic and general contact are defined as follows:
penetrating node
Shell TOP surface
Shell BOTTOM surface
Automatic Contact
General Contact
Contact
Restoring Force
March 15, 2001
Inventory #001458
6-10

11. Eroding Contacts
These are used where solid elements may fail. The purpose of eroding contact is to allow contact to occur with the remaining elements, after the elements originally forming the outer surface have failed.
March 15, 2001
Inventory #001458
6-11

12. Rigid Contacts
The contacts RNTR and ROTR are similar to NTS and OSTS except that instead of a linear stiffness to resist penetration, the user defines a force-deflection curve. These contacts are normally used for multi-body dynamics. They are intended to allow inclusion of energy absorbing compliance without the need for modeling deformable elements.
A contact of a rigid body to a deformable body must be defined with the normal, automatic or eroding contacts.
Contact of the knees
against the dashboard
March 15, 2001
Inventory #001458
6-12

13. Edge Contact
The edge contact will be used when the surface normals’ are orthogonal to the impact direction.
With EDCGEN,SE all edges will be selected automatically.
March 15, 2001
Inventory #001458
6-13

14. Tied Surfaces fn tied fs
The contacts are glued together. May be of interest when the meshes do not fit together (TDNS, TDSS, TSTS, TNTS, TSES).
Often used to model bolted parts.
With tiebreak enabled (TSTS, TNTS) failure of the connection will occur when: f n
fail m s , æ è ç ö ø ÷ + 1 2 fn
Failed (connection released)
tied fs
March 15, 2001
Inventory #001458
6-14

15. Drawbead Contact
Drawbead contact is typically used in metal forming operations when special care is need to restrain the blank.
During forming processes such as stamping, it is common for the blank to lose contact with the forming dies (i.e., wrinkling).
Drawbead contact allows implementation of bending and frictional restraining forces for ensuring the blank will remain in contact through the entire length of the drawbead depth.
Depth of drawbead
F = Ffriction+ Fbending
March 15, 2001
Inventory #001458
6-15

16. FORMING CONTACT
The forming contact options forming node to surface (FNTS), forming surface to surface (FSTS) and forming one-way surface to surface (FOSS) are primarily used in metal forming applications.
For these contact types, the tools and dies are typically defined as the target surface while the workpiece is the contact surface.
Mesh connectivity is not required for these contact options, thereby reducing the complexity of the contact specification.
Orientation of the tooling meshes must be in the same direction.
The forming contact options are based on automatic contact types and are therefore very robust.
March 15, 2001
Inventory #001458
6-16

17. TWO-DIMENSIONAL CONTACT
For models made up of PLANE162 elements, only two- dimensional contact can be defined.
The two-dimensional contact option available in ANSYS/LS-DYNA is ASS2D.
Contact component default is the entire model (Target component not used)
Contact component can be limited to a part assembly (EDASMP)
FS (static coefficient of friction) is supported with 2D contact
March 15, 2001
Inventory #001458
6-17

18. Contact Surface Definitions
There are four basic steps for defining contact within ANSYS/LS-DYNA:
Step 1: Determine the contact option that best defines your physical system
Step 2: Identify the contact entities (Not required for single surface contact)
Step 3: Specify additional input parameters that may be required
Step 4: Specify advanced contact control options
STEP 1: DETERMINING CONTACT OPTION TYPE
A large number of contact types are available in ANSYS/LS-DYNA to define a wide range of interactions between surfaces.
To determine the contact option that is best suited for a given application, use the ANSYS/LS-DYNA user guide and the descriptions found in this chapter.
For most analyses, automatic general (AG), nodes to surface (NTS), and surface to surface (STS) contact options are recommended.
March 15, 2001
Inventory #001458
6-18

19. Contact Surface Definitions - Step 2
STEP 2: DEFINE CONTACT ENTITIES
With the exception of the single surface contact (ASSC, AG, SS, ESS, ASS2D, and SE), all of the ANSYS/LS-DYNA contact options require definition of contact and target surfaces.
Defining contact and target surfaces can be accomplished by a combination of two techniques:
1. Specification of nodal components (CM command)
2. Specification of Part Ids or Part Assemblies
1. To create a nodal component that will be used in a contact definition, first select the nodes that will be used to define the contact/target surface….then create a component of the selected nodes
Utility Menu : Select -> Entities
Utility Menu: Select -> Comp/Assembly ...->Create Component
March 15, 2001
Inventory #001458
6-19

20. (continued) Contact Surface Definitions - Step 2
2. To create Part ID’s that will be used in a contact definition, first create the Parts Using the EDPART, CREATE command …
Preprocessor:LS-DYNA Optns -> Part Options
After the nodal components have been defined and the part numbers have been created, contact can be defined using the EDCGEN command.
March 15, 2001
Inventory #001458
6-20

21. (continued) Contact Surface Definitions - Step 2
The EDCGEN command automatically creates contact between the specified contact and target surfaces.
Preprocessor: LS-DYNA Options -> Contact -> Define Contact
First select the contact type and option.
Then specify the friction coefficient data and select OK.
For surface to surface and nodes to surface contact, an additional dialogue box appears so that the CONTACT and TARGET surface can be specified.
For the single surface contact options, a second dialogue box will not typically appear, as contact and target pairs are not required.
March 15, 2001
Inventory #001458
6-21

22. Contact Surface Definitions - Step 2
STEP 2 (continued): A Note on Friction Coefficient Parameters
Compared to ANSYS implicit, the capabilities for defining friction in ANSYS/LS-DYNA are much more versatile as the friction coefficient can be dependent on velocity and a limiting value can be used for the overall frictional force.
In the ANSYS/LS-DYNA program, the friction coefficient, mc, is defined by:
mc = md + (ms - md )e -(DC) (v)
where
DC = Exponential decay coefficient,
m s = the static friction coefficient,
m d = the dynamic friction coefficient,
v = relative velocity between contacting surfaces.
With DC or v = 0, mc is equal to the ms
The maximum friction force, Flim, can also be limited by the product of the coefficient for viscous friction, VC, and the area of the contact segment:
Flim = VC Asegment
The limiting friction coefficient is often used in applications where the contact causes plastic flow. The recommended value of VC = ss, where ss is the shear yield stress of the materials in contact.
March 15, 2001
Inventory #001458
6-22

23. (continued) Contact Surface Definitions - Step 2
In order to avoid undesirable oscillations during contact, damping perpendicular to the contact surface can be applied using the contact damping coefficient, VDC.
The input, VDC, requires a damping value as a percentage of critical:
x = VDC x crit = VDC (2m w)
where m is the mass and w is the natural frequency of the contact segment.
VDC is commonly used to damp out normal oscillation in metal forming analyses
All of the friction constants (m s , m d, DC, VC, and VDC) are input directly using the EDCGEN command
March 15, 2001
Inventory #001458
6-23

24. Contact Surface Definitions - Step 3
STEP 3: SPECIFY ADDITIONAL INPUT PARAMETERS
For some of the specialized contact families available in the ANSYS/LS-DYNA program, additional input is required in the fields V1-V4 of the EDCGEN command.
The following table summarizes the required additional input for each family.
Each of the additional values are input directly contact/target component or part names.
March 15, 2001
Inventory #001458
6-24

25. Listing and Deleting Contact
Because contact elements are not created, it is very important to list the defined contact surfaces before solution to ensure that the contact has been properly defined.
Listing the contact entities is performed using the EDCLIST command:
Preprocessor: LS-DYNA Options -> Contact -> List Entities
All defined contact entities are automatically listed along with the specified friction parameters. Note that each contact definition has a specific reference number
March 15, 2001
Inventory #001458
6-25

26. (continued) Listing and Deleting Contact
If it is determined that a contact surface has been incorrectly defined, it can be easily deleted using the EDDC command.
When using the EDDC command, you must specify the contact option and the contact and target components or parts. Contact entities may only be deleted in a new analysis.
Preprocessor: LS-DYNA Options -> Contact -> Delete Entity
Contact option
Contact component
Target component
March 15, 2001
Inventory #001458
6-26

27. Plotting Contact Pairs
It is often useful to plot contact pairs using the assigned contact definition number and the EDPC command
List contact with the EDCLIST command. And then, use the contact reference numbers to plot contact with the EDPC command
Specify minimum, maximum and increment contact number for EDPC
Preprocessor: LS-DYNA Options -> Contact -> Select and Plot...
Contact #1
Contact #2
Contact #3
March 15, 2001
Inventory #001458
6-27

28. Activating and Deactivating Entities
During a small restart analysis, it is also possible to deactivate and reactivate a defined contact entity.
Preprocessor: LS-DYNA Options -> Contact -> Deactivate Entities…
Preprocessor: LS-DYNA Options -> Contact -> Activate Entities...
March 15, 2001
Inventory #001458
6-28

29. Contact Boxes Explicit Dynamics with ANSYS/LS-DYNA
Training Manual
Box-shaped volumes can be used to further restrict contact searching. A Box ID number is entered along with the X, Y, and Z coordinates of the box. BoxIDs are only used with Parts and Part assemblies (nodal components are not allowed)
EDBX,,BOXID,XMIN,XMAX,YMIN,YMAX,ZMIN,ZMAX
The BOXID number is used when defining contact
Preprocessor: LS-DYNA Options -> Contact -> Define Box…
Explicit Dynamics with ANSYS/LS-DYNA
001322
15 OCT 2000
6-29

30. Advanced Contact Control Options - Step 4
Once contact has been defined between surfaces in a model, there are several advanced options in ANSYS/LS-DYNA for controlling the contact.
Almost all of the advanced contact options are controlled with the EDCONTACT command. We will highlight the following options that are most commonly used to control contact in ANSYS/LS-DYNA:
Option 1: Controlling the contact search method
Option 2: Controlling contact depth
Option 3: Controlling contact stiffness
Option 4: Contact surface birth and death times (EDCGEN command)
In ANSYS/LS-DYNA, there are 2 different contact search methods:
a. Mesh Connectivity Tracking (default for NTS, OSTS, TSTS, TNTS, TDNS)
b. Bucket Sort Method (default for all other types)
In mesh connectivity tracking, the contact search algorithm uses shared nodes of neighboring element segments to search. When a target segment loses contact with a contact node, the neighboring segment is checked.
March 15, 2001
Inventory #001458
6-30

31. Advanced Contact Control - Option 1
The mesh connectivity method is extremely fast, but can be disadvantageous since it requires that the contact surfaces have a continuous mesh.
In the bucket sort algorithm, the 3-D space occupied by the contact surface is divided into cubes (‘buckets’). Nodes can contact any segment in the same bucket or a next-door bucket. The bucket sort algorithm is extremely robust, but can be somewhat slower than mesh connectivity tracking, especially for large models.
Because many models contain meshes that are discontinuous, it is often beneficial to switch the search algorithm to the bucket sort method using the SHTK field of the EDCONTACT command:
Preprocessor: LS-DYNA Options -> Contact -> Advanced Controls
Setting the Multi-Surface Shell thickness option to Thk Incl-Exc Rgd (use shell thickness except for rigid bodies) or Thk Incl (use shell thickness, including rigid bodies) will cause the options NTS, OSTS, and TDNS to use the bucket sort algorithm.
March 15, 2001
Inventory #001458
6-31

32. Advanced Contact Control - Option 2
Option 2: Controlling contact depth
For the general contact options STS, NTS, TNTS, TSTS, and OSTS, a contact search depth of is assumed by ANSYS/LS-DYNA. Anytime a contacting node passes behind a target surface, a contact force proportional to the contact depth will be generated.
This can cause instabilities in dynamic models where components are in continuous relative motion and non-genuine contact is generated. If the contact depth is large, the spurious contact forces could become nearly infinite. If a node “appears” (slips) behind a target surface, it can shoot off into space.
In order to control the contact depth, the PENCHK field of the EDCONTACT command should be used: Preprocessor: LS-DYNA Options ->Contact -> Advanced Controls
By setting the small penetration check to ON, the program will only search for contact to a depth proportional to the target segment thickness.
March 15, 2001
Inventory #001458
6-32

33. Advanced Contact Control - Option 3
Option 3: Controlling contact stiffness
In the ANSYS/LS-DYNA program the penalty method is used for the calculation of the contact forces. In the penalty method, an ‘elastic spring’ is placed between the two bodies such that the contact interface force, F, is given by: F
d = penetration between bodies.
F = k d
where
k = contact interface stiffness, k d
Ideally there should be no penetration between surfaces during contact. This implies that the contact interface stiffness k= , which will lead to numerical instabilities.
The ANSYS/LS-DYNA program automatically calculates the contact stiffness based on the material properties and size of the contacting segments. This value will generally provide excellent results.
March 15, 2001
Inventory #001458
6-33

34. (continued) Advanced Contact Control - Option 3
The contact stiffness can be changed, however, using a contact stiffness scale factor, SFSI, that adjusts the ANSYS/LS-DYNA calculated stiffness (kcalc) by the following relationship:
k = SFSI kcalc
The default value for SFSI used by the LS-DYNA program is To increase the contact stiffness, SFSI is increased. Care should be taken, however, when doing this because of the risk of convergence instabilities. SFSI is often increased in eroding contact analysis.
In order to control the contact stiffness, the SFSI field of the EDCONTACT command should be used: Preprocessor: LS-DYNA Options -> Contact -> Advanced Controls
It is recommended that the SFSI field never be increased to a value above 1.0.
March 15, 2001
Inventory #001458
6-34

35. (continued) Advanced Contact Control - Option 3
When determining a default contact stiffness, the ANSYS/LS-DYNA program uses the material properties and the element sizes of the contact and target surfaces.
If the contacting surfaces of a model have large differences in material properties (e.g., steel impacting foam) or element size, instabilities or unrealistic behavior may arise.
When problems occur due to an incompatible contact stiffness, the contact stiffness of the contact and target surfaces can be scaled to closer values by ANSYS/LS-DYNA.
Scaling the contact stiffness can be accomplished using the PENO field of the EDCONTACT command: Preprocessor: LS-DYNA Options -> Contact -> Advanced Controls
There are five different options available for controlling the contact stiffness due to incompatibility:
1 - Use minimum of contact and target stiffness
2 - Use target surface value
3 - Use contact surface value
4 - Use area or mass weighted contact value
5 - Use slave value inversely proportional to
shell thickness (not generally recommended)
March 15, 2001
Inventory #001458
6-35

36. Advanced Contact Control - Option 4
Option 4: Contact Surface Birth and Death Time
In some applications it may become important to establish specific times for which contact can occur between surfaces.
For such cases, the ANSYS/LS-DYNA program allows the user to specify contact surface birth and death times.
At a specified birth time, the defined contact surface will become active and remain active until the specified death time.
Contact surface birth and death is controlled using the BTIME and DTIME fields of the EDCGEN command.
March 15, 2001
Inventory #001458
6-36

37. General Contact Guidelines
Initial penetrations between contact surfaces are not allowed. If ANSYS/ LS-DYNA detects initial penetration between surfaces, it will automatically move the overlapping surfaces out of contact.
Always use realistic material property and shell thickness values. The material properties and geometry of contacting surfaces are used to determine k.
Do not make multiple contact definitions between the same parts.
Use single surface contact if the exact contact behavior is not known beforehand.
List the defined contact surfaces prior to solution to ensure that contact has been properly defined.
If an analysis begins to diverge soon after starting, the following ASCII output files should be examined to determine whether contact is responsible:
GLSTAT: overall energy distribution
MATSUM: energies by PARTID
SLEOUT: contact energy output
Extremely large energies in these files will isolate the material in the contact definition that is causing problems.
March 15, 2001
Inventory #001458
6-37

38. Initial Velocity with Contact Exercise
The exercise for this chapter begins on page E6-1 of Volume II.
A wall is impacted by a cube that is subjected to an initial velocity. The LS-DYNA nodes-to-surface contact algorithm is used.
March 15, 2001
Inventory #001458
6-38