6.1. Contact Definitions

Due to complicated large deformation dynamics which typically occur during an explicit dynamic analysis, determining contact between components in a model can be extremely difficult. For this reason, special features have been included in the ANSYS LS-DYNA program to make defining contact between surfaces as efficient as possible. All contact surfaces are defined in ANSYS LS-DYNA through the use of the EDCGEN command.

Use the following steps when using the EDCGEN command:

STEP 1: Determine the type of contact surface which best defines your physical model.
STEP 2: Identify contact entities.
STEP 3: Specify friction coefficient parameters.
STEP 4: Specify any additional input which is required for a given contact type.
STEP 5: Specify birth and death times for the contact definition.

STEP 1: Determining Contact Type

In order to adequately describe interaction between complex geometries during large deformation contact and dynamic impact, a large number of contact surface options have been incorporated into the ANSYS LS-DYNA product. These contact types, which include node-to-surface, surface-to-surface, single surface, single edge, eroding, tied, tiebreak, drawbead, and rigid contact options, are discussed in detail later in this chapter (see Contact Options). For most typical analyses, the following contact options are recommended.

STEP 2: Defining Contact Entities

With the exception of the single surface (ASSC, SS, and ESS), automatic general (AG), and single edge contact (SE), all of the contact options require you to identify contact and target surfaces for which contact can occur. You can do this by using nodal components, PART ID definitions, and/or part assembly ID definitions. When using contact or target components, use select logic and the CM command to group the nodes (only nodal components are valid). Then, as shown in the sample input listing below, use the EDCGEN command to specify contact between the desired components such as the ball and bat surfaces of the example problem discussed in Loading:

NSEL,S,NODE,.... ! Select a set of nodes on ball surface
CM,BALLSURF,NODE ! Place selected nodes into component
                 ! BALLSURF
NSEL,S,NODE,.... ! Select a set of nodes on bat surface
CM,BATSURF,NODE  ! Place selected nodes into component
                 ! BATSURF
EDCGEN,NTS,BALLSURF,BATSURF,.25,.23	! Generate node-to-surface
             	    ! contact between components
                  ! BALLSURF and BATSURF

Alternatively, contact surfaces can be specified using part numbers or part assembly numbers that are currently defined within the finite element model. Part assembly numbers are defined with the EDASMP command.

The input line below demonstrates how the EDCGEN command is used to define contact between two different parts / part assemblies in a model:

EDCGEN,STS,1,2,.25,.23 ! Generate surface-to-surface contact
                       ! between PARTS 1 and 2

Additionally, contact can be defined between contact and target surfaces using a combination of PART / part assembly and component definitions, as illustrated below:

EDCGEN,NTS, N1,2,.3,.28 ! Generate node-to-surface contact
                        ! between component N1 and PART 2

EDCGEN,ESTS,1,4,.15,.15 ! Generate eroding surface-to-surface 
                         ! contact between PART 1 and part assembly 4

EDCGEN,STS,1,1,.1,.1 ! Generate surface-to-surface contact
                     ! between PART 1 and itself

You can also use the EDCGEN command for defining contact between part assemblies as shown in the following sample input:

EDCGEN,STS,5,6,.3,.28 ! Generate surface-to-surface contact 
                      ! between part assemblies 5 and 6

For the specialized case of single surface contact (ASSC, AG, ESS, and SS), no contact or target surface definitions are required. As explained later in this section, single surface contact is the most general type of contact definition as all external surfaces within a model can be in contact at any point during an analysis. The program will ignore any contact and target surfaces defined for single surface contact and will issue a warning message upon execution of the EDCGEN command. A typical command for single surface contact is presented below:

EDCGEN,ASSC,,,.34,.34 ! Generate automatic single surface
                      !  contact for the entire model

Note--When defining contact entities in an explicit analysis, no initial penetrations are allowed. Therefore, use great care when defining contact components.

STEP 3: Specifying Friction Coefficient Parameters

The frictional coefficient used for contact is determined from the static friction coefficient (FS), the dynamic friction coefficient (FD), and the exponential decay coefficient (DC). (FS, FD, and DC can be input on the EDCGEN command.) The frictional coefficient is assumed to be dependent on the relative velocity, Vrel, of the surfaces in contact:

The coefficient for viscous friction, VC (also input on EDCGEN), can be used to limit the friction force to a maximum. A limiting force is computed:

where Acont is the area of the segment contacted by the node in contact. The suggested value for VC is to use the yield stress in shear:

where σo is the yield stress of the contacted material.

In order to avoid undesirable oscillation in contact, e.g., for sheet forming simulation, a contact damping perpendicular to the contacting s

urfaces is applied. The contact damping coefficient is calculated as follows:

VDC is the viscous damping coefficient (input on EDCGEN command as percent of critical damping; e.g., VDC = 20 indicates 20%). ξcrit is determined in the following fashion by ANSYS LS-DYNA:

where

STEP 4: Specifying Additional Input

For eroding, rigid, tiebreak, and drawbead contact, additional information (fields V1-V4 on the EDCGEN command) may also be required. This information varies with contact type, as outlined below.

Eroding surface contacts (ENTS, ESS, and ESTS) are used when surfaces of solid elements fail and contact needs to be redefined with the remaining internal elements. For eroding contact, V1-V3 are defined as follows: the boundary condition symmetry option key (V1) determines whether a symmetry condition will be retained along a surface where elements fail; the interior erosion option key (V2) specifies whether erosion can subsequently occur along internal surfaces when the exterior surface fails; the adjacent material key (V3) determines whether solid element faces are included for erosion along free boundaries.

Rigid body contact (RNTR and ROTR) is normally used for multi-body dynamics. For rigid body contact, a user defined force deflection curve is used to resist penetration rather than a linear stiffness. Therefore, for rigid body contact, you must specify a data curve ID (V1), a force calculation method type (V2) applicable to the specified rigid contact option, and an unloading stiffness value (V3).

Tiebreak contact (TSTS and TNTS) is used to define contact failure when surfaces are ‘glued’ together. For both types of tiebreak contact, tensile (V1) and shear (V2) failure stresses are used to calculate the failure criterion and are required for input. For tiebreak nodes-to-surface contact, exponents for the normal force (V3) and the shear force (V4) can also be specified to define the failure criterion.

Drawbead contact (DRAWBEAD) is typically used in specialized cases to represent drawbeads, which help restrain a blank during drawing operations. In drawbead contact, you must input a load curve ID (V1), which gives the bending component of the restraining force as a function of drawbead displacement, and a drawbead depth (V3). You may optionally include a curve ID (V2), which gives the normal restraining force as a function of drawbead displacement and the number of equally spaced integration points (V4) along the drawbead.

STEP 5: Specifying Birth and Death Times

For each contact definition, you can specify a birth time and a death time by using fields BTIME and DTIME on the EDCGEN command. This allows you to activate contact at any time during the transient analysis, then deactivate it at a later time.

6.1.1. Listing, Plotting and Deleting Contact Entities

Once you define contact using the EDCGEN command, you can list, plot, or delete contact definitions. Use the EDCLIST command to list all currently defined contact entities. A sample listing is shown below. Each contact definition is given a contact entity reference number that can be used when plotting contact definitions.

CURRENT EXPLICIT DYNAMIC CONTACT DEFINITIONS
1 General Surface to Surface Contact Defined Between:
  Nodal contact Entity  N1
  And Nodal Target Entity  N2
  FS = 0.10000 FD = 0.08000 DC = 0.00000 VC = 0.00000 VDC = 0.0000

2 Automatic Single Surface Contact Defined For:
  All External Surfaces of Model
  FS = 0.20000 FD = 0.15000 DC = 0.00000 VC = 0.00000 VDC = 0.0000

You can use the EDPC command to select and plot contact entities. The plot will consist of nodes or elements, depending on the method that was used to define the contact surfaces (that is, components or parts). You can specify a minimum contact entity number, maximum contact entity number, and contact entity number increment by using the MIN, MAX, and INC fields of the EDPC command. Hence, by issuing the command EDPC,1,2,1 for the above listing, the defined entities for the STS and ASSC contact would be selected and plotted. It is important to note that for single surface contact definitions, all external surfaces in the model will be selected and plotted.


Note:   EDPC selects the nodes and/or elements of the specified contact entities. Therefore, after plotting the contact entities, you must reselect all nodes and elements required for subsequent operations (such as SOLVE). Use the NSEL,ALL and ESEL,ALL commands (or other appropriate forms of these commands).


If contact has been incorrectly specified, you can delete it using the EDDC command. To delete a specific contact definition, issue the command EDDC,DELE,Ctype,Cont,Targ, where Ctype is the contact type and Cont and Targ are the contact and target parts or components for which contact has been defined. To delete all current contact definitions, issue the command EDDC,DELE,ALL.

You cannot delete contact specifications in a small restart analysis (EDSTART,2). However, you can use the EDDC command to deactivate (EDDC,DACT,Ctype,Cont,Targ) or reactivate (EDDC,RACT,Ctype,Cont,Targ) contact in a small restart. This capability is useful when you know at what stages in an analysis certain types of contact will occur. To use this feature you must define all contact specifications (EDCGEN command) in the new analysis, and you must perform at least one small restart. Once a contact specification is defined, you can deactivate it in a restart when it is not needed, and reactivate it in a later restart when it is needed. By considering contact only when it is needed, you can achieve significant CPU time savings. (Remember that if you delete contact in a new analysis using EDDC,DELE, its definition is removed from the database and you cannot reactivate it in a later restart.)

The EDDC command is not supported in an explicit dynamic full restart analysis (EDSTART,3). Thus, you cannot delete, deactivate, or reactivate contact specifications in a full restart that were defined in a previous analysis.


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