EDCGEN

EDCGEN

EDCGEN, Option, Cont, Targ, FS, FD, DC, VC, VDC, V1, V2, V3, V4, BTIME, DTIME, BOXID1, BOXID2
Specifies contact parameters for an explicit dynamics analysis.

PREP7: Explicit Dynamics

Compatible Products: – | – | – | – | – | – | DYNA

Option

Label identifying the contact behavior (dictates the meaning of V1 through V4).

AG	—	Automatic general contact.
ANTS	—	Automatic nodes-to-surface contact.
ASSC	—	Automatic single surface contact.
ASS2D	—	Automatic 2-D single surface contact.
ASTS	—	Automatic surface-to-surface contact.
DRAWBEAD	—	Drawbead contact
ENTS	—	Eroding nodes-to-surface contact.
ESS	—	Eroding single surface contact.
ESTS	—	Eroding surface-to-surface contact.
FNTS	—	Forming nodes-to-surface contact.
FOSS	—	Forming one way surface-to-surface contact.
FSTS	—	Forming surface-to-surface contact.
NTS	—	Nodes-to-surface contact.
OSTS	—	One way surface-to-surface contact.
RNTR	—	Rigid nodes to rigid body contact.
ROTR	—	Rigid body to rigid body (one way) contact.
SE	—	Single edge contact.
SS	—	Single surface contact.
STS	—	Surface-to-surface contact.
TDNS	—	Tied nodes-to-surface contact.
TSES	—	Tied shell edge-to-surface contact.
TDSS	—	Tied surface-to-surface contact.
TNTS	—	Tiebreak nodes-to-surface contact
TSTS	—	Tiebreak surface-to-surface contact.

Cont

Contact surface identified by a component name [CM] , a part ID number [EDPART], or an assembly ID number [EDASMP]. If a component name is input, the component must contain nodes that represent the contact surface (assemblies are not valid for a component name). Alternatively, a part number may be input that identifies a group of elements as the contact surface, or an assembly number may be input containing a maximum of 16 parts. The assembly ID number must be greater than the highest number used for the part ID. Cont is not required for automatic general contact, single edge contact, and single surface contact options (Option = AG, SE, ASSC, ESS, and SS). For automatic 2-D single surface contact (ASS2D), Cont must be defined as a part assembly. For eroding node-to-surface contact (ENTS), Cont must be defined as a nodal component. For eroding single surface contact (ESS) and eroding surface-to-surface contact (ESTS), Cont must be defined as a part ID or part assembly.

Targ

Target surface identified by a component name [CM] , a part ID number [EDPART], or an assembly ID number [EDASMP]. If a component name is input, the component must contain nodes that represent the target surface (assemblies are not valid for a component name). Alternatively, a part number may be input that identifies a group of elements as the target surface, or an assembly number may be input containing a maximum of 16 parts. The assembly ID number must be greater than the highest number used for the part ID. Targ is not defined for automatic general contact, single edge contact, automatic single surface contact, eroding single surface contact, single surface contact, and automatic 2-D single surface contact options (Option = AG, SE, ASSC, ESS, SS, and ASS2D). For eroding node-to-surface contact (ENTS) and eroding surface-to-surface contact (ESTS), Targ must be defined as a part ID or part assembly.

FS

Static friction coefficient (defaults to 0).

FD

Dynamic friction coefficient (defaults to 0).

DC

Exponential decay coefficient (defaults to 0).

VC

Coefficient for viscous friction (defaults to 0).

VDC

Viscous damping coefficient in percent of critical damping (defaults to 0).

V1, V2, V3, V4

Additional input for drawbead, eroding, rigid, and tiebreak contact. The meanings of V1-V4 will vary, depending on Option. See the table below for V1-V4 definitions.

Additional input for drawbead contact (Option = DRAWBEAD):

V1	—	Load curve ID giving the bending component of the restraining force per unit draw bead length as a function of draw bead displacement. `V1` must be specified.
V2	—	Load curve ID giving the normal force per unit draw bead length as a function of draw bead displacement. `V2` is optional.
V3	—	Draw bead depth.
V4	—	Number of equally spaced integration points along the draw bead (default = 0, in which case ANSYS LS-DYNA calculates this value based on the size of the elements that interact with the draw bead).

Additional input for eroding contact (Option = ENTS, ESS, or ESTS):

—

Symmetry plane option. The purpose of this option is to retain the correct boundary conditions in a model with symmetry.

0	—	Off (default).
1	—	Do not include faces with normal boundary constraints (e.g., segments of brick elements on a symmetry plane).

—

Erosion/interior node option.

0	—	Erosion occurs only at exterior boundaries.
1	—	Interior eroding contact can occur (default).

—

Adjacent material treatment for solid elements.

0	—	Solid element faces are included only for free boundaries (default).
1	—	Solid element faces are included if they are on the boundary of the material subset. This option also allows erosion within a body and the consequent treatment of contact.

Additional input for rigid contact (Option = RNTR or ROTR):

—

Data curve id for force versus deflection behavior [EDCURVE]. Also specify V2. (No default.)

—

Force calculation method for rigid contact. (No default.)

1	—	Data curve gives total normal force on surface versus maximum penetration of any node (only applicable for `Option` = ROTR).
2	—	Data curve gives normal force on each node versus penetration of node through the surface (`Option` = RNTR or ROTR).
3	—	Data curve gives normal pressure versus penetration of node through the surface (only applicable for `Option` = RNTR).

—

Unloading stiffness for rigid contact. This should not be larger than the maximum value used in the data curve. The default is to unload along the data curve (specified on V1).

Additional input for tiebreak surface-to-surface contact (Option = TSTS). V1 and V2 are used to calculate the failure criterion:

V1	—	Normal failure stress. (No default.)
V2	—	Shear failure stress. (No default.)

Additional input for tiebreak nodes-to-surface contact (Option = TNTS). V1 through V4 are used to calculate the failure criterion:

V1	—	Normal failure force. Only tensile failure (i.e., tensile normal forces) will be considered in the failure criterion. (No default.)
V2	—	Shear failure force. (No default.)
V3	—	Exponent for normal force. (Defaults to 2.)
V4	—	Exponent for shear force. (Defaults to 2.)

BTIME

Birth time for which contact definition will become active (defaults to 0.0).

DTIME

Death time for which contact definition will become inactive (defaults to 1e21).

BOXID1

Contact volume as defined using the EDBX command (valid only when defining contact with parts or assemblies).

BOXID2

Target volume as defined using the EDBX command (valid only when defining contact with parts or assemblies).

Command Default

No contact defined.

Notes

The frictional coefficient used for contact is determined from FS, FD, and DC, and is assumed to be dependent on the relative velocity of the surfaces in contact:

µc = FD+(FS-FD) e^-DC(v_rel)

The coefficient for viscous friction, VC, is necessary to limit the friction force to a maximum. A limiting force is computed:

F_lim = VC(A_cont)

where A_cont 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 σ_o is the yield stress of the contacted material.

If a part number is input for Cont or Targ, it must represent a valid explicit dynamics part definition. For example, an elastic material for explicit dynamics requires EX, NUXY, and DENS. If any part of the material definition is missing for the part, the EDCGEN command will be ignored.

In addition to the contact parameters on this command, you can specify penalty scale factors for the contact (slave) and target (master) surfaces by using the EDCMORE command.

Duplicate definitions of the same contact type on the same components or parts will cause only one contact to be defined (previous definitions will be ignored). Duplicate definitions of different contact types on the same components or parts will cause multiple contact types to be defined.

Use the EDCLIST and EDDC commands to list and delete contact surface specifications. Use the EDPC command to select and plot contact entities.

The EDCGEN command is not supported in an explicit dynamic full restart analysis (EDSTART,3). Thus, you cannot add new contact specifications in a full restart. You can use the EDCLIST command to list any contact specifications that were defined in the previous analysis.

EDCGEN is also valid in SOLUTION.

Distributed ANSYS Restriction This command is not supported in Distributed ANSYS.

Menu Paths

Main Menu>Preprocessor>LS-DYNA Options>Contact>Define Contact