-
AUTOMATIC OVERCLOSURE RESOLUTION
-
This parameter applies only to Abaqus/Explicit analyses.
Include this parameter to store offsets instead of adjusting nodes during initial
overclosure resolution between surface pairs in the general contact domain as
specified in the data lines.
-
BEAM CROSS SECTION
-
By default, contact calculations for noncircular beams are based on the internally
generated surface-element representation of their cross-sections. For circular beams
and pipes, the contact calculations use contact edges and nodes with a radius equal to
the section radius.
Set
BEAM CROSS SECTION=EXACT
to activate contact calculations based on the internally generated surface-element
representation of the beam cross-sections for the entire model.
Set
BEAM CROSS SECTION=CIRCUMSCRIBED CIRCLE
to activate contact calculations based on the circumscribed circle representation of
the beam cross-sections for the entire model.
-
CONTACT THICKNESS REDUCTION
-
This parameter applies only to Abaqus/Explicit analyses.
Set
CONTACT THICKNESS REDUCTION=SELF
to limit automatic contact thickness reductions to only regions of potential
self-contact and the perimeters of shell surfaces for the entire model.
Set
CONTACT THICKNESS REDUCTION=NOPERIMSELF
to limit automatic contact thickness reductions to only regions of potential
self-contact for the entire model.
-
NODAL EROSION
-
This parameter applies only to Abaqus/Explicit analyses.
Set
NODAL EROSION=NO
(default) to keep a node of an element-based surface in the general contact domain as
a point mass after all contact faces and edges to which it is attached have eroded.
Set
NODAL EROSION=YES
to delete a node of an element-based surface from the general contact domain once all
contact faces and edges to which it is attached have eroded.
-
NORMAL EVOLUTION
-
This parameter applies only to Abaqus/Explicit analyses with cohesive contact behavior.
Set
NORMAL EVOLUTION=MAIN
(default) to have the contact normal direction evolve with the main surface normal
direction.
Set
NORMAL EVOLUTION=AVERAGE
to have the contact normal direction evolve with the average evolution of the main and
the secondary surface normal directions.
-
ROTATIONAL TERMS
-
This parameter applies only to Abaqus/Explicit analyses.
Set
ROTATIONAL TERMS=NONE
(default) to ignore the effects of shell and beam thickness offsets for contact.
Set
ROTATIONAL TERMS=STRUCTURAL
to account for the effects of shell and beam thickness offsets for contact.
-
SHELL REPRESENTATION
-
This parameter applies only to general contact in Abaqus/Standard analyses.
Set
SHELL REPRESENTATION=REFERENCE SURFACE
(default) to represent shells in general contact by the shell reference surface.
Set
SHELL REPRESENTATION=EXTRA PERIMETER FACES
to represent shell perimeter regions in general contact with internally generated
surface elements near the exterior of the shell, with nonperimeter regions represented
by the shell reference surface.
-
THREAD MESH GENERATION
-
This parameter applies only to general contact in Abaqus/Standard analyses.
Include this parameter to activate the surface element representations of the
external and internal threads.
-
TYPE
-
Set
TYPE=ENFORCEMENT METHOD
to assign the numerical enforcement method of the contact constraints. This option
applies only to Abaqus/Standard analyses. It cannot be used in conjunction with the SURFACE BEHAVIOR,
DIRECT; SURFACE BEHAVIOR,
AUGMENTED LAGRANGE; or SURFACE BEHAVIOR,
PENALTY options.
Set
TYPE=FOLD INVERSION CHECK
to activate the fold inversion check.
Set
TYPE=FRICTION ENFORCEMENT
to assign the numerical friction enforcement of the "stick" condition of contact
constraints. This option applies only to Abaqus/Standard analyses. It cannot be used in conjunction with the FRICTION,
SLIP TOLERANCE; FRICTION,
ELASTIC SLIP; or FRICTION,
LAGRANGE options.
Set
TYPE=PERMEABILITY CONSTRAINT METHOD
to assign the contact permeability constraint method. This option applies only to Abaqus/Standard analyses. It cannot be used in conjunction with the CONTACT PERMEABILITY,
CONSTRAINT METHOD option.
Set
TYPE=SCALE PENALTY
to assign a scale factor to the default penalty stiffnesses. This option applies only
to Abaqus/Explicit analyses.
Set
TYPE=TRACKING THICKNESS
to assign a thickness that determines the contact tracking distance. It cannot be used
in conjunction with the SURFACE INTERACTION,
TRACKING THICKNESS option.