CONTPRM
Bulk Data Entry Defines the default properties of all contacts and sets parameters that affect all contacts.
Format
(1) | (2) | (3) | (4) | (5) | (6) | (7) | (8) | (9) | (10) |
---|---|---|---|---|---|---|---|---|---|
CONTPRM | PARAM1 | VALUE1 | PARAM2 | VALUE2 | PARAM3 | VALUE3 | PARAM4 | VALUE4 | |
PARAM5 | VALUE5 |
Example
(1) | (2) | (3) | (4) | (5) | (6) | (7) | (8) | (9) | (10) |
---|---|---|---|---|---|---|---|---|---|
CONTPRM | GPAD | 0.5 | STIFF | AUTO | MU1 | 0.3 |
Definitions
Field | Contents | SI Unit Example |
---|---|---|
PARAMi | Parameter name. | |
VALi | Parameter value. |
Name | Values | SI Unit Example |
---|---|---|
ADJGRID | Creates a Bulk Data file
that contains contact grid SET's. The coordinates
of these grids are adjusted (ADJUST), and a Bulk Data file that
contains new coordinates of these contact grids after adjustment is
also created. The file names are:
filename_root.adjgset.fem and
filename_root.adjgcrd.fem. For N2N
contact, the file names are:
filename_root.n2n.adjgset.fem and
filename_root.n2n.adjgcrd.fem.
Additionally, the maximum adjusted distance is available in the
.out file.
|
|
ALM | Controls the activation of
the augmented Lagrange multiplier (ALM) method for nonlinear
contact. 9
|
|
ALMPTOL | Controls the penetration
tolerance and is effective when the augmented Lagrange multiplier
method is activated. 10
See Comment 11 for default (Real < 0.0, or Real > 0.0) |
|
ALMSFKN | Controls the relative
penalty stiffness of the contact interface with the augmented
Lagrange multiplier method disregard of any specified
STIFF options. 12
|
|
CHKDUP | Controls activation of
contact duplication check.
|
|
CONTGAP | Creates a Bulk Data file
that contains internally created node-to-surface contact elements
represented as CGAPG elements. The file name is:
filename_root.contgap.fem. 5
|
|
CONTGRID | Creates a Bulk Data file
that contains SET's of grids involved with
surface-to-surface contact elements. The file name is:
filename.root.contgrid.fem.
|
|
CONTMPC | Outputs internally created
MPC's used to generate TIE
contact. The MPC's are output to:
<filename>_contmpc.fem.
|
|
CONTOUT | Depending on the type of
contact discretization, the following file(s) are created. S2S discretization: Creates a Bulk Data file that contains internally generated Surface-to-Surface Contact elements represented as PLOTEL and RBE3 elements for visualization. The file name is: <filename>.contout.fem. N2N discretization: Creates a Bulk Data file that contains
internally generated Node-to-Node Contact elements represented
as RBEAM
JOINTG elements for visualization. The file
name is: <filename>.n2s.fem.
|
|
CORIENT | Indicates whether the main
orientation field MORIENT on the
CONTACT card applies to all surfaces or if it
excludes solid elements.
|
|
DEACTLIN | Controls how
non-FREEZE contacts are handled in linear
analysis.
|
|
DISCRET | Contact discretization
approach for all the
CONTACT/TIE entries which
do not have an explicit DISCRET specification.
|
|
FRICESL | Frictional elastic slip -
distance of sliding up to which the frictional transverse force
increases linearly with slip distance. Specified in physical
distance units (similar to U0 and
GPAD). Refer to Friction in the User Guide.
|
|
GPAD | "Padding" of main or
secondary objects to account for additional layers, such as shell
thickness, and so on. This value is subtracted from contact gap
opening as calculated from location of nodes. 1
(Real) |
|
KA0TUNE | Coefficient to decide the
initial trial penalty for adaptive contact penalty. 8 Default = 1.0 (Real > 0.0) |
|
KTLIN | Controls the tangential
stiffness KT for closed contact in linear
analysis when STIFF = Real > 0.0 and
MU1 = Real > 0.0 on PCONT
referenced by the contact.
(Integer) |
|
LSLDCLR | Indicates whether
CLEARANCE is allowed for finite/continuous
sliding
(TRACK=FINITE/CONSLI)
contact with large displacement analysis.
|
|
MAXPNTR | Coefficient to decide the
maximum allowed penetration for adaptive contact penalty. 7
Default = 0.001 (Real > 0.0) |
|
MU1 | Coefficient of static
friction (
s) 3
4 Default = 0.0 (Real ≥ 0.0 or STICK or FREEZE) |
|
MU2 | Coefficient of kinetic
friction (
k). Default = MU1 (0.0 < Real < MU1) |
|
N2SFORM | Controls the core element
formulation used for N2S contact.
No default Note: If
CONTPRM,N2SFORM,NOCGAPG
is not present, the CGAPG core based
formulation is used when possible for N2S
contact. |
|
NONTIED | Controls the output of
grids which are not tied in the TIE or
CONTACT
(TYPE=FREEZE) interfaces.
|
|
PREPRT | Prints initial contact
conditions (except for MPC-based TIE) into an
ASCII data file. The file name is:
<filename>.cpr. For more information,
refer to .cpr file.
|
|
SFPRPEN | Indicates whether initial
pre-penetrations are recognized and resolved in self-contact areas.
(This only affects self-contact areas, wherein Main and Secondary
belong to the same set or surface).
|
|
STABILIZ | Controls activation of
adaptive contact stabilization.
If CONTPRM,STABILIZ,ADAPTIVE parameter is not present, then adaptive contact stabilization is not activated. No default |
|
STIFF | Relative stiffness of the
contact interface. 2 Positive value (STIFF = Real > 0.0) is directly specified stiffness. Negative value (STIFF = Real < 0.0) defines a stiffness scaling factor. The stiffness scaling factor is equal to |Real < 0.0|. The scaling is applied to the automatic stiffness value (the stiffness value when STIFF = AUTO). Default = AUTO (AUTO, SOFT, HARD, Real > 0.0, or Real < 0.0) |
|
TIE | Indicates the type of
contact formulation that is used when the TIE Bulk Data Entry is present in
the model.
|
|
TUNESTF | Controls activation of
Adaptive Contact Penalty. Automatic tuning of contact penalty for
implicit nonlinear analysis. 6
|
Comments
- The initial gap opening is calculated automatically based on the relative location of secondary and main nodes (in the original, undeformed mesh). To account for additional material layers covering main or secondary objects (such as half of shell thickness), the GPAD entry can be used. GPAD option THICK automatically accounts for shell thickness on both sides of the contact interface (this also includes the effects of shell element offset ZOFFS or composite offset Z0).
- Option STIFF=AUTO determines the value of normal stiffness for each contact element using the stiffness of surrounding elements. Additional options SOFT and HARD create respectively softer or harder penalties. SOFT can be used in cases of convergence difficulties and HARD can be used if undesirable penetration is detected in the solution. A negative value for STIFF indicates that a stiffness scaling factor equal to |Real < 0.0| is defined. This scaling is applied on the stiffness value via STIFF=AUTO.
- MU1=STICK is interpreted in OptiStruct as an enforced stick condition - such contact interfaces will not enter the sliding phase. Of course, the enforced stick only applies to contacts that are closed.
- MU1=FREEZE enforces zero relative displacements on the contact surface - the contact gap opening remains fixed at the original value and the sliding distance is zero. The FREEZE condition applies to all secondary nodes, no matter whether their initial gap is open or closed.
- The file
filename_root.contgap.fem, produced using the
CONTGAP parameter, can be imported into HyperMesh in order to visualize internally created
node-to-surface contact elements (now converted to GAPG
entities).Note: During optimization, this file shows node-to-surface contact elements for the latest optimization iteration. In order to correctly visualize this configuration in HyperMesh for shape optimization problems, the FEA mesh shape needs to be updated by applying "Shape change" results.
Furthermore, if GAPPRM,HMGAPST,YES is activated together with CONTPRM,CONTGAP,YES, then the gap status command file, filename_root.HM.gapstat.cmf, will also include the open/closed status of these additional GAPG's that represent node-to-surface contact elements. For correct visualization of their status in HyperMesh, file filename_root.contgap.fem needs to be imported before running the gap status command file.
- Adaptive contact penalty is not
applicable to these cases:
- TIE or FREEZE contact
- Contact with nonlinear penalty
- No-separation contact
- The maximum allowed penetration for
adaptive contact penalty is selected as MAXPNTR*L.
Where, L is the characteristic edge length (the average edge length on the main surface) of the contact.
- The initial trial penalty for
adaptive contact penalty is selected as:
- KA0TUNE*K
Where, K is an automatically selected raw stiffness value, if STIFF=AUTO for the contact interface.
- The contact penalty stiffness value of STIFF option, otherwise.
- KA0TUNE*K
- The augmented Lagrange multiplier
method is applicable to nonlinear static and transient analyses except when
combined with the following features:
- FREEZE/TIE contact
- CGAP/CGAPG core N2S contact
- Nonlinear penalty or the adaptive penalty method
- The arc-length method
- If the penetration of a secondary node on the main surface exceeds the specified tolerance, additional augmentation iterations will be performed. For no-separation contact, the penetration tolerance is effective for both the penetration and the opening distance once it is closed.
- The default penetration tolerance is
defined relative to the average characteristic edge length, L, of the contact
interface as follows:
- TRACK
- Tolerance
- SMALL(SMDISP)
- L*0.1%*w
- SMALL(LGDISP)
- L*1%*w
- FINITE/CONSLI
- L*5%*w
- The penalty stiffness employed by the augmented Lagrange multiplier method is independent of the STIFF field. Option SFKN=AUTO determines the value of the normal penalty stiffness for each contact element using the stiffness of surrounding elements along the normal direction of the surface. Additional options AUTO, HARD, SOFT or Real < 0.0 are available as a scaling factor applied on the stiffness value via SFKN=AUTO.
- This card is represented as a control card in HyperMesh.