CONTPRM

Bulk Data Entry Defines the default properties of all contacts and sets parameters that affect all contacts.

The default values set here can be overridden by values explicitly specified on PCONT, PCONTX, and CONTACT cards.

Note: These defaults do not apply to properties of individual gap elements that are specified on PGAP cards.

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. NO (Default) YES
`ALM`	Controls the activation of the augmented Lagrange multiplier (ALM) method for nonlinear contact. 9 YES Activates the Augmented Lagrange Multiplier method for nonlinear contact.
`ALMPTOL`	Controls the penetration tolerance and is effective when the augmented Lagrange multiplier method is activated. 10 Negative value (`ALMPTOL` = Real < 0.0) Defines a scaling factor applied to an average characteristic edge length of the contact interface. The scaling factor is equal to \|Real < 0.0\|. Positive value (`ALMPTOL` = Real > 0.0) Defines an absolute tolerance. 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 AUTO (Default) SOFT HARD Negative value (`ALMSFKN` = Real < 0.0) Defines a stiffness scaling factor. The stiffness scaling factor is equal to \|Real < 0.0\|. The scaling is applied to an automatic stiffness value (the stiffness value when `SFKN`=AUTO). Positive value (`ALMSFKN` = Real > 0.0) Directly prescribed stiffness.
`CHKDUP`	Controls activation of contact duplication check. 0 (Default) Contact duplication check is turned off. 1 Contact duplication check is turned on. A warning is issued if any of the following cases is detected for contact interfaces A and B: Grids on the secondary side of contact A are all included by the secondary side of contact B, and grids on the main side of contact A are all included by the main side of contact B. Grids on the secondary side of contact A are all included by the secondary side of contact B, and the main side of contact A includes all the grids on the main side of contact B. Grids on the secondary side of contact A are all included by the main side of contact B, and grids on the main side of contact A are all included by the secondary side of contact B. Grids on the secondary side of contact A are all included by the main side of contact B, and the main side of contact A includes all the grids on the secondary side of contact B.
`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 NO (Default) YES
`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. NO (Default) YES
`CONTMPC`	Outputs internally created MPC's used to generate TIE contact. The MPC's are output to: <filename>_contmpc.fem. NO (Default) YES
`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. NO (Default) YES
`CORIENT`	Indicates whether the main orientation field `MORIENT` on the CONTACT card applies to all surfaces or if it excludes solid elements. ONSHELL (Default) `MORIENT` applies only to contact mains that consist of shell elements or patches of grids. Main surfaces defined as faces of solid elements always push outwards, irrespective of initially open or pre-penetrating contact. ONALL `MORIENT` applies to all contact mains including, in particular, solid elements.
`DISCRET`	Contact discretization approach for all the CONTACT/TIE entries which do not have an explicit `DISCRET` specification. N2S (Default) S2S
`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. AUTO (Default) or Blank Friction model based on Elastic Slip Distance, with the distance selected as 0.5% of the average characteristic edge length of all the CONTACTs. LONG Friction model based on Elastic Slip Distance, with the distance selected as 10% of the average characteristic edge length of all the CONTACTs. Real > 0.0 Friction model based on Elastic Slip Distance, with the distance selected as Real > 0.0. 0.0 Friction model based on fixed transverse stiffness `KT`.
`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 THICK (Default) NONE (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. 0 (Default) The value of tangential stiffness `KT` = 0.1`STIFF`. For N2S contact with CGAPG-core, the dimension of `STIFF` and `KT` is Force/Length; for N2S contact without CGAPG-core, the dimension of `STIFF` and `KT` is Force/(Length³); for S2S contact, the dimension of `STIFF` and `KT` is Force/(Length³). 1 The value of tangential stiffness `KT` = `MU1``STIFF`. The dimension of `STIFF` and `KT` is Force/(Length³). (Integer)
`LSLDCLR`	Indicates whether `CLEARANCE` is allowed for finite/continuous sliding (`TRACK`=FINITE/CONSLI) contact with large displacement analysis. YES NO (Default)
`MAXPNTR`	Coefficient to decide the maximum allowed penetration for adaptive contact penalty. 7 Default = 0.001 (Real > 0.0)
`MU1`	Coefficient of static friction ( $μ$ _s) 3 4 Default = 0.0 (Real ≥ 0.0 or STICK or FREEZE)
`MU2`	Coefficient of kinetic friction ( $μ$ _k). Default = `MU1` (0.0 < Real < `MU1`)
`N2SFORM`	Controls the core element formulation used for N2S contact. NOCGAPG CGAPG core is not 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. YES (Default) The grids which are not tied are output as a grid SET to the <filename>_nontied.fem file. NO The non-tied grids are not output.
`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. NO (Default) YES
`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). YES (Default) Initial self-penetrations are recognized and resolved in self-contact areas. There is some danger of finding false self-penetrations across solids thinner than `SRCHDIS`. Refer to Resolution of Pre-penetration (CONTPRM,SFPRPEN) in the User Guide. NO There is no pre-penetrations to be resolved in self-contact areas, except maybe minimal intrusions due to meshing, and so on. Any self-penetrations larger than minimum element size will be ignored in those areas.
`STABILIZ`	Controls activation of adaptive contact stabilization. ADAPTIVE Activates a rapid decaying 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. PENALTY (Default for Implicit Analysis) PENALTY-based formulation of the TIE contact. MPC (Default for Explicit Analysis) Activates the MPC-based formulation of TIE contact. Note: Default switched automatically to PENALTY if over-constraint condition exits.
`TUNESTF`	Controls activation of Adaptive Contact Penalty. Automatic tuning of contact penalty for implicit nonlinear analysis. 6 0 (Default) Adaptive contact penalty is turned off. 1 Adaptive contact penalty is turned on.

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.
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
For more information, refer to Augmented Lagrange Multiplier (ALM) Method (Nonlinear Analysis) in the User Guide.
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

Where, $w = \frac{1}{\sqrt{0.1 |S F K N|}}$ is an additional scaling factor effective for -10.0 ≤ SFKN ≤ 0.0. This scaling also applies to SFKN =AUTO or SOFT, and for SFKN≤10.0, or SFKN > 0.0, w = 1.0.
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.