CNCHECK

CNCHECK, Option, RID1, RID2, RINC, InterType, TRlevel, Val1, Val2, Val3
Provides and/or adjusts the initial status of contact pairs.

PREP7: Database

SOLUTION: Analysis Options

Option

Option to be performed:

DETAIL	—	List all contact pair properties (default).
SUMMARY	—	List only the open/closed status for each contact pair.
POST	—	Execute a partial solution to write the initial contact configuration to the jobname.rcn file.
ADJUST	—	Physically move contact nodes to the target in order to close a gap or reduce penetration. The initial adjustment is converted to structural displacement values (UX, UY, UZ) and stored in the jobname.rcn file.
MORPH	—	Physically move contact nodes to the target in order to close a gap or reduce penetration, and also morph the underlying solid mesh. The initial adjustment of contact nodes and repositioning of solid element nodes due to mesh morphing are converted to structural displacement values (UX, UY, UZ) and stored in the jobname.rcn file.
TADJUST	—	Physically move target body to the contact surface in order to close a gap or reduce penetration. The initial adjustment is converted to structural displacement values (UX, UY, UZ) and stored in the jobname.rcn file.
RESET	—	Reset target element and contact element key options and real constants to their default values. This option is not valid for general contact.
AUTO	—	Automatically sets certain real constants and key options to recommended values or settings in order to achieve better convergence based on overall contact pair behaviors. This option is not valid for general contact.
TRIM	—	Trim contact pair (remove certain contact and target elements).
OVER	—	When a rigid beam or a weld joint connects to a rigid surface constraint or a rigid body, automatically convert the rigid beam elements (MPC184) to rigid target or contact elements. In addition, if `Val1` = 1 is set, when a Lagrange-multiplier-based joint element connects a rigid surface constraint or a rigid body, also switch to the penalty method (KEYOPT(2) = 1 of MPC184).
UNSE	—	Unselect certain contact and target elements.
SPLIT	—	Split base (original) contact pairs into smaller sub-pairs at the preprocessing (/PREP7) level. The main intent of this option is to achieve better scalability in a distributed-memory parallel (DMP) run. The splitting operation may create additional overlapping contact elements at the split boundaries. Contact pairs can only be split once. Repeated use of this option results in no further splitting for those contact pairs already split.
DMP	—	This option is similar to the SPLIT, but it is more automatic and contact pair-splitting is done at the solution level (SOLVE) of the first load step, not at the preprocessing level. This option is activated only in a distributed-memory parallel (DMP) run. For this option, `TRlevel`, `InterType`, and `Val1` are valid. All other arguments are ignored.
MERGE	—	Merge all contact sub-pairs that were previously split (by prior `Option` = SPLIT or DMP operations) back to their original pairs. Any contact and target elements deleted due to the trim logic of the splitting operation cannot be recovered by the MERGE operation. All other arguments are ignored.

RID1, RID2, RINC

The meanings of RID1, RID2, and RINC vary depending on the contact type or the Option specified, as described below. RID1 accepts tabular input for some Option values. RID1, RID2, RINC are ignored when Option = DMP.

Pair-Based Contact — For pair-based contact, the range of real constant pair IDs for which Option will be performed. If RID2 is not specified, it defaults to RID1. If no value is specified, all contact pairs in the selected set of elements are considered.

General Contact — For general contact (InterType = GCN), RID1 and RID2 are section IDs associated with general contact surfaces instead of real constant IDs. If RINC = 0, the Option is performed between the two sections, RID1 and RID2. If RINC > 0, the Option is performed among all specified sections (RID1 to RID2 with increment of RINC).

Contact Splitting — For contact splitting at the preprocessing level (Option = SPLIT only), RID1, RID2, and RINC are used as follows:

If RID1, RID2, and RINC are non-zero and positive, split the contact pairs from real constant pair ID number RID1 to RID2 in increments of RINC. In this case, if TRlevel is non-zero, it will only be applied to these specified pairs.
If RID1 is zero or blank, TRlevel will take affect for all contact pairs in the model from largest to smallest.
If RID1, RID2, RINC, and TRlevel are not defined, the program automatically determines the number of sub-pairs for splitting each contact pair.

Tabular Input for RID1 — RID1 accepts tabular input in the form of a 2D array when Option = ADJUST, MORPH or TADJUST. In this case, RID2, RINC, Val1, Val2, and Val3 are ignored. For more information, see Physically Moving Contact Nodes Toward the Target Surface in the Contact Technology Guide.

InterType

The type of contact interface (pair-based versus general contact) to be considered; or the type of contact pair to be trimmed, unselected, or auto-set.

The following labels specify the type of contact interface:

(blank)	—	Include all contact definitions (pair-based and general contact).
GCN	—	Include general contact definitions only (not valid when `Option` = RESET or AUTO).

The following labels specify the type of contact pairs to be trimmed/unselected/auto-set (used only when Option = TRIM, UNSE, or AUTO, and only for pair-based contact definitions):

ANY	—	All types (default).
MPC	—	MPC-based contact pairs (KEYOPT(2) = 2).
BOND	—	Bonded contact pairs (KEYOPT(12) = 3, 5, 6).
NOSP	—	No separation contact pairs (KEYOPT(12) = 2, 4).
SMAL	—	Small sliding contact pairs (KEYOPT(18) = 1).
SELF	—	Self contact pairs (target surface completely overlaps contact surface).
INAC	—	Inactive contact pairs (symmetric contact pairs for MPC contact or KEYOPT(8) = 2).

The following labels specify the type of contact pairs to be split, and are used only when Option = DMP or SPLIT, and only for pair-based contact definitions:

(blank)	—	All types.
MPC	—	MPC-based contact pairs (KEYOPT(2) = 2).
BOND	—	Bonded contact pairs (KEYOPT(12) = 3, 5, 6).
NOSP	—	No separation contact pairs (KEYOPT(12) = 2, 4).
SMAL	—	Small sliding contact pairs (KEYOPT(18) = 1).

TRlevel

This argument is either the trimming level for trimming contact pairs, or the number of sub-pairs for contact splitting or executing a partial solution.

Trimming level (used only when Option = TRIM, UNSE, or MORPH):

(blank)	—	Normal trimming (default): remove/unselect contact and target elements which are in far-field.
AGGRE	—	Aggressive trimming: remove/unselect contact and target elements which are in far-field, and certain elements in near-field.

Number of sub-pairs used for contact splitting (used only when Option = SPLIT or DMP):

(blank)	—	The program automatically chooses the number of sub-pairs for splitting in order to achieve better scalability in a DMP run.
*`N`*	—	Input a non-zero positive number to indicate the maximum number of sub-pairs for splitting the largest contact pair in the model. All other smaller contact pairs will be split following this number proportionally. The number you input may not always be honored. Splitting may result in a fewer number of sub-pairs basing on many factors.

Effect of initial interface treatment used for or executing a partial solution (when Option = POST):

(blank)	—	The program follows settings of KEYOPT(9) of contact element type for every contact pair to report numerical penetration/gap.
*`1`*	—	The program ignores settings of KEYOPT(9) of contact element type for every contact pair to report geometrical penetration/gap.

The remaining arguments, Val1, Val2, and Val3, are parameters that control initial contact adjustment. They are only valid when Option = ADJUST, MORPH, TADJUST, OVER, DMP, or SPLIT. The meaning of these arguments varies depending on the Option setting.

When Option = ADJUST or MORPH, Val1, Val2, and Val3 are CGAP, CPEN, and IOFF, respectively:

CGAP: Control parameter for opening gap; must be greater than zero. Close the opening gap if the value of the gap is smaller than the CGAP value. CGAP defaults to 0.25*PINB (where PINB is the pinball radius) for bonded and no-separation contact. Otherwise, it defaults to the value of real constant ICONT.
CPEN: Control parameter for initial penetration. CPEN must be greater than zero. Close the initial penetration if the value of the penetration is smaller than the CPEN value. CPEN defaults to 0.25*PINB (where PINB is the pinball radius) for any type of interface behavior (either bonded or standard contact).
IOFF: Control parameter for initial adjustment. Input a positive value to adjust the contact nodes towards the target surface with a constant interference distance equal to IOFF. Input a negative value to adjust the contact node away from the target surface with a uniform gap distance equal to the absolute value of IOFF.

When Option = TADJUST, Val1 and Val2 are PMAX and PMIN, respectively (Val3 is not used):

*`PMAX`*	—	Upper limit of initial allowable penetration.
*`PMIN`*	—	Lower limit of initial allowable penetration.

When Option = SPLIT or DMP, Val1 is the label that specifies the type of contact pairs to be trimmed (only for pair-based contact definitions):

*`(blank)`*	—	The program automatically deletes inactive contact pairs defined by auto-asymmetric selection (KEYOPT(8) = 2). If `Option` = DMP, the program also trims split contact pairs that are associated with bonded contact (KEYOPT(12) = 5 or 6) or small sliding contact (KEYOPT(18) = 1).
*`TRIM`*	—	The program automatically deletes inactive contact pairs defined by auto-asymmetric selection (KEYOPT(8) = 2), and also trims all split contact pairs.

When Option = TRIM or DMP, Val1 is the label that specifies the "global" pinball value used by contact pairs to be trimmed. When Option = DMP, "TRIM" needs to be set at Val1 to activate this feature. The global pinball value must be positive.

Notes

The CNCHECK command provides information for surface-to-surface, node-to-surface, and line-to-line contact pairs (element types TARGE169, TARGE170, CONTA172, CONTA174, CONTA175, CONTA177). All contact and target elements of interest, along with the solid elements and nodes attached to them, must be selected for the command to function properly. For performance reasons, the program uses a subset of nodes and elements based on the specified contact regions (RID1, RID2, RINC) when executing the CNCHECK command.

CNCHECK is available in both the PREP7 and SOLUTION processors, but only before the first solve operation (that is, only before the first load step or the first substep).

If the contact and target elements were generated through mesh commands (AMESH, LMESH, etc.) instead of the ESURF command, you must issue MODMSH,DETACH before CNCHECK. Otherwise, CNCHECK will not work correctly.

The following additional notes are available:

`Option` = POST

The command CNCHECK,POST solves the initial contact configuration in one substep. After issuing this command, you can postprocess the contact result items as you would for any other converged load step. However, only the contact status, contact penetration or gap, and contact pressure will have meaningful values. Other contact quantities (friction stress, sliding distance, chattering) will be available but are not useful.

Initial contact results obtained and listed from CNCHECK,DETAIL, CNCHECK,POST, and the actual solution may not be always consistent with each other. The discrepancy is mainly due to applied boundary conditions and solution options. Contact results from CNCHECK,POST are, in general, closer to what the solution will provide than those from CNCHECK,DETAIL.

To inspect the real geometric penetration and gap, specify TRLEVEL=1. The program will set KEYOPT(9) = 0 internally during the execution of CNCHECK,POST.

Because Option = POST forces a solve operation, the PrepPost (PP) license does not work with CNCHECK,POST.

If CNCHECK,POST is issued within the solution processor, the SOLVE command that solves the first load step of your analysis should appear in a different step, as shown in the following example:

/SOLU
CNCHECK,POST
FINISH
. . .

/SOLU
SOLVE
FINISH
. . .

CNCHECK,POST writes initial contact results to a file named jobname.rcn. The command should be issued before defining analysis type, solution options, and boundary conditions. If the command is issued later, a segmentation violation error may occur. When postprocessing the initial contact state, you need to explicitly read results from this file using the FILE and SET,FIRST commands in POST1 to properly read the corresponding contact data. Otherwise, the results may be read improperly. The following example shows a valid command sequence for plotting the initial contact gap:

/SOLU
CNCHECK,POST
FINISH
/POST1
FILE,Jobname,RCN
SET,FIRST
PLNSOL,CONT,GAP,0,1
FINISH
. . .

`Option` = ADJUST or MORPH

You can issue CNCHECK,ADJUST to physically move contact nodes to the target surface. Alternatively, you can issue CNCHECK,MORPH to physically move contact nodes to the target surface and then morph the underlying mesh to improve the mesh quality. See Physically Moving Contact Nodes Toward the Target Surface in the Contact Technology Guide for more information. Similar to the POST option, if CNCHECK,ADJUST or CNCHECK,MORPH is issued within the solution processor, the SOLVE command that solves the first load step of your analysis should appear in a different step:

/SOLU
CNCHECK,ADJUST
FINISH
. . .

/SOLU
SOLVE
FINISH
. . .

After issuing the CNCHECK,ADJUST command, the initial adjustment is converted to structural displacement values (UX, UY, UZ) and stored in a file named jobname.rcn. Similarly, the CNCHECK,MORPH command converts the initial adjustment of contact nodes as well as the morphing adjustment of solid element nodes to structural displacement values (UX, UY, UZ) and stores them in the jobname.rcn file. You can use this file to plot or list nodal adjustment vectors or create a contour plot of the adjustment magnitudes via the displacements. When postprocessing the nodal adjustment values, you need to explicitly read results from this file using the FILE and SET,FIRST commands in POST1 to properly read the corresponding contact data. Otherwise, the results may be read improperly.

Note: The jobname.rcn file contains information generated from the CNCHECK,POST, CNCHECK,ADJUST, CNCHECK,MORPH, or CNCHECK, TADJUST command. If multiple commands are issued in the same analysis, the file is overwritten by the last CNCHECK command.

`Option` = TADJUST

You can issue CNCHECK,TADJUST to physically move the target body to the contact surface. This command tries to establish initial contact with penetration in a range specified by PMAX and PMIN. Similar to the ADJUST and MORPH options, the initial adjustment is converted to structural displacement values (UX, UY, UZ) and stored in the jobname.rcn file. This option accepts tabular input in the RID1 field.

You can specify either a positive or negative value for PMIN and PMAX. The program interprets a positive value as a scaling factor and interprets a negative value as the absolute value.

For more information, see Physically Moving the Target Body Toward the Contact Surface in the Contact Technology Guide.

`Option` = RESET

The command CNCHECK,RESET allows you to reset all but a few key options and real constants associated with the specified contact pairs (RID1, RID2, RINC) to their default values. This option is only valid for pair-based contact definitions.

The following key options and real constants remain unchanged when this command is issued:

Element type	Key options not affected by RESET	Real constants not affected by RESET
TARGE169, TARGE170	KEYOPT(2), KEYOPT(3)	R1, R2
CONTA172	KEYOPT(1), KEYOPT(3)	R1, R2
CONTA174, CONTA175, CONTA177	KEYOPT(1)	R1, R2

`Option` = AUTO

The command CNCHECK,AUTO automatically changes certain default or undefined key options and real constants to optimized settings or values. The changes are based on overall contact pair behaviors. In general, this command improves convergence for nonlinear contact analysis. This option is only valid for pair-based contact definitions.

The tables below list typical KEYOPT and real constant settings implemented by CNCHECK,AUTO. The actual settings implemented for your specific model may vary from what is described here. You should always verify the modified settings by issuing CNCHECK,DETAIL to list current contact pair properties.

KEYOPT

Description

Default (0 or blank)

CNCHECK,AUTO

Selects DOF set

Structural DOFs

Automatic selection based on DOFs of underlying elements.

Contact algorithm

Augmented Lagrange

1- Penalty for rigid-rigid contact [1].

Location of contact detection point

Gauss point

2 - Normal to target surface if KEYOPT(2) > 1.

CNOF/ICONT adjustment

No adjustment

1 - Auto CNOF if tiny gap exists.

Contact stiffness variation

Use default range

1 - Nominal refinement for opening contact or underlying elements having TB plasticity.

2 - Aggressive refinement for opening contact and underlying elements having TB plasticity.

Element level time increment control

No control

1 - Automatic bisection for self contact.

4 - Impact constraint for opening contact and transient analyses.

Assymetric contact selection

No action

2 - Auto selection if KEYOPT(2) > 1.

Effect of initial penetration or gap

Include all

1 - Exclude if KEYOPT(5) = 1, or if ICONT was previously specified.

Contact stiffness update

Between load steps

0 - Between iterations except when underlying elements are superelements. [2]

Set to 0 if KEYOPT(2) > 1 for debonding.
Set to 1 if underlying elements are superelements, or if KEYOPT(9) = 2 was previously specified.

Real Constants		Description	Default	CNCHECK,AUTO
No.	Name	Description	Default	CNCHECK,AUTO
3	FKN	Normal penalty stiffness factor	1	Set to 5 if KEYOPT(9) = 2 (ramp initial penetration) and KEYOPT(10) > 0.
6	PINB	Pinball region	see [1]	Cut in half if spurious contact is detected or contact searching is slow.
14	TCC	Thermal contact conductance	0	Calculated as a function of highest conductivity of underlying element and overall model size.
19	ECC	Electric contact conductance	0	Calculated as a function of highest permitivity or lowest resistivity of underlying element and overall model size.
26	MCC	Magnetic contact permeance	0	Calculated as a function of highest emissivity of underlying element and overall model size.
37	PCC	Pore fluid contact permeability coefficient	0	Calculated as a function of highest permitivity of underlying element and overall model size.

PINB default depends on contact behavior (rigid vs. flexible target), NLGEOM,ON or OFF, KEYOPT(9) setting, KEYOPT(12) setting, and the value of real constant CNOF (see Defining the Pinball Region (PINB)).

CNCHECK,AUTO also sets PRED,OFF for the case of a force-distributed constraint defined via MPC contact.

Removing or Unselecting Contact and Target Elements (`Option` = TRIM/UNSEL)

You can issue CNCHECK,TRIM or CNCHECK,UNSEL to remove or unselect contact and target elements which are in far-field (that is, open and not near contact), or even in near-field if aggressive trimming logic is used (TRlevel = AGGRE).

`Option` = SPLIT, DMP, or MERGE

The SPLIT, DMP, and MERGE options are intended for use in a distributed-memory parallel (DMP) run. Use the command CNCHECK,SPLIT or CNCHECK,DMP to split large contact pairs into smaller sub-pairs so that the smaller contact pairs can be distributed into different cores, thereby improving performance. This functionality is not the same as manually splitting contact pairs during the modeling process. The program splitting logic performs the necessary exchange of data on the boundaries between the split contact pairs to ensure that the results with and without splitting are essentially identical. CNCHECK,DMP also performs trimming for bonded, small-sliding, and removing inactive pairs from auto-asymmetric contact definition before splitting to improve load balance ratio of DMP runs.

The command CNCHECK,MERGE can be used to merge the sub-pairs together again, which is useful for postprocessing the contact results based on the original contact pair geometry. However, caution must be taken when a downstream analysis is performed since the MERGE operation may alter the database.

For more information, see Solving Large Contact Models in a Distributed-Memory Parallel Environment in the Contact Technology Guide.

Menu Paths

Main Menu> Preprocessor> Modeling> Create> Contact Pair

CNCHECK

Notes

Option = POST

Option = ADJUST or MORPH

Option = TADJUST

Option = RESET

Option = AUTO

Removing or Unselecting Contact and Target Elements (Option = TRIM/UNSEL)

Option = SPLIT, DMP, or MERGE