# 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.

## Parameters for OptiStruct Analysis

Name Values SI Unit Example
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)

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)

MU1 Coefficient of static friction ( $\mu$ s) 3 4

Default = 0.0 (Real ≥ 0.0 or STICK or FREEZE)

MU2 Coefficient of kinetic friction ( $\mu$ k).

Default = MU1 (0.0 < Real < MU1)

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

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

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

CONTMPC Outputs internally created MPC's used to generate TIE contact. The MPC's are output to: <filename>_contmpc.fem.
NO (Default)
YES

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.

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.

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.

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.

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.

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.
NO (Default)
YES

DISCRET Contact discretization approach for all the CONTACT/TIE entries which do not have an explicit DISCRET specification.
N2S (Default)
S2S

LSLDCLR Indicates whether CLEARANCE is allowed for finite/continuous sliding (TRACK=FINITE/CONSLI) contact with large displacement analysis.
YES
NO (Default)

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.

STABILIZ Controls activation of adaptive contact stabilization.
Activates a rapid decaying contact stabilization.

If CONTPRM,STABILIZ,ADAPTIVE parameter is not present, then adaptive contact stabilization is not activated.

No default

MAXPNTR Coefficient to decide the maximum allowed penetration for adaptive contact penalty. 7

Default = 0.001 (Real > 0.0)

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)

## Parameters for Explicit Dynamic Analysis via Radioss Integration (ANALYSIS = EXPDYN)

Name Values SI Unit Example
STFAC Interface stiffness scale factor.

Default = 1.0 in implicit analysis

Default = 0.1 in explicit analysis

(Real ≥ 0)

FRIC Coulomb friction.

Default = 0.0 (Real ≥ 0)

GAP Gap for impact activation. 10 11

(Real ≥ 0)

IDEL Node and segment deletion flag.
0 (Default)
No deletion.
1
When all of the elements (shells, solids) associated to one segment are deleted, the segment is removed from the main side of the interface. Additionally, non-connected nodes are removed from the secondary side of the interface.
2
When a shell or a solid element is deleted, the corresponding segment is removed from the main side of the interface. Additionally, non-connected nodes are removed from the secondary side of the interface.

(Integer)

INACTI Handling of initial penetrations flag. 13
Default as defined by CONTPRM (Integer = 0, … , 5)
0
No action.
1
Deactivation of stiffness on nodes.
2
Deactivation of stiffness on elements.
3
Change secondary node coordinates to avoid small initial penetrations.
4
Change main node coordinates to avoid small initial penetrations.
5
Gap is variable with time but initial gap is slightly de-penetrated as:
$ga{p}_{0}=gap-{P}_{0}^{}-0.05\cdot \left(gap-{P}_{0}\right)$

Valid in explicit analysis: 0, 1, 2, 3 and 5.

Valid in implicit analysis: 0, 3 and 4.

Invalid entries are ignored.

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.

IFRIC Friction formulation flag. 15
COUL (Default)
Static Coulomb friction law.
GEN
Generalized viscous friction law.
DARM
REN
Renard friction law.

In implicit computation, only IFRIC = COUL is implemented.

(Character)

IFILTR Friction filtering flag. 14
NO (Default)
No filter is used.
SIMP
Simple numerical filter.
PER
Standard -3dB filter with filtering period.
CUTF
Standard -3dB filter with cutting frequency.

(Character)

FFAC Filtering coefficient (Only with IFILTNO).

(0.0 < Real < 1.0)

IFORM Friction penalty formulation type. 16 17
VISC (Default)
Viscous (total) formulation.
STIFF
Stiffness (incremental) formulation.

(Character)

C1, C2, C3, C4, C5, C6 Friction law coefficients.

(Real > 0)

IGNORE Flag to ignore secondary nodes if no main segment is found for TIE contact. 18
0
No deletion of secondary nodes.
1 (Default)
Secondary nodes with no main segment found are deleted from the interface.
2
Secondary nodes with no main segment found are deleted from the interface; if SRCHDIS is blank, then it would be newly calculated internally.

(Integer)

MTET10 Flag for second order CTETRA as contact main surface.
0 (Default)
TETRA 10 is degenerated on the surface (middle nodes are removed from contact).
1
Four triangular segments are used on each tetra face.

(Integer)

ISYM Symmetric contact flag.
SYM (Default)
Symmetric contact.
UNSYM
Main-secondary contact.

If SSID defines a grid set, the contact is always a main-secondary contact.

(Character)

IEDGE Flag for edge generation from secondary and main surfaces.
NO (Default)
No edge generation.
ALL
All segment edges are included.
BORD
External border of secondary and main surface is used.
FEAT
External border as well as features defined by FANG are used.

(Character)

FANG Feature angle for edge generation in degrees (Only with IEDGE = FEAT).

Default = 91.0 (Real ≥ 0)

IGAP Gap definition flag.
CONST (Default)
Gap is constant and equal to GAP. 11 12
VAR
Gap is variable (in space, not in time) according to the characteristics of the impacting surfaces and nodes. 12

(Character)

ISTF Stiffness definition flag. 9
0 (Default)
The stiffness is computed according to the main side characteristics.
1
STIF1 is used as interface stiffness.
2, 3, 4 and 5
The interface stiffness is computed from both main and secondary characteristics.

(Integer)

STIF1 Interface stiffness (Only with ISTF = 1).

Default = 0.0 (Real ≥ 0)

STMIN Minimum interface stiffness (Only with ISTF > 1).

(Real ≥ 0)

STMAX Maximum interface stiffness (Only with ISTF > 1).

Default = 1030 (Real ≥ 0)

IBC Flag for deactivation of boundary conditions at impact.

(Character = X, Y, Z, XY, XZ, YZ, or XYZ)

VISS Critical damping coefficient on interface stiffness.

Default = 0.05 (Real ≥ 0)

VISF Critical damping coefficient on interface friction.

Default = 1.0 (Real ≥ 0)

BMULT Sorting factor.

Default = 0.20 (Real ≥ 0)

1. 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).
2. 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.
3. 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.
4. 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.
5. 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.

6. Adaptive contact penalty is not applicable to these cases:
• TIE or FREEZE contact
• Contact with nonlinear penalty
• No-separation contact
7. 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.

8. 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.
9. If ISTF ≠ 1, the interface stiffness K is computed from the main segment stiffness Km and/or the secondary segment stiffness Ks.

The main stiffness is computed from $Km=STFAC\cdot B\cdot S\cdot S}{V}$ for solids, $Km=0.5\cdot STFAC\cdot E\cdot t$ for shells as well as when the main segment is shared by a shell and a solid.

The secondary stiffness is an equivalent nodal stiffness computed as for solids: (1)
$Ks=STFAC\cdot B\cdot {V}^{-3}$
For Shells:(2)
$Ks=0.5\cdot STFAC\cdot E\cdot t$
Where,
$B$
Bulk modulus
$S$
Segment area
$E$
Modulus of elasticity
$t$
Shell thickness
$V$
Volume of a solid

There is no limitation to the value of stiffness factor (but a value greater than 1.0 can reduce the initial time step).

ISTF = 0, the interface stiffness $K=Km$

ISTF > 1, the interface stiffness is $K=\mathrm{max}\left(STMIN,\mathrm{min}\left(STMAX,K1\right)\right)$ with:
• ISTF = 2, $K1=0.5\cdot \left(Km+Ks\right)$
• ISTF = 3, $K1=\mathrm{max}\left(Km,Ks\right)$
• ISTF = 4, $K1=\mathrm{min}\left(Km,Ks\right)$
• ISTF = 5, $K1=Km\cdot Ks/\left(Km+Ks\right)$
10. In an implicit analysis, the contact stiffness plays a very important role in convergence. ISTF = 4 (which takes the minimum of main and secondary stiffness's for contact) is recommended. This is because the penalty contact force will be balanced with the internal force of the deformable impacted part, which means the stiffness near the effective stiffness one will converge easier than a higher one.

For small initial gaps in implicit analysis, the convergence will be more stable if a GAP larger than the initial gap is defined.

In implicit analysis, sometimes a stiffness with scaling factor reduction (for example: STFAC = 0.01) or reduction in impacted thickness (if rigid one) might reduce unbalanced forces and improve convergence, particularly in shell structures under bending where the effective stiffness is much lower than membrane stiffness; but it should be noted that too low of a value could also lead to divergence.

11. The default for the constant gap (IGAP = CONST) is the minimum of:
t
Average thickness of the main shell elements
l/10, l
Average side length of the main solid elements
lmin/2, lmin
Smallest side length of all main segments (shell or solid)
12. The variable gap (IGAP = VAR) is computed as gs + gm with:
• gm - main element gap with
• gm = t/2, t: thickness of the main element for shell elements.
• gm = 0 for solid elements.
• gs - secondary node gap:
• gs = 0 if the secondary node is not connected to any element or is only connected to solid or spring elements.
• gs = t/2, t - largest thickness of the shell elements connected to the secondary node.
• gs = 1/2√S for truss and beam elements, with S being the cross-section of the element.

If the secondary node is connected to multiple shells and/or beams or trusses, the largest computed secondary gap is used.

The variable gap is always at least equal to GAPMIN.

13. INACTI = 3 or 4 are only recommended for small initial penetrations and should be used with caution because:
• the coordinate change is irreversible
• it may create other initial penetrations if several surface layers are defined in the interfaces
• it may create initial energy if the node belongs to a spring element
INACTI = 5 works as:
14. IFILT defines the method for computing the friction filtering coefficient. If IFILTNO, the tangential friction forces are smoothed using a filter:(3)
${F}_{T}=\alpha \cdot F{\text{'}}_{T}+\left(1-\alpha \right)\cdot F{\text{'}}_{T-1}$
Where,
${F}_{T}$
Tangential force
$F{\text{'}}_{T}$
Tangential force at time $t$
$F{\text{'}}_{T-1}$
Tangential force at time $t-1$
α
Filtering coefficient
IFILT = SIMP
α = FFAC
IFILT = PER
$\alpha =2\pi dt/FFAC$ , where dt/T = FFAC, $T$ is the filtering period
IFILT = CUTF
$\alpha =2\pi \cdot FFAC\cdot dt$ , where FFAC is the cutting frequency
15. IFRIC defines the friction model.

IFRIC = COUL - Coulomb friction with ${F}_{T}\le \mu \cdot {F}_{N}$ with $\mu =FRIC$

If IFRIC is not COUL, the friction coefficient is set by a function $\left(\mu =\mu \left(p,V\right)\right)$ ,

Where,
$p$
Pressure of the normal force on the main segment
$V$
Tangential velocity of the secondary node

The following formulations are available:

IFRIC = GEN - Generalized viscous friction law(4)
$\mu =Fric+{C}_{1}\cdot p+{C}_{2}\cdot V+{C}_{3}\cdot p\cdot V+{C}_{4}\cdot {p}^{2}+{C}_{5}\cdot {V}^{2}$
IFRIC = DARM - Darmstad law(5)
$\mu ={C}_{1}\cdot {e}^{\left({C}_{2}V\right)}\cdot {p}^{2}+{C}_{3}\cdot {e}^{\left({C}_{4}V\right)}\cdot p+{C}_{5}\cdot {e}^{\left({C}_{6}V\right)}$
IFRIC = REN - Renard law(6)
$\mu ={C}_{1}+\left({C}_{3}-{C}_{1}\right)\cdot \frac{V}{{C}_{5}}\cdot \left(2-\frac{V}{{C}_{5}}\right)\mathit{if}V\in \left[0,{C}_{5}\right]$
(7)
$\mu ={C}_{3}-\left(\left({C}_{3}-{C}_{4}\right)\cdot {\left(\frac{V-{C}_{5}}{{C}_{6}-{C}_{5}}\right)}^{2}\cdot \left(3-2-\frac{V-{C}_{5}}{{C}_{6}-{C}_{5}}\right)\right)\mathit{if}V\in \left[{C}_{5},{C}_{6}\right]$
(8)
$\mu ={C}_{2}-\frac{1}{\frac{1}{{C}_{2}-{C}_{4}}+{\left(V-{C}_{6}\right)}^{2}}\mathit{if} V\ge {C}_{6}$

where,

$\begin{array}{l}{C}_{1}=C1={\mu }_{S},{C}_{2}=C2={\mu }_{d}\\ {C}_{3}=C3={\mu }_{\text{max}},{C}_{4}=C4={\mu }_{\text{min}}\\ {C}_{5}=C5={V}_{cr1},{C}_{6}=C6={V}_{cr2}\end{array}$

• The first critical velocity ${V}_{cr1}$ must be different to 0 (C5 ≠ 0). It also must be lower than the second critical velocity ${V}_{cr2}$ (C5 < C6).
• The static friction coefficient C1 and the dynamic friction coefficient C2 must be lower than the maximum friction C3 (C1C3) and C2C3).
• The minimum friction coefficient C4, must be lower than the static friction coefficient C1 and the dynamic friction coefficient C2 (C4C1 and C4C2).
16. IFORM selects two types of contact friction penalty formulation.
The viscous (total) formulation (IFORM = VISC) computes an adhesive force as:(9)
${F}_{adh}=VISF\cdot Sqrt\left(2Km\right)\cdot {V}_{T}{F}_{T}=\mathrm{min}\left(\mu {F}_{N},{F}_{adh}\right)$
The stiffness (incremental) formulation (IFORM = STIFF) computes an adhesive force as:(10)
${F}_{adh}={F}_{Told}+\text{Δ}{F}_{T}$
(11)
$\text{Δ}{F}_{T}=K\cdot {V}_{T}\cdot dt$
(12)
${F}_{Tnew}=\mathrm{min}\left(\mu {F}_{N},{F}_{adh}\right)$
17. For nonlinear implicit contact with friction, the stiffness formulation (IFORM = STIFF) is recommended.
18. If IGNORE = 1 or 2, the secondary nodes without a main segment found during the searching are deleted from the interface.

If IGNORE = 1 and SRCHDIS is blank, the default value of the distance for searching closest main segment is the average size of the main segments.

If IGNORE = 2 and SRCHDIS is blank, the distance for searching closest main segment for each secondary node is computed as:

${d}_{1}=0.6\cdot \left({T}_{s}+{T}_{m}\right)$

${d}_{2}=0.05\cdot {T}_{md}$

$SRCHDIS=\mathrm{max}\left({d}_{1},\text{\hspace{0.17em}}\text{\hspace{0.17em}}{d}_{2}\right)$

Where,
${T}_{s}$
Thickness of the element connected to the secondary node, for solids ${T}_{s}$ = 0.0
${T}_{m}$
Thickness of main segment, for solids ${T}_{m}$ = Element volume / Segment area
${T}_{\mathrm{md}}$
Main segment diagonal
19. This card is represented as a control card in HyperMesh.