#### Command list

• Input handling
• Solution control and techniques
• Output
• Mesh commands
• Nodes and connectivity
• Material properties
• Initial conditions
• Boundary conditions
• Contact and tied interfaces
• Rigid bodies
• Connectors
• Parameters and functions
• Geometries
• Sets
• Coordinate system
• Particle
• SPH

### CONTACT

###### Contact and tied interfaces
*CONTACT
"Optional title"
coid, accuracy_level
entype${}_1$, enid${}_1$, entype${}_2$, enid${}_2$, $\mu$, $pfac$, $t_{beg}$, $t_{end}$
merge, $\xi$, gid${}_0$, gid${}_1$, $\delta_{0}^{offset}$, $\delta_{0}^{max}$, $\delta^{edge}$
fid${}_{wear1}$, fid${}_{wear2}$, fid${}_{thermal}$, $\alpha_{edge}$, one_way, no_internal

#### Parameter definition

VariableDescription
coid Contact command ID
accuracy_level Accuracy level
options:
1 $\rightarrow$ low
2 $\rightarrow$ standard
>2 $\rightarrow$ high
default: 2
entype${}_1$ Entity type of Surface 1
options: P, PS, ALL
enid${}_1$ Entity identification number of Surface 1
entype${}_2$ Entity type of Surface 2
options: P, PS, ALL
enid${}_2$ Entity identification number of Surface 2
$\mu$ Coulomb coefficient of friction or FUNCTION (see example below)
options: constant, fcn
default: 0
$pfac$ Penalty stiffness (contact pressure per unit distance of penetration)
default: automatic calculaton of stiffness
$t_{beg}$ Contact activation time
default: 0
$t_{end}$ Contact deactivation time
default: 1.0e20
merge Flag to activate merged faces in the contact
options:
0 $\rightarrow$ merged faces are inactive
1 $\rightarrow$ merged faces are active
$\xi$ Fraction of critical damping
default: 0.1
gid${}_0$ Faces outside the geometry at time 0 are excluded from the contact
default: not used
gid${}_1$ Faces moving outside the geometry are deactivated from the contact
default: not used
$\delta_{0}^{offset}$ Maximum penetration offset for faces that are in contact at time zero. The offset is used to prevent unwanted contact forces
default: 0
$\delta_{0}^{max}$ Maximum initial penetration that is allowed. Faces penetrating more than $\delta_{max}$ at time 0 are released
default: 4% of element thickness
$\delta^{edge}$ Penetration tolerance for sliding across sharp edges
default: 0
fid${}_{wear1}$ ID of a FUNCTION defining the contact wear rate of Surface 1
default: no wear calculation
fid${}_{wear2}$ ID of a FUNCTION defining the contact wear rate of Surface 2
default: no wear calculation
fid${}_{thermal}$ ID of a FUNCTION defining the thermal contact conductivity
default: no contact heat transfer
$\alpha_{edge}$ Angle defining a sharp edge (minimum angle between adjacent element faces)
default: 40 deg
one_way Flag to switch from symmetric to one way contact
options:
0 $\rightarrow$ symmetric contact
1 $\rightarrow$ one way contact
no_internal Flag to disable contact surface updates at element erosion or node splitting
options:
0 $\rightarrow$ internal element faces are included
1 $\rightarrow$ internal element faces are excluded

#### Description

This command defines contact between two surfaces (here referred to as Surface 1 and Surface 2). The overlap between surfaces in contact is estimated through numerical integration. The user can specify different levels of accuracy for this numerical integration. Default value (accuracy_level=2) is a good choice for most situations. The low accuracy option is generally only recommended in situations where the total memory requirement of the model needs to be reduced.

The contact treatment is by default symmetric. The input order of Surface 1 and Surface 2 is arbitrary, unless one_way=1. If one_way=1, Surface 2 alone is used to define the contact surface. That is, in a case without friction all forces will then be perfectly perpendicular to Surface 2.

A value for the penalty stiffness ($pfac$) or a unit system (see UNIT_SYSTEM) must be defined in the command file. A unit system based stiffness is computed if $pfac$ has not been defined by the user. It is individual for each part ID and it calculated according to:

$\displaystyle{ pfac = \frac{K}{L_{min}} \times \min \left(1 + \left( \frac{v_{max}}{100} \right)^2,100 \right) } \,\,\, \mathrm{[Pa/m]}$

where $K$ is the initial linear bulk modulus, $L_{min}$ is the characteristic size of the smallest element in the part and $v_{max}$ is the highest initial velocity in the model. For rigid bodies (who do not have a bulk modulus) the penalty stiffness is defined as:

$\displaystyle{ pfac = 10^{13} \times \min \left(1 + \left( \frac{v_{max}}{100} \right)^2,100 \right) } \,\,\, \mathrm{[Pa/m]}$

Assume that two faces are in contact. Face A belongs to a part with penalty stiffness $pfac_A$ and face B belongs to a part with penalty stiffness $pfac_B$. In such case the used penalty stiffness $pfac$ is the minimum of the two values.

$\displaystyle{ pfac = \min (pfac_A, pfac_B)}$

$\delta_{edge}$ can be used in situations where elements undergoing large deformations are sliding against contact surfaces with sharp edges. It should only be used if necessary in order to prevent failing contacts, as it might lead to a certain degree of energy errors.

The calculated wear (optional) does not affect the simulation results. That is, the wear does not affect the geometry of the surfaces in contact. It is only a quantity that can be visualized in the GUI.

#### Example

Automatically defined penalty stiffness

This is a complete model of a rubber sphere impacting a block of steel at the velocity 100 m/s. The penalty stiffnesses $(pfac_{rubber}=3 \cdot 10^{12}, pfac_{steel} = 1.68 \cdot 10^{13})$ are calculated automatically based on the bulk modulus of the materials, the size of the elements and on the magnitude of the intitial velocities.

*UNIT_SYSTEM
SI
*TIME
0.001
*COMPONENT_SPHERE
1, 1, 3
0.0, 0.0, 0.03, 0.01
*COMPONENT_BOX
2, 2, 2, 2, 1
-0.03, -0.03, 0.0, 0.03, 0.03, 0.01
*CHANGE_P-ORDER
P, 1, 3
*SMOOTH_MESH
P, 1, 45.0
*MAT_MOONEY_RIVLIN
1, 1500.0, 3.0e9
1.0e6, 0, 1.0e2
*MAT_ELASTIC
2, 7800.0, 210.0e9, 0.3
*PART
"rubber"
1, 1
"steel"
2, 2
*INITIAL_VELOCITY
P, 1, 0.0, 0.0, -100.0
*CONTACT
"rubber to steel"
1
P, 1, P, 2, 0.1
*END