/INTER/TYPE2
Block Format Keyword Defines a TYPE2 tied interface that connects a set of secondary nodes to a main surface. It can be used to connect coarse and fine meshes, model spotwelds, rivets, and so on.
Format
(1)  (2)  (3)  (4)  (5)  (6)  (7)  (8)  (9)  (10) 

/INTER/TYPE2/inter_ID/unit_ID  
inter_title  
grnd_ID_{s}  surf_ID_{m}  Ignore  Spot_{flag}  Level  I_{search}  I_{del2}  d_{search} 
Read this input, if Spot_{flag} = 20, 21, or 22:
(1)  (2)  (3)  (4)  (5)  (6)  (7)  (8)  (9)  (10) 

Rupt  I_{filtr}  fct_ID_{sr}  fct_ID_{sn}  fct_ID_{st}  I_{sym}  Max_N_Dist  Max_T_Dist  
Fscale_{stress}  Fscale_{str_rate}  Fscale_{dist}  Alpha  Area 
Read this input, if Spot_{flag} = 25, 27 or 28:
(1)  (2)  (3)  (4)  (5)  (6)  (7)  (8)  (9)  (10) 

Stfac  Visc  I_{stf} 
(1)  (2)  (3)  (4)  (5)  (6)  (7)  (8)  (9)  (10) 

I_{the}  K_{the}  I_{proj} 
Definitions
Field  Contents  SI Unit Example 

inter_ID  Interface
identifier (Integer, maximum 10 digits) 

unit_ID  Unit Identifier (Integer, maximum 10 digits) 

inter_title  Interface
title (Character, maximum 100 characters) 

grnd_ID_{s}  Secondary node group
identifier. (Integer) 

surf_ID_{m}  Main surface
identifier. (Integer) 

Ignore  Flag to ignore secondary
nodes if no main segment found.


Spot_{flag}  Spotweld formulation flag.
3
4
5
6
7
11
(Integer) 

Level  Hierarchy level of the
interface. (Integer) 

I_{search}  Search formulation flag
for the closest main segment.
(Integer) 

I_{del2}  Node deletion flag. 9
10
16
(Integer) 

d_{search}  Distance for searching
closest main segment. Default value is the average size of the main segments. 13 (Real) 
$\left[\text{m}\right]$ 
Rupt  Failure model (only
available with Spot_{flag}
20, 21 or 22).
(Integer) 

I_{filtr}  Filter flag. 10
(Integer) 

fct_ID_{sr}  Stress factor vs stress
rate function identifier. 6
(Integer) 

fct_ID_{sn}  Max normal stress vs
normal relative displacement function identifier
(N_Dist). This function must be defined. 6 (Integer) 

fct_ID_{st}  Max tangential stress vs
tangential relative displacement function identifier
(T_Dist). This function must be defined.
6 (Integer) 

I_{sym}  Asymmetric rupture flag.
6
(Integer) 

Max_N_Dist  Maximum normal relative
displacement. Default = 1e+20 (Real) 
$\left[\text{m}\right]$ 
Max_T_Dist  Maximum tangential
relative displacement. Default = 1e+20 (Real) 
$\left[\text{m}\right]$ 
Fscale_{stress}  Stress scale factor. 6 Default = 1.00 (Real) 
$\left[\text{Pa}\right]$ 
Fscale_{str_rate}  Stress rate scale factor.
6 Default = 1.00 (Real) 
$\left[\frac{\text{Pa}}{\text{s}}\right]$ 
Fscale_{dist}  Distance scale factor.
6 Default = 1.00 (Real) 
$\left[\text{m}\right]$ 
Alpha  Stress filter alpha
value. Default = 1 (Real) 

Area  Area of surface which used when the area computed from
secondary node side is null or when secondary node is connected
only to 1D element. Default = 0.0 (Real) 
$\left[{\text{m}}^{2}\right]$ 
Stfac  Stiffness factor (used only with Spot_{flag}
25, 27 or
28). Default = 1.0 (Real) 

Visc  Critical damping coefficient on interface stiffness (used only
with Spot_{flag}
=25, 27 or
28). Default = 0.05 (Real) 

I_{stf}  Interface stiffness
definition flag. 16 Only used with penalty
formulations (Spot_{flag}=25,
27 or 28).
(Integer) 

I_{the}  (Optional) Heat transfer
flag.
(Integer) 

K_{the}  (Optional) Heat exchange
coefficient. Default = 0.0 
$\left[\frac{\text{W}}{{\text{m}}^{2}\cdot \text{K}}\right]$ 
I_{proj}  (Optional) Secondary node
projection flag. 18 (not available for Spot_{flag} = 1,
28 and 30).
(Integer) 
Comments
 Interface TYPE2 is a kinematic condition; no other kinematic condition should be set on any node of the secondary surface, except when Spot_{flag} =25, 27 or 28.
 The d_{search} is computed as (see Tied Interface (TYPE2) in the Radioss Theory Manual):
(1) $${d}_{\mathit{search}}=\frac{1}{n}\cdot {\displaystyle \sum _{i=1}^{n}{d}_{i}}$$with, $n$
 Being the number of main segments
 ${d}_{i}$
 Tthe total length of all the main side segments
 Main nodes of an interface TYPE2 may be
secondary nodes of another interface TYPE2 only if the hierarchy level of the
first interface is lower than the hierarchy level of the second interface.
Hierarchy levels are only available with Spot_{flag} =2. It does not
work if Spot_{flag} =0 or Spot_{flag} =1.
A possible workaround is using Spot_{flag}=2, which corresponds to the default formulation (Spot_{flag}=0); except that it is not compatible with /DT/NODA/CST.
 Spot_{flag} =2 is equivalent to formulation 0; except that it is not compatible with nodal time step /DT/NODA/CST.
 Spot_{flag} =4 is recommended to connect SPH particles to a surface (refer to Smooth Particle Hydrodynamics (SPH)).
 Spot_{flag} = 20,
21 or 22 can include falure and be used to
model a glue connection. It is not compatible with nodel time step
/DT/NODA/CST. The stress is computed for each secondary
node according to the "equivalent" surface around the node.In this case, the force in secondary node will be scaled by reduced force coefficient Fac_N (Fac_T), which is computed as:
(2) $$\mathit{Fac}\_N=\text{min}\left\{\sqrt{\frac{{\sigma}_{N\_\text{max}}{}^{2}}{\text{max}\left[{\left({\sigma}_{N}\left(t\right)\right)}^{2},\text{}{10}^{20}\right]}},\text{}1\right\}$$(3) $$\mathit{Fac}\_T=\text{min}\left\{\sqrt{\frac{{\sigma}_{T\_\text{max}}{}^{2}}{\text{max}\left[{\left({\sigma}_{T}\left(t\right)\right)}^{2},\text{}{10}^{20}\right]}},\text{}1\right\}$$The reduced force is compared to the max value:
if ${\sigma}_{N}<{\sigma}_{N\_\mathrm{max}}$ , then Fac_N =1, which means the force will not be reduced.
if ${\sigma}_{N}>{\sigma}_{N\_max}$ , then $Fac\_N=\sqrt{\frac{{\sigma}_{N\_\mathrm{max}}^{2}}{\mathrm{max}\left[{\left({\sigma}_{N}\left(t\right)\right)}^{2},{10}^{20}\right]}}$ , which means the force will be reduced.
Here the max value will be defined by the user with:(4) $${\sigma}_{{N}_{\mathrm{max}}}=\mathrm{Fscale}\left(\dot{\sigma}\right)\cdot {\mathrm{f}}_{sn}\left(\frac{\text{\Delta}{X}_{N}}{Fscal{e}_{dist}}\right)$$(5) $${\sigma}_{{T}_{\mathrm{max}}}=\mathrm{Fscale}\left(\dot{\sigma}\right)\cdot {\mathrm{f}}_{st}\left(\frac{\text{\Delta}{X}_{T}}{Fscal{e}_{dist}}\right)$$(6) $$\mathrm{Fscale}\left(\dot{\sigma}\right)=Fscal{e}_{stress}\cdot {\mathrm{f}}_{sr}\left(\frac{\dot{\sigma}}{Fscal{e}_{str\_rate}}\right)$$While, ${\mathrm{f}}_{sn}$ , ${\mathrm{f}}_{st}$ and ${\mathrm{f}}_{sr}$ are functions of fct_ID_{sn}, fct_ID_{st} and fct_ID_{sr}.
Once the rupture criterion (defined by Rupt) is reached, the contact will be deleted.
Here: ${\sigma}_{N\_\mathrm{max}}$ is the maximum normal stress value defined by fct_ID_{sn}
 ${\sigma}_{N}\left(t\right)$ is the normal stress
 $\sigma $ _{T_max} is the maximum tangential stress value defined by fct_ID_{st}
 ${\sigma}_{T}\left(t\right)$ is the tangential stress
 Fscale_{stress} is the input constant stress factor
 fct_ID_{sr} is the input variable coefficient
 fct_ID_{sn} and fct_ID_{s} are the input stressdisplacement functions
 I_{sym} permits to choose between symmetric or asymmetric rupture (traction/compression). The initial direction from main surface to the secondary node defines the positive side (traction). If the distance is zero (secondary node lies on the main surface), the rupture will be symmetric, even with I_{sym} =1.
This failure option (Spot_{flag} = 20, 21 or 22) can not be used in implicit.
 Spot_{flag} =30: Secondary
mass/inertia/stiffness distribution to the main node is based on the Kirschoff
model: bicubic form functions are used instead of linear (standard
formulation). It allows a softer contact behavior since the element shape
curvature is taken into account in the force/moment transmission.Warning: This formulation is not compatible with solid elements, as it requires rotational DOF.
 If flag I_{del2} =2, then when a 4node shell, a 3node shell or a solid element is deleted, it is also removed from the main side of the interface (the kinematic condition is suppressed on relative secondary nodes).
 The options I_{del2} =1 and I_{del2} =2 act if the main element is deleted using explicit deletion in Radioss Engine (using the keyword /DEL in Radioss Engine Input (/DEL/SHELL, /DEL/BRICK, ...)).
 If I_{filtr} is set to 1, the
normal and tangential stresses are filtered with an alpha filter, as:
(7) $${\sigma}_{N}\left(t\right)=Alpha\cdot {\sigma}_{N}\left(t\right)+\left(1Alpha\right){\sigma}_{N}\left(tdt\right)$$(8) $${\sigma}_{T}\left(t\right)=Alpha\cdot {\sigma}_{T}\left(t\right)+\left(1Alpha\right)\cdot {\sigma}_{T}\left(tdt\right)$$  Spot_{flag} =25 (penalty
formulation) will keep the penalty formulation during the whole run. The
secondary node (of this contact) could also be the secondary node of another
kinematic option, like rigid body.
The penalty stiffness is constant, calculated by default as the mean nodal stiffness of main and secondary side. The stiffness factor, Stfac, may be used to modify it, if needed. The penalty stiffness will be multiplied by Stfac.
A critical viscous damping coefficient (Visc) allows damping to be applied to the interface stiffness.
 If Ignore = 1, 2, or 3, the secondary nodes without a main segment found during the Starter, are deleted from the interface.
 If Ignore ≠ 1000, d_{search} is used.If Ignore = 2 or 3 and d_{search} = 0, d_{search} is computed, for each secondary node as:
(9) $${\delta}_{1}=0.6\left(thickness\_secondary\_node+thickness\_main\_segment\right)$$(10) $${\delta}_{2}=0.05\left(main\_segment\_diagonal\right)$$${d}_{search}=\mathrm{max}\left({\delta}_{1},{\delta}_{2}\right)$
For shells: thickness_secondary_node = shell thickness of secondary
 thickness_main_segment = shell thickness of main
For solids: thickness_secondary_node = 0
If Ignore = 2: thickness_main_segment = $\frac{Element\_volume}{Segment\_area}$
If Ignore = 3: thickness_main_segment = 0
If Ignore = 2 or = 3: Thickness is retained in the following order: first from /PART definition, from /SHELL or /SH3N definition, then from /PROP definition.
 The contact is compatible with 2Dplane and axisymmetrical simulations only for Spot_{flag}=0 and in case of connecting to solid elements with Spot_{flag}=0, then moments are not transferred.
 If flag I_{del2} =1, then when all 4node shells, all 3node shells and all solid elements belonging to a main segment are deleted, this segment is also removed from the main side of the interface (the kinematic condition is suppressed on relative secondary nodes).
 Spot_{flag} = 25,
27 or 28: Interface penalty stiffness is
computed from both main segment stiffness
K_{m} and secondary node
stiffness K_{s}, depending on I_{stf} flag:
 I_{stf} = 1: ${K}_{n}=Stfac\cdot {K}_{m}$
 I_{stf} = 2 (default): ${K}_{n}=Stfac\cdot \frac{{K}_{m}+{K}_{s}}{2}$
 I_{stf} = 3: ${K}_{n}=Stfac\cdot \mathrm{max}\left({K}_{m},{K}_{s}\right)$
 I_{stf} = 4: ${K}_{n}=Stfac\cdot \mathrm{min}\left({K}_{m},{K}_{s}\right)$
 I_{stf} = 5: ${K}_{n}=Stfac\cdot \frac{{K}_{m}\cdot {K}_{s}}{{K}_{m}+{K}_{s}}$
 If I_{the} >1, the material
of the secondary side and main need to be a thermal material, using finite
element formulation for heat transfer (/HEAT/MAT).
Thermal conduction is computed when the secondary node falls into contact.
The heat exchange is computed from main to secondary and from secondary to main:(11) $${\varphi}_{cond}={K}_{the}\left({T}_{s}^{}{T}_{m}^{}\right)$$  By default, I_{proj} =1 is used to avoid having the wrong mass distribution when the secondary node is projected outside of the main element. The mass and inertia are distributed on the closest edge based on the projection of the secondary node on this edge. Use I_{proj} =2, to obtain the same results as Radioss version 14.0 or older.
 When using the penalty formulation Spot_{flag}=25, moments cannot be transmitted from the secondary nodes to a main segment. Therefore, it is not recommended to use it for any connection where the secondary nodes have rotational degrees of freedom. This would include: shell to shell, spring to shell, shell to solid where the shell is secondary and solid is main. Due to this limitation and the lower robustness compared to kinematic formulations, it is recommended to use the mixed kinematic and penalty formulation, Spot_{flag} =27 and 28.
 Spot_{flag} =27 and
28 are a mixed kinematic and penalty formulation tied
contact. By default, the kinematic formulation is used. Any secondary nodes with
incompatible kinematic conditions are automatically switched to the penalty
formulation. Incompatible kinematic conditions with rigid bodies, imposed
displacements, imposed velocities, imposed accelerations, other tied contact
secondary nodes, or boundary conditions will cause the switch to penalty
formulation. A WARNING message is printed in the Starter output file when
secondary nodes are switched to penalty formulation.
The penalty formulation stiffness is constant and calculated using I_{stf} and Stfac. A critical viscous damping coefficient (Visc) allows damping to be applied to the interface stiffness. The penalty formulation can transfer moments from the secondary nodes to the main segment.
 Unlike Spot_{flag} =1, Spot_{flag} =28 does not add any mass at time=0 when the main surface of the tied contact is a shell element. If the main surface is a solid element there could be some mass added. No mass is added when Spot_{flag} =27 is used.