Previous Up Next

4  GROUP D—LINKS

D.10


Object:

To introduce links between degrees of freedom. Links may be subdivided into three broad categories:


Following the above subdivision, this directive admits three forms, characterized by the respective sub-directives: LINK COUP, LINK DECO or LINK LIAI. The complete syntax is summarized below. For each variation of the main directive (COUP, DECO or LIAI) the available link types are listed in the relevant column, so as to provide a compact overview.


Syntax:

 $ LINK COUP        $ LINK DECO        $ LINK LIAI        $
 $ <NONP>           $                  $                  $
 $ <SOLV  . . .>    $                  $ <SOLV  . . .>    $
 $ <RENU ; NORE>    $                  $ <RENU ; NORE>    $
 $ <VERI> <ARRA>    $                  $ <FREQ ifreq>     $
 $ <SPLT $ DOF  ;   $                  $ <VERI>           $
 $         NODE ;   $                  $                  $
 $         DOMA ;   $                  $                  $
 $         PART ;   $                  $                  $
 $         NONE $>  $                  $                  $
 $ <SOL2>           $                  $                  $
 $ <GPCG  . . .>    $                  $                  $
 $ <UPDT /CTIME/>   $                  $                  $

 |  BLOQ  . . .     ,  BLOQ . . .      ,  BLOQ . . .      |
 |  GUID  . . .     ,                  ,                  |
 |  CONT  . . .     ,                  ,  CONT . . .      |
 |  RADI  . . .     ,                  ,  RADI . . .      |
 |  RELA  . . .     ,                  ,  RELA . . .      |
 |  ARMA  . . .     ,  ARMA . . .      ,  ARMA . . .      |
 |  CROS  . . .     ,  CROS . . .      ,                  |
 |                  ,  ACBE . . .      ,                  |
 |  LCAB  . . .     ,                  ,                  |
 |  ARLQ  . . .     ,                  ,                  |
 |  DEPL  . . .     ,                  ,  DEPL . . .      |
 |  VITE  . . .     ,                  ,  VITE . . .      |
 |  ACCE  . . .     ,                  ,  ACCE . . .      |
 |  COQM  . . .     ,                  ,  COQM . . .      |
 |  INTE  . . .     ,                  ,                  |
 |  FLST  . . .     ,                  ,                  |
 |  FLSR  . . .     ,  FLSR . . .      ,                  |
 |  FS    . . .     ,                  ,  FS   . . .      |
 |                  ,                  ,  UNIL . . .      |
 |  IMPA  . . .     ,  IMPA . . .      ,  IMPA . . .      |
 |                  ,                  ,  JEUX . . .      |
 |  GLIS  . . .     ,  GLIS . . .      ,  GLIS . . .      |
 |                  ,                  ,  MPEF . . .      |
 |                  ,                  ,  SPHY . . .      |
 |  TYPL  . . .     ,                  ,                  |
 |  EDEF  . . .     ,                  ,                  |
 |  BIFU  . . .     ,                  ,  BIFU . . .      |
 |  ADHE  . . .     ,                  ,                  |
 |  TUBM  . . .     ,                  ,  TUBM . . .      |
 |  TUYM  . . .     ,                  ,  TUYM . . .      |
 |  TUYA  . . .     ,                  ,  TUYA . . .      |
 |  SOLI  . . .     ,                  ,  SOLI . . .      |
 |  COMP  . . .     ,                  ,  COMP . . .      |
 |  ARTI  . . .     ,                  ,  ARTI . . .      |
 |  ROTA  . . .     ,                  ,  ROTA . . .      |
 |  MENS  . . .     ,                  ,  MENS . . .      |
 |  DIST  . . .     ,                  ,  DIST . . .      |
 |  BARY  . . .     ,                  ,  BARY . . .      |
 |  RIGI  . . .     ,                  ,  RIGI . . .      |
 |                  ,                  ,  SPLI . . .      |
 |                  ,                  ,  COLL . . .      |
 |  FSA   . . .     ,                  ,  FSA  . . .      |
 |  FSR   . . .     ,                  ,  FSR  . . .      |
 |  PINB  . . .     ,  PINB . . .      ,  PINB . . .      |
 |  GPIN  . . .     ,  GPIN . . .      ,                  |
 |                  ,  FSS  . . .      ,                  |
 |  SH3D  . . .     ,                  ,  SH3D . . .      |
 |                  ,  FLSW . . .      ,                  |
 |  MAP2  . . .     ,                  ,  MAP2 . . .      |
 |  MAP3  . . .     ,                  ,  MAP3 . . .      |
 |  MAP4  . . .     ,                  ,  MAP4 . . .      |
 |  MAP5  . . .     ,                  ,  MAP5 . . .      |
 |  MAP6  . . .     ,                  ,  MAP6 . . .      |
 |  MAP7  . . .     ,                  ,  MAP7 . . .      |
 |  FESE  . . .     ,                  ,                  |
 |  NAVI  . . .     ,                  ,                  |
 |  BREC  . . .     ,                  ,                  |
 |                  ,  PELM . . .      ,                  |
 |                  ,  ADAP . . .      ,                  |
 |  ENGR  . . .     ,  ENGR . . .      ,                  |
COUP

Introduces the set of coupled links. All coupled links must be declared within this set (the keyword COUP may not be repeated).
DECO

Introduces the set of decoupled links. All decoupled links must be declared within this set (the keyword DECO may not be repeated).
LIAI

Introduces the set of "liaison" links. All "liaison" links must be declared within this set (the keyword LIAI may not be repeated).



Comments:

The COUP and LIAI subdirectives are mutually exclusive. However, the may be combined with the DECO links within the same calculation, with the following syntax:

    LINK $[COUP ; LIAI]$
          (declare all coupled/"liaison" links here ...)
    LINK DECO
          (declare all uncoupled links here ...)

The subdirective LIAI is not compatible with the other types of links. Only the coupled links declared with LINK COUP may be used also in conjunction with domain decomposition (see the STRU directive), while this is not the case for the LINK LIAI directive.


Beware that, for the moment, only the BLOQ, DEPL, VITE and ACCE models are accepted in calculations with sub-domains.


Note that he availability of each link formulation introduced above with one or more of the link types is given in their specific manual page below.


Warning:


The LINK COUP directive allows to build a coupling matrix between the different degrees of freedom appearing in the connections. This matrix must be invertible, and a problem occurs in this sense if the different connections are not independent from each other.


In principle, EUROPLEXUS is able to eliminate the redundant relations in order to be able to invert the connections matrix. But since this elimination is a trial-and-error process, it is preferable when possible to avoid this situation. If this is not possible, it is recommended to start by giving the most complex connections (solids or articulations), and to finish by giving the simplest ones (relations or blockages).


Comments:


Be sure to check the various options available in relation to connections: see Page H.160.

4.1  LINK CATEGORY

D.11


Object:

Choose between the available categories for links (see GBD_0010).


Syntax:

  $[ COUP ; DECO ; LIAI ]$
COUP

Introduces the set of coupled links. All coupled links must be declared within this set (the keyword COUP may not be repeated).
DECO

Introduces the set of decoupled links. All decoupled links must be declared within this set (the keyword DECO may not be repeated).
LIAI

Introduces the set of "liaison" links. All "liaison" links must be declared within this set (the keyword LIAI may not be repeated).

4.2  OPTIONS FOR COUPLED LINKS

D.12 - Oct 13


Object:

Syntax:

    LINK COUP
         <NONP>
         <SOLV  |[ CHOL                                     ;
                   PARD                                     ;
                   SPLI < TYPE  imet > < PCON ipre >
                        < PITE  prec > < IPA1 ip1  >
                        < IPA2  ip2  > < RPAR rp   >
                        < INIS  inig >                    ]| >
    $[ RENU ; NORE ]$ <VERI>
    <ARRA>
    <SPLT |[ DOF  ; NODE ; DOMA ; PART ; NONE ]| >
    <SOL2>
    <GPCG < PREC prec > < APRE apre > < DUMP > >
    <UPDT /CTIME/>


NONP

Accept the occurrance of non-permanent links (such as Lagrangian contacts for example) during the calculation even though there are no non-permanent links explicitly declared in the input. This optional keyword should be used only in the special case that there are no non-permanent links explicitly declared in the input, but at the same time there is some other model which might introduce non-permanent links during the course of the calculation. For example, the Lagrangian contact between SPH particles and structures treated by the SPHY COQU or SPHY STRU directive, when the LAGC keyword is also specified in the calculation type. In this case the model may add coupled, non-permanent links during the course of the calculation, which is only accepted if either some non-permanent links are explicitly declared, or if the present NONP keyword is specified. In the second case, just add LINK COUP NONP to your input.
imet

iterative solver number i, default 8
ipre

preconditioner number k, default 3
prec

tolerance on residual, default 1.D-6
ip1

first integer parameter, default 20
ip2

second integer parameter, default 10
rp

real parameter, default 1.D-4
inig

initial guess, default 0.0
prec

MPI Only - Relative precision for GPCG solver (see comment below)
apre

MPI Only - Absolute precision for GPCG solver (see comment below)

Comments:

The SOLV directive is fully described in 4.3 (page D.20).


Concerning imposed motions (directives DEPL, VITE and ACCE), note that no dimensions are needed relative to the motions themselves. Hovever, dimensioning relative to the time tables describing such motions is still necessary (see keywords FNOM, FTAB).


The ARMATURE directive is described in 4.11 (page D.125).


The optional keyword RENU makes it possible to renumber the links in order to minimize the size of the matrix.


By default, links are renumbered (option RENU).


If the optional keyword NORE is specified, the links are taken in the order of their definition, and the matrix can be very large and ill-conditioned. If RENU (or nothing) is specified, then the connections are renumbered in an attempt to minimize the size of the matrix.


The optional keyword VERI can be used to verify a posteriori that the imposed links are effectively satisfied. This option produces heavy output and CPU overhead and should therefore be used only for debugging purposes.


The optional keyword ARRA can be used to choose storage of the links in a dynamic array rather than in a doubly linked list of doubly linked lists. This may increase efficiency (but is still under development).


The optional keyword SPLT can be used to choose the desired strategy for splitting the constraints into groups. The following possibilities are currently available:


The optional keyword SOL2 can be used to choose closed-form solution for groups of links containing just two links (in addition to groups containing just one link). By default, all groups of links containing more than one links are solved by the general numerical method (Choleski’s method). In some cases, closed-form solution may be more efficient.


The optional keyword GPCG toggles the use of a specific Preconditioned Conjugate Gradient solver for links coupling several subdomains within parallel MPI framework. The precision of the solution is computed in terms of relative residual with respect to the norm of the right-hand side vector. Default precision is 105 and it can be changed using the keyword PREC. An additional precision acting on the absolute norm of the residual can be entered using the keyword APRE. It is useful in the rare cases where the norm of the right-hand side vector is very small. Additional information is printed on the listing output during the iterations of the algorithm if the keyword DUMP is used.


The optional keyword UPDT can be used to introduce an update frequency for time-varying links, in order to save CPU time. This is especially useful for fluid-structure interaction, when links are classically updated at each time-step, with a frequency obtained from the CFL condition, whereas their update should follow the physical structural velocity, often much smaller than sound speed in the different media.


As far as GLIS models are concerned, only 3D models (sliding surface) are currently available. For 2D models (sliding lines), please use decoupled or "liaison" links.


The EDEF directive is described in 4.30 (page D.189).

4.3  OPTIONS FOR "LIAISON" LINKS

D.20 - Oct 13


Object:


The option "SOLV" makes it possible to change the resolution method in order to reduce the time spent to solve large matrix systems. For iterative solvers ("SPLI" keyword) the data structure uses the CSR format (Compressed Sparse Rows), well suited for iterative solution and used in the SPLIB library.


The option "RENUM" makes it possible to renumber the connections in order to minimize the size of the matrix.


The optional keyword "FREQ" can be used to avoid the inversion of the connection matrix at each computation step, in the cases where this is possible (see below).


The optional keyword "VERI" can be used to verify a posteriori that the imposed liaisons are effectively satisfied. This option produces heavy output and CPU overhead and should therefore be used only for debugging purposes.


Syntax:

    < "SOLV"  |[ "CHOL"                                     ;
                 "PARD"                                     ;
                 "SPLI" < "TYPE"  imet > < "PCON" ipre > ...
                  ...   < "PITE"  prec > < "IPA1" ip1  > ...
                  ...   < "IPA2"  ip2  > < "RPAR" rp   > ...
                  ...   < "INIS"  inig >                     ]| >

    < $[ "RENU" ; "NORE" ]$ >  < "FREQ"  ifreq > <"VERI">


imet

iterative solver number i, default 8
ipre

preconditioner number k, default 3
prec

tolerance on residual, default 1.D-6
ip1

first integer parameter, default 20
ip2

second integer parameter, default 10
rp

real parameter, default 1.D-4
inig

initial guess, default 0.0
ifreq

The matrix will be inverted each ifreq computation step; by default, ifreq is 1, i.e. the matrix is inverted at each step. This has only effect in Lagrangian computations. In ALE or Eulerian cases, the matrix is inverted anyway at each time step (like if ifreq=1) because the nodal masses are continuously changing due to transport.

Comments:

If the option "CHOL" is specified, the standard direct solver is used. This is the default option.


When the keyword "PARD" is specified, the library PARDISO is used. The package PARDISO is a thread-safe, high-performance, robust, memory efficient and easy to use software for solving large sparse symmetric and unsymmetric linear systems of equations on shared-memory and distributed-memory multiprocessors. This package is include in MKL library provided by the Intel compiler.
http://www.pardiso-project.org/
http://software.intel.com/


When the keyword "SPLI" is specified, the iterative solver is used. SPLIB is a library of iterative solvers with preconditioners for symmetric and nonsymmetric systems. It has been adapted for large matrix systems in the EUROPLEXUS code and uses the Compressed Sparse Row format (CSR).
http://www.netlib.org/utk/papers/iterative-survey/node61.html


The integer parameter imet specifies which SPLIB solver to use :

imet = 1 : Bi-Conjugate Gradients
imet = 2 : Conjugate Gradients with AA’y = b, x = A’y
imet = 3 : Conjugate Gradients with A A’ x = A’b
imet = 4 : Conjugate Gradients Squared (CGS)
imet = 5 : Conjugate Gradients Stabilized
imet = 6 : GMRES(ip2)
imet = 7 : Transpose free QMR
imet = 8 : Template version of Conjugate Gradients Stabilized
imet = 9 : Template version of GMRES(ip2)


The integer parameter ip2 used in GMRES solvers defines the Krylov subspace size (default value 10). When an imet of zero or less is specified, CG-Stabilization is used.


The integer parameter ipre specifies which preconditioner to use :

ipre = 0 : no preconditioner
ipre = 1 : ILU(ip1)
ipre = 2 : MILU(ip1,rp)
ipre = 3 : ILUT(ip1,rp)
ipre = 4 : SSOR(rp)
ipre = 5 : TRID(ip1)
ipre = 6 : ILU0
ipre = 7 : ECIMGS(rp)


The integer parameter ip1 indicates the levels of fill-in to allow for ILU and MILU and the block size to use in the tridiagonal preconditioner TRID.
For ILUT, ip1 is the maximum additional entries allowed per row in the preconditioner compared to the original matrix. The real parameter rp is the relaxation parameter, the amount of multiply discarded fill-in entries before adding them to the diagonal. For SSOR it is the relaxation parameter. For ILUT, it is the drop tolerance.


For ECIMGS, rp specifies the sparsity pattern of the preconditioner :

- rp = 0 : use the non zero pattern of the matrix
- 0 < rp < 1. : use a sparser pattern than that of the matrix
- rp = 1. : use a diagonal pattern
- rp > 1. : use a denser pattern with int(rp) levels of fill-in

It is greatly recommanded to use default values by entering only the following key words : "LIAIS" "SOLV" "SPLIB".


More informations to use SPLIB options can be found in this paper : “SPLIB : A library of iterative methods for sparse linear systems” by R. Bramley and X Wang, department of computer science - Indiana University, 1995.


For information about methods implemented, see for example the following reference by Y. Saad : “Iterative Methods for Sparse Linear Systems”. This book can be found at http://www-users.cs.umn.edu/ ~ saad


By default, connections are renumbered (option "RENU").


If the option "NORE" is specified, the connections are taken in the order of their definition, and the matrix can be very large and ill-conditioned. If "RENU" (or nothing) is specified, then the connections are renumbered in an attempt to minimize the size of the matrix.


If the connections are simple fixed displacements, a new numeration is useless because the matrix is diagonal.


The option FREQ is not compulsory. If it is not specified, a new computation is done at every time step.


When the coefficients of the relations between the degrees of freedom depend on the updated geometry (see COQM and FS), it is necessary to perform new computations and to invert the matrix at each time step during a EUROPLEXUS run. This operation is very costly if there are many coupled degrees of freedom. The keyword "FREQ" requests a new computation and an inversion only every ifreq computation steps.


In the case of an uncompressible fluid or an A.L.E or Eulerian computation it is necessary to invert the matrix at each time step because the nodal masses are continuously changing due to transport. Therefore, the code ignores the user-supplied value for ifreq in these cases.


The same holds for an incompressible calculation, or for a calculation involving non-deformable sub-structures (keywords "NAVIER" and "SOLIDE").

4.4  AUXILIARY FILE

D.25


Object:


This directive allows to read the connections data from an auxiliary file.


Syntax:

    < "FICHIER"   'nom.fic'  >


In certain cases the data may be bulky. It is then recommended to store them on an auxiliary file to shorten the main input data file. The auxiliary file is activated by means of the keyword "FICHIER" that precedes the file name (complete under Unix). In the main data file then only the keywords "LIAISON" "FICHIER" remain.


The auxiliary file (in free format) contains the whole set of connections data, except the keyword "LIAISON". To return to the main input data, the auxiliary file must be terminated by the keyword "RETOUR".

4.5  BLOCKAGES

D.30


Object:


To prescribe a zero displacement to (i.e., to block) a degree of freedom, that is to say to ensure the relation U(i) = 0.


Compatibility: COUP, DECO, LIAI


Syntax:

    "BLOQ"  ( /LECDDL/  /LECTURE/  )


/LECDDL/

Reading procedure of the degrees of freedom concerned.
/LECTURE/

Reading procedure of the numbers of the blocked nodes.

Comments:


It is possible to repeat the same blockage several times. Indeed, when a boundary is described, it is often simpler to use the implicit definition of the procedure /LECTURE/; in this case the points which are located at the ends are written twice. The EUROPLEXUS program eliminates these double definitions before it builds up the matrix.


Note, however, that the program is unable to eliminate the repeated points if e.g. several "BLOQ" keywords are used.


A time-limited version (TBLO) of the BLOQ directive, which acts only until a certain time and then is automatically removed, is also available, see Page D.31.

4.6  TIME-LIMITED BLOCKAGES

D.31


Object:


To prescribe a zero displacement to (i.e., to block) a degree of freedom, that is to say to ensure the relation U(i) = 0, up to a certaint time or a certain event. After the chosen time (or event), the blockage is automatically released.


Compatibility: COUP, DECO


Syntax:

    "TBLOQ"  ( /LECDDL/ $ "UPTO" t ; "TRIG" $ /LECTURE/  )


/LECDDL/

Reading procedure of the degrees of freedom concerned.
UPTO t

Time up to which the blockage is imposed. After this time, the blockage is automatically released.
TRIG

The blockage is imposed only until a trigger is activated. The trigger refers to the TRIG keyword which activates mesh refinement in some adaptivity models, see OPTI ADAP TRIG on Page H.180. After this time, the blockage is automatically released.
/LECTURE/

Reading procedure of the numbers of the blocked nodes.

Comments:


It is possible to repeat the same blockage several times. Indeed, when a boundary is described, it is often simpler to use the implicit definition of the procedure /LECTURE/; in this case the points which are located at the ends are written twice. The EUROPLEXUS program eliminates these double definitions before it builds up the matrix.


Note, however, that the program is unable to eliminate the repeated points if e.g. several "BLOQ" keywords are used.

4.7  GUIDE (SLIDE CHANNEL)

D.35


Object:


This directive aims to model a piping guide, i.e. the support that blocks the transverse displacement of the piping at a given node, while keeping free its longitudinal motion.

The sliding direction is prescribed by giving 3 parameters DIRX, DIRY and DIRZ, which correspond to 3 components of the direction vector. Rotationary degrees of freedom are left free.


Compatibility: COUP


Syntax:

    "GUIDE"  "DIRX" rx "DIRY" ry "DIRZ" rz   /LECTURE/  )


rx ry rz

Components that define the direction of the guide.
/LECTURE/

Reading procedure of the number or of the name of the node concerned.

Comments:

Definition of the local frame (x,y,z) with respect to the global frame (X,Y,Z):

If the slider direction is vertical, the local x-axis is collinear with the sliding direction, the y-axis is collinear with Y-axis, and z-axis completes the direct orthogonal axis system.

To obtain the reaction forces in the local frame corresponding to the guide, one must define the node as a REGION and give the same components of the direction vector.

4.8  GEOMETRIC BILATERAL RESTRAINTS ("CONTACTS")

D.40


Object:


The following instructions are used to automatically write relations imposed by boundary conditions of geometrical origin. For instance, the user wants certain nodes of an element to stay on a given structure, or to impose symmetry conditions for one part of the boundary.


Compatibility: COUP, LIAI


Syntax:

    "CONT"
        |  "PLAN"  ...      |
        |  "SPHE"  ...      |
        |  "CYLI"  ...      |
        |  "CONE"  ...      |
        |  "TORE"  ...      |
        |  "SPLA"  ...      |



Comments:


Do not forget to dimension (see "RELA" n1 n2, page A80).


Here n1 represents the maximum number of nodes in contact and n2 is equal to 2 for 2-D computations and 3 for 3-D computations.


It is very important to note that the behaviour of these directives (except PLAN and SPLA) is different, according to the fact that the constraints coefficients are considered to be constant, or allowed to vary in time (the desired behaviour may be chosen via the OPTI CONT option, described in Section H). By default the constraint coefficients are determined on the initial configuration and are kept constant in time. This treatment is always adequate for the PLAN and SPLA types of constraint (since the normal to the plane does not vary in time anyway). However, for the other directives it is only adequate if the nodes do not move, i.e. for Eulerian nodes. In this case, the directives represent a handy shortcut for specifying constraints with coefficients different from point to point (but constant in time), without having to write such conditions explicitly in the input file.


But when the nodes move in time, i.e. for Lagrangian or ALE nodes, the use of constant coefficients in time is no longer adequate. The coefficients should be recomputed at each time step, which may be a costly operation. The user may require this updating of the coefficients by specifying the OPTI CONT VARI option, see Section H. Using variable coefficients has as effect that the nodes move by remaining on the imposed surface with first-order accuracy.


The instructions are described in detail on the following pages.

4.8.1  PLANE/LINEAR RESTRAINT (“CONTACT PLAN”)

D.50


Object:


The specified nodes lay (and remain) on a plane normal to a given vector. In 2D, the plane reduces to a straight line. Only translational degrees of freedom are blocked.


Compatibility: COUP, LIAI


Syntax:

   "PLAN"  |[  "NX" x  "NY" y  < "NZ" z > ;
               "NR" r  "NZ" z             ;
               "POIN" /LECT1/             ;
               "AUTO"                     ]| /LECT2/
x y

Components of the normal vector (2-D).
x y z

Components of the normal vector (3-D).
r z

Components of the normal vector (Axisymmetric).
POIN /LECT1/

Must specify a node belonging to the mesh, either via its index or via its CASTEM 2000 name. The coordinates of this node are taken as the components of the normal.
AUTO

The components of the normal are determined automatically from the position of the nodes listed in /LECT2/. Therefore, in this case, the nodes contained in the following /LECT2/ list must lie on the same line (in 2D) or plane (in 3D). In the 3D case, of course, the listed nodes must define a plane (not be along the same line).
/LECT2/

Numbers of the nodes concerned.

Comments:


It is not necessary that the normal vector be unitary, since it is automatically normalised by the program. Furthermore, it is not necessary that the nodes initially belong to the same line or plane (except in the AUTO case).


The difference between this directive and the CONT SPLA directive (see below) is that CONT PLAN blocks only translational degrees of freedom, while CONT SPLA blocks both translational and rotational degrees. Therefore, the two directives are identical for nodes of continuum elements, which do not possess rotational degrees of freedom. However, for structural nodes (with rotations), CONT PLAN represents a hinge while CONT SPLA represents a symmetry line or plane (the relevant rotations are automatically blocked in that case).

4.8.2  SPHERICAL/CIRCULAR RESTRAINT

D.60


Object:


The specified nodes lay on (a) sphere(s) of given center. In 2D, the sphere reduces to a circle.


Compatibility: COUP, LIAI


Syntax:

    "SPHE"  |[  "CX" x  "CY" y  < "CZ" z >  ;
                "CR" r  "CZ" z              ;
                "CENT" /LECT1/              ]|    /LECT2/


x y

Coordinates of the center of the sphere (2-D).
x y z

Coordinates of the center of the sphere (3-D).
r z

Coordinates of the center of the sphere (Axisymmetric).
"CENT" /LECT1/

Node at the center of the sphere. Points should be sufficiently far from the sphere center so as to define the radial direction with sufficient accuracy.
/LECT2/

Nodes located at the surface of the sphere.

Comments:


This constraint only ensures that, at each time step, the displacement increment of the specified nodes be tangent to the (current) sphere. For finite displacement increments, therefore, the nodes will only approximately remain on the initial spherical surface. It is not necessary that the nodes initially belong to the same sphere.


This directive blocks only translational degrees of freedom.


In case variable coefficients are specified (via the OPTI CONT VARI option), remember to dimension adequately by the DIME VCON directive). Each sphere/circle requires 3 coefficients.

4.8.3  CYLINDRICAL RESTRAINT

D.70


Object:


The specified nodes lay on (a) circular cylinder(s) of given axis. At each step the displacement increment along the axial direction is free, while that in the plane orthogonal to the axis is tangent to a circle.


The instruction only applies to a 3-D analysis. In 2D, the SPHE directive described in the previous Section may be used to obtain a circular restraint.


Compatibility: COUP, LIAI


Syntax:

   "CYLI"  |[ "P1X" x1  "P1Y" y1  "P1Z" z1 ; "POI1" /LECT1/ ;
              "P2X" x2  "P2Y" y2  "P2Z" z2 ; "POI2" /LECT2/ ]| /LECT3/
x1 y1 z1

Coordinates of a point of the cylinder axis.
"POI1" /LECT1/

Node at the first point of the cylinder axis.
x2 y2 z2

Coordinates of another point of the axis.
"POI2" /LECT2/

Node at the other point of the cylinder axis.
/LECT3/

Nodes concerned. Points should be sufficiently far from the cylinder axis so as to define the radial direction with sufficient accuracy.

Comments:


This constraint only ensures that, at each time step, the displacement increment of the specified nodes be tangent to the cylinder (current or initial, depending on OPTI CONT option). For finite displacement increments, therefore, the nodes will only approximately remain on the initial cylindrical surface. It is not necessary that the nodes initially belong to the same cylinder.


This directive blocks only translational degrees of freedom.


In case variable coefficients are specified (via the OPTI CONT VARI option), remember to dimension adequately by the DIME VCON directive). Each cylinder requires 6 coefficients.

4.8.4  CONICAL RESTRAINT

D.80


Object:


The specified nodes lay on (a) cone(s) of given axis.


The instruction only applies to a 3-D analysis.


Compatibility: COUP, LIAI


Syntax:

   "CONE"  $[ "SX" x1  "SY" y1  "SZ" z1 ; "APEX" /LECT1/ ]$
           $[ "PX" x2  "PY" y2  "PZ" z2 ; "POIN" /LECT2/ ]$ /LECT3/


x1 y1 z1

Coordinates of the apex of the cone.
"APEX" /LECT1/

Node at the cone apex.
x2 y2 z2

Coordinates of a point on the cone axis different from the apex.
"POIN" /LECT2/

Node along the cone axis different from the apex.
/LECT3/

Nodes concerned. Points should be sufficiently far from the cone axis so as to define the radial direction with sufficient accuracy.

Comments:


This constraint only ensures that, at each time step, the displacement increment of the specified nodes be tangent to the cone (current or initial, depending on OPTI CONT option). For finite displacement increments, therefore, the nodes will only approximately remain on the initial conical surface. It is not necessary that the nodes initially belong to the same cone.


This directive blocks only translational degrees of freedom.


In case variable coefficients are specified (via the OPTI CONT VARI option), remember to dimension adequately by the DIME VCON directive). Each cone requires 6 coefficients.

4.8.5  TOROIDAL RESTRAINT

D.90


Object:


The specified nodes lay on (a) torus(es) of given axis and center.


This instruction only applies to a 3-D analysis.


Compatibility: COUP, LIAI


Syntax:

   "TORE"  |[ "P1X" x1  "P1Y" y1  "P1Z" z1 ; "POI1" /LECT1/ ;
              "P2X" x2  "P2Y" y2  "P2Z" z2 ; "POI2" /LECT2/ ;
              "P3X" x3  "P3Y" y3  "P3Z" z3 ; "CENT" /LECT3/ ]|  /LECT4/


x1 y1 z1

Coordinates of a point on the torus (circular) axis.
"POI1" /LECT1/

First node on the torus (circular) axis.
x2 y2 z2

Coordinates of another point on the circular axis.
"POI2" /LECT2/

Second node on the torus (circular) axis.
x3 y3 z3

Coordinates of the center of the torus.
"CENT" /LECT3/

Node at the torus center.
/LECT4/

Nodes concerned.

Comments:


This constraint only ensures that, at each time step, the displacement increment of the specified nodes be tangent to the torus (current or initial, depending on OPTI CONT option). For finite displacement increments, therefore, the nodes will only approximately remain on the initial torical surface. It is not necessary that the nodes initially belong to the same torus.


This directive blocks only translational degrees of freedom.


In case variable coefficients are specified (via the OPTI CONT VARI option), remember to dimension adequately by the DIME VCON directive). Each torus requires 9 coefficients.

4.8.6  PLANE/LINE OF SYMMETRY RESTRAINT

D.100


Object:


The specified nodes lay (and remain) on (a) plane(s) of given normal vector, that defines the symmetry. In 2D, the plane reduces to a straight line.


Compatibility: COUP, LIAI


Syntax:

   "SPLA"  |[  "NX" x  "NY" y  < "NZ" z > ;
               "NR" r  "NZ" z             ;
               "POIN" /LECT1/             ;
               "AUTO"                     ]| /LECT2/
x y

Components of the normal vector (2-D).
x y z

Components of the normal vector (3-D).
r z

Components of the normal vector (Axisymmetric).
POIN /LECT1/

Must specify a node belonging to the mesh, either via its index or via its CASTEM 2000 name. The coordinates of this node are taken as the components of the normal.
AUTO

The components of the normal are determined automatically from the position of the nodes listed in /LECT2/. Therefore, in this case, the nodes contained in the following /LECT2/ list must lie on the same line (in 2D) or plane (in 3D). In the 3D case, of course, the listed nodes must define a plane (not be along the same line).
/LECT2/

Numbers of the nodes concerned.

Comments:


It is not necessary that the nodes initially belong to the same plane (except in the AUTO case).


The difference between this directive and the CONT PLAN directive (see above) is that CONT PLAN blocks only translational degrees of freedom, while CONT SPLA blocks both translational and rotational degrees. Therefore, the two directives are identical for nodes of continuum elements, which do not possess rotational degrees of freedom. However, for structural nodes (with rotations), CONT PLAN represents a hinge while CONT SPLA represents a symmetry line or plane (the relevant rotations are automatically blocked in that case).


Remember to dimension adequately with ’SYME’ (see page A.80).


When AUTO is used, the search for enough non-coincident nodes, among those contained in LECT2, so as to define a line in 2D or a plane in 3D is affected by a tolerance. In case of necessity, this tolerance may be set by OPTI TOLC, see page H.40.

4.9  IMPOSED CIRCULAR SHAPE

D.110


Object:


The displacements of the specified nodes are constrained to be in the radial direction with respect to a point (center) and to have the same modulus. If the nodes lie initially on the same circle, they remain on a circle, whose radius may vary with time.


The instruction is available for a 2-D and 3-D analysis.


For an Eulerian computation (no mesh displacements), the fluid velocities are radial and of the same modulus.


Compatibility: COUP, LIAI


Syntax:

    "RADI" "SPHE" "CENT" /LECTURE/
            ...   "CONT" /LECTURE/


"CENT" /LECTURE/

Number of the node at the center of the circle.
"CONT" /LECTURE/

Numbers of the nodes concerned.

Comments:


The instruction is used to avoid instabilities e.g. when a gas bubble collapses after an initial expansion.


For n points (n > or = 2), EUROPLEXUS writes (idim*n - 1) relations.

4.10  RELATIONS

D.120


Object:


Several displacement (or velocity) components are linked by constant coefficients during the whole computation.


Compatibility: COUP, LIAI


Syntax:

    "RELA"  ngroup*(
                  ... nrel  nterm*( coef icomp $[ nuneu ipas ;
                                                 /LECTURE/ <SHIF s> ]$ )
                  ... "EGAL"  /LECDDL/  /LECTURE/                           )


ngroup

Number of relation sets.
nrel

Number of relations to be generated in a set.
nterm

Number of terms in a relation of the set.
coef

Coefficient of a term.
icomp

Displacement component of the node "nuneu" involved in the relation.
nuneu

Number of the node concerned.
ipas

Increment on the number of the node "nuneu" in order to get the next relation of the set.
LECTURE

List of concerned nodes.
SHIFT s

Force circular permutation of the list (see example below). The increment in traversing the list circularly is indicated by the s quantity (normally 1).
/LECDDL/

Reading procedure of the numbers of the blocked nodes.
EGAL

Indicates the equality along the component /LECDDL/ of the motion of the nodes defined by the following /LECT/.

Comments:


Each displacement will be specified by the number of the node (nuneu) and its component (icomp). Formula of the relation:

        0 = coef(1)*U(1) + coef(2)*U(2) +  . . . + coef(k)*U(k)


There are two ways to define a set of relations. The first is to give the node number nuneu and the step ipas. The second is to use the procedure /LECTURE/, which allows to use object names created by GIBI. In this latter case, on passes from one relation to the next one in a set by taking the next node in the procedure /LECTURE/ associated with each term. In this case, there must be exactly nrel nodes in each one of the lists specified via the /LECT/ procedures (assuming that the optional SHIF keyword has not been specified).


The optional SHIF keyword can be used to force a circular permutation of the list. In this case, the number of nodes in the lists need not be the same. For example, assume that one wants to impose the same displacement along z (i.e. global direction 3) to all nodes of an object named “face1”. Then the command would be:

 RELA 1  0 2
      1. 3 LECT face1 TERM
     -1  3 LECT face1 TERM SHIFT 1

Note that in this case the number of relations nrel can be set to 0 because the code computes it automatically.


Example:
       RELA  5  2  2    1.  1 288 1    -1. 1 6 1
                1  3    3.4 2 287 0    -1. 2 5 0    1. 1 5 0
                3  2    0.5 3 115 7    -1. 3 9 5
                5  2    1.  3    LECT toto TERM
                       -1.  3    LECT tata TERM
                EGAL        13   LECT 228 321 842 TERM


There are five groups. The first group has 2 relations of 2 terms, the second 1 relation of 3 terms, the third 3 relations of 2 terms, the fourth 5 relations of 2 terms and the last one 2 relations of 2 terms.


In the first group, d.o.f 1 of node 288 has been linked to d.o.f 1 of node 6 (first relation), then d.o.f 1 of node 289 to d.o.f 1 of node 7 (second relation). In fact ipas=1 for the two terms.


In the second group, d.o.f. 2 of node 287 has been linked to d.o.f. 2 of node 5 and to d.o.f. 1 of the same node 5. There is just one relation since ipas = 0 for the three terms.


On the contrary, in the third group, ipas=7 for the first term and 5 for the second. Therefore, d.o.f 3 of node 115 has to be linked to d.o.f 3 of node 9 (first relation of the group), then d.o.f 3 of node 122 to d.o.f 3 of node 14 (2nd relation), and finally d.o.f 3 of node 129 to d.o.f 3 to node 19 (3rd relation).


In the fourth group, there are 5 relations between the d.o.f. 3 of the nodes belonging to objects ’toto’ and ’tata’ taken in the order in which they appear.


In the fifth group, there are 4 equalities between the d.o.f. 1 and 3 of nodes 228, 321 and 842.

                   Ux(228) = Ux(321)  ;   Uz(228) = Uz(321)
                   Ux(321) = Ux(842)  ;   Uz(321) = Uz(842)

4.11  ARMATURES

D.125


Object:


In calculations of structures made of reinforced concrete, this directive allows to link the displacements of the nodes belonging to continuum-like elements made of concrete, with those of bar-like elements made of steel.


Decoupled treatment of this link consists in introducing a penalty spring between the reference position of a steel node in the corresponding concrete element and its actual position.


The default spring’s stiffness is obtained from concrete element through the formula:

k = GL


with:

G : bulk modulus of concrete element’s material,

L : radius of a sphere whose volume equals concrete element’s volume.


Compatibility: COUP, DECO, LIAI


Syntax:
       "ARMA"         < "TSTA" ista> < "CSTI" cstif >
                      "BETO" /LECTURE/
                      "FERR" /LECTURE/


ista

DECO only: flag for stability control over the penalty spring’s stability (default: 1, see comment below)..
cstif

DECO only: coefficient multiplying default stiffness of the penalty spring (default: 1.0).
BETO

Introduces the list of the concrete (continuum-like) elements.
FERR

Introduces the list of the steel or reinforcement (bar-like) elements.

Comments:


The concrete elements must be of continuum-like type 2D or 3D. The steel or reinforcement elements must be of bar-like type (e.g. BR3D in 3D or BARR in 2D).


If ista equals 2, stiffness of the penalty spring is limited so that the associated stability time-step is not smaller that the reference concrete element’s one.

4.12  CROSSING

D.126


Object:

This directive allows the user to automatically interconnect crossing longitudinal and transverse reinforcement bars (rebars) to constitute rebar cages (carcasses) frequently used to reinforce the concrete structures. In the real life, the rebars in the cages are usually connected either by welding, tying steel wire, or with mechanical connections.

Links are created between the elements of longitudinal reinforcement and the nodes of transverse reinforcing steel (stirrups).

Both coupled and decoupled links are implemented: the coupled links are treated using Lagrange multipliers method whereas the decoupled ones are solved by the penalty method.

Only the translation degrees of freedom are concerned by this link.

Nodes of the transverse rebars may eventually coincide with the nodes of the longitudinal rebars but should remain distinct.


Compatibility: COUP, DECO


Syntax:
       "CROS"  < "TSTA" ista> < "CSTI" cstif >
               "LONG" /LECTURE/
               "TRAN" /LECTURE/
ista

DECO only: flag for stability control over the penalty spring’s stability (default: 1, see comment below)..
cstif

DECO only: coefficient multiplying default stiffness of the penalty spring (default: 1.0).
LONG

Introduces the list of longitudinal rebar elements.
TRAN

Introduces the list of transverse rebar elements.

Comments:

Both the logitudinal and transverse rebars must be modelled as POUT elements.


If ista equals 2, stiffness of the penalty spring is limited so that the associated stability time-step is not smaller that the reference longitudinal steel element’s one.

4.13  ACBE: REBAR(FEM)-CONCRETE(DEM) LINK

D.127


Object:

This directive allows creating nonlinear links between a steel reinforcement bar (rebar) modelled as FEM beam and plein concrete modelled by the discrete element method (DEM). Only one link between a given discrete element and a finite element beam may be created. Each link contains a normal and a tangential component.

A decoupled (DECO) link model is implemented only.


Syntax:
       "ACBE"  < "TSTA" ista> < "CSTI" cstif >
               "BETO" "COEF" c1 /LECTURE/
               "ARMA" "COEF" c2 /LECTURE/
               "YOUN"  youn  "TN" tn "CN" cn "ADUN" adun
              < "AMOR"  amor >
               "FTAN" "NUMF" nf
ista

Flag for stability control over the penalty link’s stability (default: 1, see comment below).
cstif

Coefficient multiplying default stiffness of the link (default: 1.).
BETO

Introduces the list of discrete elements concerned.
c1

Coefficient defining the interaction range for the discrete elements.
ARMA

Introduces the list of rebar (POUT type) elements concerned.
c2

Coefficient defining the interaction range for the beam elements.
youn

Young’s modulus used to calculate the normal stiffness of the link (kn=youn*S/L).
tn

Maximum normal tensile strength (perpendicular to the rebar direction)
cn

Maximum normal compression strength (perpendicular to the rebar direction)
adun

Softening coefficient (ratio between elastic and softening slopes >0)
amor

Reduced damping coefficient applied on steel-concrete links if needed
nf

Number of the function describing the tangential behaviour of the link.

Comments:


If ista equals 2, stiffness of the penalty spring is limited so that the associated stability time-step is not smaller that the reference concrete element’s one.

4.14  LCAB: LINK BETWEEN PRESTRESSING CABLES AND CONCRETE

D.128


Object:

This directive allows creating kinematic relations between the nodes of prestressing cables modelled as FE bars (BR3D) and the nodes of plain concrete modelled through a FE thick shell model (T3GS,Q4GS). First, a projection of cable nodes onto concrete mesh is done to determine cable node to concrete element correspondence, and then, node by node relations are written.

Adherent and sliding conditions are implemented. In the adherent case, the cable-concrete links act in 3 space directions. For the purely sliding case, only 2 relations per cable node are written (in the normal directions to the cable), the relation in the tangential direction is not written. Those relations are updated at each time step in order to account for the cable direction change when sliding in a curvilinear case.

It is possible to add friction to the sliding case. To do this, RNFR friction-spring elements must be added to the model and declared in the directive GEOM (just after BR3D cables elements). RNFR elements are of SEG2 type with the nodes that coincide geometrically at the beginning of the calculation: the first RNFR node corresponds to cable’ node (except for the cables’ extremity nodes) and the second one is automatically connected to a concrete point having the same global coordinates and being related to concrete element nodes by ADHE-type relations. The RNFR elements are detected automatically when using LINK LCAB FROT option, thus there is no need to declare them in the present directive. It should be noted that RNFR elements cannot be used outside the LCAB directive.

For theoretical description see [].

This link model is implemented in coupled (LINK COUP) version only.


Syntax:
       "LCAB" $[ "ADHE" ; "GLIS" ; "FROT" ]$
               "BETC" /LECTURE/
               "CABL" /LECTURE/
ADHE

Fully adherent option.
GLIS

Perfectly sliding option.
FROT

Sliding with friction.
BETC

Introduces the list of concrete shell (T3GS,Q4GS type) elements concerned.
CABL

Introduces the list of cable (BR3D type) elements concerned.

Comments:


This directive may by repeated as many times as necessary.

4.15  ARLQ: SHELL-3D MESH COUPLING WITHIN THE ARLEQUIN FRAMEWORK

D.129


Object:

This directive allows linking in a continuous way two (or more) sub-domains used to model a slender structure, some sub-domains modeled as thick shells (Reissner-Mindlin kinematics) and others represented through a 3D hexahedra-type mesh. The shell and 3D sub-domains are glued in a weak sense within an overlapping zone using the Arlequin method ([]).


The following hypotheses must be satisfied:


- only Q4GS quadrangular shell and CUB8 hexahedron elements can be used,


- the shell and 3D meshes in the gluing zone must be hierarchic.


This link model is implemented in coupled (LINK COUP) version only.


Syntax:
       "ARLQ" < "ROTA" >
               "COQU" /LECTURE/
               "VOLU" /LECTURE/
ROTA

Optional key-word to be used to add the gluing of rotations.
COQU

Introduces the list of shell (Q4GS) elements of the gluing zone.
VOLU

Introduces the list of 3D (CUB8) elements of the gluing zone.

Comments:


This directive may by repeated as many times as necessary.

4.16  IMPOSED MOTIONS

D.130


Object:


These instructions define imposed motions (displacements, velocities or accelerations) depending on time, for different degrees of freedom.


Compatibility: COUP, LIAI


Syntax:

    "DEPL"  ( /LECDDL/  coef  "FONC"  ifonc  < "TLIM" tlim > /LECTURE/  )
    "VITE"  ( /LECDDL/  coef  "FONC"  ifonc  < "TLIM" tlim > /LECTURE/  )
    "ACCE"  ( /LECDDL/  coef  "FONC"  ifonc  < "TLIM" tlim > /LECTURE/  )


/LECDDL/

Reading procedure of the different d.o.fs concerned.
coef

Multiplying factor of the values of the function.
ifonc

Number of the function to be used.
tlim

Time after which the imposed motion is deactivated.
/LECTURE/

Reading procedure of the numbers of the nodes concerned.

Comments:


The function to be used will be defined by means of the principal instruction "FONC" which enables the user to choose a tabulated function (linear interpolation between the points), or a function programmed by the user by means of a subroutine.


At a time t, the imposed motion is : coef*F(t). In this case, only one function is to be defined, if the motions vary only in amplitude.


If the same d.o.f is submitted to several motions, EUROPLEXUS only takes into account the motion which has been defined first.


Motion can be imposed temporarilly using the "TLIM" keyword.

4.17  CONNECTIONS BETWEEN SHELLS AND SOLID ELEMENTS

D.140


Object:


The purpose is to link together the degrees of freedom at the boundary of two parts of the structure. One part is meshed with shells, the other with solid elements. This link is available only for two-dimensional computations (plane or axisymmetric).


Compatibility: COUP, LIAI


Syntax:

    "COQM"  ngroup*(  nco  nma  /LECTURE/  )


ngroup

Number of groups of shell and solid element connections.
nco

Number of the shell node linked to a solid element.
nma

Number of the solid node linked to a shell.
/LECTURE/

Reading procedure to input the other solid element nodes which are connected (no compulsory order).

Comments:
            M1  x---------
                I
     (shell)    I
     --------x  x  M0 (nma)          R(i) : distance M0-Mi
            /   I                    D(i) : normal displacement
         nco    x  Mi                       of Mi
                I    (solid element)
           Mp   x----------


A "shell-solid element" relation is represented by the following p+2 equations.


2 equations for the displacements:

U(1,nco) = U(1,nma)

U(2,nco) = U(2,nma)


p equations for the rotations of p other solid element nodes:

U(3,nco) = R(i) * D(i)

4.18  INTERFACES

D.141


Object:


This directive allows to define an interface between two lines or two surfaces. Link relations are created so that the velocity field is continuous through the interface. In the case of non-matching meshes on both sides of the interface, continuity is imposed in a weak sense.


This directive is very similar to the INTERFACE directive used in the sub-domain calculation framework.


Compatibility: COUP


Syntax:
"INTERFACE"   |[ "COMP"    ;
                   "MORTAR"  ;
                   "OPTIMAL" ]| <"TOLE" tole> ...

          ... |[ "SIDE"    ;
                 "SCOARSE" ;
                 "SFINE"   ]| /LECTURE/ ...

          ... |[ "SIDE"    ;
                 "SCOARSE" ;
                 "SFINE"   ]| /LECTURE/


"COMP"

Keyword declaring an interface with matching meshes.
"MORTAR"

Keyword declaring an interface with non-matching meshes, treated by the mortar method (see comment below).
"OPTIMAL"

Keyword declaring an interface with non-matching meshes, treated by the optimal method.
tole

Tolerance given to find matching nodes (default=1.E-3).
"SIDE"

Keyword introducing the support of both sides of the interface for COMP and OPTI cases (see note below).
"SCOARSE"

Keyword introducing the support of the side of the interface with coarse mesh in the MORTAR case (see note below).
"SFINE"

Keyword introducing the support of the side of the interface with fine mesh in the MORTAR case (see note below).

Comments:


There MUST NOT be any coincident nodes between the two sides of an interface.


When using the mortar method, the side of the interface whose mesh is used to discretize Lagrange multipliers has to be specified. It is the mesh introduced by the SFINE keyword, the other mesh being introduced by the SCOARSE keyword.


When using interfaces with non-matching meshes, so-called CLxx elements (see pages INT.90 and INT.100) have to be affected to meshes of both sides of the interface. These elements must be given the “phantom” material (MATE FANT) with density equal to zero.


The treatment of non-matching meshes with 3D solid elements is restricted to hierarchical meshes. In this case, the mortar method and the optimal method are identical, and a mortar interface has to be declared.


The mortar method may be used with any element types in 2D, but only with shell element types in 3D. When using the mortar method with linear interfaces (2-noded element sides), there must be at least one geometrical point that has the same coordinates, within the tolerance tole defined above, in the two facing meshes. This is necessary because the interface model uses the point’s coordinates internally in order to define a reference frame on the interface.

4.19  FLUID-STRUCTURE COUPLING

D.142


Object:


This directive allows to specify the coupling between a fluid and a structure modelled by topologically independent meshes.


Compatibility: COUP


Syntax:

    FLST <SLID> STRU /LECTS/ FLUI /LECTF/
               <DGRI> $[ HGRI hgri ; NMAX nmax ; DELE dele ]$


/LECTS/

List of structural nodes concerned. They must be declared as Lagrangian.
/LECTF/

List of fluid elements concerned.
DGRI

Dump out the initial grid of cells used for fast searching on the listing (only at step 0).
HGRI

Specifies the size of the grid cell. Each cell has the same size in all spatial directions and is aligned with the global axes.
NMAX

Specifies the maximum number of cells along one of the global axes.
DELE

Specifies the size of the grid cell as a multiple of the diameter of the largest coupled fluid element. Element “diameters” are computed only along each global spatial direction and the maximum is taken. For example, by setting DELE 4 the size of the cell is four times the diameter of the largest coupled fluid element. By default, i.e. if neither HGRI, nor NMAX, nor DELE are specified, the code takes DELE 3.

4.20  FLUID-STRUCTURE COUPLING 2 (FLSR)

D.143


Object:


This directive allows to specify a “strong” coupling between a fluid and a structure modelled by topologically independent meshes. It is similar to FLSW (see page D.555) but uses a strong approach (constraint on velocity imposed by Lagrange multipliers) rather than a weak approach (direct application of the fluid pressure (constraint on velocity imposed by Lagrange multipliers).

The present FLSR directive is (primarily) intended for use with Finite Elements (FE) modeling of the fluid.


The fluid mesh may be either fully general (unstructured) or regular (structured), as specified by the STFL directive described on page C.68. In the latter case, the search operations are faster.


The FSI coupling is realized between structural points (ultimately, structural nodes) on one side, and fluid entities on the other side. The fluid entities are fluid nodes in this case, since in the FE method the velocities are discretized at the nodes of the FE.


Compatibility: COUP, DECO.


Syntax:

    FLSR     STRU /LECTS/
          |[ FLUI /LECTF/ ; STFL ]|
          $[ R r       ; GAMM gamm ; PHIS phis ]$
          $[ HGRI hgri ; NMAX nmax ; DELE dele ]$
            <DGRI>
            <BFLU bflu $[/LECTURE/]$>
            <FSCP fscp>
            <DVOF dvof $[/LECTURE/]$>
            <ADAP LMAX lmax <SCAL scal> >


STRU

Introduces the structure mesh to be coupled with the fluid. The concerned elements are specified next.
/LECTS/

List of structural elements concerned. All their nodes must be declared as Lagrangian.
FLUI

The fluid mesh to be coupled with the structure is fully general (unstructured). The concerned elements are specified next.
/LECTF/

List of fluid elements concerned. The fluid mesh is unstructured.
STFL

The fluid mesh to be coupled with the structure is regular (structured). The concerned elements need not be specified. In fact, they are simply the elements generated by the STFL directive described on page C.68, which must in this case have been specified previously in the input file.

Structural influence domain

The next three keywords (R, GAMM or PHIS) are used to set the size (thickness) of the structural influence domain surrounding the structure elements defined above by /LECTS/. All fluid nodes contained within this influence domain will be coupled to the structure. Therefore, the correct size of the influence domain is related to the size of the fluid mesh in the vicinity of the embedded structure. On one hand, if the influence domain is too thin, then some interactions between the structure and the fluid enetities might be overlooked, thus resulting in spurious passage of fluid across the structure (leakage). On the other hand, if the inluence domain is too thick, too much fluid will be interacting with the structure (excessive added mass effect). The optimal value is then the minimum value which ensures structure tightness (no leakage).

By default, i.e. f neither R nor GAMM nor PHIS are specified, the code performs an automatic determination of influence spheres at each coupled structural node by using the default value of GAMM (γ=1.01). For the choice of R, GAMM or PHIS in adaptive calculations see the ADAP keyword below and the comments at the end of this page.

R

Prescribed (fixed) radius R of influence spheres at each coupled structural node. In the special, but frequent, case of a uniform structured fluid mesh (uniform square or cube elements) it is suggested to take R slightly larger than the semi-diagonal of a fluid element. This means that, for a 2D uniform square fluid mesh of side LΦ one should take R=0.71LΦ while for a 3D uniform cube fluid mesh of side LΦ one should take R=0.87LΦ.
GAMM

Coefficient γ for the automatic determination of influence spheres at each coupled structural node, based on the size of the enclosing fluid element (which must thus be found by the code by means of a fast search algorithm, see the remarks at the end of this manual page). The sphere radius is RRF=γδ LΦ where LΦ is the local length (size) of the fluid mesh, δ is a coefficient related to the space dimension d of the problem (δ=√d /2, i.e. about 0.71 in 2D and about 0.87 in 3D calculations). The quantity indicated as RF above is the “natural” size of the sphere radius, i.e. the radius of a sphere (circle in 2D) which exactly encompasses all nodes of a regular element (regular cube in 3D or regular quadrilateral in 2D). By default it is γ=1.01. This value should ensure “tightness” of the structure, at least for a regular mesh. By increasing the value, tightness is safer but the amount of fluid “attached” to the structure also increases. By decreasing the value, some local spurious passage of fluid across a solid structure might occur.
PHIS

Coefficient φs for the automatic determination of influence spheres at each coupled structural node. The sphere radius is equal to φs times the minimum structural element length at the concerned node. By default it is φs=0.3. This option should be rarely used. It is advisable to use GAMM instead.

Fast search of coupled fluid entities

The next three keywords (HGRI, NMAX or DELE) are used to set the size of the spatial grid used for the fast search of fluid nodes contained within the influence domain of the structure. Fast search speeds up the calculation and is absolutely essential in medium and even more in large size simulations. For this reason, fast search is always active in the present FSI model. Note that this may be unlike other types of search in EPX. For example, in the pinball contact model (PINB) fast search of pinballs contact is not active by default (an option has to be activated).

By default, i.e. if neither HGRI, nor NMAX, nor DELE are specified, the code takes DELE 1.01.

A (regular) spatial grid is built up and used for the fast search. The fluid nodes contained in a cell are tested for inclusion in the structural influence subdomains contained either in the same cell or in a direct neighbor cell (there are up to 8 such cells in 2D, up to 26 cells in 3D). The cell grid can be optionally dumped out on the listing by the DGRI keyword.

For the calculation to be as fast as possible, the fast search grid must have the minimum size ensuring correctness of results, i.e. such that a (barely) sufficient number of interacting entities is detected, and thus no spurious fluid passage occurs across the structure. If hF denotes the size of the fluid mesh and hS the size of the structure mesh, then the grid size hG must be:

hG=φ·max(hF,hS)       (1)

where φ>1 is a sefety factor. A value φ=1.01 should be sufficient. Since a single grid is used for the search over the whole computational domain, hF and hS in the above expression must be the maximum sizes of the fluid and structural elements which are susceptible of interacting, i.e. which belong to the /LECTF/ and LECTS/ sets defined above.

In calculations without adaptivity one has normally hF<hS for accuracy reasons (especially if shells are used to discretize the structure), so that the grid size is (normally) dictated by the largest coupled structural element. For the case of adaptive calculations, see the Remarks at the end of this manual page.

HGRI

Specifies the size of the fast search grid cell. Each cell has the same size in all spatial directions and is aligned with the global axes.
NMAX

Specifies the maximum number of cells along one of the global axes.
DELE

Specifies the size of the fast search grid cell as a multiple of the length of the largest coupled structural element. Element “diameters” are computed only along each global spatial direction and the maximum is taken. For example, by setting DELE 2 the size of the cell is two times the length of the largest coupled structural element. By default, i.e. if neither HGRI, nor NMAX, nor DELE are specified, the code takes DELE 1.01.
DGRI

Dump out the initial grid of cells used for fast searching on the listing (only at step 0).

Additional optional parameters

Next come some additional parameters.

BFLU

Type of treatment of numerical fluxes (density and energy, but not momentum) in fluid models, when used in conjunction with the present FLSR directive. This directive applies to fluids modelled by multicomponent node-centered Finite Volumes (NCFV, i.e. MCxx ‘elements’) and to any fluid modelled by CEA Finite Elements.

In both cases, the value 0 (default) indicates that fluxes are freely computed.

For MCxx elements, the value 1 indicates that fluxes are blocked between two fluid nodes (or points) which are both within the influence domain of the structure. For CEA fluid elements, it indicates that the fluxes are blocked through a face for which one node at least is within the influence domain of the structure.

For MCxx elements, the value 2 indicates that fluxes are blocked between two fluid nodes (or points) of which at least one lies within the influence domain of the structure. For CEA fluid elements, it indicates that the fluxes are blocked through a face for which all nodes are within the influence domain of the structure.

With CEA fluid elements, the defined treatment can be restricted to the influence domain of a subset of structure elements using the LECTURE procedure.

FSCP

Type of coupling by Lagrange multipliers between fluid nodes and corresponding structural points, when used in conjunction with the present FLSR directive. The value 0 (default) indicates that coupling occurs only in the direction normal to the structure. The value 1 indicates that coupling occurs along all spatial directions.
DVOF

Locally deactivate VOFIRE anti-dissipative scheme when used in conjunction with the present FLSR directive.

The value 0 (default) indicates that no deactivation occurs.

The value 1 indicates that VOFIRE anti-dissipation is deactivated for fluid elements, it indicates that the fluxes are blocked throu for which one node at least is within the influence domain of the structure.

The value 2 indicates that VOFIRE anti-dissipation is deactivated for fluid elements, it indicates that the fluxes are blocked throu for which all nodes are within the influence domain of the structure.

The defined deactivation can be restricted to the influence domain of a subset of structure elements using the LECTURE procedure.


FSI-driven adaptivity

Finally, there are some optional keywords related to automatic (FSI-driven) adaptivity of the fluid mesh near the structure.

ADAP

Activates mesh adaptivity for automatic refinement and un-refinement of the fluid mesh specified by /LECTF/ in the vicinity of the structure specified by /LECTS/. Note that this type of mesh adaptivity is at the moment incompatible with other types of adaptivity such as those activated by the WAVE or INDI directives.
LMAX

Introduces lmax, the desired maximum adaptive refinement level Lmax of the fluid mesh in the vicinity of the structure. This value should be greater than 1, since level 1 is attributed to the base mesh (no refinement). Each level corresponds to a halving of the mesh size with respect to the immediately previous level.
SCAL

Introduces scal (s), an optional scaling factor to be used in the determination of elements to be refined. By default scal is equal to 1. When scaling the structural influence domain by successive powers of two in order to identify, at each refinement level, the fluid elements to be refined or un-refined, the code finally multiplies the result by this factor. Using a value of s greater than one, e.g. 1.5 or 2, correspondingly enlarges the zone of fluid mesh arond the structure which is refined and this may result in a smoother mesh transition (for example, as an alternative to the option OPTI ADAP RCON). Note, however, that s has no influence on the size of the structural influence domain used for the final search of fluid entities (fluid nodes or fluid cell interfaces) interacting with the structure. This search is always done by the smallest influence domain RLmax = R1/2Lmax − 1, i.e. without taking into account the s factor.

In FSI adaptive calculations, the size of the structural influence domain specified in input by R, GAMM or PHIS is related to the base (i.e. the coarsest) fluid mesh size, not to the refined one (for the user’s convenience) and is then scaled automatically by the code whenever necessary, up to the maximum chosen refinement value given by the ADAP LMAX keyword. Therefore, in order to try out different adaptive refinement levels in the vicinity of the structure the user needs only to change LMAX in the input directive (all other parameters R etc. remain the same).

In FSI adaptive calculations, that is when the FLSR ADAP LMAX optional keyword has been specified, one is certain that the fluid mesh in the vicinity of the structure will be constantly refined to the maximum level (minimum size) specified for the fluid (LMAX), given by:

hFrefined=hFbase/2Lmax−1     (2)

For this reason, in the equation (1) for the determination of the grid size HGRI (hG) one can use hFrefined instead of the base fluid mesh h+Fbase=hF, obtaining thus:

hG=φ·max(hFrefined,hS)       (3)

One should make sure to use (3) instead of (1) since it is likely to be hFrefined<hS, while it is typically hF>hS, so this may lead to important savings of CPU time.


Remarks:


In case of automatic determination of influence spheres based on the GAMM keyword in conjunction with an unstructured fluid grid, a fast search over the coupled fluid elements is needed in addition to the normal fast search over the coupled structural elements. Scope of this second search is to detemine, for each structural node, which is the fluid element currently containing the node. For this purpose, the code uses a fast search algorithm by means of the same parameters (DGRI, HGRI, NMAX, DELE) specified above for the search over structural elements. Note, however, that as concerns this second search if DELE is specified it refers to the size of the fluid element rather than to the size of the structural element. However, if a structured fluid grid is specified, then no additional search is needed because the containing fluid element can be detected directly.


Make sure you consult the additional options related to the functioning of the FLSR model in pages H.155 and H.160.


References

The FLSR model was first described in report []. A short description of the model is also given in reference [].

4.21  FLUID/IMMERSED STRUCTURE INTERACTION (FLSX)

D.144


Object:


This directive allows to specify the coupling between a fluid and a structure modelled by topologically independent meshes. The fluid can either be in finite elements or in finite volumes. This directive is more recent than FLSR and FLSW directive and is expected to provide more accurate solutions. At this time, the fluid mesh must have all of its nodes declared as EULE (i.e. Eulerian, not ALE). This directive only works in a 3D space. At this time, only thin structures are supported (the mesh of the structure must only contain shell elements).


Compatibility: COUP (for FE fluid meshes), DECO (for FV fluid meshes).


Syntax:

    FLSX     STRU /LECTS/
             FLUI /LECTF/
            <LSPC lspc>
            <LORD lord>


STRU

Introduces the structure mesh coupled with the fluid. This mesh can be meshed totally independently from the fluid mesh. The concerned elements are specified next.
/LECTS/

List of the structural elements concerned. All their nodes must be declared Lagrangian in the GRIL directive.
FLUI

Introduces the fluid mesh coupled with the structure. The concerned elements are specified next.
/LECTF/

List of the fluid elements concerned. All their nodes must be declared Eulerian in the GRIL directive (note that nodes not explicitly mentioned in the GRIL directive are Eulerian by default).

The two options LSCP and LORD are effective only if the fluid is treated with finite elements. In this case, the FLSX coupling results from a finite-element discretization of the constraint:

 


Γ


vs(x)−vf(x)
· ns(x)
λ(xdx , ∀λ∈ L2(Γ)     (4)

where Γ is the mid-surface of the structure, vf and vs the fluid and structure velocity respectively, ns the normal to Γ, and λ a test function. The two options LSCP and LORD specify the finite-element space on which the Lagrange multiplier related to the test function λ is discretized. If LSCP is set to 0 (default), the Lagrange multiplier is defined on a finite element space generated from the mesh of the structure. If LSCP is set to 1, the Lagrange multiplier is defined on the “restriction” to the structure mesh at each time step of a finite-element space generated from the mesh of the fluid. LORD, which can be 0 or 1 (default), is the polynomial degree of interpolation used to generate the finite-element space for the Lagrange multiplier.

LSCP

Finite-elements fluid only.
Specifies which mesh is used to generate a finite-element space for the lagrange multiplier enforcing the coupling. If set to 0 (default), the mesh of the structure is used. If set to 1, the mesh of the fluid is used.
LORD

Finite-elements fluid only.
Specifies the polynomial degree of interpolation used to generate the finite-element space for the Lagrange multiplier. If set to 0, constant-value elements are used. If set to 1 (default), linear elements are used.

4.22  FLUID-STRUCTURE INTERACTIONS

D.150


Object:


This is aimed at linking together the degrees of freedom at the boundary of 2 parts of the structure:


- one part meshed with shells or solid elements;


- one solid element part meshed with a fluid material.


This possibility exists for two- and three-dimensional computations.


This connection may be expressed in two ways:


- By using specific fluid-structure elements FS2D or FS3D: directive "FS";


Without using fluid-structure elements: directive "FSA".


Compatibility: COUP, LIAI


Comments:


The first directive is available for a Lagrangian or an ALE calculation. Instead, the second is only valid for ALE problems.


The elements FS2D and FS3D behave like incompressible fluids. In order to avoid spurious effects (related to the flow along the boundary), the thickness of this boundary zone must be as small as possible, and possibly 0.


The "FS" directive is described in the next page, while for the "FSA" directive please consult page D.260.

4.22.1  FLUID-STRUCTURE CONNECTION (FS)

D.152


Object:


The contact between the fluid and the structure is modelled by elements FS2D and FS3D. This directive is available for Lagrangian and ALE calculations.


Compatibility: COUP, LIAI


Syntax:

    "FS"  /LECTURE/


/LECTURE/

Numbers of the FS2D, FS3D or FS3T elements composing the boundary.

Comments:


The FS2D, FS3D and FS3T elements are in fact incompressible fluids. In order to avoid any parasitic effects (due to a potential flow along the boundary), the thickness of that boundary zone has to be as small as possible and even equal to zero.


It is strongly advised to use the new directives "FSA" and "FSR".

4.23  UNILATERAL RESTRAINT [OBSOLETE]

D.160


Foreword:


This directive is now obsolete, use the IMPACT directive described below (page D.170) which allows to compute at the same time the shock parameters (impulse, reaction, ...).

4.24  IMPACT

D.170


Object:


As for unilateral restraints, certain nodes of the structure must remain in the same half-space. However, the boundary is linked to the position of a material point and can be mobile. Impacts are possible in 2D or 3D.


The method of Lagrange multipliers may be activated by adding the keyword "LAGC" in the problem type (see page A.30). This method allows to couple the calculation of contact forces with the permanent connections (relations, boundary conditions, ...). It also allows to take into account the form of a projectile ‘nose’ in the case of a non-deformable projectile.


Compatibility: COUP, DECO, LIAI


Syntax:

    "IMPACT" "DDL" iddl "COTE" alpha       ...

              ... < "NEZ" |[ "HEMI" "RAYO" rayon1                  ;
                             "PLAT" "LARG" larg1  < "LONG" long1 > ;
                             "CONE" "LARG" larg2  < "ANGL" beta  > ;
                             "CYLI" "RAYO" rayon2 ]| >

              ... <"FROT" "MUST" must "MUDY" mudy "GAMM" gamm >

              ...  "PROJ" /LECTURE/  |["CIBL" /LECTURE/ ; "CIBD" /LECTURE/]|


iddl

Component concerned. Indicates the first direction.
alpha

Enables one to choose between the 2 half-spaces separated by the plane of equation x = x0. It must be an integer. Typically, one uses either +1 or −1.
rayon1

Radius of a projectile with hemispherical nose.
larg1

Width of a projectile with rectangular flat nose. It is in the second direction obtained by circular permutation of the Euclidean frame.
long1

Only in 3D, length of the rectangular projectile nose. It is in the third direction (obtained by circular permutation).
larg2

Width of a projectile with a conical nose.
beta

Half-angle of the cone (in degrees).
ray2

Radius of the projectile with cylindrical nose.
FROT

Introduces the (optional) declaration of friction characteristics.
must

Static friction coefficient µs: (0 < µs < 1).
mudy

High-velocity (dynamic) friction coefficient µd: (0 < µd < µs < 1).
gamm

Coefficient γ of the friction law. This law is similar to the one used for sliding lines and sliding surfaces (see page D.180). The friction coefficient µ varies from µs to µd as the relative tangential velocity Vr of the two bodies increases. The passage is governed by the exponential decay law: µ = µd + (µs − µd)e(−γ Vr).
PROJ

Introduces the number of the material point located on the boundary (if relevant, it is the tip of the projectile “nose”).
CIBL

Introduces the numbers of the nodes which are submitted to the impact.
CIBD

Used for ELDI elements only to take into account the elements’ radius for contact detection. Introduces the numbers of the discrete elements which are submitted to the impact.

Comments:


The boundary plane is perpendicular to one of the axes of the general coordinate system. This axis is defined by the component iddl, just as for unilateral contacts.


The half-space admissible for a point M (of the target) of coordinate x is such that, if x0 is the abscissa of the material point:

α (xx0) ≥ 0 


These impacts are available in 2-D or 3-D.


It is suggested to displace the projectile in such a way that the impact occurs after at least one time step.


Do not forget to dimension the keywords "IMPA" and "PSIM" correctly, see (page A.80).


The "NEZ" directive is available only with the LAGC option. When it is present, only those "CIBLE" nodes which are in contact with the geometric boundary thus defined, will be considered.


Without the option "LAGC":


It should be noted that the nodes which undergo shocks may not be connected by other imposed relations (LIAISONS).


The shock between the material point (projectile) and the point(s) of the target is treated elastically. The energy and impulse will therefore be conserved during the impact. This requires a modification of the time step so that the impact instant coincides with the beginning of a time step.


This effect introduces a small error in the work of forces during the impact, of the order: dW =F * v * dt. It is therefore advisable to shorten the time step in order to obtain better energy conservation.


These recommendation are irrelevant with the option "LAGC".

4.25  GAPS ("JEUX")

D.175


Object :


This is an impact between the (uncoupled) nodes along the direction defined by the user. This directive is available in 2D and 3D. In 3D, the gap must be defined also along a direction normal to the first one.


Compatibility: LIAI


Syntax:

  In 2D:

    "JEUX"    "AXE1" a1x a1y      "JEU1"  jeu1
       ...    "NOE1"  /LECTURE/
       ...    "NOE2"  /LECTURE/

  In 3D:

    "JEUX"    "AXE1" a1x a1y a1z   "AXE2" a2x a2y a2z
       ...    "JEU1"  jeu1     "JEU2" jeu2a jeu2b
       ...    "NOE1"  /LECTURE/
       ...    "NOE2"  /LECTURE/


a1x,a1y (,a1z)

Components of the first vector of the local reference.
a2x,a2y,a2z

Components of the second vector of the local reference (3D only).
jeu1

Gap along the direction of the first vector.
jeu2a,jeu2b

Gap along the direction of the second vector (3D only).
NOE1

Announces the first group of nodes.
NOE2

Announces the second group of nodes.

Comments:


To each node P1 belonging to the first group, is associated one node P2 of the second group, and reciprocally. In 3D, in the local frame of origin P1, defined by vectors AXE1 and AXE2, the impact occurs when: 1) the abscissa of point P2 is less than jeu1; 2) and the ordinate of point P2 lies between jeu2a and jeu2b.


In 2D, in the local reference of origin P1 of which AXE1 is the first axis, the impact occurs when the abscissa of point P2 is less than jeu1.


The direction defined by vector(s) AXE1 (or AXE2) does not change during the calculation.


Do not forget to dimension, by keyword "NBJEUX" (see page A.80).

4.26  BUTEE: LIMITED DISPLACEMENT

D.176


Object :


This directive allows limiting the displacement of a node along the direction defined by the user, when a prescribed distance is covered. This directive can be repeated several times. It is operational in MPI.


Compatibility: LINK COUP


Syntax:

    "BUTE"   "DIRE" vx vy vz
             "DMAX" dmax
             /LECTURE/


vx,vy,vz

Components of the vector indicating the direction of blocking.
dmax

Distance above which the displacement is blocked in the prescribed direction.
/LECTURE/

Name of the node for which the displacement is to be limited.

4.27  SLIDING LINES AND SLIDING SURFACES

D.180


Object:


This directive defines one or more couple(s) of mutually sliding lines (2D) or sliding surfaces (3D). In 3D the “master” and “slave” objects may be composed of continuum elements or shells. In 2D they are composed by an ordered series of nodes.


In 3D, an auto-contact model is available. An auto-contacting surface is both master and slave at the same time.


Compatibility: COUP, DECO, LIAI


LIAI only: the method of Lagrange multipliers may be activated by adding the keyword LAGC in the problem type (see page A.30, Section ??). This method allows to couple the computation of contact forces with the permanent connections (relations, boundary conditions, ...).


Penalty method is only available in 3D with DECO keyword. If not activated, the same uncoupled algorithm is used as with LIAI and LAGC deactivated (see above and comments below).


Syntax:
    "GLIS"  nglis * ( <"FROT" "MUST" must "MUDY" mudy "GAMM" gamm >

                      < "PENA" > < "PFSI" rfac > < "PGAP" rgap >
                      < "SELF" > < "ELIM" < "UPDT /CTIME/" > >
                      < "COHE" >
                      |[
                        |[ "MAIT"      <"NODE">     /LECTURE/          ;
                           "CMAI" /LECTURE/ |[ "EXTE" /LECTURE/ ;
                                               "INTE" /LECTURE/ ]| ]|

                        |[ "ESCL" ; "CESC" ; "PESC" ]|  /LECTURE/  ;

                        "AUTO" FACE iface  /LECTURE/                   ;

                        "DECO" <"SYME"> <"DBLE"> <"ELIM" <"UPDT /CTIME/">>
                               /LECTURE/
                      ]|
                      <   "COPT" 1    /LECTURE/  >              )


nglis

Number of couples of lines (or surfaces) (MAIT, ESCL) or AUTO.
FROT

Introduces the (optional) declaration of friction characteristics.
must

Static friction coefficient µs: (0 < µs < 1).
mudy

High-velocity (dynamic) friction coefficient µd: (0 < µd < µs < 1).
gamm

Coefficient γ of the friction law. This law is similar to the one used for the IMPA sirective (see page D.170). The friction coefficient µ varies from µs to µd as the relative tangential velocity Vr of the two bodies increases. The passage is governed by the exponential decay law: µ = µd + (µs − µd)e(−γ Vr).
PENA

DECO only: toggles the use of penalty method to compute contact forces (see comment below).
rfac

DECO only: scale factor for the automatically computed contact stiffness (see comment below).
rgap

Value of the gap between master surface and slave nodes (3D only). Default value is zero in the case of solid master elements and half of shell’s thickness in the case of shell master elements.
SELF

Toggles self-contact treatment for shells (3D only, see comment below).
ELIM

Toggles the elimination of the not visible faces (for each slave node) of the master elements in the detection of the contact (sometimes necessary option when the 3D master elements contain only a single element in the thickness). This elimination is only once realized during the initialization of the problem. The keyword UPDT can be used to introduce a regular update of this sorting. Indeed, the relative movement of the various elements of structure can require to redefine for each slave node the not visible faces of the master elements.
COHE

This keyword enters within the framework of the automatic separation of elements (See page A.63, Section ??, keyword DECO). Compulsory to update the list of the sliding surfaces and the list of the slave nodes.
MAIT /LECTURE/

Numbers of the master nodes (in 2D) or numbers of the continuum elements (in 3D).
MAIT NODE /LECTURE/

In 3D continuum elements: numbers of the master nodes belonging to the sliding surface.
CMAI /LECTURE/

Numbers of the master elements of the structure meshed by shell elements (“COQUES”) (in 3D).
EXTE /LECTURE/

Number of the node defining the half-space external to the solid.
INTE /LECTURE/

Number of the node defining the half-space internal to the solid.
ESCL /LECTURE/

Numbers of the slave nodes (in 2D) or numbers of the slave elements (in 3D).
CESC /LECTURE/

Numbers of the slave elements (in 3D) if the structure is meshed by shell elements (COQUES).
PESC /LECTURE/

3D only. Numbers of the slave nodes.
iface

Number (local) of the face of the elements submitted to auto-contact.
DECO /LECTURE/

Numbers of the continuum elements (only CUB8). The keyword "DECO" can appear only once and must be positioned in last position. The keyword "DECO" enters within the framework of the automatic separation of elements (See page A.63, Section ??, keyword DECO). This directive allows to treat self-contact and contacts between various pieces of wood coming from the automatic separation of elements. The creation of a new node causes the activation of a coupled link. In this link the slave node is the new node of the wood and the master faces are the free faces of the wood except the faces containing the new node and the faces already eliminated by the previous links. During the initialization NPTMAX_DECO (See page A.63, Section ??, keyword DECO) links are created but not actived (option by default). For each new node a coupled links is actived. More explanations can be found in [].
SYME

With this keyword the master faces of each new actived coupled link are the free faces of the wood except the faces containing the new node.
DBLE

With this keyword (2*NPTMAX_DECO) links (See page A.63, Section ??, keyword DECO) are created during the initialization but not actived. For each new node two coupled links are actived. In the first link the slave node is the new node. In the second link the slave node is the initial node.
ELIM

With this keyword the not visible faces (for the new slave node) of the master elements are eliminated in the detection of the contact. This elimination is only once realized during the initialization of the new actived link (option by default). The keyword UPDT can be used to introduce a regular update of this sorting. Indeed, the relative movement of the various elements of structure can require to redefine for the slave node the not visible faces of the master elements.
COPT 1

If COPT 1 is activated, the thickness of the slave surface is taken into account.

Comments:

Sliding lines (2D):


The order of the numbers of the nodes determines the orientation of the contour and defines in that way the inner side of the two domains after a rotation of +90 degrees.


The slave nodes must be located just at or above the boundary of the region defined by the line of the master nodes.


Without the LAGC option, it is preferable that the two lines have similar mesh densities. But, if the master domain presents a high convexity, it is better to have master segments which are a bit longer than the slave segments in front of them. This is aimed at minimizing the interpenetration of the two domains. It is suggested to fix a point of the master line (blocked material point) to avoid the interpenetration of the two domains.


With the LAGC option, the recommendations of the preceding paragraph are irrelevant.


When the “erosion” algorithm is activated (See page A.30, Section ??, keyword FAIL), the sliding surfaces are updated at each time step by eliminating the failed elements.


Sliding surfaces (3D):


For the sliding surfaces, the master and slave entities are defined by the elements composing them (possibly these are GIBI objects). If continuum elements are used, then it is not necessary to define the “inner” or “outer” sides of such entities. However, when shell elements are used, it is mandatory to define the outer half-space of the shell structure by a point.


SELF keyword is necessary if contact on both sides of a shell is considered with the same set of slaves (typically, the nodes of the shell itself). It prevents contact from being detected if a slave node has penetrated the shell of a value greater than the gap (see PGAP keyword). Without this, each slave node would initially be found in contact with one of the side of the shell.


With the MAIT NODE option, the master entity must be defined by the nodes belonging to the sliding surface.


It is not admitted to define master objects (nor slave objects) formed by continuum and shell elements at the same time.


Remark (2D and 3D):


The sliding nodes may not be linked by other imposed relations (LIAISONS), except in the case where the treatment of sliding lines (or surfaces) is done by the method of Lagrange multipliers (option LAGC).


Auto-contact:


This directive indicates that the surface formed by the set of faces defined by the user may be in contact. This surface is both master and slave at the same time.


The surface may only be formed by faces of continuum elements (CUBE, PRISME, etc.) or by thick shell elements with 8 nodes (SHB8). The shells with 3 or 4 nodes (DKT3, DST3, Q4GS, etc.) are currently not treated by this directive.


When using the penalty method to compute contact forces, contact stiffness is computed automatically from the stiffness of master elements using the following formulae :

k = rfac
GS2
V


in the case of solid master elements, with :

G : bulk modulus of master element’s material,

S : area of contacting face,

V : volume of master element.

k = rfac
GS
L


in the case of shell master elements, with :

G : bulk modulus of master element’s material,

S : area of master element,

L : maximum length of master element’s edges.

4.28  METHOD OF PARTICLES AND FORCES

D.185


Object:


This directive activates the (internal) interactions occurring among a set of particles (“billes”) representing a soft body, according to the so-called Method of Particles and Forces (MPEF).


Optionally, the user may require that the particles also interact with some structure, composed either of continuum or of shell elements. By omitting the definition of the structure, interaction occurs only between the particles themselves.


Compatibility: LIAI


Syntax:
    "MPEF" nbpef * (     "BILL" /LECTURE/
                    < $[ "STRU" /LECTURE/                  ;
                         "COQU" /LECTURE/ "EXTE" /LECTURE/ ]$ > )


nbpef

Number of pairs (BILL, STRU) or (BILL, COQU) or of single BILL groups (in case no structure is specified).
"BILL" /LECTURE/

Numbers of the nodes belonging to the BILL elements.
"STRU" /LECTURE/

Numbers of the “master” elements of the solid structure, meshed by continuum elements.
"COQU" /LECTURE/

Numbers of the “master” elements of the solid structure, meshed by shell elements.
"EXTE" /LECTURE/

Number of a node defining the “external” half-space to the solid shell structure. Here “external” means simply the side of the shell onto which the particles are going to impact. If the impact is going to occur on both sides of the shell, or if the shape of the shell is such that there exists no point that can be used to uniquely define the “external” space (think e.g. of a spherical structure impacted from outside the sphere), the present algorithm is inappropriate.

Comments:


If the structure domain presents a large convexity, it is advisable that the faces of the elements of the structure be longer than the diameter of the neighbouring particles. This in order to minimize the interpenetration between the two domains.


The data relative to this method are similar to those of the SPH method, described on page D.187.

4.29  SMOOTHED PARTICLE HYDRODYNAMICS METHOD (S.P.H.)

D.187


Object:


This directive activates the (internal) interactions occurring among a set of particles (“billes”) representing a soft body, according to the so-called Smoothed-Particle Hydrodynamics (SPH) method.


Optionally, the user may require that the SPH particles also interact with some structure, composed either of continuum or of shell elements. By omitting the definition of the structure, interaction occurs only between the particles themselves.


If a structure is specified in the directive described below, the interaction between the particles and the structure is treated by an algorithm of the ‘sliding surfaces’ type. The code offers also other alternative (more general and more robust) methods to describe the interaction between the SPH particles and a structure, see comments below.


Compatibility: LIAI


Syntax:
    "SPHY" nbpef * (     "BILL" /LECTURE/
                    < $[ "STRU" /LECTURE/                  ;
                         "COQU" /LECTURE/ "EXTE" /LECTURE/ ]$ > )


nbpef

Number of pairs (BILL, STRU) or (BILL, COQU) or of single BILL groups (in case no structure is specified).
"BILL" /LECTURE/

Numbers of the nodes belonging to the BILL elements.
"STRU" /LECTURE/

Numbers of the “master” elements of the solid structure, meshed by continuum elements.
"COQU" /LECTURE/

Numbers of the “master” elements of the solid structure, meshed by shell elements.
"EXTE" /LECTURE/

Number of a node defining the “external” half-space to the solid shell structure. Here “external” means simply the side of the shell onto which the particles are going to impact. If the impact is going to occur on both sides of the shell, or if the shape of the shell is such that there exists no point that can be used to uniquely define the “external” space (think e.g. of a spherical structure impacted from outside the sphere), the present algorithm is inappropriate. In such cases the user may utilize one of the alternative contact models mentioned in the comments below.

Comments:


The data relative to this method are similar to those of the PEF method, described on page D.185.


If a structure is specified in the directive described above, the interaction between the particles and the structure is treated by an algorithm of the ‘sliding surfaces’ type. Use is made of Lagrange multipliers, but by default the imposed contact constraints are decoupled from other constraints imposed e.g. vai LIAI or LINK directives.


To force coupling of the SPH contact constraints with other constraints, add the optional LAGC keyword in the calculation type, see Page A.30.


Sometimes contact detection and enforcement with the above mathod may be imprecise. In such cases, alternative (more general and robust) contact models can be used.


One possibility is to use the sliding surface algorithm via the LIAI or LINK directives. To this end, specify only the BILL keyword in the SPHY directive. Then, use the LIAI or LINK directive with the GLIS keyword to detect the contact. The LINK form of the directive can use either Lagrange multipliers (strong formulation, either in a coupled or in a decoupled manner, COUP or DECO), or a penalty method (weak formulation). On the “master” side, the MAIT keyword is used to specify a structure made of continuum elements, or the CMAI keyword for a shell structure. The SPH particles are then listed after the PESC keyword, that treats each particle as a “slave” material point. See page D.180 for further details.


Another possibility is to use the pinball method. To this end, specify only the BILL keyword in the SPHY directive. Then, embed pinballs both in the SPH particles themselves (with a diameter equal to the diameter of the particles) and in the impacted structure. The LIAI or LINK forms of the pinball contact method can be applied. The latter can use either Lagrange multipliers (strong formulation, either in a coupled or in a decoupled manner, COUP or DECO), or a penalty method (weak formulation). See page D.480 for further details.

4.30  CONNECTING FINITE AND DISCRETE ELEMENT MODELS

D.189


Object:


This directive defines a bridging (recovering) zone allowing to couple a set of discrete elements (ELDI) with a 3D finite element model (meshed with the CUB8 element only) or a shell model (Q4GS elements only).

The coupling equations are solved using Lagrange multipliers. To simplify, a diagonal matrix is used. It’s possible to couple discrete elements by using the complete matrix through the LINK procedure.


Compatibility: COUP


Syntax:
    "EDEF" nbcoup
           nbcoup*("NCOU"  ncouches
                  "ELDI"  /LECTURE/
                  "FRON"  /LECTURE/ )


nbcoup

Number of combined finite/discrete zones to connect.
"NCOU"

Number of finite element range defining the combined finite/discrete element zone.
"ELDI" /LECTURE/

List of the discrete elements concerned to research in the combined finite/discrete element zone.
"FRON" /LECTURE/

List of nodes forming the border of the finite elements mesh in the bridging finite/discrete element zone.

4.31  BIFURCATION CONNECTION

D.190


Object:


Writes the relations that ensure the conservation of mass flow rate for the fluid, and the equality of mechanical d.o.f.s if necessary (case of 1D coupled fluid calculation).


This directive may only be used in 1D.


Compatibility: COUP, LIAI


Syntax:

    "BIFU"   < LIBR >   /LECTURE/


/LECTURE/

Numbers of the BIFU elements for which the conservation of flow rate must be imposed.

Comments:


This directive may only be used in 1D, coupled or not, and for the junctions between the following elements:

               |  TUBE  |  TUYA  |  POUT  |
         ----------------------------------
         TUBE  |   yes  |   yes  |    -   |
         TUYA  |   yes  |   yes  |   no   |
         POUT  |    -   |   no   |   no   |


In the case of a bifurcation linking an element TUBE with an element TUYA, there may be only two nodes connected in the directive /LECTURE/ (no multiple branches).


In the case of bifurcations (even multiple) between TUYA, the 6 mechanical d.o.f.s are connected (continuity of the beam). In order to avoid these connections (for rxample in the case of a ‘soufflet’), add the keyword "LIBR". On the contrary, between a TUBE and a TUYA the 6 mechanical d.o.f.s are left free, and the keyword "LIBR" is irrelevant.


Outputs:


The various components of the ECR table are as follows:

ECR(1) : density (all materials)

ECR(6) : internal energy (water)

4.32  ADHESION CONNECTION

D.195


Object:


This link can describe adhesion connections between two surfaces. The contact will be opened, when a failure criterion is reached. From this point on, the link can not sustain any tension forces. But can still react to compression forces, when the gap is closed.

Until now, the adhesion connection is only implemented for 2D cases.


Compatibility: COUP


Syntax:

    "ADHE"  "AUTO" auto <"CRIT" "TENS" tens >  /LECTURE/


auto

Maximum distance for the automatic search.
tens

Maximum tensile strengthj for the difinition of the failure.
/LECTURE/

Objects which should be taken into account for the automatic search.

4.33  TUBM CONNECTION (3D-1D JUNCTION)

D.200


Object:


Write the relations ensuring the conservation of mass flow rate for the fluid (Eulerian formulation)


Compatibility: COUP, LIAI


Syntax:

    "TUBM"  /LECTURE/


/LECTURE/

Numbers of the "TUBM" elements (or names of the GIBI objects), which form the junctions.

4.34  TUYM CONNECTION (3D-1D JUNCTION)

D.203


Object:


Write the relations ensuring the conservation of mass flow rate for the fluid (moving meshes).


Compatibility: COUP, LIAI


Syntax:

    "TUYM"  /LECTURE/


/LECTURE/

Numbers of the "TUYM" elements (or names of the GIBI objects), which form the junctions.

4.35  TUYA CONNECTION (3D-1D JUNCTION)

D.205


Object:


Automatically writes the mechanical relations among d.o.f.s of a pipeline meshed by beams and a pipeline meshed by thin shells.


Compatibility: COUP, LIAI


Syntax:

    "TUYAU"  "CENTRE" /LECTURE/
             "LISTE"  /LECTURE/


"CENT" /LECTURE/

Number of the node (or name of the object) corresponding to the extremity of the pipeline meshed by beams.
"LIST" /LECTURE/

Number(s) of the node(s) (or name of the object) corresponding to the circle, extremity of the pipeline meshed by thin shells.

Comments:


This directive automatically writes the relations between the displacements of nodes belonging to the shells and the beam. All rotations are supposed to be equal.


All nodes involved by the link (including the CENT node) must have 6 dofs, since the imposed relations involve also the rotations. Therefore, the CENT node cannot be simply represented by a (stand-alone) PMAT, which has only 3 dofs. In such a case, it is sufficient to attach a (dummy) beam or shell element to the CENT.

4.36  RIGID BODY (SOLIDE INDEFORMABLE) CEA Implementation

D.210


Object:


This directive defines the sub-structures that will be considered as rigid bodies.


It also allows to impose the inertia tensor of the solid, or to leave EUROPLEXUS compute it starting from the mesh, or from a composition of simple homogeneous solids.


The directive may be used in two ways:

- The solid is meshed, i.e. its form is represented by a set of elements

- The solid is not meshed, i.e. one imposes that a small number of points be rigidly connected.


Compatibility: COUP, LIAI


Syntax:

    "SOLI" nsol*( ... )

     1st case - Solid meshed by elements:

            "ELEM" /LECTURE/  "PLIE" /LECTURE/ ...
                   $  <  "COMP" ncomp*( "INER"  ... )   >   $
                   $  <  "INER"  ...    >                   $

     2nd case - Rigidly connected points:

            "POIN" /LECTURE/


nsol

Number of non-deformable solids.
"ELEM" /LECTURE/

Numbers of the elements composing the solid.
"PLIE" /LECTURE/

Numbers of the points of the solid to be conserved because they take part in a connection (linked points).
ncomp

Number of homogeneous simple solids whose combination allows to compute the inertia tensor. In the case that ncomp = 1, this parameter is optional.
"INER"

This option allows to introduce the parameters of inertia of a solid, that will replace the ones computed starting from the mesh and the initial materials.
"POIN" /LECTURE/

Numbers of the points rigidly linked (case of the non-meshed solid).

Comments:


A sub-structure described like a non-deformable solid will reduce to a system of four material points. The calculation will be done with these points, and the solid will then be reconstructed to be viaualized.


The linked points (participatin in a connection) will be conserved in the calculation in order to be able to write down the connection relation.


The other points are not conserved in the calculation. However, they are used for the calculation of the inertia tensor. Care must then be taken that the discretization be sufficient, else the parameters related to the solid will be imprecise, and the computation will be affected by errors.


The "INER" directive is optional. It imposes to the solid inertia values coming from an external calculation. If it is absent, EUROPLEXUS computes inertias from the mesh.


If you impose the inertia tensor via "INER", you may limit the mesh to the minimum indispensable, by directly connecting the linked points (wireframe mesh). In any case, at least ONE free poit per solid is necessary, i.e. two linked points will be connected by at least two beam elements.


In the case of complex solids, it is interesting to mesh them finely from the beginning, and to let EUROPLEXUS compute the inetria tensor. The option VERIF is enough for that. For the real dynamic calculation, a coarser mesh (wireframe) will be sufficient, and one will then impose the previously found inertia tensor, by nmeans of the INER directive.


In the case that the solid is not meshed (directive "POIN"), all points of the list will be considered linked. The inertia tensor data is then useless.


Dimension sufficiently by means of directives "SOLI", "PLIE" and "PLIB" (page A.80).

4.36.1  INERTIA

D.215


Object:


This directive allows to specify inertia parameters for a non-deformable solid. It also allows to compute the inertia tensor starting from simple shapes.


Compatibility: COUP, LIAI


Syntax:

   "COMP"  ncomp*(    "INER"    "MASS"  m  ...
                  ... <"XG" xg>    <"YG" yg>    <"ZG" zg>   ...
                  ... <"IXX" ixx>  <"IYY" iyy>  <"IZZ" izz> ...
                  ... <"IXY" ixy>  <"IXZ" ixz>  <"IYZ" iyz> )


"COMP"

Announces that the inertia tensor is composed by assembly of simple tensors.
ncomp

Number of inertia tensors to be read in order to compute the inertia tensor of the composite solid.
"INER"

Announces the beginning of the data relative to an inertia tensor.
m

Mass of the isolated solid (without taking into account the added masses).
xg,yg,zg

Coordinates of the center of gravity of the solid isolated in the general reference frame (frame of the mesh).
ixx,iyy,izz

Diagonal elements of the inertia tensor of the isolated solid, in the general frame translated to the center of gravity of the solid.
ixy,iyz,ixz

Off-diagonal elements of the inertia tensor of the isolated solid, in the general frame translated to the center of gravity of the solid.

Comments:


If one single inertia tensor is given (ncomp = 1), the keywords < "COMP" ncomp > are optional. One may start directly by the keyword "INER".


If the "INER" directive is absent, the inertia values will be computed from the initial mesh and densities.


The inertia tensor has the followig form:

                      | ixx  ixy  ixz |
                      |               |
                   I= | ixy  iyy  iyz |
                      |               |
                      | ixz  iyz  izz |


If some parameters are not explicitly given, they are supposed to be zero by default.


In case of complex solids, it is interesting to discretise them finely, and let EUROPLEXUS compute the inertia tensor with high precision. When this operation is terminated, one can take a coarser mesh, by imposing the formerly obtained inertia terms. In this way, the output files will be smaller. But the precision of the calculation will ne the same.

4.37  ARTICULATION

D.220


Object:


This directive allows to link two sub-structures by meand of a kinematic relationship.


Compatibility: COUP, LIAI for VERR, ROTU, PIVO, GLIS, PIGL and DRIT


Compatibility: COUP for TGGR and CRGR


Syntax:

    "ARTI"
        |  "VERR"  ...    |
        |  "ROTU"  ...    |
        |  "PIVO"  ...    |
        |  "GLIS"  ...    |
        |  "PIGL"  ...    |
        |  "DRIT"  ...    |
        |  "TGGR"  ...    |
        |  "CRGR"  ...    |



Comments:


Articulations VERR, ROTU, PIVO, GLIS, PIGL and DRIT may only be defined by means of a mechanism element "MECA". It is therefore necessary that such elements be present in the mesh.


Articulations TGGR and CRGR may only be defined by means of a mechanism element "LIGR".


The linked sub-structures may be described as either non-deformable or deformable.


The various types of articulations are described in the following pages.

4.37.1  RIGID ARTICULATION (“VERROU”)

D.225


Object:


This directive allows to join two sub-structures by means of a blocked articulation, i.e. a rigid connection.


Compatibility: COUP, LIAI


Syntax:

    "VERR"  /LECTURE/  ...

            ... ( "NOEU" /LECTURE/  "VOIS" $[  "ABSENT"       ;
                                               "INDEF"  isol  ;
                                               /LECTURE/      ]$ )


"VERR" /LECTURE/

Number of the "MECA" element to be rigidly connected.
"NOEU" /LECTURE/

Number of the node of the "MECA" element to which the following neighbour will be associated.
"VOIS" "ABSENT"

There is no need to define a neighbour because the nodes of this sub-structure already have 6 d.o.f.s. The node of the mechanism is then sufficient.
"VOIS" "INDEF" isol

The neighbour is part of the non-deformable solid isol. The points resulting from the decomposition will be used. It seems that this directive cannot be used when the solid is defined by "POIN" (not meshed solid).
"VOIS" /LECTURE/

Number of the points forming the neighborhood (the point belonging to the mechanism must be excluded).

Comments:


The two sub-structures are rigidly connected. The six degrees of freedom are coupled on both parts of the mechanism.


The couple "NOEU" "VOIS" must be described twice, i.e. for each of the two points of the mechanism.

4.37.2  PIVOT

D.230


Object:


This option allows to link two sub-structures by a frictionless hinge.


Compatibility: COUP, LIAI


Syntax:

    "PIVOT" /LECTURE/    ...
            ...   "AXE"  "VX" vx  "VY" vy  "VZ" vz  ...

            ... ( "NOEU" /LECTURE/  "VOIS" $[  "ABSENT"       ;
                                               "INDEF"  isol  ;
                                               /LECTURE/      ]$ )


"PIVOT" /LECTURE/

Number of the "MECA" element of the hinge.
vx,vy,vz

Components of the initial direction of the hinge axis.
"NOEU" /LECTURE/

Number of the node of the "MECA" element to which the following neighborhood will be associated.
"VOIS" "ABSENT"

There is no need to define a neighborhood because the nodes of this sub-structure already possess 6 d.o.f.s. The first node of the mechanism is then sufficient.
"VOIS" "INDEF" isol

The neighbourhood is part of the non-deformable solid isol. The points resulting from the decomposition will then be used. It seems that this directive cannot be used when the solid is defined by "POIN" (not meshed solid).
"VOIS" /LECTURE/

Numbers of the points forming the neighbourhood (the point belonging to the mechanism must be excluded).

Comments:


The pivot axis is modified accounting for the motions of the sub-structures.


The pair "NOEU" "VOIS" must be described twice, once for each of the 2 points of the mechanism.


Special care must be taken for the neighborhood. In fact, these parts will be considered as rigid for the calculations of angular relations.

4.37.3  PIN JOINT (“ROTULE”)

D.240


Object:


This option allows to connect two sub-structures by a friction-less pin joint (“rotule”).


Compatibility: COUP, LIAI


Syntax:

    "ROTU"  /LECTURE/  ...

            ... ( "NOEU" /LECTURE/  "VOIS" $[  "ABSENT"       ;
                                               "INDEF"  isol  ;
                                               /LECTURE/      ]$ )


"ROTU" /LECTURE/

Number of the "MECA" element of the pin joint.
"NOEU" /LECTURE/

Number of the node of the "MECA" element to which the following neighborhood will be associated.
"VOIS" "ABSENT"

There is no need to define a neighborhood because the nodes of this sub-structure already possess 6 d.o.f.s. The first node of the mechanism is then sufficient.
"VOIS" "INDEF" isol

The neighbourhood is part of the non-deformable solid isol. The points resulting from the decomposition will then be used. It seems that this directive cannot be used when the solid is defined by "POIN" (not meshed solid).
"VOIS" /LECTURE/

Numbers of the points forming the neighbourhood (the point belonging to the mechanism must be excluded).

Comments:


The two sub-structures are linked in translation but free in rotation.


The pair "NOEU" "VOIS" must be described twice, once for each of the 2 points of the mechanism.

4.37.4  SLIDER (“GLISSIERE”)

D.250


Object:


This option allows to connect two sub-structures by a friction-less slider (“glissière”).


Compatibility: COUP, LIAI


Syntax:

    "GLIS"  /LECTURE/    ...
            ...   "AXE"  "VX" vx  "VY" vy  "VZ" vz  ...

            ... ( "NOEU" /LECTURE/  "VOIS" $[  "ABSENT"       ;
                                               "INDEF"  isol  ;
                                               /LECTURE/      ]$ )


"GLIS" /LECTURE/

Number of the "MECA" element of the pin joint.
vx,vy,vz

Components of the initial direction of the axis.
"NOEU" /LECTURE/

Number of the node of the "MECA" element to which the following neighborhood will be associated.
"VOIS" "ABSENT"

There is no need to define a neighborhood because the nodes of this sub-structure already possess 6 d.o.f.s. The first node of the mechanism is then sufficient.
"VOIS" "INDEF" isol

The neighbourhood is part of the non-deformable solid isol. The points resulting from the decomposition will then be used. It seems that this directive cannot be used when the solid is defined by "POIN" (not meshed solid).
"VOIS" /LECTURE/

Numbers of the points forming the neighbourhood (the point belonging to the mechanism must be excluded).

Comments:


The slider axis is modified to account for the motion of the sub-structures.


The pair "NOEU" "VOIS" must be described twice, once for each of the 2 points of the mechanism.


The axis defined by "AXE" is used only in case of a spring ("RESS") on the connection (to compute the forces coming from the spring) or in case of merging points of the MECA element. In general case, the sliding axis is defined by the two points of the MECA element (local axis of the element).

4.37.5  SLIDING PIVOT

D.255


Object:


This option allows to connect two sub-structures by a friction-less sliding pivot.


Compatibility: COUP, LIAI


Syntax:

    "PIGL"  /LECTURE/    ...
            ...   "AXE"  "VX" vx  "VY" vy  "VZ" vz  ...

            ... ( "NOEU" /LECTURE/  "VOIS" $[  "ABSENT"       ;
                                               "INDEF"  isol  ;
                                               /LECTURE/      ]$ )


"PIGL" /LECTURE/

Number of the "MECA" element of the sliding pivot.
vx,vy,vz

Components of the initial direction of the axis.
"NOEU" /LECTURE/

Number of the node of the "MECA" element to which the following neighborhood will be associated.
"VOIS" "ABSENT"

There is no need to define a neighborhood because the nodes of this sub-structure already possess 6 d.o.f.s. The first node of the mechanism is then sufficient.
"VOIS" "INDEF" isol

The neighbourhood is part of the non-deformable solid isol. The points resulting from the decomposition will then be used. It seems that this directive cannot be used when the solid is defined by "POIN" (not meshed solid).
"VOIS" /LECTURE/

Numbers of the points forming the neighbourhood (the point belonging to the mechanism must be excluded).

Comments:


The sliding pivot’s axis is modified to account for the motion of the sub-structures.


The pair "NOEU" "VOIS" must be described twice, once for each of the 2 points of the mechanism.


The rotational axis is supposed to be identical with the sliding axis. This single axis is defined with the "AXE" keyword. Nevertheless, for the sliding behavior, the axis defined by "AXE" is used only in case of a spring ("RESS") on the connection (to compute the forces coming from the spring) or in case of merging points of the MECA element. In general case, the sliding axis is defined by the two points of the MECA element (local axis of the element).

4.37.6  IMPOSED RELATIVE DISPLACEMENT - D.R.I.T.

D.260


Object:


This D.R.I.T. directive (Déplacement Relatif Imposé en fonction du Temps = Prescribed Time-dependent Relative Displacement) allows to link two sub-structures by an actuator (“vérin”) whose length is a prescribed time function.


Compatibility: LIAI


Syntax:

    "DRIT"  /LECTURE/    ...
            ...   "AMPLI"  ampli   "FONCTION" ifonc    ...

            ... ( "NOEU" /LECTURE/  "VOIS" $[  "ABSENT"       ;
                                               "INDEF"  isol  ;
                                               /LECTURE/      ]$ )


"DRIT" /LECTURE/

Number of the "MECA" element of the "DRIT" mechanism.
ampli

Amplification coefficient.
ifonc

Number of the function defined by the "FONCTION" directive (see page E.10).
"NOEU" /LECTURE/

Number of the node of the "MECA" element to which the following neighborhood will be associated.
"VOIS" "ABSENT"

There is no need to define a neighborhood because the nodes of this sub-structure already possess 6 d.o.f.s. The first node of the mechanism is then sufficient.
"VOIS" "INDEF" isol

The neighbourhood is part of the non-deformable solid isol. The points resultiong from the decomposition will then be used.
"VOIS" /LECTURE/

Numbers of the points forming the neighbourhood (the point belonging to the mechanism must be excluded).

Comments:


The relative displacement between the two nodes of the element is equal to the product ampli * F(ifonc,t).


The pair "NOEU" "VOIS" must be described twice, once for each of the 2 points of the mechanism.

4.37.7  TGGR

D.270


Object:


This option allows to link a node from a shell with a node from a beam. Both nodes are linked in translation. They can be connected in rotation around the axis "AXE1" and "AXE2" (local axis of the shell) by means of two springs ("MECA" "LIGR").


Not available with LIAI.


Syntax:

      "TGGR"  /LECTURE/    ...
          ...   "AXE1"  "VX" vx  "VY" vy  "VZ" vz  ...
          ...   "AXE2"  "VX" vx  "VY" vy  "VZ" vz  ...

          ... ( "NOGR" /LECTURE/  )


"TGGR" /LECTURE/

Number of the "LIGR" element.
"AXE1" vx,vy,vz

Components of the first vector (local axis of the shell).
"AXE2" vx,vy,vz

Components of the second vector (local axis of the shell).
"NOGR" /LECTURE/

Number of the node of the "LIGR" element which belong to the shell.

Comments:


The pivot axis "AXE1" and "AXE2" are modified accounting for the motions of the shell.

4.37.8  CRGR

D.275


Object:


This option allows to link a node from a shell with the beam’s node which is the closer. Both nodes are linked in translation in the plane defined by the vectors "AXE1" et "AXE2" and free in translation in the perpendicular direction of this plane. They can be connected in rotation around the axis "AXE1" and "AXE2" (local axis of the shell) by means of two springs ("MECA" "LIGR") (See C.965).


Not available with LIAI.


Syntax:

      "CRGR"  /LECTURE/    ...
          ...   "AXE1"  "VX" vx  "VY" vy  "VZ" vz  ...
          ...   "AXE2"  "VX" vx  "VY" vy  "VZ" vz  ...

          ... ( "NOGR" /LECTURE/  )
          ... ( "NOCR" /LECTURE/  )

          ... < "DMAX" dmax  >


"CRGR" /LECTURE/

Number of the "LIGR" element.
"AXE1" vx,vy,vz

Components of the first vector (local axis of the shell).
"AXE2" vx,vy,vz

Components of the second vector (local axis of the shell).
"NOGR" /LECTURE/

Number of the node of the "LIGR" element which belong to the shell.
"NOCR" /LECTURE/

List of the nodes of the "LIGR" element which belong to the beam and are candidates for the connection.
"DMAX" dmax

Optional : allows to introduce a test on the distance between both nodes of the connection. If the distance is superior to dmax then the connection is broken.

Comments:


The pivot axis "AXE1" and "AXE2" are modified accounting for the motions of the shell.


The relative perpendicular to the plan motion of the beam is free. The beam’s node considered in the link is modified accounting for the relative axial motion of the beam.

4.38  ROTATION

D.310


Object:


In the case of a rotating structure, this directive allows to define the symmetry condition with respect to a rotating plane, whose axis and rotation velocity are prescribed by the user.


This directive allows, for example, to model just one sector of a rotating disk instead of the whole disk.


Compatibility: COUP, LIAI


Syntax:

    "ROTATION"    "ORIG"   x0 y0  < z0 >
                < "VECT"   vx vy    vz >
                  "FONC"   ifonc
                  ...                           /LECTURE/


xo,yo,zo

Coordinates of the origin point (z0 is redundant in 2D).
vx,vy,vz

Components of the vector defining the rotation axis. These data are not necessary in 2D (see comments below).
ifonc

Number of the function defining the rotation velocity (in rad/s) as a function of time.
LECTURE

Numbers of the concerned nodes.

Comments:


This directive may be used at most once in a calculation.


The rotation axis is supposed fixed. The velocity of the rotation varies in time according to the user-specified function.


In 2D plane calculations, the rotation axis is normal to the plane xOy.

4.39  IMPOSED TIME-DEPENDENT ROTATIONAL MOTION

D.320


Object:


In the case of a rotating structure, this directive allows to impose a global motion of rotation to a set of nodes. The axis of rotation and the rotation velocity (as a function of time) are prescribed by the user.


Compatibility: COUP, LIAI


Syntax:

    "MENS"        "POINT"   x0 y0  < z0 >
                < "VECTEUR"   vx vy    vz >
                  "FONCTION"  ifonc
                  /LECTURE/


xo,yo,zo

Coordinates of the origin point (tail of the rotation axis). Note that z0 is redundant in 2D.
vx,vy,vz

Components of the vector defining the rotation axis. These data are not necessary in 2D (see comments below).
ifonc

Number of the function defining the rotation velocity (in rad/s) as a function of time.
LECTURE

Numbers of the concerned nodes.

Comments:


This directive may be used at most once in a calculation.


The rotation axis is supposed fixed. The velocity of rotation varies in time according to the user-specified function.


In 2D plane calculations, the rotation axis is normal to the plane xOy.


A time-limited version (TMEN) of the MENS directive, which acts only until a certain time and then is automatically removed, is also available, see Page D.321.

4.40  TIME-LIMITED IMPOSED ROTATIONAL MOTION

D.321


Object:


In the case of a rotating structure, this directive allows to impose a global motion of rotation to a set of nodes. The axis of rotation and the rotation velocity (as a function of time) are prescribed by the user. The rotation is imposed up to a prescribed time. After that time, the imposed condition is automatically removed.


Compatibility: COUP


Syntax:

    "TMEN"        "POINT"   x0 y0  < z0 >
                < "VECTEUR"   vx vy    vz >
                  "FONCTION"  ifonc
                  "UPTO"  t
                  /LECTURE/


xo,yo,zo

Coordinates of the origin point (tail of the rotation axis). Note that z0 is redundant in 2D.
vx,vy,vz

Components of the vector defining the rotation axis. These data are not necessary in 2D (see comments below).
ifonc

Number of the function defining the rotation velocity (in rad/s) as a function of time.
t

Time up to which the rotation is imposed. After this time, the rotation is automatically released.
LECTURE

Numbers of the concerned nodes.

Comments:


This directive may be used at most once in a calculation.


The rotation axis is supposed fixed. The velocity of rotation varies in time according to the user-specified function.


In 2D plane calculations, the rotation axis is normal to the plane xOy.

4.41  CONSTANT DISTANCE CONNECTION ("DIST")

D.322


Object:


Automatic prescription of the 3D mechanical relations between the translational degrees of freedom of a point with a set of points.


Compatibility: COUP, LIAI


Syntax:

    "DISTANCE"  /LECTURE/


/LECTURE/

Numbers of the two nodes (or name of the object) whose distance must be kept constant during the calculation.

4.42  BARYCENTRIC JUNCTION

D.325


Object:


Automatic prescription of mechanical relations (links) such that the displacement of a point equals the mean value of the displacements of a set of points, i.e. the displacement of the barycenter of the set of points (considered all with the same weight).


Compatibility: COUP, LIAI


Syntax:

    BARY  CENT /LECT/
          LIST /LECT/
         <VECT <VX vx> <VY vy> <VZ vz>>


CENT /LECT/

Number of the node (or name of the object) corresponding to the “central” (or reference) node. This node may be located anywhere and does not need to be at (or close to) the true center of the following points set.
LIST /LECT/

Numbers of the nodes (or name of the object) corresponding to the set of nodes, whose mean displacement will be identical to that of the reference node.
VECT

Introduces the optional definition of a direction (vector) along which the constraint will act. By default, the constraint acts along all space directions.
VX, VY, VZ

Introduce the optional components of the vector vx, vy, vz. By default, they are zero. At least one non-zero component must be specified. The vz component may only be specified in 3D. Note that only the direction, not the norm, of the vector counts. The vector is always normalized to unit length internally.

Comments:

By default (no VECT specified) this directive imposes the following (vectorial) condition on nodal velocities v:

v
C − (
v
1 + 
v
2 + ⋯ + 
v
N) / N = 
0
 

which corresponds to the following 2 or 3 scalar independent links:

vCx − (v1x + v2x + ⋯ + vNx) / N = 0 
vCy − (v1y + v2y + ⋯ + vNy) / N = 0 
vCz − (v1z + v2z + ⋯ + vNz) / N = 0    (3D  only

where C is the “central” node defined by CENT and 1, 2, ⋯ , N are the N nodes defined by LIST.


When a vector V is specified by VECT, then the following single condition on nodal velocities is imposed:

v
C · 
V
 − 
1
N
(
v
1 − 
v
2 − ⋯ − 
v
N) · 
V
 = 
0
 

which corresponds to the following scalar link (assuming a 2D case):

vCxVx + vCyVy − 
1
N
 (v1xVx + v1yVy + ⋯ + vNxVx + vNyVy) = 0 


Note that the above conditions, both without and with the definition of a vector VECT, do not strictly ensure that the displacements of all nodes in the set will be all equal among them. To obtain this effect, use the RIGI link, see page D.326.

4.43  RIGID JUNCTION

D.326


Object:


Automatic prescription of mechanical relations (links) such that the displacement of each point in a certain set of points equals the displacement of a reference point, like if all these points were all rigidly connected among them.


Compatibility: COUP, LIAI


Syntax:

    RIGI  CENT /LECT/
          LIST /LECT/
         <VECT <VX vx> <VY vy> <VZ vz>>


CENT /LECT/

Number of the node (or name of the object) corresponding to the “central” or reference node. This node may be located anywhere and does not need to be at (or close to) the true center of the following points set.
LIST /LECT/

Numbers of the nodes (or name of the object) corresponding to the set of nodes, whose displacement will be identical to that of the reference node.
VECT

Introduces the optional definition of a direction (vector) along which the constraint will act. By default, the constraint acts along all space directions.
VX, VY, VZ

Introduce the optional components of the vector vx, vy, vz. By default, they are zero. At least one non-zero component must be specified. The vz component may only be specified in 3D. Note that only the direction, not the norm, of the vector counts. The vector is always normalized to unit length internally.

Comments:

By default (no VECT specified) this directive imposes the following set of N (vectorial) conditions on nodal velocities v:

v
C − 
v
1 = 
0
 
v
C − 
v
2 = 
0
 
⋯ 
v
C − 
v
N = 
0
 

which corresponds to the following 2N or 3N scalar independent links:

vCx − v1x = 0 
vCy − v1y = 0 
vCz − v1z = 0    (3D  only
⋯ 
vCx − vNx = 0 
vCy − vNy = 0 
vCz − vNz = 0    (3D  only

where C is the “central” node defined by CENT and 1, 2, ⋯ , N are the N nodes defined by LIST.


When a vector V is specified by VECT, then the following N conditions on nodal velocities are imposed:

v
C · 
V
 −
v
1 · 
V
 = 
0
 
v
C · 
V
 −
v
2 · 
V
 = 
0
 
⋯ 
v
C · 
V
 −
v
N · 
V
 = 
0
 

which correspond to the following N scalar links (assuming a 2D case):

vCxVx + vCyVy − v1xVx − v1yVy = 0 
vCxVx + vCyVy − v2xVx − v2yVy = 0 
⋯ 
vCxVx + vCyVy − vNxVx − vNyVy = 0 

4.44  CONTACTS DEFINED BY SPLINE FUNCTIONS

D.330


Object:


In the case of a rotating structure, this directive allows to define the possible contacts between the rotationg parts (blades) with the fixed wall (carter). The geometrical forms of these parts are defined by means of spline functions starting from the positions of mesh nodes. This interpolation allows thus to approximate the real geometry of such structures.


Compatibility: LIAI


Syntax:

    "SPLINE"
    nspline * (      "SURFACE"   /LECTURE/     ...
                ...  "COURBE"  ncourbe * ( "LIGNE" /LECTURE/ )     ...
                ...  "METC"  metc   "METS"  mets   "NPTT"  nptt    ...
                ...  "DEGC"  degc   "DGST"  dgst   "DGSZ"  dgsz    ...
                ...  "EPAIS" epais  "FREQ"  freq                       )


nspline

Number of splines.
SURFACE

Defines the nodes forming the surface. This surface MUST be a cylinder,
ncourbe

Number of curves that may get in contact with the surface.
LIGNE

Introduces the nodes that compose a curve. The user must enter these nodes in the order of their position along the curve.
metc

Method for the modelisation of the curve (see comments below).
mets

Method for the modelisation of the surface (see comments below).
nptt

Number of nodes of the surface lying on the same circumference.
degc

Degree for the modelisation of the curve.
dgst

Degree for the modelisation of the surface, circumferential direction.
dgst

Degree for the modelisation of the surface, axial direction Oz.
epais

Thickness of the shell elements composing the surface.
freq

Frequency of the updationg of surface nodes.

Comments:


The methods for the modelisation (of the curve and of the surface along the circumferential and axial directions) may assume the values: 1 (direct), 2 (interpolation) or 3 (smoothing by least squares).


The surface MUST be a cylinder of axis Oz. Furthermore, the nodes composing it must be regularly spaced.

4.45  COLLISIONS

D.400


Object :

This directive allows to simulate the contact and/or shock without friction between the envelopes of 3D rigid bodies.


Compatibility: LIAI


Syntax :

      "COLL"    "REST"  crest    "SGEO"  tolgeo    "SVIT"  tolvit
              ( "CHAI"
                   ( "SOLI"  nusoli
                          "SURF"  /LECTURE/
                          "EPAI"  epais
                          "ORIE"  xp  yp  zp       )     )
           "CONT"
              ( "CHA1"  nucha1    "CHA2"  nucha2   )
           "FCON"


COLL

This keyword announces the data relative to collisions.
crest

Energy restitution coefficient.
tolgeo

Geometric tolerance of the contact.
tolvit

Kinematic tolerance of the contact.
CHAI

This keyword announces the data relative to a chain.
SOLI

This keyword announces the data relative to one of the solids that define the chain.
nusoli

Number of the solid associated to the chain. This number corresponds to the order under which the solid has been listed under the sub-directive "SOLIDE" of the directive "LIAISON".
/LECTURE/

Reading procedure of the triangular elements defining the envelope of the chain, i.e. the contact surfaces.
epais

Thickness of the contact surfaces.
xp, yp, zp

Coordinates of a point interior to the envelope, used to define the orientation of the triangular elements.
CONT

This keyword allows to introduce the list of pairs of chains for which contact may take place.
nucha1

Number of the first chain of the pair.
nucha2

Number of the second chain of the pair.
FCON

This keyword announces the end of the collisions data.

Warning :

It is mandatory:

- to mesh the surfaces by triangular elements;

- to declare these elements as “phantoms” by directive "MATE",

- to define the data block "SOLIDE" before the block "COLLISIONS",

- to specify in "DIME" the dimensioning parameter:

        "CSCO" nbpcon


With:

nbpcon

Maximum number of contact points.

Comments :

The coefficient of energy restitution is between 0 and 1. For crest = 0, one obtains a perfectly soft shock, while for crest = 1 one gets a perfectly elastic shock (the energy is conserved).


The thickness of surfaces must be of the order of the size of elements at most. If this value is too small, it is possible that the interpenetration of the two surfaces will not be detected.


The contact geometric tolerance determines the distance starting from which one considers that there is contact.


The kinematic tolerance must be of the order of the time step. The larger this tolerance, the more the discontinuity at the velocity level due to a shock is ignored.


If a contact surface is fixed (instead of being defined via a rigid body), it is sufficient to declare nusoli = 0. In this case it is redundant to block the concerned nodes, since it is done automatically by the code.


References :

For further information, please consult the reference [].

4.46  FLUID-STRUCTURE SLIDING OF THE ALE TYPE (FSA)

D.450


Object:


To define fluid-structure sliding of the ALE type according to the FSA model developed at JRC Ispra.


The program writes for each node subjected to this type of sliding a ‘liaison’ that forces the fluid (slave) velocity to be equal to the structure (master) velocity along the normal to the FS interface. In the tangent direction (tangent plane in 3D), the fluid velocity is free.


In the case of a curved interface, the normal direction is determined at each step by taking into account all the element faces that lie along the fluid-structure boundary and include the node under consideration (influence domain) and by imposing that the net flux of mass out of some faces be balanced by the flux entering the other faces.


Since the geometry varies in time, the coefficients of the liaison have to be recalculated and the matrix inverted at each step.


The nodes declared in this directive should be fluid nodes and be declared as Eulerian in the GRIL directive. The program then automatically searches for each slave node a corresponding master node: this is defined as the Lagrangian node having the same coordinates as the slave node (within a small tolerance) and if it exists (nodally conforming FS interface), it must be unique. Usually this will be a structural node, but it could be also a fluid (Lagrangian) node, in case the sliding takes place along a fluid-fluid interface.


If no such node exists, then the FS interface is nodally non-conforming and the program searches a Lagrangian master face on which the slave fluid node lies. The motion of the fluid node is automatically set so as to follow the motion of the master face.


Note that the treatment of non-conforming FS interfaces requires a special optional keyword (NCFS) to be explicitly chosen by the user. If this keyword is not specified and a non-conforming node is found, then an error message is issued and the calculation is stopped. This is to make sure that the user intentionally wanted to specify a non-conforming interface and there was not just an error in mesh specification.


Compatibility: COUP, LIAI


Syntax:

    "FSA" <"STRU" /LECT_STRU/> <"NCFS"> /LECTURE/


STRU /LECT_STRU/

Optional sub-directive used to tell the code in which object (/LECT_STRU/) it should search to determine the “structural” (i.e. the Lagrangian) nodes corresponding to the FSA fluid nodes that will be specified in the final /LECTURE/. By default, the search is extended to the whole mesh.
NCFS

The FS interface may contain non-conforming fluid nodes.
/LECTURE/

List of fluid (slave) nodes subjected to FSA sliding.

Comments:


The fluid nodes subjected to FSA sliding should preferably be declared Eulerian in the grid movement directive (GRILL). The program will automatically consider these nodes as manually rezoned when it encounters the LIAI FSA directive. The user might also declare these nodes as automatically rezoned in GRILL (e.g., as a consequence of an AUTO AUTR directive), with no effect on the results, but in this case the dimensioning for automatically rezoned nodes (DIME NBLE) should include these nodes, although this is not necessary for the actual computation.


Beware that the behaviour of the FSA algorithm may be modified by setting appropriate options, see page H.120. In particular, the FSCR option activates the correction of normals based on equilibrium considerations (FSCR algorithm).


Occasionally, the automatic search for the master node corresponding to a slave node might fail. The code then reports the concerned node number by an appropriate error message. This may happen because either the code finds zero nodes, or it finds more than one Lagrangian nodes matching the slave node.

In the first case, the tolerance for node matching determination might be too small, e.g. due to the fact that mesh coordinates are generated by an external, and not too precise, mesh generator. The user may adjust this tolerance, see OPTI TOLC on page H.40.

The second case may occur for example when there are superposed structures (coincident nodes) in the initial mesh. In such cases, there are two possibilities. Either the user specifies the required nodes correspondence by the COMP CNOD directive, see page C.92, but this is only practical if there are just a few of these nodes. Or, the user specifies the STRU /LECT_STRU/ optional sub-directive, so that the search for matching structural (more precisely, Lagrangian) nodes is confined to the specified object /LECT_STRU/ rather than to the whole mesh. This is the method of choice e.g. in case a large shell structure is subjected to FSA on one side, and to Lagrangian sliding (say, by GLIS) on the other side, so that the number of “superposed” structural nodes is potentially large.

4.47  RIGID-BOUNDARY/FLUID SLIDING OF THE ALE TYPE

D.460


Object:


To simplify the description of fluid sliding along inviscid, rigid boundaries. The simplification lies in the fact that the program automatically computes the correct sliding conditions, in particular the normal (or possibly the 2 normals, in 3D cases) to the rigid boundary and automatically prescribes the relevant "connections" (liaisons).


For complex geometric shapes this is very convenient with respect to the "manual" prescription of all such connections.


This condition is similar to the "FSA" condition, but with the following differences:


- Since the boundary is rigid, there is no need to represent it by a structure. The sliding condition therefore involves only a fluid node.


- The geometry of the boundary does not vary in time, therefore the coefficients of the liaison are constant and do not need to be recalculated during the transient.


- The program does not search for a Lagrangian node having the same coordinates as the fluid node.


The nodes declared in this directive (/LECT/) should all be fluid nodes and be declared as Eulerian in the GRIL directive.


Compatibility: COUP, LIAI


Syntax:

    "FSR"  /LECTURE/


/LECTURE/

List of fluid nodes subjected to FSR sliding.

Comments:


The fluid nodes subjected to FSR sliding should preferably be declared Eulerian in the grid movement directive (GRILLE). The program will automatically consider these nodes as Eulerian when it encounters the LIAI FSR directive. The user might also declare these nodes as automatically rezoned in GRILLE (e.g., as a consequence of an AUTO AUTR directive), with no effect on the results, but in this case the dimensioning for automatically rezoned nodes (DIME NBLE) should include these nodes, although this is not necessary for the actual computation.

4.48  IMPACT/CONTACT BY THE PINBALL MODEL (PINB)

D.480


Object:


The purpose is to define impact and contact conditions between Lagrangian subdomains (typically two or more solid bodies) by means of the “pinball” model. The model is inspired to a formulation proposed by Belytschko and co-workers in the papers: (i) Ted Belytschko and Mark O. Neal, “Contact-Impact by the Pinball Algorithm with Penalty and Lagrangian Methods”, Int. J. Num. Meths. Eng., Vol. 31, pp. 547-572 (1991), and (ii) T. Belytschko and I.S. Yeh, “The splitting pinball method for contact-impact problems”, CMAME, 105, pp. 375-393, (1993).


The user defines the elements that may enter in contact with one another and a pinball (a sphere or circle) is associated to these elements. Interpenetration is detected by comparing the distance of the centers of two pinballs with the sum of their radii. If this condition is satisfied, equal normal velocity is enforced by the method of Lagrange multipliers and the corresponding contact forces are computed.


Optionally, contact may be verified on a hierarchy of “descendent” pinballs derived from the “parent” pinballs described above by recursively halving the pinball dimensions. This allows finer spatial resolution of the contact conditions.


The uncoupled version of the pinball algorithm (DECO keyword) uses a penalty method instead of (coupled) Lagrange multipliers.


Compatibility: COUP, DECO, LIAI


Syntax:

     PINB $[ PENA <SFAC sfac> ]$
          (  $[BODY ; SELF]$
            < "FROT" "MUST" must "MUDY" mudy "GAMM" gamm >
            < $[DMIN dmin ;
                MLEV mlev ;
                DIAM diam < ADAD < UPTO lmax > >
                          < ADNP < UPTO lmax > > ]$ >
            < HARD hard >
            /LECT/ )
          < EXCL (PAIR n1 n2) >
          < ADAP LMAX lmax <SCAL scal> <SCAS scas> <NOUN> >


The input consistes of several parts. The first part is related to the chosen solution method. If LINK COUP or LIAI has been chosen, then this part may be skipped. If LINK DECO has been chosen, this part is mandatory.

PENA

DECO only: mandatory keyword (ignored with COUP or LIAI), must immediately follow the PINB keyword and indicates that a penalty method is used.
SFAC sfac

DECO only: optional scaling coefficient φ for the automatic determination of the contact stiffness (see Comments below). By default it is 1.0.

Next, comes the description of the bodies in contact, or more precisely the description of pinball sets to be embedded in the contacting bodies. The BODY or SELF (in order to activale self-contact) sub-directives should be repeated as many times as necessary to define all the contacting pinball sets.

BODY

Introduces the declaration of a set of pinballs that form one of the bodies that may come in contact with other bodies. There may not be contact between pinballs belonging to the same body.
SELF

Introduces the declaration of a set of pinballs that form one of the bodies that may come in contact with other bodies. In this case, there may be contact between different pinballs belonging to this body (this model is called self-contact or auto-contact).

The next sub-block of data concerns the optional definition of friction characteristics of the body (i.e. of the pinballs set).

FROT

Introduces the specification of (optional) friction characteristics for the current contacting body. A simple Coulomb dry friction model is assumed.
MUST must

Specifies the limiting friction coefficient for the static case µS. This is the value assumed when no sliding occurs between the contacting surfaces. It must be (0 ≤ µS < 1).
MUDY mudy

Specifies the friction coefficient for the dynamic (or kinetic) case µK. This is the (asymptotic) value assumed at very large (infinite) relative velocity of the contacting surfaces. It must be (0 ≤ µK ≤ µS < 1).
GAMM gamm

Parameter (γ) of the law of variation of the friction coefficient (µ) with the relative tangential sliding velocity (vr) of the contacting surfaces. The friction coefficient µ varies from µS to µK as the relative tangential velocity vr of the two bodies increases. The transition is governed by the exponential decay law: µ = µK + (µS − µK)e−γ |vr|.

The following sub-block of data basically defines the size of the pinballs belonging to the current body (i.e. of the current pinballs set). Three alternatives are possible: choosing the minimum diameter, choosing the maximum refinement level, or choosing a fixed diameter. In the latter case, only one pinball per element is ever generated.

DMIN dmin

Minimum diameter of descendent pinballs that will be generated from the set being declared. By default, this value is 0 for continuum elements (the size is then governed by mlev, see below), or it is the element thickness for beam or shell elements. For the choice of DMIN in adaptive calculations see the ADAP keyword below and the comments at the end of this page. Note that a modification in the effects of DMIN has been introduced recently. Thus, in order to repeat an old calculation which uses DMIN made with EPX version 3208 of 20 February 2017 or earlier, one should divide the old input value of DMIN by two, in order to obtain “exactly” the same results as previously (in the rare cases where this might have an importance).
MLEV mlev

Maximum hierarchy level for descendent pinballs that will be generated from the set being declared. The value 0 means that no descendents are generated (contact forces are computed based on interpenetration between parent or 0-level pinballs). The pinball radius is roughly divided by two at each new level produced. If specified, mlev must be greater or equal to 0. If not specified, mlev has to be computed. If dmin (dmin) is given, then the maximum level is computed such that the minimum pinball diameter is of the order of dmin. More precisely, the (0-level) pinball diameter is repeatedly halved until the result dmineff is equal to or less than twice the chosen value dmin. This algorithm guarantees that 2dmindmineff>dmin. If dmin is not given, for beam/shell elements mlev is computed by repeated halvings such that the minimum pinball diameter is of the order of (more precisely: equal to or less than) twice the element thickness h, that is: 2hdmineff>h. For continuum elements and for other element types, the default mlev value is 0. For the choice of MLEV in adaptive calculations see the ADAP keyword below and the comments at the end of this page.
DIAM diam

Fixed pinball diameter, typically to be associated with elements of the material-point type (PMAT). These elements have just one node and thus their pinball radius may not be computed by the code but must be provided by the user. In special cases this keyword can be used to assign a chosen pinball diameter also to elements not of the material point type, e.g. continuum elements. By default, the pinball diameter is never updated during the transient calculation even though the associated element undergoes large deformations, unless the UPDR option is specified. So make sure not to specify the UPDR option if you want the imposed pinball diameter to stay constant. When diam is specified, dmin may not be specified and mlev must be 0 (i.e., either unspecified, or specified to be 0). This means that no hierarchic pinballs are generated when diam is specified, i.e. only one pinball of the chosen diameter is associated with each element of the body. The pinball is placed at the centroid of the element. For the choice of DIAM in adaptive calculations see the ADAP keyword below and the comments at the end of this page.
ADAD

Adapt the diameter chosen by DIAM. Specifying this optional keyword (after choosing a diameter D by the DIAM command) adapts the diameter of pinballs associated with descendents of the elements in the current body, when such elements are refined by adaptivity. That is, first-generation descendents receive one pinball each (no hierarchy is possible with DIAM) with a diameter one half of the ancestor’s diameter (i.e. D/2), second-generation descendents get a diameter D/4 and so on. The default behaviour when DIAM is set but ADAD is not activated, is that in case of adaptive refinement of the body’s elements, the diameter of the newly generated pinballs (one per element) is constant and equal to D. The default rule seems appropriate, for example, if the body is a thin plate discretized by shells and for which a DIAM is chosen (as an alternative to other possible pinball strategies, such as hierarchic pinballs for example). In such a case one probably wants the diameter of pinballs to be equal to the thickness of the plate and to remain constant along with mesh adaptive refinement. In other applications, however, one may prefer that the imposed-diameter pinballs be scaled down as the mesh is refined, and this is the purpose of the ADAD keyword.
UPTO lmax

Limit the diameter adaptation mechanism activated by the ADAD keyword up to level lmax of the hierarchy. By default, adaptation is performed at all levels when ADAD is specified. This optional keyword can be used to avoid obtaining too small diameter pinballs in cases with deep mesh refinement (large hierarchy levels).
ADNP

Adapt nodal pinballs (more precisely: propagate nodal pinballs in adaptivity). This optional keyword has only effect if the pinballs of the current body are so-called nodal pinballs, and is ignored otherwise. So-called nodal pinballs are pinballs associated with material point elemengts (PMAT) attached (as typically mass-less geometrical supports) to the nodes of a body which is discretized by continuum or structural elements. They are not real nodal pinballs (directly associated with the nodes), because in the current implementation each pinball always requires an associated element. When the elements of the body are refined due to adaptivity, new nodes are created. By default, i.e. without specifying the ADNP optional keyword, no new pinballs would be created, because technically it is the continuum or structural elements which are refined and not the PMAT material point elements. By activating ADNP, each newly created node will receive a (new) PMAT element with an associated pinball. Note that the diameter of the newly created pinballs will be scaled or not, depending on the setting or not of the ADAD optional keyword described above for the current body.
UPTO lmax

Limit the pinball propagation mechanism activated by the ADNP keyword up to level lmax of the hierarchy. By default, propagation is performed at all levels when ADNP is specified. This optional keyword can be used to avoid obtaining too many (descendant) pseudo-nodal pinballs in cases with deep mesh refinement (large hierarchy levels).

Next comes an optional definition of some additional parameters (hardness) and the list of the elements forming the current body, i.e. the elements into which the pinballs of the current set should be embedded. This completes the definition of the current set of pinballs.

HARD hard

Optional “hardness’ value to be associated with the body. This information is only used in conjunction with options OPTI PINS MASL or OPTI PINS MAS2, see page H.160, in order to eliminate constraints in multiple flat contact situations. Values of hardness are arbitrary. The only important thing is the relative value of hardness of two bodies that come into flat contact. The body with lower hardness behaves like a “slave”, and the other one as a “master”. It is advised to use simple integer values, e.g. 1, 2, 3 etc.
/LECT/

List of the elements that will be associated with a (parent or 0-level) pinball of the set being described. For continuum-like bodies, these should typically contain only those elements along the body surface which are likely to come in contact with other objects.

Having defined all the pinball sets, next comes an optional definition of pairs of sets that should be excluded from contact. By default, the pinballs of each set are checked for contact against all pinballs of any other set (or even with pinballs of the same set if the SELF keyword has been used to define the current set). Occasionally, the user may want to disable some of these contacts.

EXCL

Introduces a list of body pairs to be excluded from contact search.
PAIR n1 n2

The body pairs of indexes n1 and n2 (in the bodies list declared above) are to be excluded from contact search.

The last part of the input is also optional and concerns the activation of contact-driven mesh adaptivity.

ADAP

Activates contact-driven mesh adaptivity, i.e. automatic refinement and un-refinement of the mesh elements containing pinballs, based on contact detection (and on contact anticipation). Note that this type of mesh adaptivity is at the moment incompatible with other types of adaptivity such as those activated by the WAVE or INDI directives.
LMAX lmax

Introduces lmax, the desired maximum adaptive refinement level Lmax of the structure mesh (elements) in the vicinity of contacting surfaces. This value should be greater than 1, since level 1 is attributed to the base mesh (no refinement). Each level corresponds to a halving of the mesh size with respect to the immediately previous level. The element level should not be confused with the pinball level, see details in the comments below.
SCAL scal

Introduces scal, an optional scaling factor φn to be used in the determination of elements to be refined belonging to non self-contacting bodies. By default φn=1.0. When scaling the structural influence domain by successive powers of two in order to identify, at each refinement level, the structure elements to be refined or un-refined, the code finally multiplies the result by this factor. Using a value of φn greater than one, e.g. 1.5 or 2, correspondingly enlarges the zone of structure mesh which is refined and this may result in a smoother mesh transition (for example, as an alternative to the option OPTI ADAP RCON).
SCAS scas

Introduces scas, an optional scaling factor φs to be used in the determination of elements to be refined belonging to self-contacting bodies. By default φs=0.55. The use of values of φs lower than 1.0 is necessary in self-contacting bodies in order to avoid a so-called chain reaction, i.e. immediate and uniform refinement of all the elements belonging to the self-contacting body up to the maximum chosen level. Theoretical values of φs can be determined for regular meshes made of continuum elements (see Table in the comments below), but not so easily for other cases. In practice, some experimentation is needed.
NOUN

When this optional keyword is specified, no element unsplitting is performed by the contact-driven adaptivity algorithm. That is, the mesh is refined near the contacting surfaces, but never unrefined.

This completes the definition of the input data.


Choice of the scaling factor for self-contacting bodies

The theoretical maximum scaling factors to be used for self-contacting bodies are shown in the following Table.


CaseEncompassing pinballsEquivalent pinballs
2D continuum (squares)2/2=0.707π/2=0.886
3D continuum (cubes)1/√3=0.577π/6=0.806
Table 3: Maximum scaling factor φmax for self-contact in 2D and 3D regular continuum meshes.


Comments:


By default, each pinball (belonging to a certain body) is checked for contact with any other pinball belonging to a different body. If the current pinball’s body is declared by the SELF keyword rather than BODY, then the pinball is checked for contact with any other pinball (including those belonging to the same body). A list of non-contacting body pairs can be optionally declared by the EXCL keyword.


For example, assume we have the following input:

   PINB ... BODY ... /LECT1/ ! first body
            SELF ... /LECT2/ ! second body, is self-contacting
            BODY ... /LECT3/ ! third body
            EXCL PAIR 2 3

Then, the pinballs in the first body interact with those of the other two bodies, the pinballs of the second body interact with those of the first and second body, while the pinballs of the third body interact with those of the first body.


The exclusion mechanism can be useful, e.g., in the presence of contact on both sides of a (thin) shell, say a thin reservoir filled of liquid, which is impacted externally by a projectile The user may want to specify that the shell is in contact both with the liquid (internally) and with the projectile (externally), but direct contact between the projectile and the liquid may not occur.


Be sure to consult also the options related to the pinball model in Section H, see Page H.160, and the interactive commands for the visualization of pinballs and of contacts, see Pages A.25 and O.10.


When using penalty method to compute contact forces, contact stiffness is computed automatically from the stiffness of master elements using the following formulae:

k = φ
GS2
V


in the case of solid master elements, with :

φ : optional scaling coefficient sfac given in input. By default φ=1.

G : bulk modulus of master element’s material,

S : area of contacting face,

V : volume of master element.

k = φ
GS
L


in the case of shell master elements, with :

φ : optional scaling coefficient sfac given in input. By default φ=1.

G : bulk modulus of master element’s material,

S : area of master element,

L : maximum length of master element’s edges.

The bulk modulus G of the material is:

G = 
E
3(1+ν)

where:

E : Young’s modulus of master element’s material,

ν : Poisson’s coefficient of master element’s material.


Distinction between element level and pinball level

Note that the above value of Lmax refers to the maximum refinement level of the elements (adaptivity) Lmaxadap, and not of the pinballs (contact) Lmaxpinb. This distinction is unfortunate and is only needed due to historical reasons: the pinball models was developed and implemented in EPX long before the adaptivity model. The relation between the levels is as follows: a base (not refined) element in adaptivity has by convention Ladap=1, while a base (parent) pinball in the contact model has by convention Lpinb=0. Thus, it should be kept in mind that:

Ladap=Lpinb+1

It seems preferable and more consistent with other adaptivity directives of EPX to use the LMAX keyword in the PINB ... ADAP directive to define Lmaxadap rather than Lmaxpinb. In any case, it should be rarely necessary to use a hierarchic pinball method in combination with contact-driven adaptivity, so the level of the generated pinballs (attached to the smaller and smaller elements) will be zero, and the user can safely ignore this.


References

Examples of application of the contact model by the pinball method are presented in the following papers: [].

4.49  CONTACT/IMPACT BY THE GENERALIZED PINBALL MODEL (GPIN)

D.490


Warning:

The present directive is currently still under implementation and validation. It may not be used yet for production runs. It is possible that not all keywords listed below be implemented yet.


Object:


The purpose is to define contact and impact conditions between Lagrangian subdomains (typically two or more solid bodies) by means of a variant of the “pinball” model, called “generalized pinballs” method. The model is inspired to the original pinball formulation proposed by Belytschko and co-workers in the papers: (i) Ted Belytschko and Mark O. Neal, “Contact-Impact by the Pinball Algorithm with Penalty and Lagrangian Methods”, Int. J. Num. Meths. Eng., Vol. 31, pp. 547-572 (1991), and (ii) T. Belytschko and I.S. Yeh, “The splitting pinball method for contact-impact problems”, CMAME, 105, pp. 375-393, (1993). However, generalized pinballs (GPINs) are not only spherical, but may assume other shapes (rectangles in 2D, cylinders, triangular prisms and hexahedra in 3D).


The user defines the elements that may enter in contact with one another and GPINs of the appropriate shapes are automatically associated with (typically the surface of) these elements. Interpenetration is detected by checking couples of GPINs. If this condition is satisfied, equal normal velocity is enforced by the method of Lagrange multipliers and the corresponding contact forces are computed.


Unlike the standard pinball model (PINB, see page D.480), the generalized pinball model does not admit (and does not need) hierarchical pinballs.


The uncoupled version of the generalized pinball algorithm (DECO keyword) uses a penalty method instead of (coupled) Lagrange multipliers.


Compatibility: COUP, DECO.


Syntax:

    "GPIN" $[ "PENA" <"SFAC" sfac> ]$
              ( $[ "BODY" ; "SELF" ]$
                  < "FROT" "MUST" must "MUDY" mudy "GAMM" gamm >
                /LECT/ )
              ( "DIAM" diam /LECT/ )
           < "EXCL" ("PAIR" n1 n2) >


PENA

DECO only: mandatory keyword (ignored with COUP), must immediately follow the GPIN keyword and indicates that a penalty method is used.
sfac

DECO only: optional coefficient φ for the automatic determination of the contact stiffness (see comments below). By default it is 1.0.
BODY

Introduces the declaration of a set of generalized pinballs (GPINs) that form one of the bodies that may come in contact with other bodies. There may not be contact between GPINs belonging to the same body. Some restrictions apply to the elements that can be declared, see the comments below.
SELF

Introduces the declaration of a set of GPINs that form one of the bodies that may come in contact with other bodies. In this case, there may be contact between different GPINs belonging to this body (this model is called self-contact or auto-contact). Some restrictions apply to the elements that can be declared, see the comments below.
FROT

Introduces the specification of (optional) friction characteristics for the current contacting body. A simple Coulomb dry friction model is assumed.
MUST

Specifies the limiting friction coefficient for the static case µS. This is the value assumed when no sliding occurs between the contacting surfaces. It must be (0 ≤ µS < 1).
MUDY

Specifies the friction coefficient for the dynamic (or kinetic) case µK. This is the (asymptotic) value assumed at very large (infinite) relative velocity of the contacting surfaces. It must be (0 ≤ µK ≤ µS < 1).
GAMM

Parameter (γ) of the law of variation of the friction coefficient (µ) with the relative tangential sliding velocity (vr) of the contacting surfaces. The friction coefficient µ varies from µS to µK as the relative tangential velocity vr of the two bodies increases. The transition is governed by the exponential decay law: µ = µK + (µS − µK)e(−γ |vr|).
/LECT/

List of the elements whose nodes (and then faces) will be associated with GPINs of the set being described.
DIAM

Introduces the declaration of a “contact diameter” to be associated with the nodes specified next. The nodes specified must be a sub-set of the nodes belonging to the elements listed in the previous BODY or SELF declarations. Some restrictions apply to the nodes that can be declared, see the comments below.
diam

Generalized pinball diameter (contact diameter) to be associated with P-GPINs attached to the nodes specified by the following /LECT/.
/LECT/

List of the nodes concerned.
EXCL

Introduces a list of body pairs to be excluded from contact search.
PAIR n1 n2

The body pairs of indexes n1 and n2 (in the bodies list declared above) are to be excluded from contact search.

Comments:


A point GPIN (P-GPIN) is associated to each node to which a contact diameter has been assigned via the DIAM directive. Then, the other GPIN types (L-GPINs in 2D, or L/T/Q-GPINs in 3D) are built for each element face whose nodes have all received a contact diameter.


The following restrictions apply to the elements that are declared in the BODY (or SELF) directive, and to the nodes that are declared in the DIAM directive described above:

Since a P-GPIN is attached to each such node, and this P-GPIN (like any other GPIN) must have one and only one associated body index, for obvious reasons, it follows that:


By default, each GPIN (belonging to a certain body) is checked for contact with any other GPIN (of suitable type) belonging to a different body. If the current GPIN’s body is declared by the SELF keyword rather than BODY, then the GPIN is checked for contact with any other GPIN of suitable type (including those belonging to the same body). A list of non-contacting body pairs can be optionally declared by the EXCL keyword.


For example, assume we have the following input:

   GPIN ... BODY ... /LECT1/ ! first body
            SELF ... /LECT2/ ! second body, is self-contacting
            BODY ... /LECT3/ ! third body
            DIAM ... /LECT123/ ! same diameter at all nodes
            EXCL PAIR 2 3

Then, the GPINs in the first body interact with those of the other two bodies, the GPINs of the second body interact with those of the first and second body, while the GPINs of the third body interact with those of the first body.


The exclusion mechanism can be useful, e.g., in the presence of contact on both sides of a (thin) shell, say a thin reservoir filled of liquid, which is impacted externally by a projectile The user may want to specify that the shell is in contact both with the liquid (internally) and with the projectile (externally), but direct contact between the projectile and the liquid may not occur.


Be sure to consult also the options related to the generalized pinball model in Section H, see Page H.160, and the interactive commands for the visualization of generalized pinballs and of contacts, see Pages A.25 and O.10.


When using penalty method to compute contact forces, contact stiffness is computed automatically from the stiffness of master elements using the following formulae :

k = φ
GS2
V


in the case of solid master elements, with :

G : bulk modulus of master element’s material,

S : area of contacting face,

V : volume of master element.

k = φ
GS
L


in the case of shell master elements, with :

G : bulk modulus of master element’s material,

S : area of master element,

L : maximum length of master element’s edges.

The bulk modulus G of the material is:

G = 
E
3(1+ν)

where:

E : Young’s modulus of master element’s material,

ν : Poisson’s coefficient of master element’s material.

4.50  FLUID-STRUCTURE SLIDING BY "FSS" (JRC)

D.510


Object:


The purpose is to define fluid-structure sliding lines of the ALE, Lagrangian or fixed type according to the models developed at JRC Ispra.


These directives are obsolete and are maintained only for compatibility with old input files. Use the "LINK COUP FSA" or "LINK COUP FSR" directives instead.


Compatibility: DECO


Syntax:

    "FSS"  | "ALE"  . . . |
           | "LAGR" . . . |
           | "FIXE" . . . |



Comments:


These directives use a rather primitive input syntax that obliges the user to use node indexes and often leads to complex and lengthy input data. A simplification of the input structure to allow the use of GIBI objects is foreseen, but not yet available.


FLUID-STRUCTURE SLIDING OF THE ALE TYPE

D.520


Object:


Defines fluid-structure sliding lines of the ALE type according to the model developed at JRC Ispra. In this type of sliding, the couples of nodes remain permanently aligned. Thus, there is sliding of the fluid along the structure or with respect to another (master) fluid, but the mesh does not slide. This type of sliding is useful for permanently submerged parts of a structure.

                      s2  m2  m4 s4
                       / /    / /
              - - -----0 0----0 0----- - -
                       | |    | |
                       | | me | |
                       | |    | |
                    F  | | S  | |  F
                       | | or | |
                       | | F  | |
                       | |    | |
                       | |    | |
              - - -----0 0----0 0----- - -
                       / /    / /
                      s1 m1  m3 s3

           F = fluid element
           S = structural element


Note:

Nodes (s1, m1) (s2, m2) (s3, m3) (s4, m4) are coincident in the real geometry.


Master (structural or fluid) nodes are Lagrangian, while slave nodes are treated by the ALE formulation and are constrained to follow the corresponding master nodes.


Compatibility: COUP


Syntax:

    "ALE"   "NCOT" nasle * ( /LECTURE/ )
            "NPOI" nasln
 where:

    /LECTURE/ = LECT me m1 m2 s1 s2 m3 m4 s3 s4 c1 c2 TERM


nasle

Number of ALE sliding element side couples of the type shown in the above sketch, to be described by the following /LECTURE/.
me

Master element index.
m1, m2

Nodes defining the first master element side.
s1, s2

Nodes defining the first slave element edge.
m3, m4

Nodes defining the second master element side (default is 0 0, i.e. sliding occurs along one side only of the master element).
s3, s4

Nodes defining the first slave element edge (default is 0 0, i.e. sliding occurs along one side only of the master element).
c1, c2

Key to define the type of connection for nodes (s1, m1, m3, s3) and (s2, m2, m4, s4), respectively. Normally these values are both 1, that means ALE sliding. A value of 0 means connection without sliding: this allows to rapidly eliminate a sliding condition, i.e. as if the nodes were rigidly connected, without modifying too much the input. Note that, when a sliding condition is eliminated by posing c1 or c2 equal 0, the corresponding slave node must be declared Lagrangian in the GRILLE directive. Finally a third possibility, indicated by the value -1, is used to model a so-called U-bend ALE sliding. This is useful for situations where a thin structure is permanently submerged in a fluid, in order to model the U-shaped flow around a tip in the structure (represented by the shell element thickness). In this case, the two structural nodes on the tip have different normals (while for ’inner’ nodes the normal is unique), so a special treatment is needed.
nasln

Total number of nodes defining each of the (slave or master) ale sliding lines.

Comments:


If a negative value is given for m1, m2, s1, s2, m3, m4 s3 or s4, then the corresponding node is not considered in the ALE sliding process. This feature is useful when modeling e.g. a continuous fluid-structure interface of which one part has a sliding condition of the ALE type, while the rest has a condition of the Lagrangian type. In this case, the element couple at the transition between the two conditions will have one couple of ALE sliding nodes, and the other one Lagrangian. This Lagrangian couple of nodes, say m2 and s2, should have negative indexes.


Finally, note that in this type of sliding the number of nodes in the fluid and in the structure must coincide (the nodes themselves must coincide two by two), so the mesh size is necessarily the same on both sides and it is not possible to use a finer mesh on one of the sides with respect to the other.


FLUID-STRUCTURE SLIDING OF THE LAGRANGIAN TYPE

D.530


Object:


Defines fluid-structure sliding lines of the Lagrangian type according to the model developed at JRC Ispra. In this type of sliding, the couples of nodes do not remain permanently aligned. Thus, there is sliding of the fluid mesh along the structure. This type of sliding is useful when the interface nodes cannot be kept permanently aligned, e.g. near free surfaces. The first side of the sliding line consists of fluid nodes only; the second side may consist either of structural or of (master) fluid nodes.

             first side  second side
                      f2 s2
                       / /
              - - -----0 0----0
                       | |    |
                   fe  | | se |
                       | |    |
                    F  | | S  |
                       | | or |
                       | | F  |
                       | |    |
                       | |    |
              - - -----0 0----0
                       / /
                      f1 s1

           F = fluid element
           S = structural element


Compatibility: COUP


Syntax:

    "LAGR"   "NCT1" lsle1 * ( /LECTURE1/ )
             "NPOI" lsln1
             "NCT2" lsle2 * ( /LECTURE2/ )
             "NPOI" lsln2
 where:

    /LECTURE1/ = LECT fe f1 f2 TERM
    /LECTURE2/ = LECT se s1 s2 TERM


lsle1

Number of element sides on the first side (slave side) of the Lagrangian sliding line.
fe

Index of the fluid (slave) element.
f1, f2

Indexes of the nodes of the slave edge (first side).
lsln1

Total number of nodes defining the slave edges.
lsle2

Number of element edges on the second side (master side) of the Lagrangian sliding line.
se

Index of the structural (or master fluid) element.
s1, s2

Indexes of the nodes of the master edge (second side).
lsln2

Total number of nodes defining the master edges.

Comments:


If a negative value is given for f1, f2, s1 or s2, then the corresponding node is not considered in the Lagrangian sliding proocess. This feature is useful when modeling e.g. a continuous fluid-structure interface of which one part has a sliding condition of the ALE type, while the rest has a condition of the Lagrangian type. In this case, the element couple at the transition between the two conditions will have one couple of ALE sliding nodes, and the other one Lagrangian. The ALE couple of nodes, say m2 and s2, should have negative indexes.


In this type of sliding, the number of nodes on the fluid side may be different from that on the structural side, since the nodes don’t have to be aligned in the initial configuration, as it is the case for ALE sliding. It is therefore possible to use meshes of different size for the fluid with respect to the structure.


FLUID-STRUCTURE SLIDING OF THE FIXED TYPE

D.540


Object:


Defines fluid-structure sliding lines of the fixed type according to the model developed at JRC Ispra. This type of sliding is sometimes useful to model rigid inviscid boundaries. Nodes belonging to a fixed sliding line are treated as Lagrangian. The fixed boundary is defined via a series of points identified by their coordinates.

                          x
                         /
            - - -----0  /
                    /  /
              F    /  /
                  /  /
        - - -----0  x
                 |  |
            F    |  |
                 |  |
                 |  |
        - - -----0  |
                    |
                    x

           F = fluid element
           0 = fluid node
           x = fixed point defining fixed sliding line


Compatibility: COUP


Syntax:

    "FIXE"   "NPOI" n1fsl /LECTURE/
             "NFIX" n2fsl * ( xcoor ycoor )


n1fsl

Number of nodes on the fixed sliding line.
n2fsl

Number pf fixed points used to define the fixed boundary.
xcoor, ycoor

Coordinates of the fixed point.

4.51  NODE TO SHELL CONNECTOR

D.550


Object:

This element is used in order to connect node to a master edge of shell. Note that the "SH3D" directive is a subdirective of the "LIAI" directive but it is needed to define an element which defines the nodes (master and slave) of the liaisons. It is listed in this Section because it consists in the definition of kinematic constraints between the dof of one slave node and 2 master nodes.


Compatibility: COUP, LIAI


                      N4-----------N3
                      |             |
                      |             |
                      |             |
                      |             x S
                      |             |
                      |             |
                      N1 --------- N2

                  N1,N2,N3,N4 = nodes shell
                  S           = Slave node

Syntax:

    "SH3D OPT 2"
             ( /LECTURE/)
/LECTURE/

Reading procedure of the elements

Comments:

Note that in the "GEOM" directive the definition of the element must be in this order : N1 N2 S ie the slave node is defined after the two master nodes.

4.52  WEAK FLUID-STRUCTURE COUPLING 2 (FLSW)

D.555


Object:


This directive allows to specify a “weak” coupling between a fluid and a structure modelled by topologically independent meshes. It is similar to FLSR (see page D2.143) but uses a weak approach (direct application of the fluid pressure onto the structure) rather than a strong approach (constraint on velocity imposed by Lagrange multipliers).

The present FLSW directive is (primarily) intended for use with cell-centered Finite Volumes (CCFV) modeling of the fluid. Recently, it is also being rendered compatible with Finite Elements, using then master/slave approach instead of (coupled) Lagrange Multipliers. However, this part of the implementation (FE coupling) is still incomplete and experimental.


The fluid mesh may be either fully general (unstructured) or regular (structured), as specified by the STFL directive described on page C.68. In the latter case, the search operations are faster.


The STFL directive produces by default a Finite Element regular mesh for the fluid domain (which is normally not suited for use in conjunction with the present FLSW model). To create a regular cell-centred Finite Volume mesh instead, for use with FLSW, add the extra VFCC keyword to the COMP STFL directive (see page C.68).


The FSI coupling is realized between structural points (ultimately, structural nodes) on one side, and fluid entities on the other side. The nature of the fluid entities depends upon the chosen options: they are fluid cell centroids if the VOLU keyword (or nothing) is specified (this is the default), while they are fluid cell interfaces if the FACE keyword is specified (see below for details).


Compatibility: DECO


Syntax:

    FLSW     STRU /LECTS/
          |[ FLUI /LECTF/ ; STFL ]|
          $[ R r       ; GAMM gamm ; PHIS phis ]$
          $[ HGRI hgri ; NMAX nmax ; DELE dele ]$
            <DGRI>
            <VOLU ; FACE>
            <BFLU bflu> <FSCP fscp>
            <ADAP LMAX lmax <SCAL scal> >

Basic parameters
STRU

Introduces the structure mesh to be coupled with the fluid. The concerned elements are specified next.
/LECTS/

List of structural elements concerned. All their nodes must be declared as Lagrangian.
FLUI

The fluid mesh to be coupled with the structure is fully general (unstructured). The concerned elements are specified next.
/LECTF/

List of fluid elements concerned. The fluid mesh is unstructured.
STFL

The fluid mesh to be coupled with the structure is regular (structured). The concerned elements (volumes) need not be specified. In fact, they are simply the elements (volumes) generated by the COMP STFL directive described on page C.68, which must in this case have been specified previously in the input file. Since by default the COMP STFL directive produces Finite Elements for the fluid domain, make sure to add the VFCC optional keyword to that directive (see page C.68), so that cell-centered Finite Volumes are created instead.

Structural influence domain

The next three keywords (R, GAMM or PHIS) are used to set the size (thickness) of the structural influence domain surrounding the structure elements defined above by /LECTS/. All fluid entities as defined above (cell centroids or cell interfaces) contained within this influence domain will be coupled to the structure.

Therefore, the correct size of the influence domain is related to the size of the fluid mesh in the vicinity of the embedded structure. On one hand, if the influence domain is too thin, then some interactions between the structure and the fluid enetities might be overlooked, thus resulting in spurious passage of fluid across the structure (leakage). On the other hand, if the inluence domain is too thick, too much fluid will be interacting with the structure (excessive added mass effect). The optimal value is then the minimum value which ensures structure tightness (no leakage).

By default, i.e. if neither R nor GAMM nor PHIS are specified, the code performs an automatic determination of influence spheres at each coupled structural node by using the default value of GAMM (γ=1.01). For the choice of R, GAMM or PHIS in adaptive calculations see the ADAP keyword below and the comments at the end of this page.

R

Prescribed (fixed) radius R of influence spheres at each coupled structural node. In the special, but frequent, case of a uniform structured fluid mesh (uniform square or cube elements) it is suggested to take R slightly larger than the semi-diagonal of a fluid element. This means that, for a 2D uniform square fluid mesh of side LΦ one should take R=0.71LΦ while for a 3D uniform cube fluid mesh of side LΦ one should take R=0.87LΦ.
GAMM

Coefficient γ for the automatic determination of influence spheres at each coupled structural node, based on the size of the enclosing fluid element (which must thus be found by the code by means of a fast search algorithm, see the remarks at the end of this manual page). The sphere radius is RRF=γδ LΦ where LΦ is the local length (size) of the fluid mesh, δ is a coefficient related to the space dimension d of the problem (δ=√d /2, i.e. about 0.71 in 2D and about 0.87 in 3D calculations). The quantity indicated as RF above is the “natural” size of the sphere radius, i.e. the radius of a sphere (circle in 2D) which exactly encompasses all nodes of a regular element (regular cube in 3D or regular quadrilateral in 2D). By default it is γ=1.01. This value should ensure “tightness” of the structure, at least for a regular mesh. By increasing the value, tightness is safer but the amount of fluid “attached” to the structure also increases. By decreasing the value, some local spurious passage of fluid across a solid structure might occur.
PHIS

Coefficient φs for the automatic determination of influence spheres at each coupled structural node. The sphere radius is equal to φs times the minimum structural element length at the concerned node. By default it is φs=0.3. This option should be rarely used. It is advisable to use GAMM instead.

Fast search of coupled fluid entities

The next three keywords (HGRI, NMAX or DELE) are used to determine the size of the spatial grid used for the fast search of fluid entities (nodes, or cell interfaces if the FACE keyword is specified, see below) contained within the influence domain of the structure. Fast search speeds up the calculation and is absolutely essential in medium and even more in large size simulations. For this reason, fast search is always active in the present FSI model. Note that this may be unlike other types of search in EPX. For example, in the pinball contact model (PINB) fast search of pinballs contact is not active by default (an option has to be activated).

By default, i.e. if neither HGRI, nor NMAX, nor DELE are specified, the code takes DELE 1.01.

A (regular) spatial grid is built up and used for the fast search. The fluid entities (centroids or interfaces) contained in a cell of the search grid are tested for inclusion in the structural influence subdomains contained either in the same cell or in a direct neighbour cell (there are up to 8 such cells in 2D, up to 26 cells in 3D). The cell grid can be optionally dumped out on the listing by the DGRI keyword.

For the calculation to be as fast as possible, the fast search grid must have the minimum size ensuring correctness of results, i.e. such that a (barely) sufficient number of interacting entities is detected, and thus no spurious fluid passage occurs across the structure. If hF denotes the size of the fluid mesh and hS the size of the structure mesh, then the grid size hG must be:

hG=φ·max(hF,hS)       (5)

where φ>1 is a sefety factor. A value φ=1.01 should be sufficient. Since a single grid is used for the search over the whole computational domain, hF and hS in the above expression must be the maximum sizes of the fluid and structural elements which are susceptible of interacting, i.e. which belong to the /LECTF/ and LECTS/ sets defined above.

In calculations without adaptivity one has normally hF<hS for accuracy reasons (especially if shells are used to discretize the structure), so that the grid size is (normally) dictated by the largest coupled structural element. For the case of adaptive calculations, see the Remarks at the end of this manual page.

HGRI

Specifies the size of the fast search grid cell. Each cell has the same size in all spatial directions and is aligned with the global axes.
NMAX

Specifies the maximum number of cells along one of the global axes.
DELE

Specifies the size of the fast search grid cell as a multiple of the length of the largest coupled structural element. Element “diameters” are computed only along each global spatial direction and the maximum is taken. For example, by setting DELE 2 the size of the cell is two times the length of the largest coupled structural element. By default, i.e. if neither HGRI, nor NMAX, nor DELE are specified, the code takes DELE 1.01.
DGRI

Dump out the initial grid of cells used for fast searching on the listing (only at step 0).

Additional optional parameters

Next come some additional parameters.

VOLU

For use with Cell Centered Finite Volumes only. The search for fluid entities “contained” in the influence domain of the structure is based upon the element volume, more precisely on the position of the element centroid. This is the default.
FACE

For use with fluid Cell Centered Finite Volumes only. The search for fluid entities “contained” in the influence domain of the structure is based directly upon the “faces” (interfaces) between neighboring cells. The centroid of the face is considered rather than the centroid of the finite volume. In this case, there is no difference between using BFLU 1 or BFLU 2, see below. However, please note that by omitting BFLU or by specifying BFLU 0 (the default value for BFLU) no numerical fluxes are blocked. So, if FACE is used and fluxes must be blocked (as is normally the case), one must specify either BFLU 1 or BFLU 2 (with no difference in the results).
BFLU

For use with cell-centered Finite Volumes only. Type of treatment of numerical fluxes (density and energy, but not momentum) in fluid models, when used in conjunction with the present FLSW directive. The value 0 (default) indicates that fluxes are freely computed. The value 1 indicates that fluxes are blocked between two fluid entities which are both within the influence domain of the structure. The value 2 indicates that fluxes are blocked between two fluid entities of which at least one lies within the influence domain of the structure. If the FACE keyword has been specified (see above), there is no difference between using BFLU 1 or BFLU 2. However, please note that by omitting BFLU or by specifying BFLU 0 (the default value for BFLU) no numerical fluxes are blocked. So, if FACE is used and fluxes must be blocked (as is normally the case), one must specify either BFLU 1 or BFLU 2 (with no difference in the results).
FSCP

For use with cell-centered Finite Volumes only. Type of weak coupling between fluid entities and corresponding structural points, when used in conjunction with the present FLSW directive. The value 0 (default) indicates that coupling occurs only in the direction normal to the structure. The value 1 indicates that coupling occurs along all spatial directions.

FSI-driven adaptivity

Finally, there are some optional keywords related to automatic (FSI-driven) adaptivity of the fluid mesh near the structure.

ADAP

Activates mesh adaptivity for automatic refinement and un-refinement of the fluid mesh specified by /LECTF/ in the vicinity of the structure specified by /LECTS/. Note that this type of mesh adaptivity is at the moment incompatible with other types of adaptivity such as those activated by the WAVE or INDI directives.
LMAX

Introduces lmax, the desired maximum adaptive refinement level Lmax of the fluid mesh in the vicinity of the structure. This value should be greater than 1, since level 1 is attributed to the base mesh (no refinement). Each level corresponds to a halving of the mesh size with respect to the immediately previous level.
SCAL

Introduces scal (s), an optional scaling factor to be used in the determination of elements to be refined. By default scal is equal to 1. When scaling the structural influence domain by successive powers of two in order to identify, at each refinement level, the fluid elements to be refined or un-refined, the code finally multiplies the result by this factor. Using a value of s greater than one, e.g. 1.5 or 2, correspondingly enlarges the zone of fluid mesh around the structure which is refined and this may result in a smoother mesh transition (for example, as an alternative to the option OPTI ADAP RCON). Note, however, that s has no influence on the size of the structural influence domain used for the final search of fluid entities (fluid nodes or fluid cell interfaces) interacting with the structure. This search is always done by the smallest influence domain RLmax = R1/2Lmax − 1, i.e. without taking into account the s factor.

In FSI adaptive calculations, the size of the structural influence domain specified in input by R, GAMM or PHIS is related to the base (i.e. the coarsest) fluid mesh size, not to the refined one (for the user’s convenience) and is then scaled automatically by the code whenever necessary, up to the maximum chosen refinement value given by the ADAP LMAX keyword. Therefore, in order to try out different adaptive refinement levels in the vicinity of the structure the user needs only to change LMAX in the input directive (all other parameters R etc. remain the same).

In FSI adaptive calculations, that is when the FLSW ADAP LMAX optional keyword has been specified, one is certain that the fluid mesh in the vicinity of the structure will be constantly refined to the maximum level (minimum size) specified for the fluid (LMAX), given by:

hFrefined=hFbase/2Lmax−1     (6)

For this reason, in the equation (5) for the determination of the grid size HGRI (hG) one can use hFrefined instead of the base fluid mesh h+Fbase=hF, obtaining thus:

hG=φ·max(hFrefined,hS)       (7)

One should make sure to use (7) instead of (5) since it is likely to be hFrefined<hS, while it is typically hF>hS, so this may lead to important savings of CPU time.


Remarks:


In case of automatic determination of influence spheres based on the GAMM keyword in conjunction with an unstructured fluid grid, a fast search over the coupled fluid elements is needed in addition to the normal fast search over the coupled structural elements. Scope of this second search is to determine, for each structural node, which is the fluid element currently containing the node. For this purpose, the code uses a fast search algorithm by means of the same parameters (DGRI, HGRI, NMAX, DELE) specified above for the search over structural elements. Note, however, that as concerns this second search if DELE is specified it refers to the size of the fluid element rather than to the size of the structural element. However, if a structured fluid grid is specified, then no additional search is needed because the containing fluid element can be detected directly.


Make sure you consult the additional options related to the functioning of the FLSW model in pages H.155 and H.160.


References

The FLSR model (similar to FLSW in many aspects) was first described in report []. A short description of the model is also given in reference [].

4.53  NODE ON FACET ELEMENT

D.560


Object:

Note that the "MAPi" directive (i = 2,..7) is a subdirective of the "LIAI" directive but it is needed to define an element which defines the nodes (master and slave) of the liaisons. It is listed in this Section because it consists in the definition of kinematic constraints between the dof of one slave node and master nodes.

The purpose is to to glue one slave node to a master face. It can be used in 2-D (the face is a line) or in 3-D.


Compatibility: COUP, LIAI

Different cases can be used and are listed below.

 ---------------------------------------------------------------------------------
| Name | Dimension  | Npt |  Dof  |  Nb. of  |             Remarks                |
|      |            |     |       | liaisons |                                    |
 ---------------------------------------------------------------------------------
| MAP2 |     2      |  3  |   2   |     2    |  point on solid line               |
| MAP3 |     3      |  4  |   3   |     3    |  point on triangular solid facet   |
| MAP4 |     3      |  5  |   3   |     3    |  point on quadrangular solid facet |
| MAP5 |     2      |  3  |   3   |     3    |  point on 2D shell line            |
| MAP6 |     3      |  4  |   6   |     6    |  point on triangular shell facet   |
| MAP7 |     3      |  4  |   6   |     6    |  point on quadrangular shell facet |
 ---------------------------------------------------------------------------------

Note:

In 3-D the slave node S should be on the face.

               MAP2      |          MAP7

                 N1      |       N1-------N2
                  |      |       |         |
                  |      |       |      S  |
                S x      |       |      x  |
                  |      |       |         |
                 N2      |       N3-------N4
                         |
                         |

              N1,N2,N3,N4 = Master nodes
              S           = Slave node

Syntax:

 "MAPi"
      ( /LECTURE/ )
/LECTURE/

Reading procedure of the elements.

Comments:

Note that in the "GEOM" directive the declaration of the element must be in this order : S N1 N2 (N3 N4), ie the slave node is the first node of the list.

4.54  FINITE-ELEMENT/SPECTRAL-ELEMENT INTERFACE

D.570


Object:


This directive allows to specify the interface between a Finite Element domain and a Spectral Element domain in a coupled analysis.

It replaces the former principal directive FESE, which is no longer accepted. The difference is that FE/SE interfacing is now coupled with any other (coupled) links specified in the calculation (LINK COUP), while formerly the FE/SE interface conditions were treated as a separate set of conditions.


Compatibility: COUP


Syntax:

    "FESE" "FNOD" /LECT1/
           "SNOD" /LECT2/


/LECT1/

List of Finite Element nodes along the FE/SE interface.
/LECT2/

List of (micro) Spectral Element nodes along the FE/SE interface.

Remarks:


The model is quite general and accepts the node lists in any order. It is even possible to define interfaces formed by several disjoint lines (or surfaces, in 3D).


The only restriction is that FE and (micro) SE nodes must lie with sufficient precision on the interface, which is defined geometrically by the macro Spectral Element faces.


Furthermore, note that to every macro Spectral Element node on the interface, there must exist one and only one FE node in LECT1 that has the same coordinates. This is necessary in order to ensure that to every FE face on the interface there correspond one and only one opposite macro Spectral Element face (the reverse is not true, in general).

4.55  NAVIER-STOKES (INCOMPRESSIBILITY)

D.580


Object:


This directive allows to specify an incompressible or quasi-incompressible behaviour for selected fluid elements. These elements must possess the LIQU material (see page C.390).

It replaces the former NAVI problem type directive (see page A.30) which automatically generated liaison conditions for all elements containing a LIQU material.


Compatibility: COUP


Syntax:

    "NAVI" /LECT/


/LECT/

List of Finite Elements concerned. These must possess the LIQU material.

Remarks:


With this directive, it is not allowed to specify the NAVI keyword in the problem type. Use either the old (NAVIER problem type) directive or the present one, but not together in the same run.


For the moment, only elements of type CAR1, TUBE and TUYA are accepted.


Be aware the verification of a link of type NAVI, as activated by the optional keyword VERI of the LINK directive (see page D2.10), makes sense only when the corresponding LIQU material is perfectly incompressible. In fact, when the material is (even slightly) compressible, as indicated by a finite sound speed C specified in the material parameters, an extra term is added to the diagonal of the assembled links matrix during the solution process. Therefore, it is normal that the original link specification does not hold any more.

4.56  PIPELINE RUPTURE CONNECTION

D.590


Object:


This FSI model allows modelling a break of a pipeline discretized with TUYA elements. Prior to the pipeline rupture instant, the conservation of the internal fluid mass flow rate and the continuity of the mechanical degrees of freedom are ensured.


Compatibility: COUP


Syntax:

    "BREC"   < "TRUP" trup >   /LECTURE/


trup

Rupture instant (no breaking by default).
/LECTURE/

Number or the name of the BREC element.

Comments:


This directive may only be used to connect two TUYA elements.



Outputs:


The components of the ECR table are as follows:

ECR(25): pipeline rupture area (water)

ECR(26): mass flow (water)

ECR(27): total ejected mass (water)

4.57  SURFACE PRESSURE MEASURED IN AN ELEMENT (PELM)

D.600


Object:


This directive allows to apply a pressure on structural facets (referred to as slave facets), which is measured in a given fluid element of the model (referred to as master element).


It is typically useful when a cavity is modelled by an equivalent pipe network instead of a full 3D mesh, but the pressure on its structural envelop must still be taken into account. Reference element would then be one of the TUBE or TUYA elements used for the cavity and the facets the structural envelop.


Compatibility: DECO


Syntax:

    PELM   ( MAIT /LECTURE/
             ESCL /LECTURE/
             < NOEX /LECTURE/ >
             < |[ INTE ; EXTE ]| /LECTURE/ >
             < PREF pref > )


pref

Reference pressure.

Comments:


Only one master element must be provided for each set of slave facets.


If slave elements are 3D continuum elements, pressure is applied on any of their free facets, along the inward normal direction.


If slave elements are 3D shell elements, keywords INTE or EXTE are used to enter a node defining the internal or external side of the structure respectively and again, pressure is applied along the inward normal direction. Option NOEX allows excluding some slave nodes from applying pressure.


No retroaction occurs from the structure onto the fluid element, which is licit only in the case of a large cavity which imposes its pressure and for limited structural displacements.

4.58  UNCOUPLED HANGING LIKNS

D.610


Object:


This directive allows to toggle uncoupled master/slave algorithm to handle hanging links with ADAPTIVITY instead of the fully coupled Lagrange Multipliers approach.[MPI only].


Compatibility: DECO


Syntax:
    ADAP



Comments:


No further subdirective is currently needed.

4.59  PRESCRIBED DAMAGE FOR GRADIENT DAMAGE MATERIALS

D.620


Object:

This directive defines imposed damage values for gradient damage materials ENGR, see ??. Concretely this routine will simply update the lower and upper bounds of the damage minimization problem.


Compatibility: COUP, DECO


Syntax:
   "ENGR" ( alpha0 /LECTURE/ )


alpha0

Prescribed damage value.
LECTURE

List of the nodes concerned.

Previous Up Next