D.10
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 subdirectives:
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.
$ 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 . . . , 
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
subdomains.
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.
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 trialanderror 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).
Be sure to check the various options available in relation to
connections: see Page H.160.
Choose between the available categories for links (see GBD_0010).
$[ COUP ; DECO ; LIAI ]$
D.12  Oct 13
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/>
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 illconditioned.
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 closedform
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, closedform 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 righthand side vector. Default precision is
10^{−}5 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 righthand 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 timevarying links, in order to save CPU time. This is especially useful
for fluidstructure interaction, when links are classically updated at each
timestep, 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).
D.20  Oct 13
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.
< "SOLV" [ "CHOL" ; "PARD" ; "SPLI" < "TYPE" imet > < "PCON" ipre > ... ... < "PITE" prec > < "IPA1" ip1 > ... ... < "IPA2" ip2 > < "RPAR" rp > ... ... < "INIS" inig > ] > < $[ "RENU" ; "NORE" ]$ > < "FREQ" ifreq > <"VERI">
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 threadsafe, highperformance, robust,
memory efficient and easy to use software for solving large sparse symmetric
and unsymmetric linear systems of equations on sharedmemory and
distributedmemory multiprocessors. This package is include in MKL library
provided by the Intel compiler.
http://www.pardisoproject.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/iterativesurvey/node61.html
The integer parameter imet specifies which SPLIB solver to use :
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, CGStabilization is used.
The integer parameter ipre specifies which preconditioner to use :
The integer parameter ip1 indicates the levels of fillin 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 fillin 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 :
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://wwwusers.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 illconditioned.
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 usersupplied
value for ifreq in these cases.
The same holds for an incompressible calculation, or for a
calculation involving nondeformable substructures (keywords
"NAVIER" and "SOLIDE").
D.25
This directive allows to read the connections data from
an auxiliary file.
< "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".
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
"BLOQ" ( /LECDDL/ /LECTURE/ )
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 timelimited 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.
D.31
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
"TBLOQ" ( /LECDDL/ $ "UPTO" t ; "TRIG" $ /LECTURE/ )
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.
D.35
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
"GUIDE" "DIRX" rx "DIRY" ry "DIRZ" rz /LECTURE/ )
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 xaxis is collinear with the sliding direction, the yaxis is collinear with Yaxis, and zaxis 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.
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
"CONT"  "PLAN" ...   "SPHE" ...   "CYLI" ...   "CONE" ...   "TORE" ...   "SPLA" ... 
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 2D computations and 3 for 3D 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 firstorder accuracy.
The instructions are described in detail on the following pages.
D.50
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
"PLAN" [ "NX" x "NY" y < "NZ" z > ; "NR" r "NZ" z ; "POIN" /LECT1/ ; "AUTO" ] /LECT2/
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).
D.60
The specified nodes lay on (a) sphere(s) of given center.
In 2D, the sphere reduces to a circle.
Compatibility: COUP, LIAI
"SPHE" [ "CX" x "CY" y < "CZ" z > ; "CR" r "CZ" z ; "CENT" /LECT1/ ] /LECT2/
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.
D.70
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 3D analysis. In 2D, the SPHE
directive described in the previous Section may be used
to obtain a circular restraint.
Compatibility: COUP, LIAI
"CYLI" [ "P1X" x1 "P1Y" y1 "P1Z" z1 ; "POI1" /LECT1/ ; "P2X" x2 "P2Y" y2 "P2Z" z2 ; "POI2" /LECT2/ ] /LECT3/
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.
D.80
The specified nodes lay on (a) cone(s) of given axis.
The instruction only applies to a 3D analysis.
Compatibility: COUP, LIAI
"CONE" $[ "SX" x1 "SY" y1 "SZ" z1 ; "APEX" /LECT1/ ]$ $[ "PX" x2 "PY" y2 "PZ" z2 ; "POIN" /LECT2/ ]$ /LECT3/
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.
D.90
The specified nodes lay on (a) torus(es) of
given axis and center.
This instruction only applies to a 3D analysis.
Compatibility: COUP, LIAI
"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/
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.
D.100
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
"SPLA" [ "NX" x "NY" y < "NZ" z > ; "NR" r "NZ" z ; "POIN" /LECT1/ ; "AUTO" ] /LECT2/
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 noncoincident 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.
D.110
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 2D and 3D analysis.
For an Eulerian computation (no mesh displacements),
the fluid velocities are radial and of the same modulus.
Compatibility: COUP, LIAI
"RADI" "SPHE" "CENT" /LECTURE/ ... "CONT" /LECTURE/
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.
D.120
Several displacement (or velocity) components
are linked by constant coefficients
during the whole computation.
Compatibility: COUP, LIAI
"RELA" ngroup*( ... nrel nterm*( coef icomp $[ nuneu ipas ; /LECTURE/ <SHIF s> ]$ ) ... "EGAL" /LECDDL/ /LECTURE/ )
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.
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)
D.125
In calculations of structures made of reinforced concrete,
this directive allows to link the displacements of the nodes belonging
to continuumlike elements made of concrete, with those
of barlike 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
"ARMA" < "TSTA" ista> < "CSTI" cstif > "BETO" /LECTURE/ "FERR" /LECTURE/
The concrete elements must be of continuumlike type 2D or 3D.
The steel or reinforcement elements must be of barlike 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 timestep is not smaller that the
reference concrete element’s one.
D.126
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
"CROS" < "TSTA" ista> < "CSTI" cstif > "LONG" /LECTURE/ "TRAN" /LECTURE/
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 timestep is not smaller that the
reference longitudinal steel element’s one.
D.127
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.
"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
If ista equals 2, stiffness of the penalty spring is limited so that
the associated stability timestep is not smaller that the
reference concrete element’s one.
D.128
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 cableconcrete 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 frictionspring 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 ADHEtype 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.
"LCAB" $[ "ADHE" ; "GLIS" ; "FROT" ]$ "BETC" /LECTURE/ "CABL" /LECTURE/
This directive may by repeated as many times as necessary.
D.129
This directive allows linking in a continuous way two (or more) subdomains used to model a slender structure, some subdomains modeled as thick shells (ReissnerMindlin kinematics) and others represented through a 3D hexahedratype mesh. The shell and 3D subdomains 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.
"ARLQ" < "ROTA" > "COQU" /LECTURE/ "VOLU" /LECTURE/
This directive may by repeated as many times as necessary.
D.130
These instructions define imposed motions (displacements,
velocities or accelerations) depending on time, for different
degrees of freedom.
Compatibility: COUP, LIAI
"DEPL" ( /LECDDL/ coef "FONC" ifonc < "TLIM" tlim > /LECTURE/ ) "VITE" ( /LECDDL/ coef "FONC" ifonc < "TLIM" tlim > /LECTURE/ ) "ACCE" ( /LECDDL/ coef "FONC" ifonc < "TLIM" tlim > /LECTURE/ )
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.
D.140
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
twodimensional computations (plane or axisymmetric).
Compatibility: COUP, LIAI
"COQM" ngroup*( nco nma /LECTURE/ )
M1 x I (shell) I x x M0 (nma) R(i) : distance M0Mi / I D(i) : normal displacement nco x Mi of Mi I (solid element) Mp x
A "shellsolid 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)
D.141
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 nonmatching 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 subdomain
calculation framework.
Compatibility: COUP
"INTERFACE" [ "COMP" ; "MORTAR" ; "OPTIMAL" ] <"TOLE" tole> ... ... [ "SIDE" ; "SCOARSE" ; "SFINE" ] /LECTURE/ ... ... [ "SIDE" ; "SCOARSE" ; "SFINE" ] /LECTURE/
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 nonmatching meshes, socalled 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 nonmatching 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 (2noded 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.
D.142
This directive allows to specify the coupling between a fluid
and a structure modelled by topologically independent meshes.
Compatibility: COUP
FLST <SLID> STRU /LECTS/ FLUI /LECTF/ <DGRI> $[ HGRI hgri ; NMAX nmax ; DELE dele ]$
D.143
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.
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> >
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.
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 h_{F} denotes the size of the fluid mesh and h_{S} the size of the structure mesh, then the grid size h_{G} must be:
h_{G}=φ·max(h_{F},h_{S}) (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, h_{F} and h_{S} 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 h_{F}<h_{S} 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.
Next come some additional parameters.
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.
The value 0 (default) indicates that no deactivation occurs.
The value 1 indicates that VOFIRE antidissipation 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 antidissipation 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.
Finally, there are some optional keywords related to automatic (FSIdriven) adaptivity of the fluid mesh near the structure.
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:
h_{F}^{refined}=h_{F}^{base}/2^{Lmax−1} (2) 
For this reason, in the equation (1) for the determination of the grid size HGRI (h_{G}) one can use h_{F}^{refined} instead of the base fluid mesh h+F^{base}=h_{F}, obtaining thus:
h_{G}=φ·max(h_{F}^{refined},h_{S}) (3) 
One should make sure to use (3) instead of (1) since it is likely to be h_{F}^{refined}<h_{S}, while it is typically h_{F}>h_{S}, so this may lead to important savings of CPU time.
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.
The FLSR model was first described in report []. A short description of the model is also given in reference [].
D.144
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).
FLSX STRU /LECTS/ FLUI /LECTF/ <LSPC lspc> <LORD lord>
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 finiteelement discretization of the constraint:
∫ 
 ⎡ ⎣  ⎛ ⎝  v_{s}(x)−v_{f}(x)  ⎞ ⎠  · n_{s}(x)  ⎤ ⎦  λ(x) dx , ∀λ∈ L^{2}(Γ) (4) 
where Γ is the midsurface of the structure, v_{f} and v_{s} the fluid and structure velocity respectively, n_{s} the normal to Γ, and λ a test function. The two options LSCP and LORD specify the finiteelement 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 finiteelement 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 finiteelement space for the Lagrange multiplier.
D.150
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 threedimensional
computations.
This connection may be expressed in two ways:
 By using specific fluidstructure elements FS2D or
FS3D: directive "FS";
Without using fluidstructure elements:
directive "FSA".
Compatibility: COUP, LIAI
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.
D.152
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
"FS" /LECTURE/
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".
D.160
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, ...).
D.170
As for unilateral restraints, certain nodes of the structure must
remain in the same halfspace. 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 nondeformable projectile.
Compatibility: COUP, DECO, LIAI
"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/]
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 halfspace admissible for a point M (of the target)
of coordinate x is such
that, if x_{0} is the abscissa of the material point:
α (x−x_{0}) ≥ 0 
These impacts are available in 2D or 3D.
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.
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".
D.175
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
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/
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).
D.176
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
"BUTE" "DIRE" vx vy vz "DMAX" dmax /LECTURE/
D.180
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 autocontact model is available.
An autocontacting 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).
"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/ > )
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.
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 halfspace 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.
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).
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 = r_{fac} 

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 = r_{fac} 

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.
D.185
This directive activates the (internal) interactions occurring
among a set of particles
(“billes”) representing a soft body, according to the
socalled 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
"MPEF" nbpef * ( "BILL" /LECTURE/ < $[ "STRU" /LECTURE/ ; "COQU" /LECTURE/ "EXTE" /LECTURE/ ]$ > )
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.
D.187
This directive activates the (internal) interactions occurring
among a set of particles
(“billes”) representing a soft body, according to the
socalled SmoothedParticle 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
"SPHY" nbpef * ( "BILL" /LECTURE/ < $[ "STRU" /LECTURE/ ; "COQU" /LECTURE/ "EXTE" /LECTURE/ ]$ > )
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.
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
"EDEF" nbcoup nbcoup*("NCOU" ncouches "ELDI" /LECTURE/ "FRON" /LECTURE/ )
D.190
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
"BIFU" < LIBR > /LECTURE/
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.
The various components of the ECR table are as follows:
ECR(1) : density (all materials)ECR(6) : internal energy (water)
D.195
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
"ADHE" "AUTO" auto <"CRIT" "TENS" tens > /LECTURE/
D.200
Write the relations ensuring the conservation of
mass flow rate for the fluid (Eulerian formulation)
Compatibility: COUP, LIAI
"TUBM" /LECTURE/
D.203
Write the relations ensuring the conservation of
mass flow rate for the fluid (moving meshes).
Compatibility: COUP, LIAI
"TUYM" /LECTURE/
D.205
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
"TUYAU" "CENTRE" /LECTURE/ "LISTE" /LECTURE/
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 (standalone) PMAT, which has only 3 dofs.
In such a case, it is sufficient to attach a (dummy) beam or
shell element to the CENT.
D.210
This directive defines the substructures 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
"SOLI" nsol*( ... ) 1st case  Solid meshed by elements: "ELEM" /LECTURE/ "PLIE" /LECTURE/ ... $ < "COMP" ncomp*( "INER" ... ) > $ $ < "INER" ... > $ 2nd case  Rigidly connected points: "POIN" /LECTURE/
A substructure described like a nondeformable 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).
D.215
This directive allows to specify inertia parameters for
a nondeformable solid. It also allows to compute the inertia tensor
starting from simple shapes.
Compatibility: COUP, LIAI
"COMP" ncomp*( "INER" "MASS" m ... ... <"XG" xg> <"YG" yg> <"ZG" zg> ... ... <"IXX" ixx> <"IYY" iyy> <"IZZ" izz> ... ... <"IXY" ixy> <"IXZ" ixz> <"IYZ" iyz> )
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.
D.220
This directive allows to link two substructures by meand
of a kinematic relationship.
Compatibility: COUP, LIAI for VERR, ROTU,
PIVO, GLIS, PIGL and DRIT
Compatibility: COUP for TGGR and CRGR
"ARTI"  "VERR" ...   "ROTU" ...   "PIVO" ...   "GLIS" ...   "PIGL" ...   "DRIT" ...   "TGGR" ...   "CRGR" ... 
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 substructures may be described as either
nondeformable or deformable.
The various types of articulations are described in the
following pages.
D.225
This directive allows to join two substructures by means of
a blocked articulation, i.e. a rigid connection.
Compatibility: COUP, LIAI
"VERR" /LECTURE/ ... ... ( "NOEU" /LECTURE/ "VOIS" $[ "ABSENT" ; "INDEF" isol ; /LECTURE/ ]$ )
The two substructures 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.
D.230
This option allows to link two substructures by a
frictionless hinge.
Compatibility: COUP, LIAI
"PIVOT" /LECTURE/ ... ... "AXE" "VX" vx "VY" vy "VZ" vz ... ... ( "NOEU" /LECTURE/ "VOIS" $[ "ABSENT" ; "INDEF" isol ; /LECTURE/ ]$ )
The pivot axis is modified accounting for the
motions of the substructures.
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.
D.240
This option allows to connect two substructures by a
frictionless pin joint (“rotule”).
Compatibility: COUP, LIAI
"ROTU" /LECTURE/ ... ... ( "NOEU" /LECTURE/ "VOIS" $[ "ABSENT" ; "INDEF" isol ; /LECTURE/ ]$ )
The two substructures 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.
D.250
This option allows to connect two substructures by a
frictionless slider (“glissière”).
Compatibility: COUP, LIAI
"GLIS" /LECTURE/ ... ... "AXE" "VX" vx "VY" vy "VZ" vz ... ... ( "NOEU" /LECTURE/ "VOIS" $[ "ABSENT" ; "INDEF" isol ; /LECTURE/ ]$ )
The slider axis is modified to account for
the motion of the substructures.
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).
D.255
This option allows to connect two substructures by a
frictionless sliding pivot.
Compatibility: COUP, LIAI
"PIGL" /LECTURE/ ... ... "AXE" "VX" vx "VY" vy "VZ" vz ... ... ( "NOEU" /LECTURE/ "VOIS" $[ "ABSENT" ; "INDEF" isol ; /LECTURE/ ]$ )
The sliding pivot’s axis is modified to account for
the motion of the substructures.
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).
D.260
This D.R.I.T. directive (Déplacement Relatif Imposé en fonction du
Temps = Prescribed Timedependent Relative Displacement)
allows to link two substructures by an actuator (“vérin”)
whose length is a prescribed time function.
Compatibility: LIAI
"DRIT" /LECTURE/ ... ... "AMPLI" ampli "FONCTION" ifonc ... ... ( "NOEU" /LECTURE/ "VOIS" $[ "ABSENT" ; "INDEF" isol ; /LECTURE/ ]$ )
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.
D.270
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.
"TGGR" /LECTURE/ ... ... "AXE1" "VX" vx "VY" vy "VZ" vz ... ... "AXE2" "VX" vx "VY" vy "VZ" vz ... ... ( "NOGR" /LECTURE/ )
The pivot axis "AXE1" and "AXE2" are modified accounting for the
motions of the shell.
D.275
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.
"CRGR" /LECTURE/ ... ... "AXE1" "VX" vx "VY" vy "VZ" vz ... ... "AXE2" "VX" vx "VY" vy "VZ" vz ... ... ( "NOGR" /LECTURE/ ) ... ( "NOCR" /LECTURE/ ) ... < "DMAX" dmax >
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.
D.310
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
"ROTATION" "ORIG" x0 y0 < z0 > < "VECT" vx vy vz > "FONC" ifonc ... /LECTURE/
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 userspecified function.
In 2D plane calculations, the rotation axis is normal
to the plane xOy.
D.320
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
"MENS" "POINT" x0 y0 < z0 > < "VECTEUR" vx vy vz > "FONCTION" ifonc /LECTURE/
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 userspecified function.
In 2D plane calculations, the rotation axis is normal
to the plane xOy.
A timelimited 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.
D.321
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
"TMEN" "POINT" x0 y0 < z0 > < "VECTEUR" vx vy vz > "FONCTION" ifonc "UPTO" t /LECTURE/
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 userspecified function.
In 2D plane calculations, the rotation axis is normal
to the plane xOy.
D.322
Automatic prescription of the 3D mechanical relations
between the translational degrees of freedom of a point
with a set of points.
Compatibility: COUP, LIAI
"DISTANCE" /LECTURE/
D.325
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
BARY CENT /LECT/ LIST /LECT/ <VECT <VX vx> <VY vy> <VZ vz>>
By default (no VECT specified) this directive imposes the following (vectorial) condition on nodal velocities v:
 _{C} − ( 
 _{1} + 
 _{2} + ⋯ + 
 _{N}) / N = 

which corresponds to the following 2 or 3 scalar independent links:
v_{Cx} − (v_{1x} + v_{2x} + ⋯ + v_{Nx}) / N = 0 
v_{Cy} − (v_{1y} + v_{2y} + ⋯ + v_{Ny}) / N = 0 
v_{Cz} − (v_{1z} + v_{2z} + ⋯ + v_{Nz}) / 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:
 _{C} · 
 − 
 ( 
 _{1} − 
 _{2} − ⋯ − 
 _{N}) · 
 = 

which corresponds to the following scalar link (assuming a 2D case):
v_{Cx}V_{x} + v_{Cy}V_{y} − 
 (v_{1x}V_{x} + v_{1y}V_{y} + ⋯ + v_{Nx}V_{x} + v_{Ny}V_{y}) = 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.
D.326
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
RIGI CENT /LECT/ LIST /LECT/ <VECT <VX vx> <VY vy> <VZ vz>>
By default (no VECT specified) this directive imposes the following set of N (vectorial) conditions on nodal velocities v:
 _{C} − 
 _{1} = 

 _{C} − 
 _{2} = 

⋯ 
 _{C} − 
 _{N} = 

which corresponds to the following 2N or 3N scalar independent links:
v_{Cx} − v_{1x} = 0 
v_{Cy} − v_{1y} = 0 
v_{Cz} − v_{1z} = 0 (3D only) 
⋯ 
v_{Cx} − v_{Nx} = 0 
v_{Cy} − v_{Ny} = 0 
v_{Cz} − v_{Nz} = 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:
 _{C} · 
 − 
 _{1} · 
 = 

 _{C} · 
 − 
 _{2} · 
 = 

⋯ 
 _{C} · 
 − 
 _{N} · 
 = 

which correspond to the following N scalar links (assuming a 2D case):
v_{Cx}V_{x} + v_{Cy}V_{y} − v_{1x}V_{x} − v_{1y}V_{y} = 0 
v_{Cx}V_{x} + v_{Cy}V_{y} − v_{2x}V_{x} − v_{2y}V_{y} = 0 
⋯ 
v_{Cx}V_{x} + v_{Cy}V_{y} − v_{Nx}V_{x} − v_{Ny}V_{y} = 0 
D.330
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
"SPLINE" nspline * ( "SURFACE" /LECTURE/ ... ... "COURBE" ncourbe * ( "LIGNE" /LECTURE/ ) ... ... "METC" metc "METS" mets "NPTT" nptt ... ... "DEGC" degc "DGST" dgst "DGSZ" dgsz ... ... "EPAIS" epais "FREQ" freq )
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.
D.400
This directive allows to simulate the contact and/or shock without friction between the envelopes of 3D rigid bodies.
Compatibility: LIAI
"COLL" "REST" crest "SGEO" tolgeo "SVIT" tolvit ( "CHAI" ( "SOLI" nusoli "SURF" /LECTURE/ "EPAI" epais "ORIE" xp yp zp ) ) "CONT" ( "CHA1" nucha1 "CHA2" nucha2 ) "FCON"
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:
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.
For further information, please consult the reference [].
D.450
To define fluidstructure 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 fluidstructure 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 fluidfluid
interface.
If no such node exists, then the FS interface is nodally nonconforming
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 nonconforming FS interfaces requires a
special optional keyword (NCFS) to be explicitly
chosen by the user.
If this keyword is not specified and a nonconforming 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
nonconforming interface and there was not just an error in
mesh specification.
Compatibility: COUP, LIAI
"FSA" <"STRU" /LECT_STRU/> <"NCFS"> /LECTURE/
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 subdirective, 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.
D.460
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
"FSR" /LECTURE/
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.
D.480
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 coworkers in the papers:
(i) Ted Belytschko and Mark O. Neal,
“ContactImpact by the Pinball Algorithm
with Penalty and Lagrangian Methods”, Int. J. Num. Meths. Eng., Vol. 31,
pp. 547572 (1991), and (ii) T. Belytschko and I.S. Yeh,
“The splitting pinball method for contactimpact problems”,
CMAME, 105, pp. 375393, (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
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.
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 selfcontact) subdirectives should be repeated as many times as necessary to define all the contacting pinball sets.
The next subblock of data concerns the optional definition of friction characteristics of the body (i.e. of the pinballs set).
The following subblock 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.
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.
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.
The last part of the input is also optional and concerns the activation of contactdriven mesh adaptivity.
This completes the definition of the input data.
The theoretical maximum scaling factors to be used for selfcontacting bodies are shown in the following Table.
Case Encompassing pinballs Equivalent pinballs 2D continuum (squares) √2/2=0.707 √π/2=0.886 3D continuum (cubes) 1/√3=0.577 ∛π/6=0.806
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 noncontacting 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 selfcontacting 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 

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 

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 = 

where:
E : Young’s modulus of master element’s material,ν : Poisson’s coefficient of master element’s material.
Note that the above value of L_{max} refers to the maximum refinement level of the elements (adaptivity) L_{max}^{adap}, and not of the pinballs (contact) L_{max}^{pinb}. 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 L^{adap}=1, while a base (parent) pinball in the contact model has by convention L^{pinb}=0. Thus, it should be kept in mind that:
L^{adap}=L^{pinb}+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 L_{max}^{adap} rather than L_{max}^{pinb}. In any case, it should be rarely necessary to use a hierarchic pinball method in combination with contactdriven 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.
Examples of application of the contact model by the pinball method are presented in the following papers: [].
D.490
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.
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 coworkers in the papers:
(i) Ted Belytschko and Mark O. Neal,
“ContactImpact by the Pinball Algorithm
with Penalty and Lagrangian Methods”, Int. J. Num. Meths. Eng., Vol. 31,
pp. 547572 (1991), and (ii) T. Belytschko and I.S. Yeh,
“The splitting pinball method for contactimpact problems”,
CMAME, 105, pp. 375393, (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.
"GPIN" $[ "PENA" <"SFAC" sfac> ]$ ( $[ "BODY" ; "SELF" ]$ < "FROT" "MUST" must "MUDY" mudy "GAMM" gamm > /LECT/ ) ( "DIAM" diam /LECT/ ) < "EXCL" ("PAIR" n1 n2) >
A point GPIN (PGPIN) is associated to each node to which a contact
diameter has been assigned via the DIAM directive.
Then, the other GPIN types (LGPINs in 2D, or L/T/QGPINs
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 PGPIN is attached to each such node, and this PGPIN (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 noncontacting 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 selfcontacting 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 

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 

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 = 

where:
E : Young’s modulus of master element’s material,ν : Poisson’s coefficient of master element’s material.
D.510
The purpose is to define fluidstructure 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
"FSS"  "ALE" . . .   "LAGR" . . .   "FIXE" . . . 
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.
D.520
Defines fluidstructure 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 00 0         me       F   S   F   or     F             0 00 0   / / / / s1 m1 m3 s3 F = fluid element S = structural element
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
"ALE" "NCOT" nasle * ( /LECTURE/ ) "NPOI" nasln where: /LECTURE/ = LECT me m1 m2 s1 s2 m3 m4 s3 s4 c1 c2 TERM
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
fluidstructure 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.
D.530
Defines fluidstructure 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 00    fe   se     F   S    or    F          0 00 / / f1 s1 F = fluid element S = structural element
Compatibility: COUP
"LAGR" "NCT1" lsle1 * ( /LECTURE1/ ) "NPOI" lsln1 "NCT2" lsle2 * ( /LECTURE2/ ) "NPOI" lsln2 where: /LECTURE1/ = LECT fe f1 f2 TERM /LECTURE2/ = LECT se s1 s2 TERM
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
fluidstructure 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.
D.540
Defines fluidstructure 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
"FIXE" "NPOI" n1fsl /LECTURE/ "NFIX" n2fsl * ( xcoor ycoor )
D.550
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
N4N3        x S     N1  N2 N1,N2,N3,N4 = nodes shell S = Slave node
"SH3D OPT 2" ( /LECTURE/)
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.
D.555
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 cellcentered 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 cellcentred 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
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> >
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.
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 h_{F} denotes the size of the fluid mesh and h_{S} the size of the structure mesh, then the grid size h_{G} must be:
h_{G}=φ·max(h_{F},h_{S}) (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, h_{F} and h_{S} 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 h_{F}<h_{S} 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.
Next come some additional parameters.
Finally, there are some optional keywords related to automatic (FSIdriven) adaptivity of the fluid mesh near the structure.
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:
h_{F}^{refined}=h_{F}^{base}/2^{Lmax−1} (6) 
For this reason, in the equation (5) for the determination of the grid size HGRI (h_{G}) one can use h_{F}^{refined} instead of the base fluid mesh h+F^{base}=h_{F}, obtaining thus:
h_{G}=φ·max(h_{F}^{refined},h_{S}) (7) 
One should make sure to use (7) instead of (5) since it is likely to be h_{F}^{refined}<h_{S}, while it is typically h_{F}>h_{S}, so this may lead to important savings of CPU time.
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.
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 [].
D.560
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 2D (the face is a line) or in 3D.
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  
In 3D the slave node S should be on the face.
MAP2  MAP7 N1  N1N2        S  S x   x      N2  N3N4   N1,N2,N3,N4 = Master nodes S = Slave node
"MAPi" ( /LECTURE/ )
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.
D.570
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
"FESE" "FNOD" /LECT1/ "SNOD" /LECT2/
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).
D.580
This directive allows to specify an incompressible or
quasiincompressible 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
"NAVI" /LECT/
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.
D.590
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
"BREC" < "TRUP" trup > /LECTURE/
This directive may only be used to connect two TUYA elements.
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)
D.600
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
PELM ( MAIT /LECTURE/ ESCL /LECTURE/ < NOEX /LECTURE/ > < [ INTE ; EXTE ] /LECTURE/ > < PREF pref > )
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.
D.610
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
ADAP
No further subdirective is currently needed.
D.620
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
"ENGR" ( alpha0 /LECTURE/ )