These directives enable the user to complete the geometry.
"COMPLEMENT"
These directives are described in detail on the following pages.
The keyword "COMPLEMENT" and the associated data are compulsory only
if required by the elements (shells, beams and 1D elements) or
if the user enters added masses.
Do not forget the corresponding dimensioning (page A.70).
C.25
This directive allows to read complementary data from
an auxiliary file.
< "FICHIER" 'nom.fic' >
In certain cases the data may be bulky. It is then advisable
to store the data on an auxiliary file in order to shorten
the main input data file. The auxiliary file is activated
by the keyword "FICHIER" that precedes the full name of
the file (under Unix). Then, only the keyword "COMPLEMENT" preceding
the keyword "FICHIER" remains in the main input file.
The auxiliary file (in free format) will contain the whole set
of geometry complement data, with the exception of the keyword
"COMPLEMENT" itself.
To resume reading from the main input data file, the auxiliary
file must be terminated by the keyword "RETOUR".
This instruction enables the user to define the masses
which are added to certain nodes, along certain degrees
of freedom.
< "MASS" ( /LECDDL/ xm /LECTURE/ ) >
1/ Several added masses may be defined without repeating
the keyword "MASS".
Example:
"MASS" /LECDDL/ xm1 /LECTURE/ /LECDDL/ xm2 /LECTURE/ . . .
2/ Use:
"MASS" 1342 xm "SUIT" 1 2 3 "TERM"
The degrees of freedom 1,3,4,2 of the nodes 1,2,3 are modified
by the mass xm (this mass is added to the initial one).
In axisymmetric cases, do not forget to divide the "true"
mass by 2π.
Material points ("PMAT" elements) may be used too, in order
to enter added masses (see page C.200).
1/ Thickness:
By means of this directive the user specifies the thickness
of two and threedimensional shells. A thickness must also
be specified
for elements of types Q92, Q93, Q92A, ED01, ED41, COQI, Q41, Q41N,
Q42, Q42N, Q41L, Q42L, Q95, CQD4, CQD9, CQD3, CQD6, FUN2, FUN3.
The directive is mandatory if the mesh contains any of these elements.
2/ Section:
This directive is similar to the preceding one, but
it is only applied to beams and bars.
< [ "EPAI" ( ep /LECTURE/ ) ; "EPAI" ( "CQDX" /LCHP/ /LECTURE/ ) ] > Or: < "SECT" ( ep /LECTURE/ ) >
Various thicknesses can be defined for different elements
without repeating the keyword "EPAI". It is the same for "SECT".
Example:
"EPAI" ep1 /LECTURE/ ep2 /LECTURE/ ep3 /LECTURE/
A special syntax is foreseen to define the thickness
of degenerated shell elements CQDx. For these elements, the
thickness should be defined at the nodes. The most accurate way
of doing this is to prepare a ’champoint’ object with CASTEM2000
and store it together with the mesh in the CASTEM2000 file
(see directive "SAUV’ in CASTEM2000). This file is then read
by EUROPLEXUS using the directive "CASTEM (see page A.30)
and can then be referred to from other directives.
The keyword "CQDX" introduces this kind of syntax: the
reference to the CASTEM2000 champoint object is read by the
/LCHP/ procedure (see page INT.57) and the associated
geometrical support (object of type ’maillage’ containing
the shell elements) is indicated by the following /LECT/.
Note that /LCHP/ and /LECT/ must be given in this order.
A simpler, but not as precise, way of specifying the thicknesses
of these shells is to assign a single value to each element
by the standard "EPAI" directive, without using the
CASTEM2000 objects for this purpose. In this case, the
program itself estimates values for the thicknesses
(and fiber orientations) at each node
based on the values of the surrounding
elements.
C.42
This directive allows to choose some geometrical parameters
for shell, plate and beam elements.
For example, the type of spatial integration through the thickness or
in the lamina directions, for certain types of shell/plate elements.
<"NGPZ" ngpz /LECT/ > <"INTE" typl /LECT/> <"ALPH" alpha /LECT/ > <"BETA" beta /LECT/> <"SK" sk /LECT/ > <"REFE" refe /LECT/>
The number of gauss points through the thickness for a sandwich element
is defined by COMP SAND NGPZ, see Page C.45.
Therefore, an additional COMP NGPZ for the same
element should be avoided.
The ‘mean tau’ procedure may be applied to CQD3, CQD4, CQD6, CQD9
degenerated shell elements.
However, it simply sets the transverse shear values to a
mean value, not to a linearly variable pattern. This is likely
to be too simplistic for the 9node element CQD9 (and also for
the 6node CQD6).
The parameter alpha is used to modify the bending coefficient
for the global shell models. The program will use the
following criterion:
sig* = SQRT (sigm ** 2 + (alph * sigf) ** 2)
In this formula, sig*, sigm and sigf represent the
Von Mises equivalent stress, the membrane stress and the bending
stress, respectively. By default, α=0.666 (i.e. 2/3) .
Of course, this parameter only makes sense for shell elements
that use a global model (i.e. which are not integrated through
the thickness).
Each of the above directives may be repeated as needed to associate appropriate
values of the parameters to each concerned element.
This (optional) directive allows to specify excentricity for
thick shell elements.
<"EXCE" exce /LECT/ >
For the moment, this feature concerns only T3GS and Q4GS shells [877].
C.45
To define sandwiches, each composed of several layers, for use with
some types of shell elements.
Each SAND directive defines a new sandwich composed of
several layers and associates it with a group of elements.
( "SAND" nl "FRAC" nl*fracl "NGPZ" nl*ngpzl /LECTURE/ )
For the moment, only the elements of type ED01, COQI,
CQD3, CQD4, CQD6 and CQD9 may be chosen to be multilayered sandwiches.
The directive SAND may be repeated as necessary
(by repeating each time also the SAND keyword itself) in order
to define all the geometrical information related to sandwiches.
There may e.g. be a sandwich (and therefore elements) with, say,
3 layers, and another (other elements) with,
say, 5 layers, in the same calculation.
Each sandwich stores all the geometrical information related to
the layered structure.
However, elements within the same sandwich may be made of
different materials (or material combinations in the various layers).
Remember to assign a material to each layer, see page C.750.
The total number of integration points through the
thickness of each element is defined by the sum of the ngpzl
values over the layers of its sandwich. This value should not exceed the
maximum value available for each element type. The value can be uncreased by using
DIME ... NGPZ.
The number of Gauss points through the thickness for each layer is defined
by ngpzl. Therefore, an additional COMP NGPZ
for the same elements should be avoided.
The set of sandwiches defined in the SAND directive(s) is stored
in an array. Each layer receives an index corresponding to its
definition order within the corresponding sandwich. This index is then used
in order to assign a material (see page C.1110)
or a set of orthotropy directions (see page C.97) to each layer.
For example, suppose that we define two sandwiches, the first with
3 layers and the second with 5 layers. The layers of the first sandwich
will be identified by indexes 1 to 3 while those of the second
sandwich by indexes 1 to 5. These are the indexes to be used
in successive directives to assign materials and/or orthotropy
characteristics to each layer within the corresponding sandwich
(i.e., within the associated element).
C.50
Description of the characteristics of beam elements.
There are four possible shapes:
 arbitrary section QUEL;
 rectangular section RECT;
 circular section CIRC;
 annular section (pipe) TUYA.
Moreover, in the case of pipes, it is possible to enter a
curvature in order to model the elbows.
For an example of use of the various cross sections see e.g. reference [650]. For an example of use of annular sections see also reference [714]. Finally, reference [719] gives an overview of pipelines.
"GEOP" [ "QUEL" "VX" vx "VY" vy "VZ" vz "AIRE" aire "IY" iy "IZ" iz "HY" hy "HZ" hz < "J" j > "R" r < "EXCE" ex > ; "RECT" "VX" vx "VY" vy "VZ" vz "AY" ay "AZ" az < "GAUC" gauch > < "J" j > < "EXCE" ex > ; "CIRC" "VX" vx "VY" vy "VZ" vz "DEXT" diam < "EXCE" ex > ; "TUYA" "VX" vx "VY" vy "VZ" vz "DEXT" diam "EP" ep <"COUR" co > < "RAYC" rayco > < "SFY" sfy "SFZ" sfz "SFT" sft > < "EXCE" ex > ; ] < "VMIS" "APRS" aprs "AMMB" ammb "ATRS" atrs "AFLX" aflx > /LECTURE/
A local reference system oxyz is attached to each beam element.
The origin o of the system is in node 1 of the element.
The second node (node 2) of the element then defines the
longitudinal direction of the beam, which is assumed to correspond
to the local x axis.
Then, to complete the definition of the local reference frame,
another direction corresponding to the local y axis must be specified.
This is done by giving a vector v (by means of its global
components vX, vY and vZ), which is located in the oxy plane
and completely defines this plane. Thus, the v vector may not
coincide with x. The length of the v vector is irrelevant
(but of course it may not be zero).
The y vector is then computed as the vector normal to x and lying in the
plane defined by x and v. Finally, the z vector is computed as the vector
normal to x and y.
In the case of an elbow, the vector v must be in the elbow plane
and directed to the inner side of the elbow, however it
is not compulsory that v is radial (directed
exactly towards the “center” of the elbow).
Bending around the y axis is therefore
outside the elbow plane, while bending around the z axis is
in the plane of the elbow.
In case of arbitrary cross section, the equivalent stress corresponding
to the moment around y (respectively z) is computed for a distance
h_{z} from the axis (respectively h_{y}) according to the following
formula:
σ_{y} = M_{y} 

In the other cases, the formula is identical but the distance h becomes:
In the case of torsion, it is again the same formula,
and the h distance is then:
In the case of a rectangular crosssection, it is possible to give
either a “gauchissement” coefficient allowing to compute the
torsional inertia starting from the inertia terms iy and iz,
or to give directly the torsional inertia j.
For a square cross section this “gauchissement” coefficient has the value 0.844.
The bending inertias are modified in the case of elbows in order to
account for the flexibility produced by the curvature as :
I_{coude} = I_{droit} / k 
where k is sfy, sfz or sft.
ATTENTION: these coefficients are associated with the parameters of the
von Mises criterion. A modification of the default values of sfy,
sfz and sft imposes a different set of input values
for aprs, ammb, atrs and aflx.
By default, these coefficients are computed as follows, according
to RCCMR 3644.31:
i) it is assumed that there is no change for the torsion (sft=1).
ii) it is also assumed that the flexibility is the same in the plane
sfy = sfz = k 
.
The coefficient k is a function of the elbow parameter λ ,
defined as follows: k = 1.65 / λ .
By definition, the elbow parameter λ is of the form :
λ = e R_{c} /R_{m}^{2} 
where e is the thickness and R_{m} the mean radius of the tube, and R_{c} the curvature radius of the elbow. In practice, EUROPLEXUS computes and prints the inverse of this value, that vanishes for a straight tube.
The used Von Mises criterion σ^{*} is of the form :
σ^{*} = √α_{p} P^{2} + α_{n} σ_{n}^{2} +
α_{t} σ_{t}^{2} + α_{f} σ_{f}^{2}
In this formula, coefficients α_{p}, α_{n},
α_{t} and α_{f} are respectively the parameters
aprs, ammb, atrs and aflx defined above.
By default, these coefficients assume the following values (which
are those for a pipeline):
α_{p} = 0.75 , α_{n} = 1 , α_{t} = 3 and
α_{f} = π^{2}/16 .
In the case of elbows, the coefficients α_{t} and α_{f} are modified. The default values are: α_{t} = 0.75 and α_{f} = ( γ π / 4 ) ^{2} .
The coefficient γ has the expression:
γ = max( 1 ; 8/9 λ^{−2/3} )
C.60
Diameters of the onedimensional elements "TUBE", "TUYA", "CL1D" and
"CLTU".
The elements "TUBE" and "TUYA" may be straight (constant diameter)
or conical, but the
elements "CL1D" et "CLTU" are always straight.
For practical reasons, there are always two diameters per element
(at the inlet and at the outlet, respectively).
"DIAM" $[ "ELAS" ; "ELAT" "EPAI" epai "YOUN" youn "NU" nu ]$ [ "DROI" d1 /LECTURE/ ; "CONE" "D1" d1 "D2" d2 "ORIG" /LECTURE/ "LIST" /LECTURE/ ]
If the element is straight: d1 = d2. If the element is
conical, d1 is different from d2.
If a conical pipe is composed of several elements, EUROPLEXUS
automatically computes the inlet and outlet diameters
of each of them.
If some friction (material PAROI) is associated to the fluid
material, only cones with a vertex angle α less
than 20 degrees are allowed.
In the last case, EUROPLEXUS computes the friction correction
factor C_{frot}, according to the formulas of IDEL’CIK
(diagram 5.2), where R is the ratio of the areas at
the inlet and outlet of the cone
(R < 1), and λ the loss coefficient for a straight tube:
C_{frot} = 
 ( 1 − R^{2} ) 
According to IDEL’CIK, the loss coefficients are then,
C_{div} for a divergent pipe and C_{conv} for a convergent
pipe (diagrams 3.7 and 5.2) :
C_{div}=C_{frot} + 3.2 tan(α) 
 (1 − R)^{2} 
C_{conv} = C_{frot} + 0.45 (1 − R) 
C.61
To define named groups of elements.
"GROU" ngro * ('nom_grou' [ /LECT/ ; STFL FLUI ; STFL CLXS ; DEBR ] <conditions> <"CENT" cx cy cz> <"SHRI" sh> <"SHFT" sx sy sz>)
Object names are not casesensitive: they are converted internally to uppercase before being used.
After their definition, group names may be used to specify in input
directives lists of
elements (or of the associated nodes), in exactly the same way
as GIBI object names
are, within a /LECT/ directive.
The set of nodes ‘associated’ with a group of elements is the
union of all nodes belonging to the elements in the group.
GIBI object names, or universal format groups or IDEAS groups
have the precedence over the present element groups, in case
they are present (and in case of homonimy).
Note that, if element groups are to be passed to the OpenGLbased
visualization module, they should preferably be disjoint, i.e.
such that each element belongs to (at most) one group.
This would ensure independence of rendering from the order in which
group selection/unselection operations are performed.
However, the code does not enforce this requirement, so that
the graphical results are under full control (and responsibility)
of the user.
The optional center, shrink and shift definitions may be used
e.g. to obtain special graphical rendering effects such as an
“exploded” view of a geometrical model. Be aware that the
code applies shrinkage by the chosen factor around the centerpoint
first, then followed by the chosen shift, if any.
Various types of conditions may be imposed. The first one
compares the position of the element’s barycenter to a given value.
Another one selects the (single) element whose barycenter is nearest
to a given node or point.
Other directives allow to identify all elements within a certain
geometric shape (a box, a sphere, a cylinder, a cone).
The last one allows to build up the complement (symmetric
difference) of the chosen object with respect to a second object.
(COND  $ XB ; YB ; ZB $ $ LT ; GT $ val   NEAR $ NODE /LECT/ ; POIN x y <z> $   BOX <X0 x0> <Y0 y0> <Z0 z0> DX dx DY dy <DZ dz>   SPHE <XC xc> <YC yc> <ZC zc> R r   CYLI <X1 x1> <Y1 y1> <Z1 z1> <X2 x2> <Y2 y2> <Z2 z2> R r   CONE <X1 x1> <Y1 y1> <Z1 z1> <X2 x2> <Y2 y2> <Z2 z2> R1 r1 R2 r2   COMP /LECT/ )
If any of the above coordinates (x0, y0 etc.) is omitted, it is assumed to be 0.
Suppose that we want to select all the elements of a 2D object
ob1 that lie in the first quadrant. The syntax would be:
COMP ... GROU 1 'firqua' LECT ob1 TERM COND XB GT 0 COND YB GT 0
The group is from now on accessible under the name firqua.
Suppose then that we want to do the same thing as in the
previous example, but also get access to the parts of ob1
in the other three quadrants, under the name others.
The syntax would be:
COMP ... GROU 2 'firqua' LECT ob1 TERM COND XB GT 0 COND YB GT 0 'others' LECT ob1 TERM COND COMP LECT firqua TERM
Note that the firqua object becomes available immediately
after its definition, and may therefore be used in the
definition of the others group.
C.62
To define named groups of nodes.
"NGRO" nngr * ('nom_grou' /LECT/ <conditions>)
Object names are not casesensitive: they are converted internally to uppercase before being used.
After their definition, group names may be used to specify
in input directives lists of
nodes (or of the associated elements), in exactly the same way
as GIBI object names
are, within a /LECT/ directive.
An element is considered ‘associated’ with a group of nodes if
and only if all its nodes belong to the group.
GIBI object names, or universal format groups or IDEAS groups
have the precedence over the present node groups, in case
they are present (and of homonimy).
Moreover, named groups of elements (see page C.61) also have
the precedence over the present node groups, in case
they are present (and of homonimy).
Note that, if node groups are to be passed to the OpenGLbased
visualization module, they should preferably be disjoint, i.e.
such that each node belongs to (at most) one group.
This would ensure independence of rendering from the order in which
group selection/unselection operations are performed.
However, the code does not enforce this requirement, so that
the graphical results are under full control (and responsibility)
of the user.
Various types of conditions may be imposed. The first one
compares the node position to a given value.
Other directives allow to identify all nodes within a certain
geometric shape (a box, a sphere, a cylinder, a cone).
The last one allows to build up the complement (symmetric
difference) of the chosen object with respect to a second object.
(COND  $ X ; Y ; Z $ $ LT ; GT $ val   NEAR $ NODE /LECT/ ; POIN x y <z> $   BOX <X0 x0> <Y0 y0> <Z0 z0> DX dx DY dy <DZ dz>   SPHE <XC xc> <YC yc> <ZC zc> R r   CYLI <X1 x1> <Y1 y1> <Z1 z1> <X2 x2> <Y2 y2> <Z2 z2> R r   CONE <X1 x1> <Y1 y1> <Z1 z1> <X2 x2> <Y2 y2> <Z2 z2> R1 r1 R2 r2   LINE X1 x1 Y1 y1 <Z1 z1> X2 x2 Y2 y2 <Z2 z2> TOL tol <DIST d>   COMP /LECT/ )
In 3D space, the line passing through 2 points P_{1}(x_{1},y_{1},z_{1}) and P_{2}(x_{2},y_{2},z_{2}) has the following parametric equations:
x = x_{1} + dx t, dx = x_{2}−x_{1} 
y = y_{1} + dy t, dy = y_{2}−y_{1} 
z = z_{1} + dz t, dz = z_{2}−z_{1} 
From each equation a value for t can be defined:
t_{x} = 

t_{y} = 

t_{z} = 

These 3 quantities are calculated for each point of the geometrical object to which the LINE condition is being applied and, if the 3 following conditions are satisfied, then the point is retained.
If any of the above coordinates (x0, y0 etc.) is omitted, it is assumed to be 0.
Suppose that we want to select all the nodes of a 2D object
ob1 that lie (strictly) within the first quadrant. The syntax would be:
COMP ... NGRO 1 'firqua' LECT ob1 TERM COND X GT 0 COND Y GT 0
The group is from now on accessible under the name firqua.
Suppose then that we want to do the same thing as in the
previous example, but also get access to the nodes of ob1
in the other three quadrants, under the name others.
The syntax would be:
COMP ... NGRO 2 'firqua' LECT ob1 TERM COND X GT 0 COND Y GT 0 'others' LECT ob1 TERM COND COMP LECT firqua TERM
Note that the firqua object becomes available immediately
after its definition, and may therefore be used in the
definition of the others group.
C.63
To define or redefine (e.g. in the case of a mesh generated by Cast3m)
the colors of elements, for visualization purposes.
"COUL" (nom_coul /LECT/)
Repeat as many times as necessary to define all the desired colors.
This directive is particularly useful in conjunction with the definition
of element groups (see GROU) to assign colors to groups
of elements.
If there are several colors to be defined, be sure not to
repeat the keyword COUL, but only the color name nom_coul
followed by the corresponding /LECT/.
In fact, each time the keyword COUL is encountered, all
colors defined so far are reset to the default color (black).
For example:
COUL roug LECT explosive TERM vert LECT structure TERM
is correct, while:
COUL roug LECT explosive TERM COUL vert LECT structure TERM
would be wrong (the explosive object would appear black and not red).
C.64
This directive allows to define values to used by a composite material
made by a RTM process ie. the CRTM material (page C264).
"RTMVF" vf /LECTURE/ "RTMRCT" rct /LECTURE/ "RTMANGL" angle /LECTURE/
C.65
Warning: the present model is under development at JRC and not all
the directives described below are available yet!
This directive sets some parameters used by the PFEM method.
PFEM H h ALPHA alpha
C.66
This directive allows to model flying debris resulting from an
explosion or an impact. Each piece of debris is modeled by a
particle, optionally embedded in the surrounding fluid and optionally
subjected to the gravity force. This latter force, if present,
must be specified via the CHAR CONS GRAV directive, see page F.30.
The fluid surrounding the debris particles may be modeled either as
a uniform field with constant properties (velocity, density), or
as an evolving fluid field, discretized by Finite Elements or
Finite Volumes, or even as a combination of the two (e.g., FE fluid field
near the explosive source, uniform field far away).
The debris particles may either be active from the very
beginning of the calculated transient (thus assuming that they result
from a fragmentation process that occurred at a previous time), or
they may be associated with certain finite elements representing a
structure, and be activated automatically by the code only when the
element undergoes complete failure.
In any case, since particles are represented by the specialized
DEBR elements, and since the topology is basically constant in time
in EUROPLEXUS, all particles must be declared
(and thus they are present in the model) from the beginning of the
calculation. However, some of them may be already active at the initial time,
some not.
The model includes the optional treatment of the impact of debris particles
against the surrounding structure. This is accomplished by the
pinball method.
DEBR <ROF rof> <VFX vfx> <VFY vfy> <VFZ vfz> <FLUI /LECT/ <DGRI> $[ HGRI hgri ; NMAX nmax ; DELE dele ]$ > (PART particle_description) (FILL fill_description)
Dimensioning for the flying debris cannot be made fully automatic, because of the FILL command which generates a variable number of particles depending upon which finite element type it is applied to and upon how many such elements will actually fail.
The number given in the dimensioning is the maximum number of debris particles that can be generated in the calculation. If the number given is not sufficient, the code will issue a warning message but the calculation will be continued (without generating any more debris particles). At the end of the run, the code will print out the exact number of particles needed (should the calculation be repeated).
The following twostep procedure is suggested:
In case of a calculation with domain decomposition (MPI), the dimensioning for the flying debris can assume two forms:
Debris particles may be subjected to the gravity force. This latter force, if present, must be specified via the CHAR CONS GRAV directive, see page F.30.
The drag force acting on a particle is
F_{d}=−C_{d}ρ_{f}Aw^{2}w/w,
where C_{d} is the particle’s drag coefficient (see below), ρ_{f} is
the fluid’s density, A=π /4d^{2} is the particle’s crosssection,
d is the particle’s diameter and w is the particle’s
velocity v relative to the fluid velocity v_{f}:
w=v−v_{f}.
The total number of particles described by the PART and FILL
subdirectives must be less than or equal to the number of elements
of type DEBR that has been reserved in the dimensioning
of the problem.
To describe a single particle of debris. The particle is already active
at the beginning of the transient calculation. Therefore, it results
from the fragmentation of a structure which has occurred at a previous time.
PART <X x> <Y y> <Z z> <VX vx> <VY vy> <VZ vz> RO ro D d DRAG drag <COUP> <IMPA> <TRAJ> <RISK>
To fill by debris particles an element or a mesh.
Particles are automatically generated uniformly within the volume
of the element or mesh (element by element). The particles inherit the
density of the parent element’s material when they are generated.
The particles may either: 1) be already active
at the beginning of the transient calculation (in this case they result
from the fragmentation of a structure which has occurred at a previous time),
or 2) be activated automatically by the code when the associated
element(s) undergo complete failure.
In case 1) above,
the associated element or mesh is defined at the geometric level only
as a geometric support for the particles generation. This element
or mesh bf must be associated with a FANT material so as to
exclude it from the transient computation. Assign to the FANT
material the desired density, which will be inherited by the generated
particles.
In case 2) above, the associated element or mesh must be assigned a
structural material with a failure model (thus not
the FANT material). When the element(s) fail, the
associated particles are suddenly activated while at the same time
the element is deactivated, so it no longer contributes to the model.
FILL $<VX vx> <VY vy> <VZ vz> ; <VR vr <CX cx> <CY cy> <CZ cz>>$ PLEV plev DRAG drag <AFLY afly> <COUP> <IMPA> <TRAJ> <RISK <MACR <RMAC rmac>>> OBJE /LECT/
The initial velocity of each group of particles defined by the
FILL directive described above may be defined in two ways:
C.67
This directive allows to define an erosion (failure) criterion,
which uses a maximum displacement of a given node.
The model can be used for calculations of laminated windows. The criterion of the complete erosion of a laminated window can be set to 30% of the span.
The model can be combined with any other erosion criterion.
FAIL ( DISP disp NODE /LECT/ OBJE /LECT/ ) ( AUTO rati DIRE disp /LECT/ )
The set of keywords DISP ... OBJE may be repeated
as many times as needed to define all the desired
displacementbased erosion criteria.
C.68
This directive allows to define a structured, Eulerian fluid grid
consisting of either Finite Elements (FE) or of
Cell Centred Finite Volumes (VFCC)
that is added to the mesh specified in the GEOM directive.
The grid has the form of a rectangular parallelepiped, is aligned along
the global axes, and has a uniform spacing in each
of the three global directions.
Using a structured fluid grid may substantially speed up the
numerical calculations because many operations (especially
those related to searching) can be highly optimized.
In particular, this model is useful in conjunction with
the FLSR model for fluidstructure interaction,
see page D.143, in the case of fluid FE, or with the
FLSW model, see page D.555, in the case of fluid VFCC.
If FE are chosen for the fluid,
special fluid elements of type FL2S (in 2D) or FL3S (in 3D) are
automatically built up and used to discretize the structured grid.
The former is a simplified version of FL24 while the latter is a
simplified version of FL38.
If VFCC are chosen for the fluid,
fluid volumes of type Q4VF (in 2D) or CUVF (in 3D) are
automatically built up and used to discretize the structured grid.
All nodes of the structured fluid grid (which are also
generated automatically) must be declared Eulerian
in the GRIL directive, see page B.60. Note that nodes not
mentioned in the GRIL directive are indeed considered Eulerian.
This directive may only be used in ALE or purely Eulerian calculations.
In addition to the fluid elements (or volumes),
special boundary condition elements of type CL2S (in 2D) or CL3S (in 3D)
(for the FE fluid case)
or of type CL2D (in 2D) or CL3D (in 3D) (for the fluid VFCC case)
may be optionally generated along the appropriate faces
of the fluid domain (see CLij input directives below).
These may be used, for example, to specify
absorbing boundary conditions.
STFL <VFCC> X0 x0 Y0 y0 <Z0 z0> LX lx LY ly <LZ lz> NX nx NY ny <NZ nz> <CLX1> <CLX2> <CLY1> <CLY2> <CLZ1> <CLZ2>
Each cell (element) of the grid is a rectangle
(rectangular parallelepiped in 3D)
with sides of length l_{x}/n_{x}, l_{y}/n_{y} (and l_{z}/n_{z} in 3D).
Nodes and elements in the grid are numbered progressively
starting from the chosen origin (x_{0}, y_{0}, z_{0}),
first along the global Xdirection,
then along the Ydirection (in 3D, finally along the Zdirection).
Once the additional elements and nodes have been generated by
the STFL directive, they are considered like any other
elements and nodes, in particular as concerns the rest of the input
file and the postprocessing.
Appropriate materials must be assigned, in the usual way, to all
the automatically generated elements. For example, a lowpressure
gas to all fluid elements except those in a bubble zone,
representing an explosion, in which a highpressure gas is assigned.
In order to identify the concerned elements, use may be made
e.g. of directives for the definition of element groups,
see page C.61. A special command to choose the STFL elements is provided,
see STFL FLUI or STFL CLXS on page C.61.
In the frequent case of absorbing boundaries of the fluid domain,
the concerned CL2S/CL2D or CL3S/CL3D elements must be identified in order
to assign an adequate impedance material to them.
The rule for automatic numbering of the generated elements is as follows:
first, all fluid elements are generated (their number may be computed
as specified above). Next, any specified CL2S/CL2D or CL3S/CL3D
elements are generated,
in the following order: CLX1, CLX2, CLY1, CLY2,
CLZ1, CLZ2.
Appropriate boundary conditions may also be specified
(e.g. via LINK) at the boundary nodes (e.g.
to block a certain face of the fluid domain).
The STFL directive requires no dimensioning since the code is able
to determine the number of necessary nodes and elements automatically.
The directive is also compatible with fluid mesh adaptivity (ADAP).
For example, the user may activate FSIdriven fluid mesh adaptivity via the
FLSR or FLSW directives by specifying as fluid domain
a domain generated by STFL. See pages D.143 and D.555, respectively,
for more information.
C.68b
This directive allows to automatically generate a Spectral Element (SE)
“micro” mesh starting from an SE “macro” mesh and a given degree (N)
of the interpolation polynomial. The degree of the polynomial is
the same for all spectral elements, and along each of the spatial
directions.
The “macro” spectral element mesh is composed of
either MS24 4node quadrilateral elements (in 2D) or of MS38 8node
hexahedral elements (in 3D), and must have been specified
in the previous GEOM directive. The generated micro SE mesh will be
composed of S24 4node quadrilaterals in 2D or of S38 8node hexahedra
in 3D.
SPEC GMIC NSPE nspe
Each macro SE generates exactly N^{2} micro SE in 2D or N^{3} micro SE in 3D.
The number of micro SE nodes generated is roughly (by excess)
(N+1)^{2} in 2D or (N+1)^{3} in 3D, for each macro SE.
The exact number of generated nodes is difficult to determine a priori
because it depends upon the connectivity of the macro SE mesh
(coincident nodes of adjacent micro SE and coincident nodes of
micro and macro SE are eliminated).
After the calculation of the exact number of nodes (and elements)
required, the code prints out this information in case the user
wants to keep the memory to a minimum (by giving minimum dimensioning
commands).
The generated micro SE are available in an automatically created element
group named _S24 if the calculation is 2D, or _S38
if the calculation is 3D.
Note that, like for other directives which change the mesh topology
(by adding new elements and new nodes), the dimensioning related
to geometrical data cannot be fully automatic. The user must
in this case dimension the total number of nodes, the total number of
degrees of freedom and the total number of micro SE generated
elements (S24 in 2D or S38 in 3D), like in the following example:
. . . DIME NPOI 9 NDDL 18 S24 4 TERM . . . GEOM . . . COMP SPEC GMIC NSPE 2 . . .
C.69
This directive allows to define an erosion criterion
for a specific subset only of the elements. A global definition of the
erosion criterion is given in the definition of the problem (see
directive EROS <ldam> on GBA_0030)).
The global value given there can be overridden for
one or more subsets of the elements by using the present directive.
EROS $[ eros ; NOER ]$ /LECT/
The set of keywords EROS ... /LECT/ may be repeated
as many times as needed to define all the desired
elementbased erosion criteria.
To orient or reorient those elements of the mesh for
which a specific orientation is important. Typically, these
are 3D shell elements without a topological thickness.
Normally, proper orientation should be done in the mesh generator,
but the present directive may be useful to correct any
problems in case one uses a mesh whose generator is not available.
This subdirective should be used only in emergency cases,
e.g. when the mesh used in a calculation (especially flat 3D shell
elements) has the wrong orientation and comes from a mesh generator
that is not available. This command has the last word on the orientation
of the elements, since it comes after the automatic
reorientation which is done in the SENS routine (called from the
geometry reading routine). The user is therefore fully responsible
of the use of this command.
"ORIE" < "OBJE" /LEC1/ $[ "POIN" x y z ; "NODE" /LECN/ ]$ > < "INVE" /LEC2/ >
Only some element types admit reorienting: typically, these
are 3node or 4node “thin” elements in 3D, such as
shell, membrane or CLxx elements.
Note that the ORIE subdirective may be repeated any
number of times, if needed.
For example, this may be useful to reorient a randomly oriented
closed surface so that it points outwards. Use a first ORIE
subdirective to orient the all the surface elements consistently towards
an internal point (e.g. its barycenter).
Then, use a second ORIE subdirective to invert the orientation:
COMP ... ORIE OBJE LECT toto TERM POIN x y z ORIE INVE LECT toto TERM
C.72
To generate automatically SPH particles within userdefined volumes.
"GBIL" ngen * (RBIL r <RESE rese> (INSI  BOX <X0 x0> <Y0 y0> <Z0 z0> DX dx DY dy <DZ dz>   SPHE <XC xc> <YC yc> <ZC zc> R r   CYLI <X1 x1> <Y1 y1> <Z1 z1> <X2 x2> <Y2 y2> <Z2 z2> R r   CONE <X1 x1> <Y1 y1> <Z1 z1> <X2 x2> <Y2 y2> <Z2 z2> R1 r1 R2 r2   MESH /LECT/ ) (OUTS  BOX <X0 x0> <Y0 y0> <Z0 z0> DX dx DY dy <DZ dz>   SPHE <XC xc> <YC yc> <ZC zc> R r   CYLI <X1 x1> <Y1 y1> <Z1 z1> <X2 x2> <Y2 y2> <Z2 z2> R r   CONE <X1 x1> <Y1 y1> <Z1 z1> <X2 x2> <Y2 y2> <Z2 z2> R1 r1 R2 r2   MESH /LECT/ ))
If any of the above coordinates (x0, y0 etc.) is omitted, it is assumed to be 0.
Suppose that we want to generate SPH particles within a cylinder
representing a pipe full of fluid. Then the syntax would be simply:
GBIL 1 RBIL 0.001 INSI CYLI X0 0 Y0 0 Z0 0 X1 0 Y1 0 Z1 10 R 0.1
The group of particles is from now on accessible
under the name _gbil001.
Suppose then that the pipe of the previous example
is submerged in the sea. To generate also the particles in a prismatic sea
region around the pipe, the syntax would be:
GBIL 2 RBIL 0.001 INSI CYLI X0 0 Y0 0 Z0 0 X1 0 Y1 0 Z1 10 R 0.1 RBIL 0.001 INSI BOX X0 1 Y0 1 Z0 0 DX 2 DY 2 DZ 10 OUTS CYLI X0 0 Y0 0 Z0 0 X1 0 Y1 0 Z1 10 R 0.1
The two group of particles are from now on accessible
under the names _gbil001 and _gbil002, respectively.
The presence of the (mandatory) RBIL keyword starts a
new group of particles. Each group must contain at least one
INSI condition. All INSI conditions must be
specified before the OUTS conditions (if any).
C.74
These directives create tables containing the physical properties of water, according to one of the following textbooks:
1) Directive "TEAU" : Properties of water and steam in SI  units
(E.Schmidt Springer Verlag, Berlin 1979)
or
2) Directive "TH2O" (letter O) : NBS/NRC Steam Tables 1984
(Extended tables)
$[ "TEAU" ; "TH2O" ]$ "TMIN" tmin "TMAX" tmax "PMIN" pmin "PMAX" pmax "UNIL" cl "UNIM" cm "DBTE" nbte "DSAT" nsat "DHTE" nhte < "DPHY" nhy > For the tests: < "DESS" > < "PERF" > < "TEST" ( "CAS" ... ) "FINT" > With : "CAS" num "P1" p1 $ "T1" t1 ; "X1" x1 $ $ "P2" p2 $ "T2" t2 ; "X2" x2 $ $ $ "DVS" dvs "DH" dh $
For the tests:
nbr
is a simple identification number.
If one intends just to run a test without a real EUROPLEXUS transient calculation, it is preferable to put the keyword "FIN" immediately after the directive "COMPLEMENT". This test is recommended, because it allows to verify the initial conditions (pressure, temperature, void fraction) and to check the composition of the tables.
A portion of the saturation curve must be included in the PressureTemperature domain chosen.
The nbte
temperature intervals start from the minimum water temperature
to the saturation temperature (for the minimum pressure).
It is the same for the nhte
intervals
between the saturation temperature and the maximum temperature,
for the maximum pressure.
The nsat
pressure intervals lie
between minimum pressure and maximum pressure, if this is in the
subcritic domain ; else, they go from the minimum pressure to
the critical pressure.
In the case of a maximum pressure above 221 bars (hypercritic domain),
a further parameter is needed : the number nhy
of intervals
between the critical pressure and the maximum pressure.
For low temperatures ("DBTE"), the subdivision is linear in the
temperature. Along the saturation curve ("DSAT"),
the subdivision is initially linear in the temperature, then linear
in the pressure, in order to obtain a regular subdivision
along this curve. Beyond the critical point ("DHTE" and "DPHY"),
the subdivison is logarithmic in temperature and in pressure.
When the "TEAU" directive is used, the pressure must be
between 0.0062 bar and 1000 bar, and the temperature
between 0 and 800 degrees Celsius.
If the extended tables are used (directive "TH2O"), the pressure
must be between 0.0062 bar and 30000 bar, and the temperature
between 0 and 2000 degrees Celsius.
If the user enters his data in the SI unit system, it is
cl=cm=1. Otherwise, cl or cm represent the value
of the SI unit expressed in the user’s unit. For example,
if the lengths are in mm, then cl=1000.
C.75
These directives create tables containing the physical properties of helium, according to CEA/IRF/DPC (1985).
"THEL" "UNIL" cl "UNIM" cm For the tests: < "TEST" <"DETA" > ( "CAS" ... ) "FINT" > With : "CAS" num "P1" p1 $ "T1" t1 ; "X1" x1 $ $ "P2" p2 $ "T2" t2 ; "X2" x2 $ $ $ "DVS" dvs "DH" dh $
For the tests:
nbr
is a simple identification number.
If one intends just to run a test without a real EUROPLEXUS transient calculation, it is preferable to put the keyword "FIN" immediately after the directive "COMPLEMENT". This test is recommended, because it allows to verify the initial conditions (pressure, temperature, void fraction).
The pressure must be above 0.042 bar, and the temperature above 2.1 Kelvin.
The critical point of helium is at 2.27 bars and 5.19 Kelvin.
Beyond these values there is only one phase.
Only the gas and the liquid are considered. In the case of
high pressures and very low temperatures, the latter must be
higher tan the melting temperature: solid → liquid.
Unlike the water tables (page C.74), the thermodynamic parameters
of helium are directly calculated starting from the interpolation
polynomials. Therefore, calculations may at times become
very timeconsuming.
If the user enters his data in the SI unit system, it is
cl=cm=1. Otherwise, cl or cm represent the value
of the SI unit expressed in the user’s unit. For example,
if the lengths are in mm, then cl=1000.
Join together different branches of a pipeline.
"RACC" [ "BIFU" ; "CAVI" ; "BREC" ] $[ n1 ... nk ; "LECT" racname "TERM" "LECT" P1 ....PK "TERM" ]$ .... "DSOR" d1...dk < "VOLU" v >
One may distinguish two cases:
"BIFU" or "BREC" : bifurcation with a small volume (acoustic continuity)
"CAVI" : cavity with a large volume (with a law describing its behaviour)
In the case of a bifurcation or a pipeline rupture, EUROPLEXUS recomputes
a fictitious volume, which corresponds to the sphere having the same area as
the sum of the areas of the branches that arrive at
the bifurcation.
The exact number of junction elements must be specified in the
"GEOM" directive (see page B.30), and the order of junctions is the
same as in the "GEOM" directive if GIBI is not used.
Example:
"GEOM" . . . "CAVI" 2 "BIFU" 1 "BREC" 1 "TERM"
corresponds to:
"CAVI" .... ) 2 cavities "CAVI" .... ) "BIFU" ......... 1 bifurcation "BREC" ......... 1 pipeline rupture
If GIBI is used, the number of junction elements specified may be
larger than the exact number, and the order is not compulsory,
because the name of each junction is specified in the directive.
Example:
"GEOM" ... "CAVI" cav_one "CAVI" cav_two "BIFU" my_bif "BREC" my_bre ..."TERM"
corresponds to (in the RACC directive) :
"CAVI" "LECT" cav_one "TERM" "LECT" P1 "TERM" .... "CAVI" "LECT" cav_two "TERM" "LECT" P2 P3 "TERM" .... "BIFU" "LECT" my_bif "TERM" "LECT" P4 P5 P6 "TERM" .... "BREC" "LECT" my_bre "TERM" "LECT" P7 P8 "TERM" ....
C.90
To connect, by means of a "TUBM" element, a pipeline
meshed in 1D with a fluid meshed in 3D.
"RACC" ( "TUBM" /LECTURE/ "NTUB" /LECTURE/ "DTUB" dtub ... "FACE" /LECTURE/ "COEF" coef )
These elements are created by CASTEM, by means of the following syntax:
mon_tubm = MANU SUPERELEMENT (p_tube ET s_face) ;
where p_tube
is the object corresponding to the 1D point,
and s_face
the object corresponding to the nodes of the 3D face.
All nodes of the 3D face must be coplanar.
In case of a mesh in the MED format, in which the SUPERELEMENT
structure does not exist, the required procedure is the following:
"raccord"
, to which the suffixes "_n"
and "_s"
must respectively be added.
"splm_raccord"
.
It is automatically created when a TUBM element is declared.
"TUBM" connects the fluid of the continuum elements (3D) with the
fluid of a "TUBE" element (continuity of the mass flow rate).
The velocities of nodes belonging to the 3D face are all
equal and normal to the face itself.
The type of elements whose face(s) participate in forming the
3D face is irrelevant: therefore it is possible to use
cubes, prisms or even tetrahedrons for the mesh.
A material must be associated to the "TUBM" element, although this
has no behaviour law.
It is mandatory to specify in the dimensioning the parameter
"JONC", in order to reserve the space indispensable
for the relations associated to the junction (see page A.80).
Do not forget to mention "TUBM" also in the "LIAISON" directive
(page D.200).
C.91
To connect, by means of a "TUYM" element, a pipeline
meshed ("TUYA" element) in 1D with a fluid meshed in 3D
for moving meshes (A.L.E computation).
"RACC" ( "TUYM" /LECTURE/ "NTUB" /LECTURE/ "DTUB" dtub ... "FACE" /LECTURE/ "COEF" coef )
These elements are created by CASTEM, by means of the following syntax:
mon_tuym = MANU SUPERELEMENT (p_tuya ET s_face) ;
where p_tuya
is the object corresponding to the 1D point,
and s_face
the object corresponding to the nodes of the 3D face.
All nodes of the 3D face must be coplanar.
In case of a mesh in the MED format, in which the SUPERELEMENT
structure does not exist, the required procedure is the following :
"raccord"
, to which the suffixes "_n"
and "_s"
must respectively be added.
"splm_raccord"
.
It is automatically created when a TUYM element is declared.
"TUYM" connects the fluid of the continuum elements (3D) with the
fluid of a "TUYA" element (continuity of the mass flow rate).
The velocities of nodes belonging to the 3D face are all
equal and normal to the face itself.
The type of elements whose face(s) participate in forming the
3D face is irrelevant: therefore it is possible to use
cubes, prisms or even tetrahedrons for the mesh.
A material must be associated to the "TUYM" element, although this
has no behaviour law.
It is mandatory to specify in the dimensioning the parameter
"JONC", in order to reserve the space indispensable
for the relations associated to the junction (see page A.80).
Do not forget to mention "TUYM" also in the "LIAISON" directive
(page D.200).
C.92
The purpose of this directive is to define a onetoone correspondence
between couples of nodes.
This userdefined correspondence may be useful in various situations,
in which the code needs to find a onetoone correspondence between
nodes in the mesh and the automatic determination of such a correspondence
is impossible. For example, this might happen under exceptional circumstances
in the following cases:
In such cases, the code tries to automatically determine the structural (or other Lagrangian) node “corresponding” to a certain fluid node. This node is defined as the Lagrangian node having the same initial coordinates as the fluid node under consideration, within a certain small tolerance (that may be changed via the OPTI TOLC, page H.40). If there is no such node or if more than one candidate node is found (e.g. because there are several superposed structures in the mesh), then the automatic search would fail. In this case, the user may assume control by explicitly specifying the corresponding Lagrangian node to each “ambiguous” fluid node.
It is advised to use this directive only in case of necessity.
First, an input without this directive should be prepared. Then,
in case the code produces some error messages related to the
impossibility of automatically determining the node correspondence,
the present directive may be added to resolve the identified conflicts.
"CNOD" "NODF" /LECT1/ "NODS" /LECT2/
The order in which nodes are listed in /LECT1 or /LECT2 is
retained. To the ith node of /LECT1 corresponds the ith
node of /LECT2. The number of nodes in /LECT1 and /LECT2
must be the same.
Note that the directive CNOD may be specified only once
in each calculation (i.e. it should not be repeated).
In other words, all correspondent nodes should be specified in
just one /LECT1/ and /LECT2/.
In case of problems with the FSA directive, please note that another
way of resolving node conflicts, alternative to
the present CNOD directive, is the STRU subdirective
of FSA, see page D.450, which is more practical
in case there is a large number of conflicting nodes.
C.93
This instruction introduces characteristics for the SPH shell elements (SPHC)
which allow discretizing shell structures with a single layer of particles.
"CSPH" "RAYO" rbille "EPAI" ep "ORX" orx "ORY" ory "ORZ" orz < "LINE" cl > < "QUAD" cq > < "RLIM" rlim > < "RESEAU" ires > < "VOIS" nvoi > ( "STRP" istrp /LECT/ )
For the quadratic damping, it is advised to take
cq=4.
To damp out the highfrequency oscillations it is advisable to use
a value of cl between 0.1 and 0.5.
At least one set of stress points must be entered. Several sets can be entered
by repeating the STRP keyword.
Two types of particle lattice are possible: for ires = 1 a cubic
lattice is adopted; in the case ires = 0 (default value), a
compact hexagonal lattice is adopted.
The number of sought neighbouring particles is by default 12.
This number may not be changed for the PEF algorithm.
Its modification is accepted only for the SPH method.
For a given particle, the search considers the neighbours
whose center is within a distance of rlim*rbille from its center.
By default, rlim=1.3.
C.94
This instruction is mandatory in the input file when using discrete elements (ELDI).
It allows printing out to the output listing the value of the radius of each
discrete element and to impose the correct masses of different parts of the
discrete element model (element density will be corrected).
This directive is used to define a bridging (recovering) zone allowing to couple a set of discrete elements (ELDI) with a 3D finite element model (meshed with the CUB8 elements only) or a shell model (Q4GS elements only).
"CELDI" < "IMPR" > < "MASS" nval nval*(val /LECTURE/ ) > < "ARMA" /LECTURE/ > < "LTM" nbse nbse*(beta plas /LECTURE/) > "TYPL" nbtypl*([ "COHE" <"IMPR"> <"COEF" val> /LECTURE/ ; "BIMA" <"IMPR"> "MAT1" <"COEF" val> /LECTURE/ "MAT2" <"COEF" val> /LECTURE/ ; "CONT" <"IMPR"> <"COEF" val> /LECTURE/ ] ) < "CSTE" coef > < "EDEF" nbcoup nbcoup*("NCOU" ncouches "ELDI" /LECTURE/ "FRON" /LECTURE/ ) > < "CBOX" xmin xmax ymin ymax zmin zmax >
To guarantee the masses of different parts of the discrete
element model are correct, each discrete element should belong to
one group only.
To identify the interacting neighbors, a grid subdivision method
is used.
An interaction between elements a and b of radius R^{a} and R^{b}
respectively, is defined within an interaction range val and does not
necessarily imply that two elements are in contact (for cohesive interactions).
Then, these elements will interact if,
val * (R^{a} +R^{b}) > or = D^{a,b}
where D^{a,b} is the distance between the centroids of element a and b
and where val is the interaction range. val is mandatory and must be
> or = 1.
C.95
The characteristics of CMC3 elements are described when they
have not been defined by CASTEM2000.
"CORTHO" "EPAISSEUR" ep "EXCENTREMENT" ex $[ "ANGLE" angle ; "VECTEUR" vx vy vz ]$ /LECTURE/
The sign of the excentricity is defined by the orientation
of the normal. This depends on the numbering
of the nodes of the CMC3
element (see Maxwell’s corkscrew rule).
The first side of the element is the one formed by the first 2 nodes.
C.96
Description of the orthothropy directions for continuum elements
in 2D and 3D.
"MORTHO" $[ "ALPHA" angle1 ; "TETHA" angle2 ; "AXE1" e11 e12 e13 "AXE2" e21 e22 e23 ; "COCY" "POINT" $[ /LECTURE1/ ; xx yy zz ]$ "VECT" v1 v2 v3 ; "V1LC" v1x v2x v3x "V2LC" v2x v2y v2z ]$ /LECTURE/
One can define several orthotropy directions by repeating
each time the keyword MORT.
It is also possible to repeat it starting from different items.
The ALPHA or TETHA keywords are used in 2D,
the AXE1 ... AXE2
or COCY directive are used in 3D.
The vectors V1(e11,e12,e13 or v1x,v1y,v1z) and
V2(e21,e22,e23 or v1x,v1y,v1z) are not necessarily unit vectors,
and V2 is not necessarily normal to V1.
Starting from these input data, EUROPLEXUS computes and stores
the values in the local reference frames relatives to each element.
These local values will be utilised during the transient calculation.
For this reason, the calculation remains valid also for large
rotations.
C.97
Description of the orthotropy characteristics for 3D (layered)
shell elements using JRC’s “sandwiches” and “layers” model
(see SAND and LAYE keywords).
The directive defines the orthotropy characteristics related to the following material types: HILL (3), ORTS (46), ORPE (55), COMM (88), GLRC (92), and to the following element types: QPPS (35), COQI (40), T3GS (51), DST3 (83), DKT3 (84), CQD4 (91), CQD9 (92), CQD3 (93), CQD6 (94), Q4GR (111), Q4GS (112), Q4MC (138), T3MC (139).
The othotropy characteristics are stored in the ECR() table of each GP of each concerned element. If the element has layers (LAYE directive) then the characteristics may vary from layer to layer. Here is how the characteristics are stored, for each material type:
HILL (3) ! ECR(8) = ANGLE ORTS (46) ! ECR(3) = ANGLE ORPE (55) ! ECR(21) = ANGLE COMM (88) ! ECR(6:8) = VX, VY, VZ GLRC (92) ! ECR(11:13) = VX, VY, VZ
Note that the GLRC material may not be associated with a layer because this is a global material model.
For historical reasons, two alternative input syntaxes can be used:
"ORTS" [ vx vy vz ; $[ "ANGL" alpha ; "AXE1" a1x a1y a1z ]$ ] /LECT/ < "LAYE" /LECT_LAY/>
Note that the directive COMP ORTS must be specified
after the definition of the material characteristics
(MATE directive). If other quantities (e.g. thickness, etc.)
are to be specified via the COMP directive, then two COMP
directives should be used: the first one, immediately after
the GEOM directive, and the second one (COMP ORTS)
immediately after the MATE directive.
C.99
Description of the characteristics of the BILLE element
(particle element).
"CBILLE" "RAYON" rbille < "LINEAIRE" cl > ... ... < "QUADRATIQUE" cq > < "RESEAU" ires > ... ... < "VOISIN" nvoi > ... < "RLIM" rlim >
For the quadratic damping, it is advised to take
cq=4.
To damp out the highfrequency oscillations it is advisable to use
a value of cl between 0.1 and 0.5.
Two types of particle lattice are possible: for ires = 1 a cubic
lattice is adopted; in the case ires = 0 (default value), a
compact hexagonal lattice is adopted.
The number of sought neighbouring particles is by default 12.
This number may not be changed for the PEF algorithm.
Its modification is accepted only for the SPH method.
For a given particle, the search considers the neighbours
whose center is within a distance of rlim*Diameter from its center.
By default, rlim=1.3.
C.99B
To define one or more rigid (nondeformable) bodies.
The geometrical characteristics of each rigid body are specified here.
The material characteristics (basically, the density) are specified
by assigning to each rigid body a RIGI (rigid) material,
see Page C.295.
RIGI nrigi * ( <MASS mass <MTOT mtot> > <BARY bary <GX gx GY gy <GZ gz>> > <INER iner <JXX jxx JYY jyy JZZ jzz JYZ jyz JXZ jxz JXY jxy> > /LECT/ )
The elements belonging to a rigid body must be assigned a rigid (RIGI) material, which is used to define the density of the rigid body and thus to compute the mass, the barycenter and the inertia moments of the body (unless they are specified by the user).
Only elements belonging to a rigid body RIGI can be assigned a rigid material RIGI.
A named elements group _RIGI<nnn> is automatically created for each rigid body. The <nnn> is the rigid body index (001, 002, ..., nrigi) in the order of definition of the rigid bodies. Each group contains only one element and only one node: the “lumped” element and the “lumped” node that represent the rigid body as a whole. These names can be used to apply external loads, boundary conditions, etc., to a rigid body as a whole.