Previous Up Next

6  GROUP C—GEOMETRIC COMPLEMENTS

C.10


Object:


These directives enable the user to complete the geometry.


Syntax:
    "COMPLEMENT"

Comments:


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 1-D elements) or if the user enters added masses.


Do not forget the corresponding dimensioning (page A.70).

6.1  AUXILIARY FILE

C.25


Object :


This directive allows to read complementary data from an auxiliary file.


Syntax :

    < "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".

6.2  ADDED MASSES

C.30


Object:


This instruction enables the user to define the masses which are added to certain nodes, along certain degrees of freedom.


Syntax:
    <  "MASS"  (  /LECDDL/   xm  /LECTURE/  )  >


LECDDL

List of the degrees of freedom concerned.
xm

Value of the added mass.
LECTURE

List of the nodes concerned.

Comments:


1/ Several added masses may be defined without repeating the key-word "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.


Remark:


Material points ("PMAT" elements) may be used too, in order to enter added masses (see page C.200).

6.3  THICKNESS OR SECTION

C.40


Object:


1/ Thickness:


By means of this directive the user specifies the thickness of two- and three-dimensional 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.


Syntax:

    < |[ "EPAI"  (  ep   /LECTURE/  )           ;
         "EPAI"  (  "CQDX" /LCHP/ /LECTURE/  )  ]| >

Or:

    <  "SECT"  (  ep   /LECTURE/  )  >


ep

Thickness or section.
LECTURE

List of the elements concerned.

Comments:


Various thicknesses can be defined for different elements without repeating the key-word "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.

6.4  GEOMETRICAL PARAMETERS FOR SHELL ELEMENTS

C.42


Object:


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.


Syntax:

   <"NGPZ" ngpz  /LECT/ > <"INTE" typl /LECT/>
   <"ALPH" alpha /LECT/ > <"BETA" beta /LECT/>
   <"SK"   sk    /LECT/ > <"REFE" refe /LECT/>


ngpz

Number of gauss points in the thickness for shell, plate or beam elements. This value must not exceed the maximum value specified in the dimensioning (see DIME ... NGPZ on page A.66). The default value for the CQDx elements is 3.
typl

Type of lamina integration for 3D degenerated shell elements (CQD3, CQD4, CQD6, CQD9), SELE means selective reduced, REDU means reduced, FULL means full, SELM means selectively reduced with ‘mean tau’ procedure and FULM means full with ‘mean tau’ procedure; the default is reduced.
alpha

Participation to bending (only for some shell elements). Default is 2/3. This parameter is only used by elements which adopt a global model: elements integrated through the thickness ignore the value of this parameter.
beta

Participation to membrane (only for some shell elements). Default is 1. This parameter is only used by elements which adopt a global model: elements integrated through the thickness ignore the value of this parameter.
sk

Shear correction factor for 3D degenerated shell elements (CQD3, CQD4, CQD6, CQD9), default value is 5/6.
refe

Location of the reference surface. refe = -1, 0, +1 indicates that the surface is located at the bottom, middle, and top surface of the shell, respectively. The shell element is moved in the positive direction of the element normal.
/LECT/

List of the concerned elements.

Comments:


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 9-node element CQD9 (and also for the 6-node 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.

6.5  EXCENTRICITY FOR SHELL ELEMENTS

C.44


Object:


This (optional) directive allows to specify excentricity for thick shell elements.


Syntax:

   <"EXCE" exce  /LECT/ >


exce

Distance between the shell mean surface and the reference surface used in the calculation. The default value is 0 (no excentricity).
/LECT/

List of the elements concerned.

Comments:


For the moment, this feature concerns only T3GS and Q4GS shells [877].

6.6  SANDWICHES AND LAYERS

C.45


Object:


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.


Syntax:

      ( "SAND"   nl "FRAC" nl*fracl "NGPZ" nl*ngpzl  /LECTURE/  )


nl

Number of layers in the sandwich, which is associated with each of the elements given in the following /LECT/.
fracl

Thickness fraction of each layer: this is the ratio of the layer thickness to the total thickness of the element.
ngpzl

Number of integration points through the thickness in each layer.
LECTURE

Elements concerned.

Comments:


For the moment, only the elements of type ED01, COQI, CQD3, CQD4, CQD6 and CQD9 may be chosen to be multi-layered 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).

6.7  GEOMETRY OF BEAMS

C.50


Object:


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.


References:

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.


Syntax:

       "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/


vx vy vz

Global coordinates X, Y, Z of a vector v defining the local system (oxyz), see comments below.
aire

Area of the cross section of the beam.
iy iz

Bending inertias around the local axes y and z.
hy

Distance along y used to estimate an “equivalent bending stress” around the local axis z.
hz

Distance along z used to estimate an “equivalent bending stress” around the local axis y.
j

Torsional inertia, if different from iy+iz.
r

Distance used to estimate an “equivalent torsional stress”.
ex

Excentricity along y (optional).
ay az

Length of the sides for a rectangular beam section (along y and z, respectively)
diam

External diameter for a beam with a circular section or for a pipe.
ep

Thickness of the pipe making up the beam.
co

Curvature of the elbows. It is the inverse of the curvature radius. In the case of a straight pipe: co = 0.0 This curvature radius stays constant during a calculation.
rayco

Curvature radius for the elbows. It is infinite for straight pipes.
sfy sfz sft

Coefficients of “surflexion” of the elbow: in the elbow plane (sfy), out of the plane (sfz) and in torsion (sft). The moment of inertia corresponding to the straight pipe is divided respectively by sfy (or sfz or sft) in order to account for the increased flexibility of the elbows (see also the comments below).
gauch

Coefficient of “gauchissement” for the cross-section, allowing to compute the torsional inertia starting from Jo = Iy + Iz by means of a multiplicative coefficient: Jp = gauch * Jo.
VMIS

This keyword states that the weighting coefficients that allow to compute the Von Mises criterion starting from the different “equivalent stresses” are given by the user.
aprs

Weighting coefficient in the Von Mises criterion for the internal pressure of pipes.
ammb

Weighting coefficient in the Von Mises criterion for the membrane stress (normal stress).
atrs

Weighting coefficient in the Von Mises criterion for the equivalent torsional stress.
aflx

Weighting coefficient in the Von Mises criterion for the equivalent bending stress.
LECTURE

List of the elements concerned.

Comments:


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 hz from the axis (respectively hy) according to the following formula:

σy = My 
hz
Iy
 

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 cross-section, 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 :

Icoude = Idroit / 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   Rc /Rm2 

where e is the thickness and Rm the mean radius of the tube, and Rc 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* = √αp   P2 + αn   σn2 + αt   σt2 + αf   σf2


In this formula, coefficients αp, αn, αt and αf 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): αp = 0.75 , αn = 1 , αt = 3 and αf = π2/16 .

In the case of elbows, the coefficients αt and αf are modified. The default values are: αt = 0.75 and αf = ( γ   π / 4 ) 2 .


The coefficient γ has the expression: γ = max( 1 ; 8/9 λ−2/3 )


Important: please consult also GBG_0025 for the printout of the results.

6.8  DIAMETERS

C.60


Object :


Diameters of the one-dimensional 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).


Syntax:

       "DIAM" $[ "ELAS" ;
                 "ELAT" "EPAI" epai "YOUN" youn "NU" nu ]$
              |[ "DROI" d1 /LECTURE/ ;
                 "CONE" "D1" d1 "D2" d2 "ORIG" /LECTURE/
                                        "LIST" /LECTURE/ ]|


"ELAS"

This optional key-word activates an elastic correction of the speed of sound in the fluid of the straight (DROI) TUYA elements listed in the followed /LECT/ sequence. By default, the fluid vena section is rigid. For information about this correction see reference [865].
"ELAT"

This optional key-word activates an elastic correction of the speed of sound in the fluid of the TUBE elements listed in the followed /LECT/ sequence. When specified, this key-word must be associated with the key-words "EPAI", "YOUN" and "NU" defining the Allievi correction (characteristics of an equivalent pipe structure). By default, the fluid vena section is rigid. For information about this correction see reference [878].
epai

Pipe thickness (optional key-word associated with "ELAT" key-word)
youn

Young modulus (optional key-word associated with "ELAT" key-word)
nu

Poisson coefficient (optional key-word associated with "ELAT" key-word)
"DROI"

Introduces the characteristics of a straight tube.
d1

Diameter of the straight tube.
LECTURE

List of the concerned elements.
"CONE"

Introduces the characteristics of a conical tube.
d1

Inlet diameter, corresponding to node "ORIGINE".
d2

Outlet diameter.
"ORIG"

The following directive /LECTURE/ allows to specify the origin node, where the diameter is d1.
"LIST"

The following directive /LECTURE/ lists the elements concerned.

Comments :


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 Cfrot, 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:

Cfrot = 
λ
8   sin(α)
   ( 1 − R2 ) 


According to IDEL’CIK, the loss coefficients are then, Cdiv for a divergent pipe and Cconv for a convergent pipe (diagrams 3.7 and 5.2) :

Cdiv=Cfrot + 3.2 tan(α)
5
4
 
  (1 − R)2
Cconv = Cfrot + 0.45  (1 − R)

6.9  NAMED ELEMENT GROUPS

C.61


Object:


To define named groups of elements.


Syntax:

       "GROU"  ngro * ('nom_grou' |[ /LECT/ ; STFL FLUI ; STFL CLXS ; DEBR ]|
                                         <conditions>
                                         <"CENT" cx cy cz>
                                         <"SHRI" sh>
                                         <"SHFT" sx sy sz>)


ngro

Total number of groups that will be defined.
nom_grou

Name associated with the group, enclosed in quotes.
/LECT/

List of the concerned elements.
STFL FLUI

Instead of the explicit elements list /LECT/, all structured fluid elements (defined using STFL command, see page C.68) are taken. Of course, if present this command must be specified after the definition of the structured fluid mesh.
STFL CLXS

Instead of the explicit elements list /LECT/, all CLxS elements attached to structured fluid elements (defined using STFL CLxx command, see page C.68) are taken. Of course, if present this command must be specified after the definition of the structured fluid mesh.
DEBR

Instead of the explicit elements list /LECT/, all DEBR elements are taken. Of course, if present this command must be specified after the definition of the debris particles.
<conditions>

An optional set of conditions that allow to restrict the chosen elements to a subset of the list specified in the preceding /LECT/. See below for the syntax of conditional statements.
CENT

Introduces the optional definition of a centerpoint for the group, of coordinates cx, cy, cz, to be used in graphical rendering. In particular, this point is used for shrinking operations (see SHRI below). If omitted, the code computes it automatically as the (unweighted) average of the center points of the elements belonging to the group.
SHRI

Introduces the optional definition of a shrinkage factor for the group, of value sh, to be used in graphical rendering. If omitted, a factor 1.0 is assumed.
SHFT

Introduces the optional definition of a shift vector for the group, of components sx, sy, sz, to be used in graphical rendering. If omitted, zero shift is assumed.

Comments:

Object names are not case-sensitive: they are converted internally to upper-case 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 I-DEAS 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 OpenGL-based 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.


Conditional statements


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/                                                       |)


COND

Introduces a condition. This keyword may be repeated as many times as necessary to specify multiple conditions, which are applied in sequence.
XB

X-coordinate of the element’s barycenter.
YB

Y-coordinate of the element’s barycenter.
ZB

Z-coordinate of the element’s barycenter.
LT

Less than operator.
GT

Greater than operator.
val

Value.
NEAR

Selects the (single) element whose centroid is nearest to a given node or point. If there is more than one element at the minimum distance, then only the first one found is retained.
NODE

Specify the node by the following /LECT.
POIN

Specify the point by its coordinates x, y and z. The last coordinate is needed only in 3D calculations.
BOX

Introduces the definition of a “box”, (a quadrilateral in 2D or a parallelepiped in 3D) with the sides aligned with the global axes.
x0, y0, z0

Coordinates of the ‘origin’ of the box.
dx, dy, dz

Lengths of the box sides.
SPHE

Introduces the definition of a sphere (in 3D, or a circle in 2D).
xc, yc, zc

Coordinates of the centre of the sphere (or of the circle).
r

Radius of the sphere or of the circle.
CYLI

Introduces the definition of a cylinder (3D only). The cylinder is defined by the two extremities of its axis (P1, P2) and its radius.
x1, y1, z1

Coordinates of the first extremity P1 of the cylinder axis.
x2, y2, z2

Coordinates of the second extremity P2 of the cylinder axis.
r

Radius of the cylinder.
CONE

Introduces the definition of a (truncated) cone (3D only). The cone is defined by the two extremities of its axis (P1, P2) and its radii.
x1, y1, z1

Coordinates of the first extremity P1 of the cone axis.
x2, y2, z2

Coordinates of the second extremity P2 of the cone axis.
r1

Radius of the cone at the first extremity.
r2

Radius of the cone at the second extremity.
COMP

Introduces a second object to be used for the symmetric difference (complement) operation.
/LECT/

List of the concerned elements.

Comments:

If any of the above coordinates (x0, y0 etc.) is omitted, it is assumed to be 0.


Example:


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.

6.10  NAMED NODE GROUPS

C.62


Object:


To define named groups of nodes.


Syntax:

       "NGRO"  nngr * ('nom_grou' /LECT/ <conditions>)


nngr

Total number of node groups that will be defined.
nom_grou

Name associated with the group, enclosed in quotes.
/LECT/

List of the concerned nodes.
<conditions>

An optional set of conditions that allow to restrict the chosen nodes to a subset of the list specified in the preceding /LECT/. See below for the syntax of conditional statements.

Comments:

Object names are not case-sensitive: they are converted internally to upper-case 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 I-DEAS 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 OpenGL-based 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.


Conditional statements


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/                                                       |)


COND

Introduces a condition. This keyword may be repeated as many times as necessary to specify multiple conditions, which are applied in sequence.
X

X-coordinate of the node.
Y

Y-coordinate of the node.
Z

Z-coordinate of the node.
LT

Less than operator.
GT

Greater than operator.
val

Value.
NEAR

Selects the (single) node nearest to a given node or point. If there is more than one node at the minimum distance, then only the first one found is retained.
NODE

Specify the node by the following /LECT. This node is of course excluded from the search of the nearest node to it.
POIN

Specify the point by its coordinates x, y and z. The last coordinate is needed only in 3D calculations.
BOX

Introduces the definition of a “box”, (a quadrilateral in 2D or a parallelepiped in 3D) with the sides aligned with the global axes.
x0, y0, z0

Coordinates of the ‘origin’ of the box.
dx, dy, dz

Lengths of the box sides.
SPHE

Introduces the definition of a sphere (in 3D, or a circle in 2D).
xc, yc, zc

Coordinates of the centre of the sphere (or of the circle).
r

Radius of the sphere or of the circle.
CYLI

Introduces the definition of a cylinder (3D only). The cylinder is defined by the two extremities of its axis (P1, P2) and its radius.
x1, y1, z1

Coordinates of the first extremity P1 of the cylinder axis.
x2, y2, z2

Coordinates of the second extremity P2 of the cylinder axis.
r

Radius of the cylinder.
CONE

Introduces the definition of a (truncated) cone (3D only). The cone is defined by the two extremities of its axis (P1, P2) and its radii.
x1, y1, z1

Coordinates of the first extremity P1 of the cone axis.
x2, y2, z2

Coordinates of the second extremity P2 of the cone axis.
r1

Radius of the cone at the first extremity.
r2

Radius of the cone at the second extremity.
LINE

Introduces the definition of a straight line. The line is defined by the two extremities (P1, P2), a relative tolerance є (TOL) and an optional relative spacing δ (DIST) between the nodes to be retained. Nodes on the line are kept in the order in which they occur passing from P1 to P2 (included).

In 3D space, the line passing through 2 points P1(x1,y1,z1) and P2(x2,y2,z2) has the following parametric equations:

x = x1 + dx   t,   dx = x2x1 
y = y1 + dy   t,   dy = y2y1 
z = z1 + dz   t,   dz = z2z1 

From each equation a value for t can be defined:

tx = 
xx1
dx
 
ty = 
yy1
dy
 
tz = 
zz1
dz
 

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.

x1, y1, z1

Coordinates of the first extremity P1 of the line.
x2, y2, z2

Coordinates of the second extremity P2 of the line.
tol

Tolerance (relative) є for searching the nodes on the line. The absolute tolerance τ is equal to the relative tolerance multiplied by the distance L between P1 and P2: τ=Lє.
d

Parametric (relative) distance δ between two consecutive nodes retained on the line. If omitted, all nodes on the line are retained. If specified, then the relative distance between two consecutive retained nodes will be greater or equal to δ (and so possibly some nodes on the line will be skipped). The absolute distance d is equal to the relative distance multiplied by the distance L between P1 and P2: d=Lδ.
COMP

Introduces a second object to be used for the symmetric difference (complement) operation.
/LECT/

List of the concerned nodes.

Comments:

If any of the above coordinates (x0, y0 etc.) is omitted, it is assumed to be 0.


Example:


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.

6.11  ELEMENT COLORS

C.63


Object:


To define or re-define (e.g. in the case of a mesh generated by Cast3m) the colors of elements, for visualization purposes.


Syntax:

       "COUL" (nom_coul /LECT/)


nom_coul

Name of the color (not enclosed in quotes). The valid names are those of Cast3m, i.e. bleu, roug, rose, vert, turq, jaun, blan or noir, plus the following nine gray levels: gr10 (almost black), gr20, gr30, gr40, gr50, gr60, gr70, gr80 and gr90 (almost white). Elements not assigned a color have a default color.
/LECT/

List of the concerned elements.

Comments:

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).

6.12  RTM COMPOSITE MATERIALS

C.64


Object:


This directive allows to define values to used by a composite material made by a RTM process ie. the CRTM material (page C264).


Syntax:

  "RTMVF"   vf      /LECTURE/

  "RTMRCT"  rct     /LECTURE/

  "RTMANGL" angle   /LECTURE/


vf

Value of the volumic fraction
rct

Value of the ratio between warp and weft
angle

Value of the angle between warp and weft directions.
LECTURE

List of the elements concerned.

6.13  PFEM METHOD

C.65


Object:


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.


Syntax:

  PFEM  H h ALPHA alpha


h

Expected distance between nodes in the Bowyer-Watson triangulation.
alpha

Alpha coefficient for the Alpha-shape method to determine the contour of the triangulation.

6.14  FLYING DEBRIS MODEL

C.66


Object:


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.


Syntax:

  DEBR  <ROF rof>
        <VFX vfx> <VFY vfy> <VFZ vfz>
        <FLUI /LECT/ <DGRI> $[ HGRI hgri ; NMAX nmax ; DELE dele ]$ >
        (PART particle_description)
        (FILL fill_description)


rof

Density of the uniform fluid field in which the particle is embedded. This value is 0.0 by default, meaning that the particle moves in vacuum.
vfx, vfy, vfz

Components of the velocity of the surrounding uniform fluid field. These values are 0.0 by default.
FLUI

Introduces the /LECT/ of the discretized fluid domain with which the particles motion should be coupled. When a particle traverses this domain, the (local) fluid velocity and density are automatically computed by the code, instead of using the constant user-given values rof, vfx, vfy, vfz described above. A fast search algorithm based on a grid of cells (as in bucket sorting) is used to compute the fluid element (if any) encompassing each debris particle.
DGRI

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

Specifies the size of the grid cell. Each cell has the same size in all spatial directions and is aligned with the global axes. Note that the size of this grid is related to the size of the fluid elements specified in FLUI, not of the structural elements producing the flying debris.
NMAX

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

Specifies the size of the grid cell as a multiple of the diameter of the largest coupled fluid element. Element “diameters” are computed only along each global spatial direction and the maximum is taken. For example, by setting DELE 4 the size of the cell is four times the diameter of the largest coupled fluid element. By default, i.e. if neither HGRI, nor NMAX, nor DELE are specified, the code takes DELE 3 (this value is probably too large, a value of 1.1 or so should be more appropriate in most cases).
PART

Introduces the description of a single particle, see details below. Such particles are active from the very beginning of the calculation. This directive may be repeated any number of times.
FILL

Fill by particles a single finite element or a finite element mesh. Such particles may either be active from the very beginning of the calculation, or be activated upon failure of the associated element(s). See below for the details of this directive. This directive may be repeated any number of times.

Dimensioning for the flying debris:

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 two-step procedure is suggested:


Dimensioning in case of domain decomposition (MPI):

In case of a calculation with domain decomposition (MPI), the dimensioning for the flying debris can assume two forms:


Comments:

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 Fd=−CdρfA||w||2w/||w||, where Cd is the particle’s drag coefficient (see below), ρf is the fluid’s density, A=π /4d2 is the particle’s cross-section, d is the particle’s diameter and w is the particle’s velocity v relative to the fluid velocity vf: w=vvf.


The total number of particles described by the PART and FILL sub-directives must be less than or equal to the number of elements of type DEBR that has been reserved in the dimensioning of the problem.


Describing a single particle

Object:


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.


Syntax:

  PART  <X x> <Y y> <Z z>   <VX vx> <VY vy> <VZ vz>
        RO ro  D d  DRAG drag
        <COUP> <IMPA> <TRAJ> <RISK>


x, y, z

Coordinates of the particle at the initial time. These values are 0.0 by default.
vx, vy, vz

Velocity components of the particle at the initial time. These values are 0.0 by default.
ro

Density of the particle.
d

Diameter of the particle.
drag

Drag coefficient of the particle. This is a number usually between 0.3 and 1.1 for a sphere. In the supersonic region the value is almost constant and close to 1.0, while it drops rapidly in the transonic region.
COUP

Couple the particle’s motion with the surrounding fluid domain defined by the FLUI directive above.
IMPA

Treat the impact of the particle against surrounding structures (by the pinball method). One (parent) pinball is embedded in the particle, of diameter equal to that of the particle. Pinballs for the potentially impacted structures must be defined separately by the PINB directive, see page D.480.
TRAJ

Save the particle’s trajectory, e.g. for visualization purposes. By default, the particle trajectory will consist of 100 points equispaced in time between the initial and final times of the calculation, but the number of points can be set by the OPTI DEBR NTRA option (see page H.45). Beware that, by default, the trajectory data are not stored in the ALIC results file. Therefore, visualization of the particles trajectory can only be done during the main calculation. In order to draw the trajectories when reading back results RESU from an ALIC file, one must activate the OPTI DEBR STTR option (see page H.45), which stores the trajectory data on the ALIC file (beware that the size of the file may increase considerably if there are many particles and many points per trajectory).
RISK

The risk of death due to the impact of the current flying debris particle on the human body is calculated. The risk calculation is based on the Lewis model and requires the presence of a (discretized) fluid domain. In fact, the risk is evaluated in each fluid element (or volume) as this is traversed by the flying debris particles.

Filling an element or a mesh by particles

Object:


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.


Syntax:

  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/


vx, vy, vz

Components of the velocity of the particles at the initial time. This value is 0.0 by default.
vr

Radial velocity of the particles at the initial time. This value is 0.0 by default.
cx, cy, cz

Coordinates of the particles centroid with respect to which the radial velocity is expressed. By default this is the centroid of the geometrical object defined by the /LECT/ directive given below.
plev

Level of hierarchic subdivision of the parent element(s) along each spatial direction in order to generate the particles. The particles’ diameter is automatically determined so as to conserve the element’s total volume. For example, a level of 3 means that 23=8 subdivisions along each spatial direction to generate the particles. A 2D quadrilateral element would in this case be filled by 8· 8=64 particles.
drag

Drag coefficient of the particles. This is a number usually between 0.3 and 1.1 for a sphere. In the supersonic region the value is almost constant and close to 1.0, while it drops rapidly in the transonic region.
afly

The drag forces and the AIRB forces depend on the area of the spherical particle, which can be different from the “true” debris cross section. For each shell element and beam element a minimum and a maximum area are estimated. By using the keyword AFLY the minimum (afly = 0.0) or the maximum (afly = 1.0) value is used. Values of afly between 0.0 and 1.0 interpolate linearly between these two values. The default value is 0.5. For solid elements, the cross section of the spherical particle is used and so afly is ignored.
COUP

Couple the particles’ motion with the surrounding fluid domain defined by the FLUI directive above.
IMPA

Treat the impact of the particles against surrounding structures (by the pinball method). One (parent) pinball is embedded in each particle, of diameter equal to that of the particle. Pinballs for the potentially impacted structures must be defined separately by the PINB directive, see page D.480.
TRAJ

Save the particle’s trajectories, e.g. for visualization purposes. By default, the particle trajectory will consist of 100 points equispaced in time between the initial and final times of the calculation, but the number of points can be set by the OPTI DEBR NTRA option (see page H.45). Beware that, by default, the trajectory data are not stored in the ALIC results file. Therefore, visualization of the particles trajectory can only be done during the main calculation. In order to draw the trajectories when reading back results RESU from an ALIC file, one must activate the OPTI DEBR STTR option (see page H.45), which stores the trajectory data on the ALIC file (beware that the size of the file may increase considerably if there are many particles and many points per trajectory).
RISK

The risk of death due to the impact of the active flying debris particles on the human body is calculated. The risk calculation is based on the Lewis model and it is applied to the active debris particles which are produced after the erosion of an element. The risk calculation requires the presence of a (discretized) fluid domain. In fact, the risk is evaluated in each fluid element (or volume) as this is traversed by the flying debris particles.
MACR

This keyword adds to the risk calculation described above (related to the flying debris particles produced after erosion of an element) also the calculation of the risk related to the impact of macro fragments (i.e., before the erosion of an element). To estimate such risk, “spurious” (inactive) particles (“markers”) are attached to the elements (one particle per element) from the very beginning of the calculation (i.e., as long as the elements do not fail). The risk estimation takes into account not only the mass of the current particle (current element) but also the mass of the surrounding (unfailed) elements, up to a certain influence radius that can be specified by the user (RMAC, see below). If an element fails and is eroded, the corresponding marker particle is suppressed and a suitable number of debris particles are activated (for which the impact risk is then computed normally).
RMAC

Introduces the influence radius (rmac) for the evaluation of the impact risk of macro fragments. If a marker impacts (penetrates through) a fluid element, the risk is estimated by using the mass of all (unfailed) elements connected with the current one within a distance equal to rmac. By specify inc RMAC 0 an infinite radius of influence is taken. This means that the total mass of the macro fragment is considered in the impact.
OBJE

Introduces the list of the elements to be filled.
/LECT/

List of the elements to be filled.

Comments:


The initial velocity of each group of particles defined by the FILL directive described above may be defined in two ways:

6.15  DISPLACEMENT EROSION

C.67


Object:


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.


Syntax:

  FAIL  ( DISP disp NODE /LECT/ OBJE /LECT/ )
        ( AUTO rati DIRE disp /LECT/ )


disp

Displacement of the node given by the keyword NODE, which results in an erosion (failure) of the elements given by the keyword OBJE.
node

Node used for the displacement criterion. The following /LECT/ must contain just one node index.
OBJE

Introduces the /LECT/ of the elements which are eroded, if the criterion is reached.
AUTO

The keyword AUTO introduces an automatic development of the nodes used for the displacement criterion and the element which should eroded. The elements given by /LECT/ are separated to several subsets, the node near the barycentre is used for the criterion, the full subset is used for the elements which could be eroded.
rati

Ratio of the minimum span which should be used for the displacement criterion.
dire

The maximum span is defined in this direction.

Remarks:


The set of keywords DISP ... OBJE may be repeated as many times as needed to define all the desired displacement-based erosion criteria.

6.16  STRUCTURED FLUID GRID MODEL

C.68


Object:


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 fluid-structure 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.


Syntax:

 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>


STFL

Introduces the parameters for the generation of a structure fluid mesh.
VFCC

Use VFCCs for the structure fluid mesh. If this optional keyword is not specified, by default the structured mesh will be made of fluid FE.
x0, y0, z0

Coordinates of the origin of the structured fluid grid. The z-coordinate z0 is only needed in 3D calculations.
lx, ly, lz

Total lengths of the sides of the structured fluid grid. The z-length lz is only needed in 3D calculations.
nx, ny, nz

Number of cells of the structured fluid grid in each direction. The z-number of cells nz is only needed in 3D calculations. Cells have a uniform length in each direction.
CLX1

Automatically generate CL2S/CL2D elements (CL3S/CL3D in 3D) along the face of the fluid domain of equation x=x0.
CLX2

Automatically generate CL2S/CL2D elements (CL3S/CL3D in 3D) along the face of the fluid domain of equation x=x0+lx.
CLY1

Automatically generate CL2S/CL2D elements (CL3S/CL3D in 3D) along the face of the fluid domain of equation y=y0.
CLY2

Automatically generate CL2S/CL2D elements (CL3S/CL3D in 3D) along the face of the fluid domain of equation y=y0+ly.
CLZ1

Useful only in 3D. Automatically generate CL3S/CL3D elements along the face of the fluid domain of equation z=z0.
CLZ2

Useful only in 3D. Automatically generate CL3S/CL3D elements along the face of the fluid domain of equation z=z0+lz.

Comments:


Each cell (element) of the grid is a rectangle (rectangular parallelepiped in 3D) with sides of length lx/nx, ly/ny (and lz/nz in 3D).


Nodes and elements in the grid are numbered progressively starting from the chosen origin (x0, y0, z0), first along the global X-direction, then along the Y-direction (in 3D, finally along the Z-direction).


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 post-processing.


Appropriate materials must be assigned, in the usual way, to all the automatically generated elements. For example, a low-pressure gas to all fluid elements except those in a bubble zone, representing an explosion, in which a high-pressure 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 FSI-driven 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.

6.17  AUTOMATIC GENERATION OF SPECTRAL MICRO MESH

C.68b


Object:


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 4-node quadrilateral elements (in 2D) or of MS38 8-node hexahedral elements (in 3D), and must have been specified in the previous GEOM directive. The generated micro SE mesh will be composed of S24 4-node quadrilaterals in 2D or of S38 8-node hexahedra in 3D.


Syntax:

 SPEC GMIC NSPE nspe


GMIC

Introduces the automatic generation of micro SE elements according to the parameters given in the following.
nspe

Degree N of the interpolation polynomial for the SE mesh.

Comments:


Each macro SE generates exactly N2 micro SE in 2D or N3 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
 . . .

6.18  ELEMENT-SPECIFIC EROSION

C.69


Object:


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.


Syntax:

  EROS  $[ eros ; NOER ]$ /LECT/


eros

Erosion criterion for the elements given by /LECT/. If no erosion limit is needed for a set of elements the keyword NOER can be taken. Negative erosion limit indicates also no erosions for the elements.

Remarks:


The set of keywords EROS ... /LECT/ may be repeated as many times as needed to define all the desired element-based erosion criteria.

6.19  MESH ORIENTATION

C.70


Object:


To orient or re-orient 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 sub-directive 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 re-orientation 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.


Syntax:

  "ORIE"   < "OBJE" /LEC1/ $[ "POIN" x y z ; "NODE" /LECN/ ]$ >
           < "INVE" /LEC2/ >

OBJE

The elements in object /LEC1/ have to be oriented so that their outwards normal direction points towards a certain point or node in space, to be specified next. By “pointing” we intend here simply that the scalar product of the unit normal with the line joining the element’s center to the given point or node should be positive.
POIN

Introduces the coordinates of the point.
x y z

Coordinates of the point. Note that three coordinates should always be given even in 2D cases (but the ORIE directive is only useful in 3D cases anyway).
NODE

Introduces the index of the node.
/LECN/

One node index or the name of an object with just one node (e.g. a Cast3m point name if the mesh has been produced by Cast3m).
INVE

The orientation of elements in object /LEC2/ has to be inverted without any checking.

Comments:


Only some element types admit re-orienting: typically, these are 3-node or 4-node “thin” elements in 3D, such as shell, membrane or CLxx elements.


Note that the ORIE sub-directive may be repeated any number of times, if needed. For example, this may be useful to re-orient a randomly oriented closed surface so that it points outwards. Use a first ORIE sub-directive to orient the all the surface elements consistently towards an internal point (e.g. its barycenter). Then, use a second ORIE sub-directive to invert the orientation:

   COMP ... ORIE OBJE LECT toto TERM POIN x y z
            ORIE INVE LECT toto TERM

6.20  AUTOMATICALLY GENERATED SPH PARTICLES

C.72


Object:


To generate automatically SPH particles within user-defined volumes.


Syntax:

"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/                                                       |))


ngen

Total number of groups of SPH particles that will be generated.
r

Radius for the particles of this group.
rese

Type of spheres packing: 0 means compact hexagonal (default), 1 means compact cubic (to be implemented), 2 means trivial (non-compact) cubic (normally to be used only for tests and debugging).
INSI

Introduces an “inside” condition: all particles “within” a certain geometrical shape are to be generated. This keyword can be repeated as many times as necessary to specify multiple conditions, which are applied in sequence. As a result, all the particles “inside” the union of the specified geometrical shapes will be generated.
OUTS

Introduces an “outside” condition: from all particles in the set generated by the previously specified INSI condition(s), only those “external” to a certain geometrical shape are to be retained. This keyword can be repeated as many times as necessary to specify multiple conditions, which are applied in sequence. As a result, only the particles “outside” the union of the specified geometrical shapes will be retained.
BOX

Introduces the definition of a “box”, (a quadrilateral in 2D or a parallelepiped in 3D) with the sides aligned with the global axes.
x0, y0, z0

Coordinates of the ‘origin’ of the box.
dx, dy, dz

Lengths of the box sides.
SPHE

Introduces the definition of a sphere (in 3D, or a circle in 2D).
xc, yc, zc

Coordinates of the centre of the sphere (or of the circle).
r

Radius of the sphere or of the circle.
CYLI

Introduces the definition of a cylinder (3D only). The cylinder is defined by the two extremities of its axis (P1, P2) and its radius.
x1, y1, z1

Coordinates of the first extremity P1 of the cylinder axis.
x2, y2, z2

Coordinates of the second extremity P2 of the cylinder axis.
r

Radius of the cylinder.
CONE

Introduces the definition of a (truncated) cone (3D only). The cone is defined by the two extremities of its axis (P1, P2) and its radii.
x1, y1, z1

Coordinates of the first extremity P1 of the cone axis.
x2, y2, z2

Coordinates of the second extremity P2 of the cone axis.
r1

Radius of the cone at the first extremity.
r2

Radius of the cone at the second extremity.
MESH /LECT/

Introduces the definition of an arbitrary volume, represented by a mesh whose elements are specified in the following /LECT/. This mesh must have been defined in the GEOM directive and may be composed of elements of Cast3m shape CUB8, PRI6, TET4 and PYR5. Since these elements are probably useless for the calculation (they only serve to define the volume), they should be assigned the FANT material.

Comments:

If any of the above coordinates (x0, y0 etc.) is omitted, it is assumed to be 0.


Example:


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).

6.21  WATER TABLES

C.74


Object :

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)


Syntax :

    $[ "TEAU" ; "TH2O" ]$   "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         $

tmin

Minimum temperature in the tables (this must be lower than the saturation temperature corresponding to pmin).
tmax

Maximum temperature in the tables (this must be higher than the saturation temperature corresponding to pmax, in the case of a sub-critical domain, or to 374 degrees Celsius in the case of a hyper-critical domain).
pmin

Minimum pressure in the tables.
pmax

Maximum pressure in the tables.
cl

Conversion factor of the length units adopted, towards metres.
cm

Conversion factor of the mass units adopted, towards kilograms.
nbte

Number of intervals into which the low-temperature domain. is subdivided.
nhte

Number of intervals into which the high-temperature domain. is subdivided.
nsat

Number of intervals into which the pressure in the saturation curve is subdivided.
nhy

Number of intervals into which the pressure in the hypercritic domain is subdivided.


For the tests:

"DESS"

Allows to draw a cross-section of the tables in the plane (temperature, pressure).
"PERF"

Allows to output on a file (logical unit 7) the tables of water properties.
"TEST"

This keyword provides a trace of the work performed by the algorithm that searches the thermodynamic parameters of the one-phase or two-phase water, by giving an initial and a final state.
"FINT"

End of the sequence opened by keyword TEST.
"CAS" nbr

Number of the treated case. nbr is a simple identification number.
p1,t1 or p1,x1

Initial state of the water. If this state is two-phase, it is sufficient to specify p1 and x1. Attention: temperatures are expressed in degrees Celsius, pressures in bar and concentrations are per unit mass.
p2,t2 or p2,x2

Final state of the water. If this state is two-phase, it is sufficient to specify p2 and x2. Attention: temperatures are expressed in degrees Celsius, pressures in bar and concentrations are per unit mass.
dvs,dh

Instead of p2 and t2 (or p2 and x2), it is possible to specify the variation of specific volume (in m3/kg) and the variation of specific enthalpy (dh) in J/kg.

Warning :

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.


Comments :

A portion of the saturation curve must be included in the Pressure-Temperature 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 sub-critic 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.

6.22  HELIUM TABLES

C.75


Object :

These directives create tables containing the physical properties of helium, according to CEA/IRF/DPC (1985).


Syntax :

    "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         $

cl

Conversion factor of the length units adopted, towards metres.
cm

Conversion factor of the mass units adopted, towards kilograms.


For the tests:

"TEST"

This keyword provides a trace of the work performed by the algorithm that searches the thermodynamic parameters of the one-phase or two-phase helium, by giving an initial and a final state.
"FINT"

End of the sequence opened by keyword TEST.
"CAS" nbr

Number of the treated case. nbr is a simple identification number.
p1,t1 or p1,x1

Initial state of helium. If this state is two-phase, it is sufficient to specify p1 and x1. Attention: temperatures are expressed in degrees Kelvin, pressures in bar and concentrations are per unit mass.
p2,t2 or p2,x2

Final state of helium. If this state is two-phase, it is sufficient to specify p2 and x2. Attention: temperatures are expressed in degrees Kelvin, pressures in bar and concentrations are per unit mass.
dvs,dh

Instead of p2 and t2 (or p2 and x2), it is possible to specify the variation of specific volume (in m3/kg) and the variation of specific enthalpy (dh) in J/kg.

Warning :

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).


Comments :

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 time-consuming.


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.

6.23  PIPE JUNCTIONS

C.80


Object :

Join together different branches of a pipeline.


Syntax:
    "RACC" |[ "BIFU" ;
              "CAVI" ;
              "BREC" ]|

           $[        n1 ... nk                              ;
             "LECT" racname "TERM" "LECT" P1 ....PK "TERM"  ]$

          ....   "DSOR" d1...dk < "VOLU" v >
n1 ... nk

Numbers of the nodes connected by the junction (the order is irrelevant).
racname

LECTURE of the name of the junction element in GIBI.
P1....PK

LECTURE of the names of the connected points as given in GIBI.
d1 ... dk

Internal diameters of the pipelines joined together (the order must correspond to that of the node numbers or names given above).
v

Volume of the junction: mandatory for a cavity, useless for a bifurcation or a pipeline rupture.

Comments:

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 re-computes 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" ....

6.24  TUBM (3D-1D JUNCTION)

C.90


Object:


To connect, by means of a "TUBM" element, a pipeline meshed in 1-D with a fluid meshed in 3-D.


Syntax:
    "RACC" ( "TUBM" /LECTURE/  "NTUB" /LECTURE/  "DTUB" dtub  ...
                               "FACE" /LECTURE/  "COEF" coef  )

"TUBM" /LECTURE/

The /LECTURE/ procedure allows to specify the name of the GIBI object associated with the junction element. In case of a mesh in the MED format, the name of the junction element must follow a specific rule, see comments below.
"NTUB" /LECTURE/

The /LECTURE/ procedure allows to specify the name of the GIBI object or MED group associated with the 1D node of the tube.
dtub

Internal diameter of the connected tube.
"FACE" /LECTURE/

The /LECTURE/ procedure allows to specify the name of the GIBI object or MED group associated with nodes of the 3D face. The object must be composed of surface elements (typically CL3D), which are used to identify the 3D part of the junction. These CL3D elements should not be assigned any material, since EPX automatically assigns them a FANT material.
coef

This coefficient allows to take into account of possible symmetries in the 3D mesh. The area of the face meshed in 3D is multiplied by coef in order to find out the same area as that of a non-symmetrised face.

Comments :


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:


"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.


Warning:


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).

6.25  TUYM (3D-1D JUNCTION)

C.91


Object:


To connect, by means of a "TUYM" element, a pipeline meshed ("TUYA" element) in 1-D with a fluid meshed in 3-D for moving meshes (A.L.E computation).


Syntax:
    "RACC" ( "TUYM" /LECTURE/  "NTUB" /LECTURE/  "DTUB" dtub  ...
                               "FACE" /LECTURE/  "COEF" coef  )

"TUYM" /LECTURE/

The /LECTURE/ procedure allows to specify the name of the GIBI object associated with the junction element. In case of a mesh in the MED format, the name of the junction element must follow a specific rule, see comments below.
"NTUB" /LECTURE/

The /LECTURE/ procedure allows to specify the name of the GIBI object or MED group associated with the 1D node of the tube ("TUYA" element).
dtub

Internal diameter of the connected tube ("TUYA" element).
"FACE" /LECTURE/

The /LECTURE/ procedure allows to specify the name of the GIBI object or MED group associated with nodes of the 3D face. The object must be composed of surface elements (typically CL3D), which are used to identify the 3D part of the junction. These CL3D elements should not be assigned any material, since EPX automatically assigns them a FANT material.
coef

This coefficient allows to take into account of possible symmetries in the 3D mesh. The area of the face meshed in 3D is multiplied by coef in order to find out the same area as that of a non-symmetrised face.

Comments :


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 :


"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.


Warning:


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).

6.26  CORRESPONDENCE BETWEEN NODES

C.92


Object:


The purpose of this directive is to define a one-to-one correspondence between couples of nodes. This user-defined correspondence may be useful in various situations, in which the code needs to find a one-to-one 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.


Syntax:

     "CNOD"   "NODF"  /LECT1/     "NODS"   /LECT2/
/LECT1/

List of first nodes of each node couple. Typically, these are fluid nodes.
/LECT2/

List of second nodes of each node couple. These nodes must be Lagrangian. Typically, these are structure nodes, but Lagrangian fluid nodes are also accepted.

Comments:


The order in which nodes are listed in /LECT1 or /LECT2 is retained. To the i-th node of /LECT1 corresponds the i-th 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 sub-directive of FSA, see page D.450, which is more practical in case there is a large number of conflicting nodes.

6.27  SPH SHELL ELEMENT (SPHC)

C.93


Object :


This instruction introduces characteristics for the SPH shell elements (SPHC) which allow discretizing shell structures with a single layer of particles.


Syntax:

     "CSPH"   "RAYO" rbille   "EPAI" ep
              "ORX" orx  "ORY" ory  "ORZ" orz
            < "LINE" cl >   < "QUAD" cq >
            < "RLIM" rlim > < "RESEAU" ires >
            < "VOIS" nvoi >
            ( "STRP" istrp /LECT/ )


rbille

Radius of the SPH shell particles.
ep

Thickness of the shell particles.
orx, ory, orz

x,y,z co-ordinates of a point used to orient normals of the SPH shell particles.
cl

Linear damping coefficient.
cq

Quadratic damping coefficient.
rlim

Multiplicative coefficient for the search radius.
ires

Type of particles lattice (1: cubic, 0: hexagonal).
nvoi

Number of neighbouring particles sought.
istrp

Type of stress points (1: free, 2: clamped) read in the following /LECTURE/ sequence (see comment below).

Comments :


For the quadratic damping, it is advised to take cq=4.


To damp out the high-frequency 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.

6.28  DISCRETE ELEMENT MODEL (ELDI)

C.94


Object :


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).


Syntax:

   "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 >


"IMPR"

This optional keyword allows printing out in the output listing the value of the radius of each discrete element.
"MASSE"

This optional keyword enables the user to impose the masses of discrete elements lists.
nval

Number of imposed masses.
val

Value of the imposed mass.
"ARMA"

Indicates the presence of steel reinforcement modeled with aligned steel discrete elements. Caculates the main direction of the reinforcement used for steel-concrete interaction.
LECTURE

List of the discrete elements concerned.
"LTM"

Indicates the presence of bending properties (rotation stiffnesses for discrete elements).
nbse

Number of sequences with different bending properties.
beta

Coefficient used to calculate the bending stiffness: Kr=beta*EI/R.
plas

Coefficient used to calculate the plastic torque: Mp=plas*sigma*I/R. In elastic calculations, one should use plas=0 (no test on Mp) or put plas>>1 to guarantee Mp is very high.
"TYPL"

This keyword defines different types of links (interactions) between discrete elements (ELDI) within one or several sets of particles. Links may be of two kinds : cohesive links and contacts. The interaction forces between the discrete elements are then computed with respect to the types of material used.
nbtypl

Number of sequences beginning from one of the following words : "COHE" or "BIMA" or "CONT".
"COHE"

This keyword initializes the search of cohesive interactions within a set of discrete elements.
<"COEF" val>

Interaction range. The default value of the interaction range val is 1.
"BIMA"

This keyword initializes the search of cohesive interactions between two sets of discrete elements (permanent contact of two materials).
"MAT1" <"COEF" val>

This keyword allows to define the first set of discrete elements and its interaction range val. The default value is 1.
"MAT2" <"COEF" val>

This keyword allows to define the second set of discrete elements and its interaction range val. The default value is 1.
"CONT"

This keyword initializes the search of contact interactions inside one or several sets of discrete elements specified in /LECTURE/. In this case, the value of the interaction range is 1.
<"IMPR">

This optional keyword allows to print out in the output listing the result of the interactions search.
"CSTE"

This optional keyword enables the user to define the security coefficient of the time step.
coef

Security coefficient (by default 0.1) : dt=coef*dtcrit
nbcoup

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

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

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

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

Allows defining a box restraining search for DE contacts. Six reals must be given: xmin,xmax,ymin,ymax,zmin,zmax.

Comments :


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 Ra and Rb 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 * (Ra +Rb) > or = Da,b


where Da,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.

6.29  MULTILAYER ELEMENT CMC3

C.95


Object:


The characteristics of CMC3 elements are described when they have not been defined by CASTEM2000.


Syntax:

     "CORTHO"   "EPAISSEUR"  ep     "EXCENTREMENT"   ex
             $[  "ANGLE"      angle       ;
                 "VECTEUR"    vx  vy  vz  ]$           /LECTURE/


ep

Thickness of the element.
ex

Element eccentricity with respect to the plane defined by the 3 nodes of the mesh.
angle

Angle (in degrees) formed by the first side of the element and the first axis of the orthotropic system.
vx,vy,vz

The 3 components in the global frame of the vector that defines the first orthotropy direction.
LECTURE

List of the elements concerned.

Comments:


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 cork-screw rule).


The first side of the element is the one formed by the first 2 nodes.

6.30  ORTHOTROPY

C.96


Object:


Description of the orthothropy directions for continuum elements in 2D and 3D.


Syntax:

     "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/


angle1

Angle (in degrees) formed by the Ox axis (in 2D plane cases or 3D) or the Or axis (in axisymmetric) and the first axis of the orthotropy reference frame.
angle2

Angle (in degrees) formed by the first side of the element and the first orthotropy axis (in 2D or axisymmetric). The first side of the element is the segment connecting the first two nodes declared for the element in the GEOM directive.
e11, e12, e13

First vector defining the orthotropy plane of the material.
e21, e22, e23

Second vector defining the orthotropy plane of the material.
COCY

This directive allows to define a “cylindrical” type of orthotropy, that may be used for example by the BOIS (wood) material. The first axis of orthotropy is parallel to the vector defined by the VECT directive described above. The second axis of orthotropy (perpendicular to the first one) lies on the plane formed by a straight line passing through the POINT defined below and parallel to VECT, and the barycenter of the element.
POINT

This directive allows to define a point which is either a node of the mesh (option /LECTURE1/), or a geometric point defined by its three coordinates (xx yy zz).
v1 v2 v3

First vector defining the orthotropy reference frame of the COCY directive.
v1x, v1y, v1z

First vector defining the orthotropy plane of the material in the local repere of the element.
v2x, v2y, v2z

Second vector defining the orthotropy plane of the material in the local repere of the element.
LECTURE

List of the elements concerned.

Comments:


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.

6.31  ORTHOTROPY FOR 3D SHELLS

C.97


Object:


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:

  1. ORTS vx vy vz /LECT/ <LAYE /LECT_LAY/>: This syntax specifies directly vx, vy, vz i.e. a vector whose projection on the lamina (local) reference of the (shell) element is the first orthotropy direction of the material which is sufficient to define the orthotropy for shell elements. This syntax applies directly to elements (or element layers) using the COMM or GLRC material, since such materials require the values of VX, VY, VZ. For elements (or element layers) using the HILL, ORTS or ORPE material the vx, vy, vz are converted internally to an angle, (by projecting the vector onto the shell’s lamina plane), which is then stored in the ECR() table.
  2. ORTS $ ANGL angl ; AXE1 a1x a1y a1z $ /LECT/ <LAYE /LECT_LAY/>:
    This syntax specifies either an angle angl or a vector a1x, a1y, a1z.

Syntax:

    "ORTS" |[ vx vy vz                                ;
              $[ "ANGL" alpha ;  "AXE1" a1x a1y a1z ]$
           ]|
           /LECT/   < "LAYE" /LECT_LAY/>


vx vy vz

Components, in the global reference frame, of a vector whose projection on the lamina (local) coordinate system of the 3D shell element indicates the orthotropy direction (one such direction is sufficient, for shell elements).
ANGL alpha

Angle between the first direction of the shell element and the first direction of the orthotropic frame (in radians). It can only be used with Q4GS, Q4GR, Q4MC, DKT3, DST3 or T3MC elements associated either with HILL or with ORTS material.
AXE1 a1x a1y a1z

Components, in the global reference frame, of a vector whose projection on the lamina (local) coordinate system of the 3D shell element indicates the orthotropy direction (one such direction is sufficient, for shell elements). It can only be used with Q4GS, Q4GR, Q4MC, DKT3, DST3 or T3MC elements associated either with HILL or with ORTS material
/LECT/

Concerned elements.
/LECT_LAY/

Concerned layers. Layers are identified by their indexes, as described in the SAND directive on page C.45.

Comments:


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.

6.32  PARTICLE ELEMENT (BILLE)

C.99


Object :


Description of the characteristics of the BILLE element (particle element).


Syntax:

     "CBILLE"   "RAYON"  rbille    < "LINEAIRE"   cl    >    ...
          ... < "QUADRATIQUE" cq > < "RESEAU"     ires  >    ...
          ... < "VOISIN"      nvoi >
          ... < "RLIM"        rlim >


rbille

Radius of the particles.
cl

Linear damping coefficient.
cq

Quadratic damping coefficient.
ires

Type of particles lattice.
nvoi

Number of neighbouring particles sought.
rlim

Multiplicative coefficient for the search radius.

Comments :


For the quadratic damping, it is advised to take cq=4.


To damp out the high-frequency 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.

6.33  RIGID BODIES (JRC Implementation)

C.99B


Object :


To define one or more rigid (non-deformable) 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.


Syntax:

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/ )


nrigi

Total number of rigid bodies. Each rigid body is geometrically defined by a set of elements.
MASS

Optional specification of the method that should be used to compute the total mass of the body. The value 0 (default) means using the nodal masses as computed by EPX using standard procedures. The value 1 means using the element masses as computed by EPX using standard procedures. The value 2 means decomposing each element into simplexes (triangles or tetrahedrons) and then using analytical formulas over each simplex in order to assemble the total mass of the whole body. The value 3 means that the user specifies the total mass by the following MTOT keyword. In this latter case the value of the RIGI material density is not used, but it must be specified anyway for input completeness, see Page C.295.
BARY

Optional specification of the method that should be used to compute the center of gravity (barycenter) of the body. The value 0 (default) means using the nodal masses, located at the rigid nodes composing the body. The value 1 means using the element masses, located at the centroids of the rigid elements composing the body. An element’s centroid is computed as the (non-weighted) arithmetic average of the element’s nodal positions. In general, this is only an approximation of the real center of gravity (barycenter) of the element. The value 2 means decomposing each element into simplexes (triangles or tetrahedrons) and then using analytical formulas over each simplex in order to compute the barycenter of the whole body. The value 3 means that the user specifies the coordinates of the barycenter, by the following GX, GY and GZ (3D only) keywords. In this latter case the value of the RIGI material density is not used, but it must be specified anyway for input completeness, see Page C.295.
INER

Optional specification of the method that should be used to compute the tensor of inertia of the body with respect to three mutually perpendicular axes parallel to the global axes and passing through the barycenter of the body. The value 0 (default) means using the nodal masses, located at the rigid nodes composing the body. The value 1 means using the element masses, located at the centroids of the rigid elements composing the body. An element’s centroid is computed as the (non-weighted) arithmetic average of the element’s nodal positions. In general, this is only an approximation of the real center of gravity (barycenter) of the element. The value 2 means decomposing each element into simplexes (triangles or tetrahedrons) and then using analytical formulas over each simplex in order to assemble the inertia tensor of the whole body. The value 3 means that the user specifies the tensor of inertia by the following JXX, JXY, JZZ, JYZ, JXZ and JXY keywords. In this latter case the value of the RIGI material density is not used, but it must be specified anyway for input completeness, see Page C.295.
/LECT/

List of the elements defining the rigid body.

Comments :

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.


Previous Up Next