Previous Up Next

5  GROUP B—MESH AND GRID MOTION

B.10


Object:


The following directives enable to define the mesh.


Syntax:

Comments:


These directives are described in detail on the following pages.


The GEOM directive accepts some simple optional mesh manipulation commands that can be used to scale, shift, etc. the mesh read from an external mesh generator before starting the transient calculation. These commands affect only the nodal coordinates, but not the mesh connectivity. They are described below on page B.15.

5.1  OPTIONAL MESH MANIPULATION COMMANDS

B.15


Object:


To manipulate the mesh coordinates read from an external mesh generator before starting the transient calculation. For example, the mesh can be scaled, translated, centred, etc. Note that these commands only affect the (initial) nodal coordinates, they do not affect the elements (i.e. the connectivity).


Syntax:

    < SCAL $[ FACT fc ;
              FACX fx ; FACY fy ; <FACZ fz> ]$ >
    < SHIF $[ CENT ;
              SHIX sx SHIY sy <SHIZ sz> ]$ >


SCAL

Scale the coordinates of the mesh to be subsequently read in input either isotropically (i.e. by the same factor fc along all axes), or anisotropically.
fc

Isotropic scaling factor.
fx

Scaling factor along the x direction (by default 1.0).
fy

Scaling factor along the y direction (by default 1.0).
fz

Scaling factor along the z direction (by default 1.0).
SHIF

Shift the coordinates of the mesh to be subsequently read in input either in such a way that it is centered around the origin, or by specified amounts in each spatial direction.
CENT

Shift the coordinates of the mesh to be read in input in such a way that it is centered around the origin.
sx

Shift along the x direction (by default 0.0).
sy

Shift along the y direction (by default 0.0).
sz

Shift along the z direction (by default 0.0).

Comments:


The above commands, in particular the scaling commands, can be useful e.g. in case the geometry has been produced by an external mesh generator in some non-standard units. For example, assume the mesh has been generated in millimetres rather than metres. To convert to metres use the command GEOM SCAL FACT 0.001 ...


Note that the mesh manipulation occurs immediately after reading the nodal coordinates, so that the coordinates printed on the listing are the corrected ones, not the ones read from the input file.


Note that in case of simultaneous mesh scaling and shifting, the scaling occurs first, then the shifting is applied. Therefore, the shift amounts should be given in the corrected (scaled) mesh units, not in the original mesh units.

5.2  MESH IN COCO-LIKE OR IN FREE FORMAT

B.20

5.2.1  GEOMETRY


Object:


To read the mesh (i.e. the nodal coordinates and the elements connectivity) either in “free” format or in a fixed (COCO-like) format.


In the first case, the mesh data are read directly from the input file.


In the second case, the (fixed) format used for the mesh data must be specified and then the mesh data can either be read directly from the main input file, or from an external file whose unit number (nl in the following) is specified by the user. This second possibility can be handy e.g. to un-clutter the main input file in case of large mesh data, or to read a (formatted) mesh data set produced by an exotic mesh generator for which no direct EPX interface exists.


Syntax:

    "GEOM"  $[        < "LIBR" >   < "POLA" >      ;
              < nl > < '(format1)'  '(format2)' > ]$

    "POIN"  npoin


LIBR

The file describing the geometry will be read in free format.
POLA

Nodes are specified by their polar coordinates (by default Cartesian coordinates). In 2D, first enter the radius (R), then the angle (θ) in degrees for each node. In 3D, the third coordinate is interpreted as the elevation Z, thus the coordinate system is cylindrical. The corresponding Cartesian coordinates are computed according to: x=Rcos(θ), y=Rsin(θ) and z=Z (3D only).
nl

Logical number of input unit (file) from which the geometry will be read. By default, nl=5 (15 at JRC). If it is omitted, then the core will read the mesh data directly from the (main) input file.
format1

Reading format of nodal coordinates. By default format1=6E12.5.
format2

Reading format of the numbers of the nodes composing the elements (i.e. the elements connectivity). By default format2=18I4.
npoin

Exact number of mesh nodes.

Comments:


If nothing is specified after the word "GEOM", the file describing the geometry is assumed to be in COCO format, it is read from logical unit 5 (15 at JRC) with the formats: format1 and format2.


If the formats are modified, they must be enclosed in parentheses AND in apostrophes.


Example:

    "GEOM"  '(5E20.12)' '(16I5)'  "POIN" 123


The option "LIBR" is particularly useful for a simple mesh when the user himself prepares the coordinates and the topology.


In the case of polar coordinates, EUROPLEXUS transforms them into Cartesian coordinates for the following computations. If outputs in polar coordinates are desired, see keyword "OPTION".


The number of nodes npoin must not be greater than the number declared for the dimension (page A.40).


In order to read the mesh data from an external file, specify the nl unit number (an integer value) just after the GEOM keyword. This is treated as a file without a name. In Fortran, the actual (default) name of the file may vary depending upon the platform. For example, under Windows by choosing unit number 9, the code will try to open a file called fort.9 for reading and will attempt reading the mesh data from this file. It is the responsibility of the User (or of the code-launching procedure) to make such a file available on the current directory. Under Windows, for example, unit 9 is the unit normally devoted to the .msh file, in case of mesh produced by Cast3m. Therefore the launching procedure automatically creates a fort.9 file by copying the .msh file (if this exists). So the simplest way to read the mesh from an external file under Windows is to use the value 9 for nl (GEOM 9 ...) and to put the formatted mesh data in a file called <base>.msh where <base> is the base name of the main input file. See also the practical examples below.

5.2.2  ELEMENT ZONES

B.30


Object:


Each of the following keywords defines a zone of elements of the given type, that are sequentially numbered.


Syntax:
    | "typ1" n1 "typ2" n2 ... |

      "TERM"

    ...   COCO data set with its title
            (title is optional if free format, see "LIBR")  ...


typi

Name of an element type (see page I.80).
ni

Number of elements in the zone
TERM

Marks the end of the directive GEOMETRY.

Comments:


The various elements are described on page INT.80.


The number of the elements announced for a zone must correspond exactly to the elements defined in the COCO data set.


The same type of element can occupy several zones.


The number of zones must be less than or equal to the one given during the dimensioning (p. A.40).


In the COCO data set, the topology of the elements must be read by zones, and these zones are arranged in the order of their definition in the directive "GEOM".


The word "TERM" is compulsory to indicate the end of the keyword GEOMETRY.


The title appearing before the coordinates of the points is not compulsory when reading in FREE format (see "LIBR").


In order to become acquainted with the keyword "GEOM" the user may have a look at the examples on pages EX 10 and on the following ones.


Warning


There is a mandatory logical order for the 1-D elements (except ED1D). These elements are to be subdivided in 3 groups, which are respectively:

- 1st group: TUBE and TUYA,
- 2nd group: CL1D and CLTU,
- 3rd group: CAVI and BIFU.


Further information allowing to completely define the properties of "CAVI" and "BIFU" elements are given by the "RACCORD" sub-directive of the "COMPLEMENT" directive (GBC_0080).


The elements of type "BIFU" cause the automatic generation of connections between the concerned d.o.f.s. It is therefore mandatory to list them again in the "LIAISON" directive: see this directive.


The junction elements "CAVI" and "BIFU" must possess the same materials as the neighbour elements of which they ensure the continuity.

5.2.3  EXAMPLE: MESH FROM FORMATTED EXTERNAL FILE

B.35


Hereafter a simple example is given of how to read the mesh data with a fixed (COCO-like) format. In a first case, we will read the data directly from the (main) input file. Then we will show how to read the data from an auxiliary file, so that the (main) input file is more compact and legible.


Here is the complete input file with formatted mesh read directly from the main input file (test00.epx):

TEST00 - MESH READ FROM THE MAIN INPUT FILE WITH FIXED FORMAT
LAGR AXIS
GEOM '(2E22.15)' '(7I10)' POIN 18
     Q92 1 Q93 1 ED01 2 TERM
The following is the mesh data in fixed format
 1.000000000000000E+00 0.000000000000000E+00
 1.500000000000000E+00 0.000000000000000E+00
 2.000000000000000E+00 0.000000000000000E+00
 2.500000000000000E+00 0.000000000000000E+00
 3.000000000000000E+00 0.000000000000000E+00
 1.000000000000000E+00 0.500000000000000E+00
 1.500000000000000E+00 0.500000000000000E+00
 2.000000000000000E+00 0.500000000000000E+00
 2.500000000000000E+00 0.500000000000000E+00
 3.000000000000000E+00 0.500000000000000E+00
 1.000000000000000E+00 1.000000000000000E+00
 1.500000000000000E+00 1.000000000000000E+00
 2.000000000000000E+00 1.000000000000000E+00
 2.500000000000000E+00 1.000000000000000E+00
 3.000000000000000E+00 1.000000000000000E+00
 0.000000000000000E+00 0.000000000000000E+00
 1.000000000000000E+00 1.000000000000000E+00
 1.000000000000000E+00 2.000000000000000E+00
         1         2         3         8        13        12        11
         6         7
         3         4         5        10        15        14        13
         8         9
        16        17        17        18
* Mesh data is finished, we continue reading the (main) input data
COMP EPAI 1. LECT 1 PAS 1 4 TERM
MATE VM23 RO 8000. YOUN 1.D11 NU 0.3 ELAS 2.D8
          TRAC 3 2.D8 2.D-3 3.D8 1. 3.1D8 2.
          LECT 1 2 TERM
     VM23 RO 4000. YOUN 2.D11 NU 0.2 ELAS 4.D8
          TRAC 2 4.D8 2.D-3 6.D8 1.
          LECT 3 4 TERM
LINK COUP
     BLOQ 12 LECT 5 PAS 5 15 TERM
     BLOQ 123 LECT 16 TERM
INIT VITE 2 300 LECT 6 PAS 1 9 TERM
     VITE 1 -200 LECT 6 PAS 1 8 TERM
     VITE 2 -100 LECT 17 TERM
     VITE 1 200 LECT 18 TERM
ECRI DEPL VITE ACCE FINT FEXT FLIA FDEC CONT ECRO FREQ 100
     FICH ALIC FREQ 1
OPTI PAS UTIL NOTE LOG 1
CALCUL TINI 0. TEND 0.001D0 PASF 1.D-5
FIN


The data are read directly from the main input file because no unit number (nl) is specified after the GEOM keyword. Instead of using the default reading formats we choose a format 2E22.15 for the nodal coordinates and a format 7I10 for the connectivity.


Note that a comment line (reading “The following is the mesh data in fixed format”) must be put before the actual mesh data.


The mesh data start with the nodal coordinates. Two values (in 2D cases) or three values (in 3D cases) must be specified for each node, and this for the exact number of nodes (POIN) chosen by the user. Coordinates are read as a single block of data using the user-specified format.


Then, the element connectivity has to be specified, i.e. the nodes of each element. These data are read element zone by element zone, since each element type may have a different number of nodes. The element zones correspond to the declaration of the element types given by the user (Q92 1 Q93 1 ED01 2, i.e. three zones in the example).


In this example, the first zone has a single Q92 element, which has 9 nodes. This takes two lines of input to specify, since we have chosen to put only seven values per line. The second zone has one Q93 element and is similar to the first one. The third and last zone contains two ED01 elements, each with two nodes. Only one line (4 values) of input is needed for this.


Now we show how to modify the previous example in order to read the mesh data from an external input file.


The main input file (test01.epx) reads:

TEST01 - MESH READ FROM AN AUXILIARY INPUT FILE WITH FIXED FORMAT
LAGR AXIS
GEOM 9 '(2E22.15)' '(7I10)' POIN 18
     Q92 1 Q93 1 ED01 2 TERM
* Mesh data is finished, we continue reading the (main) input data
COMP EPAI 1. LECT 1 PAS 1 4 TERM
MATE VM23 RO 8000. YOUN 1.D11 NU 0.3 ELAS 2.D8
          TRAC 3 2.D8 2.D-3 3.D8 1. 3.1D8 2.
          LECT 1 2 TERM
     VM23 RO 4000. YOUN 2.D11 NU 0.2 ELAS 4.D8
          TRAC 2 4.D8 2.D-3 6.D8 1.
          LECT 3 4 TERM
LINK COUP
     BLOQ 12 LECT 5 PAS 5 15 TERM
     BLOQ 123 LECT 16 TERM
INIT VITE 2 300 LECT 6 PAS 1 9 TERM
     VITE 1 -200 LECT 6 PAS 1 8 TERM
     VITE 2 -100 LECT 17 TERM
     VITE 1 200 LECT 18 TERM
ECRI DEPL VITE ACCE FINT FEXT FLIA FDEC CONT ECRO FREQ 100
     FICH ALIC FREQ 1
OPTI PAS UTIL NOTE LOG 1
CALCUL TINI 0. TEND 0.001D0 PASF 1.D-5
FIN

We have chosen 9 as the unit number for the external file from which the mesh data will be read (GEOM 9 ...). Under Windows, this unit is automatically connected to the file .msh corresponding to the main input file, i.e. the launching procedure copies the .msh file onto a local file called fort.9, from which the mesh data will be read. If a different unit number is chosen, say 34, it is the responsibility of the user to provide a file fort.34 containing the mesh data in the current directory.


The mesh file (test01.msh) reads:

The following is the mesh data in fixed format
 1.000000000000000E+00 0.000000000000000E+00
 1.500000000000000E+00 0.000000000000000E+00
 2.000000000000000E+00 0.000000000000000E+00
 2.500000000000000E+00 0.000000000000000E+00
 3.000000000000000E+00 0.000000000000000E+00
 1.000000000000000E+00 0.500000000000000E+00
 1.500000000000000E+00 0.500000000000000E+00
 2.000000000000000E+00 0.500000000000000E+00
 2.500000000000000E+00 0.500000000000000E+00
 3.000000000000000E+00 0.500000000000000E+00
 1.000000000000000E+00 1.000000000000000E+00
 1.500000000000000E+00 1.000000000000000E+00
 2.000000000000000E+00 1.000000000000000E+00
 2.500000000000000E+00 1.000000000000000E+00
 3.000000000000000E+00 1.000000000000000E+00
 0.000000000000000E+00 0.000000000000000E+00
 1.000000000000000E+00 1.000000000000000E+00
 1.000000000000000E+00 2.000000000000000E+00
         1         2         3         8        13        12        11
         6         7
         3         4         5        10        15        14        13
         8         9
        16        17        17        18

5.3  MESH BY MEANS OF GIBI OR CASTEM2000

B.40


Object:


To define the objects associated to each element type.


Syntax:
    "GEOM"  (  "nomelm"  (  'nomobjet'  )  )  "TERM"

nomelm

Name defining the type of element to be taken from the list of available elements.
’nomobjet’

Name of the GIBI object(s)
TERM

End of the directive "GEOM"

Comments:


The names of the available elements may be found on page INT.80, the same keywords are used as in the case of COCO or free-format data (see the chapter ELEMENT ZONES).


The names of the elements cannot be used for other purposes. This explains why the names of the GIBI objects cannot begin with the same first four letters as the name of an element.


Several objects may be associated to a certain type of element. In order to obtain, on the GIBI drawings, the same node and element numbers as on EUROPLEXUS, write in GIBI:


    "TRAC" ('objet1' "ET" 'objet2' "ET" 'objet3') ...;


in the same order as for the instruction "GEOM" of the EUROPLEXUS program.


There is a zone each time a name of an element is specified. Do not forget to sufficiently dimension the number of zones (page A.40).


Warning


The elements with variable number of nodes such as "CAVI" and "BIFU" may be simply generated by GIBI by means of so-called super-elements:

    my_junction = 'MANU' 'SUPE' pt1 pt2 ... ptn ;


It is also possible to use topologically equivalent elements:

    my_junct_1 = 'MANU' 'POI1' pt1 ;
    my_junct_2 = 'MANU' 'SEG2' pt1 pt2 ;
    my_junct_3 = 'MANU' 'TRI3' pt1 pt2 pt3 ;
    my_junct_4 = 'MANU' 'QUA4' pt1 pt2 pt3 pt4 ;
    my_junct_5 = 'MANU' 'PYR5' pt1 pt2 pt3 pt4 pt5 ;
       etc...


However, in order to generate a K2000 file correct for post-treatment, it is necessary that such objects be formed by one single element.


The elements of type "BIFU" cause the automatic generation of connections between the concerned d.o.f.s. It is therefore mandatory to list them again in the "LIAISON" directive: see this directive.

5.4  Superposed elements in a Cast3m mesh (color problem)

B.41


A problem may arise with meshes generated by Cast3m containing superposed elements, for example a structure made of 3D shells to which a layer of CLxx elements is attached in order to apply an external pressure. In this case, each structural element has the same nodes as the corresponding CLxx element.


EPX treats superposed elements correctly (i.e., in the way that is probably expected by the user) only if the two elements have different colors. If the color is the same, the two superposed elements are accepted (without error messages) and are made part of the EPX mesh. However, they are eliminated from the Cast3m object names, and therefore these objects contain the wrong elements (the structural objects end up containing the CLxx elements). The problem seems to occur only when the CLxx object is a complex one (i.e. if it has sub-objects), that is when there is more than one pressure sub-object.


To avoid the problem the following simple rule may be used: to generate CLxx elements (say object pres) in Cast3m, starting from a set of existing (shell-like) structural elements (say object stru), use the following syntax:

  pres = stru COUL ROUG;

where it is assumed that the stru object either has no color or has a color different from ROUG. This ensures that the pres and stru objects have different colors and will be correctly read in by EPX.


The frequently used alternative syntax:

  pres = stru PLUS (0 0 0);
  ELIM tol (pres ET stru);

is strongly discouraged (although as said it seems to work when stru is a single object, without sub-objects).

5.5  MESH BY MEANS OF I-DEAS

B.50


Object:


To read the coordinates of the nodes and the topology of the elements from an I-DEAS universal file. The elements are declared through a list of keywords defining zones of elements of the given type, that are sequentially numbered.


Syntax:

  "GEOM" | "typ1" n1 "typ2" n2 ... | "TERM"

  (same as "Mesh by means of GIBI or CASTEM 2000")


Comments:


Even when reading from an I-DEAS mesh, the topology of the elements has to be read by zones, as defined in the directive GEOM. The user has to be sure that the list of zones declared is consistent with the data contained in the I-DEAS universal file used. In order to make this easy, a first run using the REWR option (see Page A.30) can be carried out; the informations to be set into the GEOM list can be obtained from the table printed on the listing file.


The word TERM is compulsory to indicate the end of the keyword GEOM.

5.6  MESH BY MEANS OF LS-DYNA K-FILE

B.55


Object:


To read the coordinates of the nodes and the topology of the elements from an LS-DYNA k-file. The elements can be defined in the k-file by using the PART command. No materials or element type must be assigned to the PART in the k-file. The elements are simply defined by a list and can be grouped by node lists. The k-file can be created by using the free LS-PREPOST software.


Syntax:

  "GEOM" | "typ1" PART n1 "typ2" PART n2 "typ3" ESET n3 ... | "TERM"
n1, n2

Elements taken from PART n1, n2 (also the part name can be used with a maximum length of 4 characters)
n3

Elements taken from element set n3 (also the set name can be used with a maximum length of 4 characters)

In the same way, the geometry objects (PART, ESET, NSET, NODE, ELEM) can be addressed later on e.g. for the material or the boundary conditions (see also GBINT_0050).


Comments:


The following k-file keywords are interpreted:


The word TERM is compulsory to indicate the end of the keyword GEOM.


The names of the available elements may be found on GBINT_0080.

5.7  GRID MOTION IN AN A.L.E. COMPUTATION

B.60


Object:


These keywords enable the user to impose the motion of the mesh under the Arbitrary Lagrangian Eulerian (ALE) formulation. Therefore, this directive can only be used in an ALE computation (see keyword "ALE" on page A.30).


Attention!


If you use any "RACCORDS" 1D ("CAVI" and "BIFU"), the "GRIL" directive must be placed after the directive "COMPLEMENT" (see GBC_0010).


Syntax:

    "GRILLE"  <  "LAGRANGE"   /LECTURE/      >
              <  "EULE"       /LECTURE/      >
              <  "FS"         /LECTURE/      >
              <  "BFIXE"      /LECTURE/      >
              <  "GRFS"       /LECTURE/      >

              <  "SUIVRE"  ... >
              <  "LIGNE"   ... >
              <  "CONTOUR" ... >
              <  "PLAN"    ... >
              <  "TETR"    ... >
              <  "HEXA"    ... >
              <  "PRIS"    ... >
              <  "PYRA"    ... >
              <  "SLIP"    ... >
              <  "AUTO"    ... >
              <  "MEAN"    ... >
              <  "DIRE"    ... >
              <  "QUAD"    ... >
              <  "SPEC"    ... >
              <  "MECA"    ... >
              <  "GLOB"    ... >
LAGRANGE

The following nodes are Lagrangian: the mesh is fixed to material particles.
EULE

List of nodes explicitly declared Eulerian, they are fixed in space but they correspond to different material particles at different times, in general.
FS

The user has to mention all the elements of the fluid-structure type in contact with ALE continuum (fluid) elements. In this case, the keyword "SUIVRE", to ensure the continuity of the mesh, is redundant: the keyword "FS" will do it automatically.
"BFIXE"

The following nodes will be considered as fixed (purely Eulerian). This directive allows thus to specify all the fixed nodes that will serve as base points for manual rezoning options to be entered successively.
"GRFS"

The following elements must be of the CLxx type and their nodes must be geometrically coincident with structural nodes belonging to shell elements. During the calculation, the fluid nodes will be piloted by the corresponding structural nodes like if the "SUIVRE" directive would have been specified. These elements must always be associated to the "IMPE" "GRFS" material.

Comments:


If the motion of a node is not specified, then it is supposed to be Eulerian (fixed mesh).


Several options may be set for the fine-tuning of the automatic rezoning algorithms. For more information, please see the OPTI REZO directive in GBH_0150.


For the directive GLOB see section GBB_0136.


Warning:


Do not repeat the fluid-structure couplings in the instruction "LIAISON" (except in very specific cases: perforated plates described on GBC_0330).


Do not forget to dimension sufficiently: "NALE" described on GBC_0040 (number of A.L.E. or Eulerian nodes).


The order in which the different directives appear (LAGRANGE, BFIXE, FS, SUIVRE, CONTOUR...) is important: EUROPLEXUS follows the same order during the remeshing operations.

The following rule holds:

1) A node that has to be used as base (master) point for the motion of other points must have a defined motion, else it will be considered as fixed.

2) When a point is already used as base point, its motion may no longer be re-defined.


The order of instructions use more often is:

1) First, the LAGRANGIAN nodes are defined;

2) Then, one passes to a first manual rezoning directive among (SUIVRE, LIGNE, ...) by respecting the following rule: a node may be used as base point only if its motion is already defined previously.

The points defined by this directive may then be used as base points for the following directives.


Restrictions for 1-D problems:


In the presence of bifurcations or cavities (elements "BIFU" and "CAVI"), their junctions must be defined BEFORE specifying grid motions. For further details see the directive "COMPLEMENT", sub-directive "RACCORD".


It is useless to define a grid motion for elements "TUYA". In fact, they result from the assembly of an element of type "POUT" and one of type "TUBE", and the "grid" for the internal fluid is nothing but the set of nodes that define the tube walls. EUROPLEXUS automatically ensures their motion.


In the case of "TUBE" elements, as they have just one d.o.f., this will necessarily be the first one, and only the first component will be driven. Therefore, make sure that these elements are parallel to the Ox axis.


Furthermore, for "TUBE" elements for which the length must change, one should first make sure that the orientation of the global Ox axis and the local orientations of the nodes belonging to the "TUBE" elements to be driven are coherent. In fact the velocity computed by EUROPLEXUS in these nodes has a sign which depends from this orientation.

5.7.1  AUXILIARY FILE

B.65


Object :


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


Syntax :

    "GRILLE"     < "FICHIER"   'nom.fic'  >


In certain cases these data may be bulky. Then it is advisable to store them on an auxiliary file in order to shorten the main data file. The auxiliary file is activated by means of the directive "FICHIER", followed by the name (complete under Unix) of the file. Then, in the main data file remains only the keyword "GRILLE", followed by "FICHIER".


The auxiliary file (in free format) will contain all grid rezoning data, except the "GRILLE" keyword. In order to return to reading from the main input file, the auxiliary file must terminate by the keyword "RETOUR".

5.7.2  “SUIVRE”

B.70


Object:


To force one or more A.L.E. mesh nodes to follow the motion of a "base" node.


Syntax:

    "SUIVRE"    "BASE"   /LECTURE/
                "LIST"   /LECTURE/
BASE /LECTURE/

Number of the "base" node to be followed.
LIST /LECTURE/

Numbers of the A.L.E. nodes with an imposed motion.

Comments:


The particle which is present at the node is changing all the time. This instruction is therefore very different from imposing a node to be Lagrangian.


Warning:


Please read the rule for defining the base points, page B.60.

5.7.3  “LIGNE”

B.80


Object:


To impose the motion of several nodes so that they remain aligned between two “base” nodes . The initial subdivision is maintained: the segments remain in the same relation.


Syntax:

    "LIGNE"     "BASE"   /LECTURE/
                "LIST"   /LECTURE/
"BASE" /LECTURE/

Numbers of the 2 base nodes which will impose the motion.
"LIST" /LECTURE/

Numbers of A.L.E. nodes lying between the two proceeding points and following the motion. The list can safely include also the two base nodes: if present, they are automatically discarded from the list.

Comments:


It is possible to have roughly aligned points, but if the basic points are very distant from each other, the computation tends to realign the points (and vice versa).


Warning:


Please read the rule for defining the base points, page B.60.

5.7.4  “PLAN”

B.90


Object:


To impose a homeomorphic motion to several nodes of the grid describing a triangle or a quadrangle. This command is available both in 2D and in 3D. In the 3D case, all slave points should lie at least approximately on the plane defined by the triangle or quadrangle.


Syntax:

    "PLAN"      "BASE"   /LECTURE/
                "LIST"   /LECTURE/
"BASE" /LECTURE/

Numbers of the base points composing a triangle (3 points) or a quadrangle (4 points).
"LIST" /LECTURE/

Numbers of A.L.E. points submitted to homeomorphic motion. These nodes must be located inside the basic triangle or quadrangle, or on their boundaries. The list can safely include also the base nodes: if present, they are automatically discarded from the list.

Comments:


It is strongly recommended to use quadrangles. Triangles are only useful if the initial mesh already has a triangular shape.


Warning:


Please read the rule for defining the base points, page B.60.

5.7.5  “TETR”

B.95


Object:


To impose a homeomorphic motion to several nodes of the grid describing a tetrahedron. This command is available only in 3D.


Syntax:

    "TETR"      "BASE"   /LECTURE/
                "LIST"   /LECTURE/
"BASE" /LECTURE/

Numbers of the 4 (usually Lagrangian) base points defining the tetrahedron. These points should not be coplanar.
"LIST" /LECTURE/

Numbers of A.L.E. points submitted to homeomorphic motion. These nodes must be located inside the basic tetrahedron or along its boundaries. The list can safely include also the base nodes: if present, they are automatically discarded from the list.

Warning:


Please read the rule for defining the base points, page B.60.

5.7.6  “HEXA”

B.97


Object:


To impose a homeomorphic motion to several nodes of the grid describing a hexahedron. This command is available only in 3D.


Syntax:

    "HEXA"      "BASE"   /LECTURE/
                "LIST"   /LECTURE/
"BASE" /LECTURE/

Numbers of the 8 (usually Lagrangian) base points defining the hexahedron.
"LIST" /LECTURE/

Numbers of A.L.E. points submitted to homeomorphic motion. These nodes must be located inside the basic hexahedron or along its boundaries. The list can safely include also the base nodes: if present, they are automatically discarded from the list.

Warning:


Please read the rule for defining the base points, page B.60.

5.7.7  “PRIS”

B.98


Object:


To impose a homeomorphic motion to several nodes of the grid describing a prism. This command is available only in 3D.


Syntax:

    "PRIS"      "BASE"   /LECTURE/
                "LIST"   /LECTURE/
"BASE" /LECTURE/

Numbers of the 6 (usually Lagrangian) base points defining the tetrahedron.
"LIST" /LECTURE/

Numbers of A.L.E. points submitted to homeomorphic motion. These nodes must be located inside the basic prism or along its boundaries. The list can safely include also the base nodes: if present, they are automatically discarded from the list.

Warning:


Please read the rule for defining the base points, page B.60.

5.7.8  “PYRA”

B.99


Object:


To impose a homeomorphic motion to several nodes of the grid describing a pyramid. This command is available only in 3D.


Syntax:

    "PYRA"      "BASE"   /LECTURE/
                "LIST"   /LECTURE/
"BASE" /LECTURE/

Numbers of the 6 (usually Lagrangian) base points defining the pyramid.
"LIST" /LECTURE/

Numbers of A.L.E. points submitted to homeomorphic motion. These nodes must be located inside the basic pyramid or along its boundaries. The list can safely include also the base nodes: if present, they are automatically discarded from the list.

Warning:


Please read the rule for defining the base points, page B.60.

5.7.9  “CONTOUR”

B.100


Object:


To impose a homeomorphic motion to the grid nodes inside a given bounded area.


Syntax:

    "CONT"  <"NORM" "NX" nx "NY" ny <"NZ" nz> <"ORDB">>
                                               "BASE" /LECTURE/
                                               "LIST" /LECTURE/
"NORM"

Introduces the optional definition of the normal direction. This is the direction along which the contour will be deformed. For example, in case of impact on a circular pipe, the contour is initially a circle but later on is squeezed to an ellipsis or even a concave shape. In this case the normal direction coincides with the direction of the impact.
"NX"

Component of the normal along x.
"NY"

Component of the normal along y.
"NZ"

Component of the normal along z (3D only).
"ORDB"

Let the code try to order the base nodes given (in random order) in the following BASE sub-directive.
"BASE" /LECTURE/

Numbers of the base nodes defining the boundary. If no normal is specified, these can be given in any order. However, if a normal is specified, the nodes are assumed to be listed in the order they occur along the contour (starting from any node on the contour). If an odered list is not available, by specifying the optional ORDB keyword, the code itself tries to order the base nodes. Note, however, that the ordering can only succeed if the base nodes lie approximately on a plane and form a convex contour.
"LIST" /LECTURE/

Numbers of the ALE nodes submitted to the homeomorphic motion (in any order). In principle these nodes should be located inside the bounded area, they may not be on the contour. However, the list can safely include also the base nodes (on the contour): if present, they are automatically discarded from the list.

Comments:


It is recommended to use the facilities offered in GIBI by the keywords "CONTOUR" and "ENVELOPPE".


For ease of use, EUROPLEXUS accepts that among the points defined by "LIST" there be also the base points. These points will be then removed by a special treatment within the code.


Otherwise, one can also separate the internal points from those on the contour, as shown in the following example.


Given an object "LIQ", the user wants to distinguish its internal nodes (ALE) from the nodes defining the outline of the surface (Lagrangian).

  In GIBI:

    TLIQ = LIQ changer POI1   ;
    CLIQ = contour LIQ        ;
    CLIQ = CLIQ changer POI1  ;
    ILIQ = TLIQ differ  CLIQ  ;

  In EUROPLEXUS:

    CONTOUR BASE LECTURE CLIQ TERM
            LIST LECTURE ILIQ TERM


This directive should be relatively robust for translation and rigid rotation of the contour. It should perform well also for moderate deformation of the contour itself, provided the contour is initially convex (ideally, similar to a circle).

If the contour is (or becomes, due to deformation) concave, then the algorithm does not perform well in general. In this case, if the direction of the (predominant) deformation of the contour is known a priori, it is advised to specify it via the optional NORM keyword.

Recall, however, that in this case the list of base nodes (on the contour) should normally be given in the order they occur along the contour (starting from an arbitrary node). If an ordered list of the nodes is not available, you can try giving them in random order and specifying the optional ORDB keyword.

5.7.10  “SLIP”

B.108


Object:


Define 2D curves consisting of nodes that are allowed to slip tangentially to the curve itself. This only applies to ALE models in structures or fluids.


Syntax:

    "SLIP"    |[ "NORM" /LECTURE/  ;
                 "EQUI" /LECTURE/ ]|
"SLIP"

The following nodes belong to a curve (in 2D) that is Lagrangian in the normal direction but ALE in the tangential direction. Examples are free surfaces in fluids, free boundaries in solids treated by the ALE method for structures, or interfaces between different materials that should not be mixed. Sliding in the tangential direction can be of two types: a) no sliding (only normal motion) or b) slide tangentially so as to keep nodes nearly equidistant.
"NORM" /LECTURE/

The specified nodes will only move along the normal direction to the curve.
"EQUI" /LECTURE/

The specified nodes will move both along the normal and along the tangential direction, so as to remain nearly equidistant from each other.

Comments


The nodes have to be listed in /LECTURE/ in the order in which they appear along the curve, and by leaving the body on the left side (for free surfaces).


Each list must include an initial and a final node, not subject to the imposed "SLIP" motion, whose positions are used to evaluate the normal direction for each triple of nodes. Therefore, each /LECTURE/ must contain at least three numbers.


Restrictions


The algorithms implemented here are only valid for "nearly straight" curves, in the sense that the angle between successive segments of the curve (element sides) must be close to 180 degrees. If this is not the case, then the mesh should be refined locally.

5.7.11  “AUTO”

B.120


Object:


Use Giuliani’s (automatic) rezoning algorithm to determine the motion of the nodes specified next.


Syntax:

   "AUTO"    |[ "AUTRES"            ;
                "NOEUDS" /LECTURE/ ]|
"AUTRES"

All the ‘remaining’ A.L.E. nodes (i.e. those which have not been forced by a ‘manual’ command such as SUIVRE, LIGNE, ...) will be automatically rezoned.
"NOEUDS" /LECTURE/

Allows to list explicitly the nodes which have to be automatically rezoned.

Comments:


Use of the automatic rezoning technique is encouraged when tackling a new problem or in cases when the node pattern and the deformation process cannot be described by simple laws such as those provided by the ‘manual’ rezoning commands. However, compatibility is ensured so that manual commands can still be used in conjunction with the automatic option in case some nodes (usually few) are not properly treated by the automatic technique.


The algorithm starts by estimating node by node, and on the basis of purely geometric criteria, the best grid velocity W that would bring to an optimal rezoning in just one step.

Then, this velocity is projected onto the fluid velocity V at the node concerned: this in order to take automatically into account possible boundary conditions imposed at the node.

Finally, the resulting module is limited in order to avoid too high remeshing velocities. This limitation is done by a coefficient γ0, i.e :

−γ0   V < W < (1 + γ0)   V 


The coefficient γ0 may be defined by the option OPTI REZO GAM0, see page H.150. This parameter does not have a large influence on remeshing, but in any case with small values of γ0 one should get a slightly more effective remeshing. Suggested values are between 0.1 and 0.8, the default is 0.2.


Note that GAM0 is a global parameter, and hence it is the same for the whole mesh. Consequently, it is recommended to "help" the remeshing algorithm, in case of need, by the manual remeshing directives such as SUIVRE, LIGNE, etc.


Note that ALE nodes lying on fluid-structure sliding lines of the ALE type (see directive FSS ALE) have to be declared as automatically rezoned. The program then automatically applies the correct sliding conditions.


The list of nodes can be given either explicitly, by a /LECTURE/, introduced by keyword NOEU, or implicitly, by keyword AUTR. In the latter case, the nodes considered are all nodes that have not been assigned any rezoning method up to the current point in the input file. The GAM0 parameter should be specified in the OPTI directive, since it applies not only to Giuliani’s but also to the other automatic remeshing methods (in fact, it is used in the mesh velocity restriction algorithm).


Several options may be set for the fine-tuning of the automatic rezoning algorithms. For more information, please see the OPTI REZO directive in Section 12.


Warning:


To date, the automatic rezoning facility is only implemented in 2D for nodes belonging to elements of type TRIA, CAR1, CAR4, FLU1, FL23, FL24, Q41, Q41N, Q42, Q42N, TRIA, CVL1, TVL1, MC23, MC24. In 3D, it is implemented for nodes belonging to elements of type FLU3, FL34, FL35, FL36, FL38, TETR, PRIS, CUBE.

5.7.12  “MEAN”

B.130


Object:


Use the mean algorithm to determine the motion of the nodes specified next. This rezoning method is available for all ALE element types.


Syntax:

    "MEAN"    $[ "NOEU" /LECTURE/  ;
                 "AUTR"           ]$
"NOEU"

The following (ALE) nodes will be rezoned by the "mean position" algorithm. The position of each node will tend to become the mean of the position of neighbour nodes. For a generic node I, neighbour nodes are those connected to it in the mesh by a straight (two-noded) element side.
"AUTR"

All other ’remaining’ ALE nodes, i.e. those that have not been forced to move by a ’manual’ command such as "SUIVRE", "LIGNE", etc., will be rezoned by the "MEAN" algorithm.

Comments:


Several options may be set for the fine-tuning of the automatic rezoning algorithms. For more information, please see the OPTI REZO directive in Section 12.

5.7.13  “DIRE”

B.131


Object:


Use the direct algorithm to determine the motion of the nodes specified next. Note, however, that this algorithm is experimental and is currently implemented only for 2D quadrilateral ALE finite elements and finite volumes.


Syntax:

   "DIRE"    $[ "NOEU" /LECTURE/  ;
                "AUTR"           ]$
"NOEU"

The following (ALE) nodes will be rezoned by the "direct" algorithm.
"AUTR"

All other ’remaining’ ALE nodes, i.e. those that have not been forced to move by a ’manual’ command such as "SUIVRE", "LIGNE", etc., will be rezoned by the "DIRE" algorithm.

Comments:


Several options may be set for the fine-tuning of the automatic rezoning algorithms. For more information, please see the OPTI REZO directive in Section 12.


Warning


This algorithm is experimental and is currently implemented only for 2D quadrilateral ALE finite elements and finite volumes.

5.7.14  “QUAD”

B.132


Object:


Use the specific quadrilateral algorithm to determine the motion of the nodes specified next. Note, however, that this algorithm is experimental and is currently implemented only for 2D quadrilateral ALE finite elements and finite volumes.


Syntax:

   "QUAD"    $[ "NOEU" /LECTURE/  ;
                "AUTR"           ]$
"NOEU"

The following (ALE) nodes will be rezoned by the "quadrilateral" algorithm.
"AUTR"

All other ’remaining’ ALE nodes, i.e. those that have not been forced to move by a ’manual’ command such as "SUIVRE", "LIGNE", etc., will be rezoned by the "QUAD" algorithm.

Comments:


Several options may be set for the fine-tuning of the automatic rezoning algorithms. For more information, please see the OPTI REZO directive in Section 12.


Warning


This algorithm is experimental and is currently implemented only for 2D quadrilateral ALE finite elements and finite volumes.

5.7.15  “SPEC”

B.133


Object:


Use the element-specific algorithm to determine the motion of the nodes specified next. Note, however, that this algorithm is experimental and is currently implemented only for 2D quadrilateral and triangular ALE finite elements and finite volumes.


Syntax:

   "SPEC"    $[ "NOEU" /LECTURE/  ;
                "AUTR"           ]$
"NOEU"

The following (ALE) nodes will be rezoned by the "specific" algorithm.
"AUTR"

All other ’remaining’ ALE nodes, i.e. those that have not been forced to move by a ’manual’ command such as "SUIVRE", "LIGNE", etc., will be rezoned by the "SPEC" algorithm.

Comments:


Several options may be set for the fine-tuning of the automatic rezoning algorithms. For more information, please see the OPTI REZO directive in Section 12.


Warning


This algorithm is experimental and is currently implemented only for 2D quadrilateral and triangular ALE finite elements and finite volumes.

5.7.16  “MECA”

B.134


Object:


Use the mechanical algorithm to determine the motion of the nodes specified next.


Syntax:

   "MECA"    $[ "NOEU" /LECTURE/  ;
                "AUTR"           ]$
"NOEU"

The following (ALE) nodes will be rezoned by the "mechanical" algorithm.
"AUTR"

All other ’remaining’ ALE nodes, i.e. those that have not been forced to move by a ’manual’ command such as "SUIVRE", "LIGNE", etc., will be rezoned by the "MECA" algorithm.

Comments:


Several options may be set for the fine-tuning of the automatic rezoning algorithms. For more information, please see the OPTI REZO directive in Section 12.


Warning


This algorithm is experimental and is currently implemented only for 2D quadrilateral ALE finite elements and finite vol- umes. Finally, in order to use this model the problem type keyword MECA must be specified in the initial part of the input file (see Section 4.2).

5.7.17  “ELAS”

B.135


Object:


Affects a fictitious elastic material to grid elements to control the motion of the ALE nodes.


Syntax:

   "ELAS"  "RO" ro "YOUNG" young "NU" nu "DAMP" damp /LECTURE/
"ro"

Fictitious material’s density.
"young"

Fictitious material’s Young modulus.
"nu"

Fictitious material’s Poisson ratio.
"damp"

Inertial damping.
/LECT/

List of the fluid elements concerned.

Comments:


At the moment, this type of rezoning is available for the following element types: TRIA, CAR1, TETR, PRIS, CUBE, T3VF, Q4VF, TEVF, PRVF, CUVF, FL23, FL24, FL34, FL36, FL38. Note that the model is not yet available for the pyramid elements (FL35 for example).


Be aware that a critical time step is computed for the explicit elastic rezoning problem to remain stable. A soft fictitious material should be used so that this time step is not smaller than the "physical" critical time step.


An large inertial damping coefficient (i.e. from 1.E3 to 1.E4) should be used to prevent vibrating oscillations of the deformed grid.


Do not forget to set option OPTI REZO LIAI (see Page H.150, Section 12.16 ), so that nodes subjected to kinematic links are rezoned accordingly.

5.7.18  “GLOB”

B.136


Object:


Option which gives the possibility to link a fluid grid to a structure


Syntax:

   "GLOB"  "DACT"  /LECDDL/ "STRU" /LECTURE/
            /LECTURE/
"DACT"

Activation of the dlls to be linked
/LECDDL/

Reading procedure of the degrees of freedom concerned.
"STRU"

/LECT/

List of the structure elements concerned.
/LECT/

List of the fluid elements concerned.

Comments:


Multiphasic law is not available with this option

5.7.19  USER’S ROUTINE “COOGRI”

B.140


Object:


This routine can be written by the user and exploited in order to specify the motion of fluid nodes when using the ALE description. Its use should be only needed in exceptional cases, because normally the automatic and manual rezoning directives are perfectly appropriate.


Since this routine is called last by routine NVCOOR any motion specified in it will overwrite any other motion, either automatic or by means of manual rezoning directives, specified by the user.


Normally, the routine does nothing.


The listing of the sample routine is included hereafter.

      SUBROUTINE COOGRI(V,WG,posp,mvgril)
C-----------------------------------------------------------------
C     ---  ROUTINE UTILISATEUR ( vitesses DE LA GRILLE )
C-----------------------------------------------------------------
c v     : fluid velocities
c wg    : mesh grid velocities
c posp  : pointer in both v and wg
C MVGRIL(I,1)
c              -1=LAGRANGIAN
c               0=EULERIAN
C               1=A.L.E.,AUTOMATICALLY REZONED (JRC);
C               2=A.L.E.,MANUALLY REZONED (CEA),
c               3=A.L.E, rezoned by FSS ALE (ALE sliding JRC)
c               4=A.L.E, "MEAN" rezoned (JRC)
C MVGRIL(I,2)   NODAL INDEXES IN THE FOLLOWING ORDER :
C                - FIRST LAGRANGIAN NODES (GROWING ORDER)
C                - THEN NON-LAGRANGIAN BASE NODES (USED AS MASTER
C                  NODES FOR MOTION OF SLAVE A.L.E. NODES)
C                - FINALLY ALL OTHER NODES
C MVGRIL(I,3)   IAD (ADDRESS IN <NBALE> AND <CBALE>) IF MVGRIL(I,1)=2
c               -1  IF NODE IS SUBJECT TO "LIAISON" AND MVGRIL(I,1)=1
C               0   IN ALL OTHER CASES
C-----------------------------------------------------------------
c
      implicit none
      include 'CONTRO.INC'
C
      double precision V(*), WG(*)
      integer posp, mvgril
C
      dimension posp(*), mvgril(*)
c
c Insert hereafter the user's definition of the appropriate
c grid velocities:
c
C
      RETURN
      END

5.8  MESH REFINEMENT FOR WAVEFRONT TRACKING

B.200


Object:


This directive enables the user to impose the refinement of the computational mesh grid to follow the propagation of one or more prescribed wave fronts. It should be used in conjunction with mesh adaptivity dimensioning directive ADAP, see page A.62. However, note that this directive is incompatible with “true” adaptivity (piloted by an error indicator) which is activated by the ADAP directive of page B.210.


Note that this model does not represent a true implementation of adaptivity, since the mesh refinement and de-refinement is entirely piloted by the user with the present directive. However, it may be useful to check the mesh refinement and de-refinement processes in simple test cases, where the propagation of wave fronts is known a priori.


For a true implementation of adaptivity (piloted by an error indicator) see the ADAP directive on page B.210.


Syntax:

    WAVE  nwav * ($ SPHE ; PLAN ; CYLI $
                  X x Y y <Z z> <NX nx NY ny <NZ nz>>
                  T0 t0 <T1 t1> C c MAXL m H1 h1 H2 h2)
WAVE

Prescribe one or more wave fronts to be tracked.
nwav

Number of wave fronts to be defined.
SPHE

The wave being defined is a spherical wave.
PLAN

The wave being defined is a plane wave.
CYLI

The wave being defined is a cylindrical wave.
x

X-coordinate of the wave source point.
y

Y-coordinate of the wave source point.
z

Z-coordinate of the wave source point (0 by default).
nx

X-component of the normal vector to the plane (for PLAN waves). X-component of the cylinder axis vector (for CYLI waves). Note that the vector need not be normalized to unit length.
ny

Y-component of the normal vector to the plane (for PLAN waves). Y-component of the cylinder axis vector (for CYLI waves).
nz

Z-component of the normal vector to the plane (for PLAN waves). Z-component of the cylinder axis vector (for CYLI waves). This is 0 by default.
t0

Time instant at which wave propagation starts from the corresponding source point.
t1

Time instant at which wave propagation terminates. The mesh is completely un-refined (thus returning to the base mesh) at times greater than this value.
c

Propagation speed of the wavefront. For spherical waves, propagation is assumed isotropic in all space directions.
m

Maximum level of mesh refinement at the wave front.
h1

Thickness of maximum refined mesh layer normally to the wave front.
h2

Thickness of refined mesh layer normally to the wave front. Refinement passes from level m to level 0 (no refinement) linearly when passing from a distance h1 to a distance h2 from the wave front.

5.9  ADAPTIVITY

B.210


Object:


This directive enables the user to impose the refinement or un-refinement of the computational mesh grid (adaptivity) in accordance to some chosen error indicator. The error indicator can be:


The directive should be used in conjunction with mesh adaptivity dimensioning directive ADAP, see page A.62.


This directive enables automatic mesh refinement and un-refinement based on some criteria chosen by the user. At the moment, no mesh unrefinement is performed by threshold-based indicators. However, note that at the moment this directive is incompatible both with the wave front tracking directive WAVE of page B.200 and with the FSI-related adaptivity directives associated with the FLSR and FLSW directives, see page D2.143 and D.555, respectively.


In contrast to the WAVE directive of page B.200, the present model represents a “true” implementation of adaptivity.


Syntax:

    ADAP  < UPDT /CTIME/ >
          ( INDI |[ DEPL ; VITE ; ACCE ;
                    PRES ; DENS ; CONT icon ; ECRO iecr ]|
            < TYPE |[ CURV ; GRAD ]| >
            STRA $[ PERR perr ; PELE pele ALFA alfa ; PEMA pema ]$
            CERR ( cerr /LECTURE/ ) )

          ( THRS |[ PRES ; DENS ; PEPS ; FAIL ;
                    CONT icon ; ECRO iecr; EPST icon ]|
                 TMIN tmin TMAX tmax MAXL maxl
                 <CRIT crit>
                 /LECTURE/ )

         $[ PCLD ( |[ INDI NIND nind MAXL maxi ELEM /LECTURE/ ;
                      THRS MAXL maxt ELEM /LECTURE/ ;
                      FSI  FLUI /LECTURE/
                           STRU /LECTURE/
                           MAXL maxf RADI radf ;
                      GAP  MAST /LECTURE/
                           SLAV /LECTURE/
                           MAXL maxg RADI radg
                      EDGE MAST /LECTURE/
                           SLAV /LECTURE/
                           MAXL maxe RADI rade
                      VOFI FLUI /LECTURE/
                           CLIM clim
                           MAXL maxv RADI radv ]| ) ]$
ADAP

Activates true adaptivity according to the error indicator(s) chosen next.

Directives related to classical error indicators
UPDT

MPI Only - Introduces an update frequency for the mesh adaptation to save computation time.
INDI

Introduces the variable(s) used as “classical” error indicator(s). Note that exactly ni variables must be specified next, where ni is the number given in the dimensioning (NIND ni), see page A.62. If the keyword NIND has been omitted in the dimensioning, then by default ni = 1.
DEPL

Use nodal displacement (norm) as error indicator.
VITE

Use nodal velocity (norm) as error indicator.
ACCE

Use nodal acceleration (norm) as error indicator.
PRES

Use (fluid) element pressure as error indicator. Only GRAD type of indicator can be used in this case.
DENS

Use (fluid) element density as error indicator. Only GRAD type of indicator can be used in this case.
CONT icon

Use element stress component icon as error indicator. Only GRAD type of indicator can be used in this case.
ECRO iecr

Use element hardening component iecr as error indicator. Only GRAD type of indicator can be used in this case.
TYPE

Introduces the types of error indicator(s). Note that exactly ni variables must be specified next, where ni is the number given in the dimensioning (NIND ni), see page A.62. The types must be entered in the same order as the indicator variables, i.e. the first type corresponds to the first indicator variable, and so on. If the keyword NIND has been omitted in the dimensioning, then by default ni = 1. If the TYPE sub-directive is omitted, all indicators are assumed to be of the curvature type.
CURV

Error indicator is of curvature type, i.e. the curvature of the indicator variable is used to compute the error indicator. This type of error indicator can be used only for the node-based indicator variables listed above (i.e. only for DEPL, VITE or ACCE).
GRAD

Error indicator is of gradient type, i.e. the gradient of the indicator variable is used to compute the error indicator. This type of error indicator can be used for all indicator variables listed above.
STRA

Introduces the strategy used for the error indicator. At the moment, two strategies are available: prescribing the error or prescribing (approximately) the number of used elements.
PERR perr

Introduces the prescribed error perr (ẽ). This is then used to compute the prescribed element size hk, see formula below.
PELE pele

Introduces the prescribed number of adaptive elements pele ( ñ ).
ALFA alfa

Coefficient α used in the formula to estimate the predicted number of elements in memory (see below). This is an empirical value. The suggested value is 4 for 2D calculations.
PEMA pema

Introduces the prescribed number of adaptive elements pema ( ñ ). This version of the command is suited for use in conjunction with the OPTI ADAP MAXL option, see page H.180. In fact when this option is specified, the PELE strategy respects very badly the prescribed number of elements. Note that the PEMA strategy requires additional calculations with respect to PELE and is therefore more expensive. Note also that the PEMA strategy makes no use of the ALFA coefficient.
CERR cerr

Introduces the choice of the constant C (cerr) appearing in the expression of the error indicator (see below). The value may vary from element to element (e.g., due to different element types). Each (parent) element in the adaptive mesh must receive a value. Descendent elements inherit the value from their own parent element.
/LECTURE/ (CERR keyword)

List of the elements to which the value cerr is assigned.

Directives related to point-cloud indicators
PCLD

Introduce point cloud-based indicators.
INDI

Base the point-cloud indicator upon one of the “classical” adaptivity indicators that have been listed above.
NIND nind

Rank nind of the concerned indicator in the INDI list of original adaptivity indicators specified above.
MAXL maxi

Maximum refinement level maxi for this indicator as a PCLD indicator.
ELEM /LECTURE/

List of the elements concerned by this PCLD indicator.
THRS

Base the point-cloud indicator upon the threshold indicator that has to be defined above.
MAXL maxt

Maximum refinement level maxi for this indicator as a PCLD indicator.
ELEM /LECTURE/

List of the elements concerned by this PCLD indicator.
FSI

Base the point-cloud indicator upon Fluid-Structure Interaction.
FLUI /LECTURE/

List of the fluid elements concerned by this PCLD indicator.
STRU /LECTURE/

List of the structure elements defining the points of the cloud.
MAXL maxf

Maximum refinement level for this PCLD indicator.
RADI radf

Influence radius associated with the structure.
GAP

Base the point-cloud indicator upon contact (gap).
MAST /LECTURE/

List of the elements defining the point cloud.
SLAV /LECTURE/

List of the slave elements concerned by this PCLD indicator.
MAXL maxg

Maximum refinement level for this PCLD indicator.
RADI radg

Influence radius associated with the master elements.
EDGE

Base the point-cloud indicator upon distance from a free shell edge (3D only).
MAST /LECTURE/

List of the shell elements defining the point cloud.
SLAV /LECTURE/

List of the slave elements concerned by this PCLD indicator.
MAXL maxg

Maximum refinement level for this PCLD indicator.
RADI radg

Influence radius associated with the free edges of the master elements.
VOFIRE

Base the point-cloud indicator upon VOFIRE anti-dissipation fo physical interface tracking.
FLUI /LECTURE/

List of the concerned fluid elements..
CLIM clim

Minimum concentration for any fluid component to identify an interface cell. One cloud point is placed at the centroid of each interface cell.
MAXL maxv

Maximum refinement level for this PCLD indicator.
RADI radv

Influence radius associated with the interface cells.

Directives related to threshold-based indicators
THRS

Introduce threshold-based indicators. Note that, at the moment, no mesh unrefinement is performed by threshold-based indicators.
PRES

Use element pressure as threshold-based indicator.
DENS

Use element density as threshold-based indicator.
PEPS

Use element principle strain as threshold-based indicator.
CONT icon

Use element stress component icon as threshold-based indicator.
EPST icon

Use element strain component icon as threshold-based indicator.
ECRO iecr

Use element hardening component iecr as threshold-based indicator.
TMIN min

Introduces the minimum threshold value tmin above which the mesh starts to be refined.
TMAX max

Introduces the maximum threshold value tmax at which the mesh refinement reaches the maximum level (specified below).
MAXL maxl

Maximum level of mesh refinement, which is reached at the value tmax of the threshold specified above.
CRIT crit

Optional criterion to be used to compute the monitored quantity’s representative value over an element. By default (or by specifying CRIT 0) the average value of the monitored quantity over all Gauss points of the element is taken. Alternatively, 1 means taking the maximum value of all the Gauss points of the element, 2 means the minimum value, 3 means the maximum absolute value. Note that alternative criteria (other than the default one based on the average) are not available at the moment for monitored quantities of type PEPS and FAIL. Therefore, the value of crit is ignored in these two cases.
/LECTURE/

List of the elements concerned by this type of mesh adaptation.

Comments for classical indicators:


For a curvature-based indicator, the expression used to compute the error indicator is:

|e| ≈ C h2 max (|k1|,|k2|) 

where C is the constant cerr given in input for the current element, h is the local mesh size (i.e. the characteristic length of the element under consideration), k1 and k2 are the principal curvatures of the variable chosen as error indicator on a patch composed by the element itself and by all its direct neighbors.


For a gradient-based indicator, the expression used to compute the error indicator is:

|e| ≈ C h ||G|| 

where C is the constant cerr given in input for the current element, h is the local mesh size (i.e. the characteristic length of the element under consideration), ||G|| is the norm of the gradient of the variable chosen as error indicator on a patch composed by the element itself and by all its direct neighbors.


The expression used to compute the prescribed element size hk is:

hk = 
ek
 hk,   k=1,…,N 

where N is the current number of active elements in the mesh, and ek in the estimated error in the k-th element.


The expression used to estimate the number of elements ñ in memory is:

ñ ≈ 
α
 
N
k=1
 ek 

This formula is actually used to compute ẽ:

ẽ ≈ 
α
ñ
 
N
k=1
 ek 

and then the above formula gives hk .


Comments for PCLD indicators:


The PCLD subdirective introduces particular indicators designed to be combined with one another.


They are mainly based on simple distance relations between the centroids of slave elements and some master points attached to chosen elements, defining a cloud of points. The minimum distance between a slave centroid and any point of the cloud (which can be seen as the projection of the point onto the cloud) defines the refinement level of the slave element, according to the ratio between this distance and the given radius. The given maximum refinement level is applied to the elements closest to the cloud, and then decreasingly for farther elements.


To be combined with other PCLD indicators, original adaptivity indicators must be slightly reformulated. This is the goal of the PCLD INDI sub-option.


Comments for threshold-based indicators:


Note that, at the moment, no mesh unrefinement is performed by threshold-based indicators.


The mesh refinement level varies linearly between 1 and maxl as the monitored value passes from tmin to tmax.


Previous Up Next