Previous Up Next

11  GROUP G—PRINTOUT AND STORAGE OF RESULTS

G.10


Object:


The ECRITURE directive enables the user to specify the requested printouts and data storages during a computation (including data saving for successive restart).


The REGION directive enables to define certain “regions” of the mesh, on which the printout of results will then be performed.


The MEASURE directive enables to request the printout of various “measurements” on the current geometrical mesh.


Syntax:
  < ECRITURE  . . .  /CTIM/
        <  NOPO  ;  POIN  /LECTURE/  >
        <  NOEL  ;  ELEM  /LECTURE/  >
        <  FICH . . .                > >

  < REGION  ( 'nom region'  . . .  )   >

  < MEASURE ...                        >



Comments:


The keyword ECRI must only appear once in an input sequence. It allows to specify the values to be printed on the listing file, and the nodes and elements for which these values must be printed.


Furthermore, the directive allows to define which results files should be produced, in view of a subsequent post-processing.


If the keyword ECRI is absent, a printout is performed for all the time steps, all the nodes and all the elements of the mesh.


In the following subsections, first a general description of the ECRI directive is given. Then, all the optional keywords (NOPO ...) and optional sub-directives (FICH ...) are described below. Output regions created by the directive REGI are described on page G.100. Finally, the MEAS directive is described on page G.105.

11.1  SELECTIVE PRINTOUTS ("ECRITURE")

G.20


Object:


The "ECRITURE" directive can be used to select specific quantities to be printed out in the output listing at user-chosen times. It allows also to choose the nodes and elements for which the quantities will be printed.


The various quantities are associated to nodes or elements as described on page G.30 and following ones.


Syntax:

   "ECRITURE"
              < "COOR" > < "DEPL" > < "VITE" >
              < "ACCE" > < "FINT" > < "FEXT" > < "FLIA" >
              < "FDEC" > < "CONT" > < "EPST" > < "ECRO" >
              < "ENER" > < "MCVA" > < "MCVC" > < "MCVS" >
              < "FAIL" > < "VFCC" >


COOR

Printout of nodal coordinates.
DEPL

Printout of nodal displacements.
VITE

Printout of nodal velocities. In ALE cases, both fluid and grid velocities are printed out.
ACCE

Printout of nodal accelerations.
FINT

Printout of nodal internal forces.
FEXT

Printout of (total) nodal external forces.
FLIA

Printout of nodal forces due to liaisons (coupled links: LINK COUP).
FDEC

Printout of nodal forces due to decoupled links: LINK DECO.
CONT

Printout of element stresses.
EPST

Printout of element total strains.
ECRO

Printout of element material parameters (hardening for solids, pressure and density for fluids, etc.).
ENER

Printout of energies.
MCVA

Printout of nodal quantities related to multicomponent fluids: pressure, density, temperature, sound speed and mass fractions. Note that this type of printout is incompatible with MCVC and MCVS.
MCVC

Printout of conserved variables (nodal quantities) related to multicomponent fluids: partial densities (ρi) of the various components i, momentum (ρ u) (each spatial component separately), energy (ρ E). Note that this type of printout is incompatible with MCVA.
MCVS

Printout of secondary variables (nodal quantities) related to multicomponent fluids: total density (ρ), total pressure p, sound speed c, pressure derivative (∂ p/∂ (ρ e)), absolute temperature (T), pressure derivative (∂ p/∂ (ρi)) for each component, mass fraction (µi) for each component. Note that this type of printout is incompatible with MCVA.
MCFL

Printout of MC numerical fluxes: partial densities (first two components), momentum (each spatial component separately) and total energy. In case of FLSR fluid-structure interaction, print out also the list of blocked MC fluxes (in the form of node couples).
MCEF

Printout of MC numerical "external" fluxes: partial densities (first two components), momentum (each spatial component separately) and total energy.
MCMU

Printout of MC "MUSCL" conserved variables (2nd order in space and time): partial densities (first two components), momentum (each spatial component separately) and total energy.
MCVM

Printout of MC volumes (at n, n+1/2 and n+1) and masses (at n+1/2, n+1 and n+3/2).
FAIL

Printout of reached failure level of the elements. This is only available if the element erosion model has been activated by means of the EROS keyword in the problem type declaration, see page A.30. A value of 0 indicates a virgin element, a value of 100 indicates a completely failed element, an intermediate value indicates the ratio (in per cent) between the number of failed Gauss points and the total number of Gauss points in the element.
VFCC

Printout at each selected output time of “element” quantities related to cell-centred Finite Volumes: various volume-related quantities and conserved variables.

Comments


The keyword "ECRITURE" should only appear once in an input data sequence. Keywords "COOR", "DEPL", etc. should immediately follow the "ECRI" keyword.


Warning:


If none of the preceding keywods is specified, nothing will be printed.


In a standard calculation (not a restart), EUROPLEXUS always prints the last computed time step.


Take care when choosing output frequencies, because the size of listing files may grow very fast.


Note that the results file of type "ALICE" allows to re-construct a listing. You may therefore choose to print out the bare minimum. Later on, if additional results need to be printed, you may do so by re-reding the "ALICE" file (which must have been specified, of course).

11.2  PRINTABLE QUANTITIES

G.25

11.2.1  NODE-RELATED QUANTITIES


For each chosen node, one may ask to print:

- current coordinates;

- displacements;

- velocities;

- accelerations;

- internal forces;

- total external forces;

- external reaction (coupled link) forces for the nodes sujected to “coupled” conditions (see LINK COUP);

- external reaction (decoupled link) forces for the nodes sujected to “decoupled” conditions (see LINK DECO);

- multi-component flow-related data (finite volumes).

Coordinates


For each chosen node, the code prints X,Y or R,Z o X,Y,Z.

Displacements, velocities, accelerations and forces


The chosen nodes are grouped by increasing number of degrees of freedom (d.o.f.). First all the nodes with 1 d.o.f. are printed, then those with 2 d.o.f.s, etc.

11.2.2  ELEMENT-RELATED QUANTITIES


For each chosen element and each integration point one may ask to print:

- the stress components (SIG);

- the deformation (EPST);

- the hardening parameters (ECR).

Stresses and material parameters


The stress tensor and the total deformation tensor are related to the element, and independent from the material.


The material parameters, contained in the ECR table, sre independent of the element, and are only function of the material.


The choices done in EUROPLEXUS for these two quantities are detailed in the following pages.

11.3  STRESSES AND DEFORMATIONS

G.30


For a given element type, the stress components have always the same meaning, for whatever material is assigned to the element. On the contrary, the hardening values (ECR) are strictly related to the chosen material, and do not depend upon the element type.


The stress tensor is stored and printed in vector form, and is printed for each integration point of the element.


Remark 1:


In 2D, it will be necessary to distinguish the axisymmetric case (AXIS) from the plane strain (DPLA) and plane stress (CPLA) cases.


Remark 2:


For continuum-like elements, the stresses are written in the global reference frame, while for the other types of elements (shells, beams, bars) they are expressed in a local frame attached to the element.


Remark 3:


Instead of computing a bending moment, one computes a “bending stress” (sigf), that may be directly compared with the membrane stresses. This bending stress is related to the bending moment as follows:

      Moment = E * I * Khi              Khi : curvature

      sigf   = E * (h/2) * Khi          h   : thickness

      Hence:     Moment = 2 * ( I / h ) * sigf

      For a shell:    Moment = ( h * h / 6 ) * sigf

2D ELEMENTS

BARR and PONC


These elements may only work in traction and compression. There is just one stress component (scalar).


COQU


This element works in membrane and bending. There are 4 stress components per element, expressed in a local reference frame.


The first direction of the local frame is along the element from node 1 to node 2. The second, located in the mesh plane, is normal to the first. The third direction is such that the reference (u, v, w) be right-handed.

     sig(1) : membrane (u)          sig(3) : bending (v)
     sig(2) : membrane (w)          sig(4) : bending (w)

COQC


Also this element works in membrane and bending. But besides the 4 preceding stress components, there is a fifth one for the shear, which is treated elastically.

     sig(1) : membrane (u)          sig(3) : bending (v)
     sig(2) : membrane (w)          sig(4) : bending (w)
                      sig(5) : shear

CONTINUUM ELEMENTS


The stress components are expressed in the global frame. For a calculation in plane stress, there are three stresses expressed in the (x, y) frame. For an axisymmetric calculation or a plane strain calculation there are 4 stress components, expressed in the frame (x, y, z). The z direction is the normal to the mesh plane, and such that (x, y, z) be right-handed.

     1) CPLA:

                    ( SIG(1)  SIG(3) )
           (sig) =  (                )
                    ( SIG(3)  SIG(2) )

     2) AXIS or DPLA:

                    ( SIG(1)  SIG(3)    0    )
                    (                        )
           (sig) =  ( SIG(3)  SIG(2)    0    )
                    (                        )
                    (   0       0     SIG(4) )

3D ELEMENTS

BR3D


Like for the BARR and PONC elements in 2D, these elements may only work in traction and compression. The stress tensor has just one component.


POUT


This element works in traction, torsion and bending. There are always 4 stresses per Gauss point, expressed in the local frame.


The first direction of the local frame (u) is along the element, from node 1 to node 2. The second (v) is in the plane defined by u and the local vector V, on the same side as V. The third one (w) is deduced from the others.


Here, due to beam assumptions, the bending stresses are expressed in the frames (u, v) and (u, w):

     sig(1) : traction (u)          sig(3) : bending (u,v)
     sig(2) : torsion  (u)          sig(4) : bending (u,w)

Important:


In order to determine the local state of the beam, only the moments and the deformation have a sense! It is therefore mandatory to estimate the moments starting from the stresses, by the following relation:

M = σ 
I
h
 

The value of σ is read on the listing, I and h are specified in the input data set (see Chapter C1). The deformations are read directly from the listing.


For an elastic calculation ONLY, it is then possible to compute the stresses in any point of the cross-section.


COQ3 and COQ4


These elements work in membrane and bending. There are always 6 stress components per Gauss point, expressed in a local frame.


For the triangular elements COQ3, the first direction of the local frame (u) is along the first side of the element, from node 1 to node 2. The second (v) lies on the element plane, such that node 3 is on the positive side.


Because of shell hypotheses, the stresses are expressed in the (u, v) frame.


The quadrangular elements COQ4 are composed by 4 triangles:

1-2-3 3-4-1 1-2-4 3-4-2


Each of these triangles has a local reference frame as defined above. If the quadrangle is a parallelogram, the 4 local frames are identical.


The 4 Gauss points of element COQ4 are at the centers of the triangles mentioned above. If the element has an irregular shape, the stresses at the various Gauss points will not be directly comparable.

     sig(1) : membrane (u)          sig(4) : bending (u)
     sig(2) : membrane (v)          sig(5) : bending (v)
     sig(3) : membrane (uv)         sig(6) : bending (uv)

Continuuum elements


The stresses are expressed in the global frame (x, y, z).

                    ( SIG(1)  SIG(4)  SIG(6) )
                    (                        )
           (sig) =  ( SIG(4)  SIG(2)  SIG(5) )
                    (                        )
                    ( SIG(6)  SIG(5)  SIG(3) )

11.3.1  TOTAL DEFORMATIONS


The tensor of total deformations is the dual of the stress tensor. Its structure is therefore the same as that of the stresses (see the previous Section).

11.4  MATERIAL PARAMETERS ("ECROU")

G.35


All internal variables pertaining to the different materials are stored in the ECR table. Initially reserved only for the hardening parameters, this table has been considerably enlarged, as more complex materials have been implemented in EUROPLEXUS.


Only the simplest materials use just the first hardening quantities. For the others, the meaning of the ECR components are described within each material law description (see page C.100 and following ones).

    ECR     |      shells       | continua (solids) | continua (fluids)
    --------+-------------------+-------------------+------------------
    ECR(1)  |   V.M. membrane   |      Pressure     |      Pressure
    ECR(2)  | V.M. memb. + bend.|      Von Mises    |      Density
    ECR(3)  |   plast. deform.  |   plast. deform.  |         -

Remarks:


The equivalent plastic deformation (ECR(3)) is only printed for elasto-plastic calculations.


The Von Mises criterion for the shells is expressed as:

        sig(*) = SQRT( sig(m)*sig(m) + (alpha**2)*sig(f)*sig(f))


with sig(m) and sig(f) Von Mises stresses in membrane and bending and alpha = 2/3 by default.


The Von Mises criterion for the beams is expresses as:

        sig(*) = SQRT( ap * press*press + am * sig(1)*sig(1) +
                       at * sig(2)*sig(2) +
                       af * (sig(3)*sig(3) + sig(4)*sig(4)) )


The sig(i) are defined above, and press is the internal pressure, if the beam is a pipe. The coefficients ap (pressure), am (membrane), at (torsion) and af (bending) are computed by EUROPLEXUS according to the type of beam, of the existence or not of a curvature, etc.

11.5  TIME CHOICE (PROCEDURE /CTIME/) FOR THE PRINTOUTS

G.40


Object:


The /CTIME/ procedure, described in the introduction (see page INT.57) is used to specify when printouts should take place during a computation.


Comments:


If nothing is specified, the printouts are performed for all time steps.


If the keyword "NUPA" is used, do not forget to dimension adequately by means of the word "MNTI" as described on page A.100.


If the keyword "TIME" is used, do not forget to dimension adequately by means of the word "MTTI" as described on page A.100.


Be aware that printout times specified via "TFRE" or "TIME" are rounded to the closest time unit, that can be chosen via the "OPTI TION" directive.


Warning:


Be careful in the choice of your printouts if you do not want to produce unnecessarily large listings. In general, it is advisable to use graphics post-processing in order to analyse the results, instead of reading values on a listing.


It is useful to know that the output file of the results ( "FICH" "ALICE" ), enables to print selected results on a listing after completion of a calculation. Therefore it is advisable to print only the bare minimum, although it will be necessary to read the results file again, in order to output interesting things after a calculation has been completed.

11.6  NODES OR ELEMENTS TO BE PRINTED

G.50


Object:


The user can choose the nodes and/or elements where he wants to print the results.


Syntax:

    $["NOPOINT"  ;  "POINT"  /LECTURE/  ]$
    $["NOELEM"   ;  "ELEM"   /LECTURE/  ]$


"NOPOINT"

No point is printed.
"POINT"

Selection of the points which have to be printed.
"NOELEM"

No element is printed.
"ELEMENT"

Selection of the elements which have to be printed.
/LECTURE/

List of the points or elements for which the results are printed.

Comments:


The two options "POINT" and "NOPOINT" are mutually exclusive, and the same is true for the two options "ELEMENT" and "NOELEM".


If none of the two options is specified, the results are printed for all nodes and for all elements.

11.7  RESULT FILES

G.70 - Feb 13


Object:

This directive is aimed at creating files for the post-processing of the computation results or a saving file to restart the calculation. The following file types are available:

     -  SAUVER file             (saving file for successive restart)
     -  ALICE file              (postprocessor: EUROPLEXUS)
     -  ALIT (ALICE TEMP) file  (postprocessor: EUROPLEXUS)
     -  PVTK file               (postprocessor: PARAVIEW VTK format)
     -  TABL file               (a simple formatted table)
     -  POCH file               (for Pochhammer-Chree post-treatment by EPX)
     -  MAPB file               (for storing a blast wave to a later mapping)
     -  MED file                (compatible with many softwares)

The following file types are available but not developed further:

     -  SPTAB file              (postpr.: SUPERTAB (old I-DEAS interface))
     -  TPLOT file              (postprocessor: TPLOT)
     -  XPLOT file              (postprocessor: TPLOT)
     -  K2000 file              (postprocessor: CAST3M)
     -  AVS file                (postprocessor: AVS and old ParaView)
     -  PLOT-MTV file           (postprocessor: PLOT-MTV)
     -  UNIV file               (postprocessor: I-DEAS)


The SAUVER file is used to restart the calculation. It is described in detail on GBG_0110.


CAST3M is the product of CEA (see http://www-cast3m.cea.fr), SUPERTAB is a commercial software by SDRC, TPLOT is a software by JRC, AVS is a commercial product by Advanced Visual Systems, PLOT-MTV is a public utility (2D plotting only), I-DEAS is a commercial software by SDRC. The MED format is a format co-developed by the CEA and EDF which is compatible with many softwares. PARAVIEW is an open-source multi-platform application designed to visualize data sets of size varying from small to very large (see http://www.paraview.org).


Note that, besides the I-DEAS interface (UNIV keyword) described hereafter, another version is available, that had been independently developed by the CESI (formerly ENEL) group, and which is described on GBG_0072.


Syntax:

< FICHIER    |[ "SAUV" <ndsauv> <"PROT" 'maclef'> <"LAST"> </CTIME/> ;

                "ALICE" <"FORMAT"> <"SPLIT"> <ndgrap>   /CTIME/ ;

                "ALIT"   <"FORMAT">          <ndalic>    /CTIME/  ...
                                    ... < "POINT" /LECTURE/ > ...
                                    ... < "ELEM"  /LECTURE/ >     ;

                "PVTK"  < $["FORM" ; "FOLD"]$ > <ndpara> /CTIME/
                      <"PINB"> <"MPI"> <"FLSW">
                      <"GROU" |[ "AUTO" ;  nobj*("OBJE" <'groupname'>
                               $[ "GAUS" ngaus ; "GAUZ" ngauz ]$ /LECT/) ]| >
                      <"VARI"  <"DEPL"> <"VITE"> <"ACCE"> <"FEXT">
                               <"FINT"> <"FLIA"> <"MCXX"> <"SIGN">
                               <"ECRN"> <"RISK"> <"FAIL"> <"VCVI">
                               <"CONT"> <"EPST"> <"ECRO"> <"XLVL">
                               <"DTST"> <"EPAI"> <"PCLD">
                      <"SHEL" vx vy vz /LECTURE/ >  ;

                "TABL" <ndtabl> /CTIME/
                    "VARI" nv * (
                    |[ "COOR" "COMP" ic "NOEU" /LECT/              ;
                       "DEPL" "COMP" ic "NOEU" /LECT/              ;
                       "VITE" "COMP" ic "NOEU" /LECT/              ;
                       "ACCE" "COMP" ic "NOEU" /LECT/              ;
                       "FINT" "COMP" ic "NOEU" /LECT/              ;
                       "FEXT" "COMP" ic "NOEU" /LECT/              ;
                       "CONT" "COMP" ic "GAUS" gp "ELEM" /LECT/    ;
                       "ECRO" "COMP" ic "GAUS" gp "ELEM" /LECT/    ;
                       "EPST" "COMP" ic "GAUS" gp "ELEM" /LECT/    ;
                       "FONC" ifon                                 ]| ) ;


                "POCH"  <"FORMAT"> <"SPLIT">  <ndpoch>    /CTIME/  ...
                             ... "NLIN" nl * ( /LECT/ )   ...
                             ... "VARI" $[ "DEPL" ;"VITE" ; "ACCE" ]$ ;

                "MAPB" | "MSPA" ; "MTIM" | "DIPR" dipr "PCHE" pche /CTIME/

                "SPTAB" <ndspta>   /CTIME/ ;

                "TPLOT" <"FORMAT"> <ndtplo>   /CTIME/               ...
                                    ... "DESC" 'dddddd'       ...
                                    ... < "POINT" /LECTURE/ > ...
                                    ... < "ELEM"  /LECTURE/ >     ;

                "XPLOT" <"FORMAT">   <ndxplo>  /CTIME/        ...
                                    ... "DESC" 'dddddd'       ...
                                    ... < "POINT" /LECTURE/ >     ;

                "K2000" < $[ "FORM" ; "XDR" ;  "BINA" ]$ >  <"SPLIT"> ...
                                    ... <ndcast>   /CTIME/    ...
                                    ... < "POINT" /LECTURE/ > ...
                                    ... < "ELEM"  /LECTURE/ > ...
                            ... <"SHEL" vx vy vz /LECTURE/ >
                            <"CHAMELEM">
                     <"VARI" < "DEPL">  <"VITE"> <"FEXT"> <"ACCE"> <"MCXX">
                                <"SIGN">  <"ECRN">
                                <"CONT">  <"EPST">  <"ECRO">
                                <"ECRC" /LECT/> >    ;
                "AVS" "FORMAT" <"PRVW">  <ndavs>    /CTIME/
                     <"VARI" <"DEPL">  <"VITE">  <"FEXT">  <"ACCE">  <"MCXX">
                                <"CONT">  <"EPST">  <"ECRO">  <"XLVL">
                                <"ECRC"> >           ;

                "PMTV" "FORMAT"   <npmtv>  /CTIME/
                     <"VARI" < "DEPL"> <"VITE">  <"SIGN"> <"ECRN"> >   ;

                "UNIV" <FORMAT>  $["CURR" ; "OBSO"]$ <nuniv>
                                                          /CTIME/ ;

                "MED"         /CTIME/
                              < "POINT" /LECTURE/ >
                              < "ELEM"  /LECTURE/ > ;
                 ]| >


FORMAT

If this keyword is present, the file will be formatted, otherwise it will be unformatted ("BINA") (but only where both possibilities exist).
XDR

Only for K2000 file if this keyword is present, the K2000 file will be independent of hardware and operating systems. This is the default option for K2000 file.
ALICE

A file of results is written in the standard ALICE format. This file can be read again by the EUROPLEXUS or ALICE programs.
SPLI

Split the ALICE or K2000 (formatted file only) or Pochhammer-Chree results into several files, one for each time instant, instead of producing just a single, big file. Useful e.g. to produce animations of results, which require typically many tens or even a few hundred time instants and to overcome the file size limitations that hold under some operating systems (e.g., under 32 bit MS-Windows maximum file size is 2 GB).
ALIT

A file of results is written in the ALICE format as a function of time. This file will only contain the results at the nodal points and elements defined with the keywords POIN and ELEM. This file can be read again by the EUROPLEXUS or ALICE programs.
SPTAB

An output results file in the SUPERTAB universal file format is produced (old I-DEAS version).
TPLOT

A file of results is written in the standard TPLOT format. This file can be further processed by the TPLOT program.
XPLOT

A file of results is written in the XPLOT format. This file can be further processed by the TPLOT program.
K2000

A file of results is written in the CAST3M format. The default mode of K2000 output is XDR. It can be read by CAST3M by using the keyword RESTITUER. The file format is the standard format of a CAST3M file obtained with the SAUVER directive. It is mandatory in this case to indicate the list of the nodes for which the results have to be stored (possibly TOUS). The directive CHAMELEM is optional. The values defined on the elements (stresses, hardening quantities, strains) are only stored if this keyword is specified. Note that these element values are averaged on the element GPs (or on the GPs of a specific fibre of the element: see K2FB option) and are affected either to the nodes or to the barycentre of the element (see K2CH option).
CHAM

This keyword introduces the the definition of “chamelems” in the K2000 results file. If it is omitted, the latter will only contain the selected “champoints”, defined on the nodes chosen by directive POIN above.
VARI

Alternatively to CHAM, one can use the directive VARI which allows finer-grain control over the quantities effectively stored. Each nodal quantity (DEPL, VITE, FEXT, ACCE, MCXX in case of multicomponent gases, SIGN + ECRN in case of spectral elements, VCVI in case of finite volumes) and each element quantity (CONT, ECRO, EPST) may be specified separately. Furthermore, one may specify exactly which components of the ECR vector are to be stored, via the ECRC /LECT/ directive. This mechanism allows to greatly reduce the size of output files in large complex 3D calculations.
DEPL

Nodal displacements.
VITE

Nodal velocities.
FEXT

Nodal external forces (including reactions).
FINT

Nodal internal forces.
ACCE

Nodal accelerations.
MCXX

Nodal variables for multicomponent fluids (pressure, density, temperature, sound speed and component mass fractions).
SIGN

Nodal stress components (only for spectral elements).
ECRN

Nodal hardening variables (only for spectral elements).
VCVI

Velocity in the centre of finite volumes (CEA formulation, only available for PVTK).
FLSW

Face or volume blocked by FLSW (only available for PVTK).
RISK

Risk limit for eardrum failure and death. In addition, the maximum pressure and the total impulse are written to the result file. The risk types can also be split by using the SPLI command when the risk is defined (see A.30). (only available for PVTK).
FAIL

Failure level. Not active debris get a failure level of -1.0. (only available for PVTK).
XLVL

Level set of XFEM (only available for PVTK).
FLIA

Nodal forces due to liaisons (links) (only available for PVTK).
DTST

Stable time step (only available for PVTK).
EPAI

Thickness (and other COMP parameters) (only available for PVTK).
PCLD

Outputs related to point cloud adaptivity: point could index, distance to point could, adaptivity level (only available for PVTK).
SHEL

Option which enables to print in the K2000 output file or PVTK output file the stress (CONT) and strain (EPST) of shells according to specific axes rather than local axes (default). vx vy vz are the coordinates of the vector which is projected onto the shells read in /LECTURE/ in order to define the first direction of the posttreatment axes. The third posttreatment direction is identical with the third one in local axes. This definition of the posttreatment axes is made in the initial configuration and is not updated ; that means this option is only relevant for small strains. This command may be repeated as many times as needed. This option is available only for DST3, DKT3, T3GS and Q4GS shells.
AVS

A set of result files (see note below) are written in the AVS format. For the moment, only a formatted output is available for AVS, so the FORM option is actually mandatory in this case.
PRVW

The AVS files are modified to be imported into PARAVIEW software (see note below). This is only compatible with older versions of ParaView (less than 2.9 or so). For newer versions, use the PVTK type of output, which produces files in the VTK format.
UNIV

A results file in “universal” (I-DEAS) format is to be written. This file may be of two types: “current” or “obsolete”. By default it is of “current” type.
CURR

The universal results file will be of type “current”. This is the default.
OBSO

The universal results file will be of type “obsolete”.
PVTK

A set of result files (see note below) are written in the PARAVIEW format (.pvd and .vtu files). This is the VTK format, compatible with the newer versions of ParaView. By default, use is made of the library LIB_VTK_IO, written by Stefano Zaghi (see http://stefano.zaghi.googlepages.com/lib_vtk_io), which allows to produce either ASCII or binary output formats. However, if the (obsolete) keyword FOLD is specified in place of FORM, then formatted output is produced without making use of the LIB_VTK_IO library (note that in this case only ASCII format, not binary format, is possible).
PINB

The geometry of the pinballs are written in a separate vtu-file.
MPI

MPI calculations only. One set of vtu-files is written for each subdomain, to avoid centralizing data from all subdomains on one thread before writing.
GROU

Groups can be defined automatically (using keyword AUTO) or manually by entering nobj objects defined with the OBJE keyword (which must be repeated exactly nobj times). A name can be optionally given to each manually defined group. Automatic groups were generated for each material definition and for each element class (not element type). Each separate group is written as output files (see comments below for syntax). For manually defined groups, the number of the Gauss point ngaus or the number of the layer ngauz, which is used for output, can be defined for each group with GAUS or GAUZ respectively. The logic of the VTK format is not the same as the one of CAST3M and EUROPLEXUS. If an element is contained in several groups, the element will be written to the output files several times. This element is also repeated in the output of ParaView. If present, only the elements (and nodes) defined by the GROU keyword are written to the output.
MSPA

Introduces the writing of a blast field into a map file for one specific time step over a certain geometry.
MTIM

Introduces the writing of a blast field into a map file for one specific distance over the given time.
DIPR

For MSPA: Distance in which the pressure is checked and the output is written when the pressure reaches a certain value.
For MTIM: distance where the pressure history is saved.
PCHE

Pressure value which is used for the check to write the map file. For the MTIM option this is the start point of the output. The CTIME parameter should be set small in order to check the limits often.
ndgrap

Number of the logical unit of the ALICE file or file name in quotes. If omitted, the program chooses a file name by default (see page A.27). The default extension is .ALI. For the special case of split ALICE files, see comments below.
ndalic

Number of the logical unit of the ALICE TEMPS file or file name in quotes. If omitted, the program chooses a file name by default (see page A.27). The default extension is .ALT.
ndspta

Number of the logical unit of the SPTAB file or file name in quotes. If omitted, the program chooses a file name by default (see page A.27). The default extension is .SPT.
ndtplo

Number of the logical unit of the TPLOT file or file name in quotes. If omitted, the program chooses a file name by default (see page A.27). The default extension is .TPL.
ndxplo

Number of the logical unit of the XPLOT file or file name in quotes. If omitted, the program chooses a file name by default (see page A.27). The default extension is .XPL.
ndcast

Number of the logical unit of the CAST3M file or file name in quotes. If omitted, the program chooses a file name by default (see page A.27). The default extension is .K20. For the special case of split CAST3M files, see comments below.
ndavs

Number of the logical unit of the AVS file(s) or file name in quotes. If omitted, the program chooses a (base) file name by default (see page A.27). The default extension is .AVS. Split files are generated for this type of output. See comments below.
ndpara

Number of the logical unit of the PARAVIEW file(s) or file name in quotes. If omitted, the program chooses a (base) file name by default (see page A.27). The default extension is .pvd. This file contains links to files with the data (vtu-format, extension .vtu). See comments below.
npmtv

Number of the logical unit of the PLOT-MTV file or file name in quotes. If omitted, the program chooses a (base) file name by default (see page A.27). Split files are generated for this type of output. The default extension is .MTV. See comments below.
nuniv

Number of the logical unit of the universal file or file name in quotes. If omitted, the program chooses a file name by default (see page A.27). The default extension is .UNV.
ndtabl

Number of the logical unit of the table file or file name in quotes. If omitted, the program chooses a file name by default (see page A.27). The default extension is .TAB.
/CTIM/

This procedure is described in the introduction (page INT.57). If the keywords NUPA or TIME are used, do not forget to dimension adequately by means of keywords MNTI, MTTI (see also page A.100).
DESC ’dddddd’

Six-character descriptor to identify the run for the TPLOT (or XPLOT) data-base. Note that this item is in text format, therefore it must be enclosed in quotes. When loading data on the TPLOT database, a prefix PL is automatically placed in front of this descriptor. Thus, the full descriptor on the database will be PLdddddd. For XPLOT, the prefix is XL, so the full descriptor will be XLdddddd.
POIN /LECTURE/

List of nodes for which the results have to be stored for successive treatment by TPLOT or XPLOT.
ELEM /LECTURE/

List of elements for which the results have to be stored for successive treatment by TPLOT.
MED

A file of results is written in the MED format. This file will only contain the results based on the nodes and the elements selected with the keywords POIN and ELEM. For the selected nodes, nodal displacements, nodal velocities, nodal accelerations, nodal external forces (including reactions), nodal internal forces are stored. Only elements with one integration point and the POUT elements are treated. For these elements, stresses and strains fields are stored. Do not forget to create the MED file before with the keyword MEDE (see page A.30).
TABL

A file of results is written in a simple text file in tabular form. This type of output is meant to monitor just a few variables, say a nodal displacement and an element stress component, but with great precision. Results are always written formatted, and with full double precision (16 significant digits). The table contains one line per storage station (typically, each time step). The first two columns of the table always contain the current time step (npas) ad the current time (t). The following columns contain the chosen variables. Obviously, no more than just a few variables can be specified, in practice, else the length of the table line would become excessive. The keyword VARI introduces the chosen variables. Their number is given by nv and thereafter exactly nv variable specifications must be given, chosen among the following possibilities: COOR for nodal coordinates, DEPL for nodal displacements, VITE for nodal velocities, ACCE for nodal accelerations, FINT for nodal internal forces, FEXT for nodal external forces, CONT for elemental stresses, ECRO for elemental hardening quantities, EPST for elemental total strains, FONC for the value of a specified function. The keyword COMP introduces the component, GAUS the Gauss point, NOEU the node and ELEM the element. Note that the /LECT/ directives must specify one single node or element. The value ifon after FONC specifies the function identifier (see the FONCTION directive).
ndpoch

Number of the logical unit of the Pochhammer-Chree file(s) or file name in quotes. If omitted, the program chooses a (base) file name by default (see page A.27). The default extension is .poc.
NLIN

Introduces the number of “lines” along which the results will be sampled for the successive Pochhammer-Chree post-treatment. Each line is formed by an ordered sequence of nodes and is defined by the following /LECT/.

Comments:


The keyword FICHIER is not compulsory. If it is used, the last step is systematically saved.


Do not forget to define the logical unit(s) of the file(s), on the control cards. As an alternative, EUROPLEXUS accepts the name of the file enclosed in quotes.


If one does not pay attention, result files may become very bulky, because the total number of computed time steps is often very large. It is then advisable to estimate the total number of steps from the stability step computed by the program, and then choose a reasonable number of storages on the ALICE file. It is also possible to obtain a smaller results file by using the ALICE TEMPS (ALIT) directive: in this case only the variables relative to the nodes and elements given in directives POIN and ELEM will be stored.


It is rare that one needs more than a dozen of time stations to plot the deformed shapes of the mesh — in this case the ALICE directive will be used. It is also infrequent that one needs more than a few hundred points to plot curves as a function of time — it is suggested to use the directive ALIT which allows to obtain a file reduced to just the selected points. Therefore it is possible to specify a much larger number of saving stations on an ALIT file than on an ALIC one.


For ALICE, the SPLI option allows to split the results into many small files, one for each stored time instant, rather than producing just one big file. This option is useful for very large computations and/or for producing animations, which typically require many saved instants. In this case, ndgrap is just the base name of the output files. The single file names are automatically given progressive numbers (_0001, _0002, etc.) appended to the name, which identify the storage index. A file with suffix _0000 is also produced, which contains the initial mesh topology.


In order to post-treat these split results with EUROPLEXUS, proceed exactly as if the results would be in a single file, but remember to specify the SPLIT keyword in the RESU ALIC directive, see page ED.20.


XPLOT storage is intended to perform pseudo-1D visualization of data in a 2D or 3D run. A curvilinear abscissa is built up passing through the nodes defined in POIN /LECT/. Then, nodal and element quantities are stored as a function of this abscissa. By using the TPLOT program, the relevant quantities can then be plotted along the curvilinear abscissa (either initial or current). Note that nodal quantities (displacements, velocities, etc.) are stored without modification at the specified nodes. Element quantities, however, (such as stresses and hardening parameters), that are usually defined only at points internal to the elements, are first extrapolated to the nodes, then stored. Currently, the extrapolation consists of simply: 1/ averaging each quantity over each element (by using the values at the different Gauss points), 2/ averaging all neighbour element contributions to obtain nodal values. Neighbour elements to a node are those elements that contain that node.


Note also that, in the extrapolation process, only certain types of elements are considered. For example, shell or beam elements are rejected, because the mean value of the stress components on all the Gauss points is likely to be meaningless for such elements. Only the following element types are considered: TRIA( 2), CAR1( 8), CAR4( 9), CUBE(11), CUB6(13), PR6 (20), TETR(21), PRIS(27), FLU1(52), FLU3(53), FL23(64), FL24(65), FL34(66), FL35(67), FL36(68), FL38(69), Q41 (71), Q42 (72), Q41N(73), Q42N(74).


In order to read with CAST3M a file written by EUROPLEXUS, use the following CAST3M commands:


1/ Formatted file:

    OPTI REST FORM 'file';
    REST FORM;
    . . . (post-treatment commands)


2/ Unformatted file:

    OPTI REST BINA 'file';
    REST BINA;
    . . . (post-treatment commands)


3/ XDR file:

    OPTI REST 'file';
    REST ;
    . . . (post-treatment commands)


For K2000, note that two syntaxes are possible. With the ‘old’ syntax (the keyword VARI does not appear), all nodal quantities are always stored. Furthermore, all element quantities are stored if CHAM appears. The components of the ECR table which are stored depends in this case from the material: they are the same components of ECR that are printed on the listing.


With the new syntax (the keyword VARI appears) only the specified nodal quantities, element quantities and ECR table components are actually stored.


Note that, strictly speaking, it is only possible to produce an output file for K2000 when the input mesh has also been produced (and read into EUROPLEXUS) in this format. However, if this is not the case but you still desire to postprocess your EUROPLEXUS calculation with K2000, consider transforming your mesh in K2000 by the option K2MS (see Section H, output options). Beware, however, that this may require some manual intervention and in any case the obtained mesh will be less flexible to use than a “real” K2000 mesh.


In the case of standard AVS storage, a set of files is written, one for each stored variable. The files basename is given by ndavs. If ndavs as given by the user contains the extension .avs or .AVS, this extension is removed by the program. An extension of the form .VARI.N.inp is then automatically provided by EUROPLEXUS. Here VARI is the variable type (DEPL, VITE , ...) and N an integer counter which is automatically incremented by 1 at each successive storage in time.


Recall that AVS storage can also be requested interactively, i.e. during an interactive execution of EUROPLEXUS (See Group A, Interactive (Foreground) Execution).


In the case of AVS storage modified for usage with PARAVIEW, elements are split into groups with same element topology and same material law. One file is stored for each group of elements at each successive storage in time. This file contains geometry and both nodal fields and elemental fields required by the user. It is named from the name given by ndavs, with its extension removed. An extension of the form _N1_N2.inp is is then added to the name. N1 is the number of the element group and N2 is an integer counter as for standard AVS files. If ndavs is not defined, the base of the EUROPLEXUS input file name is used to build AVS-PARAVIEW file names.


If a directory name is provided for AVS-PARAVIEW files with the OPNF directive, files are written in this directory, excepted if ndavs represents a name with full path. In this latter case, the above given directory is ignored.


The AVS-PARAVIEW format is only readable with older versions of PARAVIEW (less than 2.9). For newer versions of PARAVIEW, the PARAVIEW output (see PVTK) with a .pvd and .vtu files is recommended.


Automatic group definition for PARAVIEW output (with keyword GROU AUTO) consists in the same splitting of elements as described above for the AVS-PARAVIEW output.


The PLOT-MTV output is only available in 2D and for spectral elements. the program will only include spectral elements and nodes in these files. A separate file with the extension .mtv is produced for each nodal quantity and at each selected storage time.


The SIGN keyword produces storage of 4 nodal stress (6 in 3D) components (SGXX, SGYY, SGZZ, SGXY, SGYZ, SGZX). The ECRN keyword produces storage of 2 nodal hardening quantities: the hydrostatic stress (HYDR) and the Von Mises stress (VMIS).


When using SPTAB output format, a file named sptab.param must exist in the current directory, containing the following key-words useful to declare the variables to print out: DISP, VELO, ACCE, INTF, EXTF, MCVAR, MCVEL, MCMFR, FLVAR, SCUB8, ECOQI.


For CAST3M , the SPLI option allows to split the results into many small files, one for each stored time instant, rather than producing just one big file. In this case, the chosen output type MUST be formatted (FORM). This option is useful for very large computations and/or for producing animations, which typically require many saved instants. In this case, ndcast is just the base name of the output files. The single file names are automatically given progressive numbers (_0001, _0002, etc.) appended to the name, which identify the storage index. A file with suffix _0000 is also produced, which contains the initial mesh topology.


In order to post-treat one of these split results with CAST3M, proceed as follows: choose the instant to be treated, say number 3 i.e. the third storage performed; then, produce a file by concatenating the ‘zero’ file (_0000) and the file for the chosen instant; finally, read and post-process the resulting file with CAST3M. In this example:

     cat mytest_0000.k20 mytest_0003.k20 >out.k20

     K2000

     opti rest form 'out.k20'; rest form; ...

Warning :


Be careful: output files may become very large, because the total number of the time steps computed is often large. Therefore it is better to estimate that number from the stability step computed by the program. Then, the user can choose a reasonable number of writings on the output files.


The user seldom needs more than a dozen storage stations (‘cases’) to draw deformed structures and no more than fifty points to draw time functions.

11.8  POST-PROCESSING BY I-DEAS MASTER SERIES

G.72


Object:


This is aimed at creating files for the post-processing of computation results by I-DEAS master series.


This model is part of the models developed by the CESI team (formerly at ENEL, Milano) in collaboration with JRC.


I-DEAS is a commercial software by SDRC.


Syntax:

    <  "FICHIER" <FORMAT> "IDEA" ndidea   /CTIME/
                                    ... < "POINT" /LECTURE/ > ...
                                    ... < "ELEM"  /LECTURE/ > ...
                 < "VARI" < "DEPL" "VITE" "FEXT" "ACCE" "MCXX" >
                          < "CONT" "MESH" "MCVA" "MCVE" "MCMF" >
                          < "FLVA" "ECOQ" >             >         >


"FORMAT"

If present, the file is formatted, otherwise it is unformatted.
"IDEA"

An output results file in the I-DEAS universal file format is produced (new version).
ndidea

File name in quotes of the universal output file for I-DEAS.
"POIN" /LECT/

Same meaning as for the other result files, see page G.70.
"ELEM" /LECT/

Same meaning as for the other result files, see page G.70.
"CTIM" .. "CONT"

Same meaning as for the other result files, see page G.70.
"VARI"

Introduces the list of variables to be stored.
"DEPL"

The I-DEAS universal file in output will contain the displacements.
"VITE"

The I-DEAS universal file in output will contain the velocities.
"FEXT"

The I-DEAS universal file in output will contain the external forces.
"ACCE"

The I-DEAS universal file in output will contain the accelerations.
"MCXX"

The I-DEAS universal file in output will contain the MC variables.
"CONT"

The I-DEAS universal file in output will contain the stresses.
"MESH"

The I-DEAS universal file in output will contain the mesh data (only node and element datasets).
"MCVA"

The I-DEAS universal file in output will contain the MC conserved variables: pressure, density, internal energy, maximum pressure, minimum pressure, temperature.
"MCVE"

The I-DEAS universal file in output will contain the MC velocities: x, y, z velocity components, velocity modulus, sound speed and Mach number.
"MCMF"

The I-DEAS universal file in output will contain the MC mass fractions.
"FLVA"

The I-DEAS universal file in output will contain the fluid finite elements variables (FLxx family with FLUT material): pressure, density, internal energy, max pressure, min pressure, sound speed.
"ECOQ"

The I-DEAS universal file in output will contain the COQI element ECR variables: hydrostatic pressure, Von Mises, plasticity flag, current yield stress.

Comments:


The general comments of page G.70 apply to the I-DEAS results file as well.


When using "IDEA" output format, the default options for the selection of the results are: whole geometry (i.e. all nodes/elements are treated if "POIN", "ELEM" are omitted), no variable (i.e. only the variables specified in the "VARI" option are stored).


Element output in I-deas universal file format is only available for FLxx, MCxx, CUB8, COQI, CQD3, CQD4 elements at the moment.

11.9  OUTPUT REGIONS

G.100


Object:


This directive enables the printing of physical values within a given region.


A region is defined by the list of the elements which compose it. The region could correspond to a GIBI object.


Syntax:

       "REGION"  ( 'nom region'
            $[ "RMAS" ; "VOLU" ; "BARY" ; "DIMX" ; "DIMN" ;
               "DMOY" ; "VEMX" ; "VEMN" ; "VMOY" ; "ACMX" ;
               "ACMN" ; "AMOY" ; "IMPU" ; "ECIN" ; "WINT" ;
               "WEXT" ; "PDV"  ; "WINJ" ; "RESU" ; "IRES" ;
               "ECRG" ; "ECRM" ; "EMAS" ; "FLIR" ; "RISK" ;
               "EROD" ; "ENDO" ; "CLAS' ; "EPSM" ; "TOUT" ]$
             < "DIRX" rx "DIRY" ry "DIRZ" rz >
            |[     /LECTURE/     ;
               "POIN" /LECTURE/  ]| )


nom region

Name of the region given by the user (in apostrophes).
RMAS

Mass (components, computed via XMEL).
VOLU

Volume.
BARY

Center of gravity (barycentre) of the region.
DIMX

Maximum displacement (absolute) of the region (vector), only components 1 to 3.
DIMN

Minimum displacement (absolute) of the region (vector), only components 1 to 3.
DMOY

Average displacements (components).
VEMX

Maximum velocity (absolute) of the region (vector), only components 1 to 3.
VEMN

Minimum velocity (absolute) of the region (vector), only components 1 to 3.
VMOY

Average velocity (components).
ACMX

Maximum acceleration (absolute) of the region (vector), only components 1 to 3.
ACMN

Minimum acceleration (absolute) of the region (vector), only components 1 to 3.
AMOY

Average acceleration (components).
IMPU

Impulse (components).
ECIN

Kinetic energy (norm and components).
WINT

Internal energy.
WEXT

Work of external forces applied to the nodes of the region.
PDV

Work of pressure forces in ALE for a stand-alone domain.
WINJ

Injected energy (only for material EAU).
RESU

Resultant of the external forces applied at the nodes.
IRES

Impulse corresponding to the above resultant.
ECRG

For each component of ECR (in fact, for the first 10 components), sum of the values on the Gauss points of the region.
ECRM

Average of the ECR over the region.
EMAS

Mass (scalar, computed via the element’s mass XM0).
FLIR

Resultant of the force due to LINK/LIAI applied at the nodes.
RISK

Global risk (average).
EROD

Number of eroded elements.
ENDO

Number of damaged elements (A damaged element contains a least a Gauss point which is not broken.) - (See A.30 : EROS ldam)
CLAS

Number of eroded classes and number of damaged classes - A class is eroded as soon as an element of this class is eroded - A class is damaged if the class is not eroded and if the class contains at least a damaged element.
EPSM

Average of the EPST (strain variables) over the region.
TOUT

All possible physical values are required.
DIRX, DIRY, DIRZ

Components of the direction vector specifying the user-defined frame. Definition of the local frame (x,y,z) with respect to the global frame (X,Y,Z):

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

Only the following quantities can be written in this frame: MASS, ECIN, AMOY, ACMX, ACMN, VMOY, VEMX, VEMN, DMOY, DIMX, DIMN, BARY, IMPU, QMVT, RESU, ECRG, FLIR

LECTURE

List of the elements composing the region.
POIN /LECTURE/

List of the nodes composing the region.

Comments:


The computation takes place within the elements.


It is possible to have elements which belong to several regions.


If the region is only known by its nodes (it has not been defined in the directive "GEOM"), the only possible balances are WEXT, RESU and IRES. In this case, it is mandatory to use the keyword "POIN" before the /LECTURE/ procedure, to avoid confusion between nodes and elements.


If the region is nothing else but the whole structure, the values of WINT and ECIN are the same as those printed in the energy balance.


The physical values of the regions are computed during the printing.


Important: restart calculation (see page ED.10)


There is no problem if the computed quantity does not depend on masses (WINT). If the physical values are dependant on the masses (ECIN BARY VMOY IMPU RMAS VOL PDV), the computation will be correct only if the masses are constant during the EUROPLEXUS computation. In fact, in order to lighten the file of the results (FICHIER ALICE), only the initial masses are copied out. There is no problem concerning a Langrangian computation. For an Eulerian or A.L.E computation, the masses change. Therefore, the physical values will not be correct.


All this happens during a restart; if the physical values are computed during a normal (non restart) EUROPLEXUS run, all the results are correct.

11.10  MEASUREMENTS AND MESH QUALITY

G.105


Object:


This directive enables: 1) the printout of various types of simple measurements taken on the current geometrical mesh; 2) the verification of mesh quality (MQUA) on the initial configuration as well as at chosen later times during the simulation by choosing appropriate criteria; 3) the use of such mesh quality criteria to get rid of heavily distorted elements via the element erosion mechanism.


Normally, it is called from the input file and the requested measurements are then printed on the listing. However, the same directive (same syntax) is available also from the command line during an interactive execution (see pages A.25 and O.10). For this reason, the present directive must be terminated by the keyword TERM, as shown below in the syntax. In case of interactive use, the requested measurements are printed on the console window, not on the listing.


Syntax:

        MEASURE   $[ ELEM e ;
                     NODE n ;
                     OBJE /LECT/ ;
                     EMIN /LECT/ ;
                     EMAX /LECT/ ;
                     DIST <POIN> /LEC1/ <POIN> /LEC2/ ;
                     MQUA nmq <mesh quality assessment commands> ]$
                  TERM


ELEM e

Returns information about the chosen element e: its type, the associated nodes (with their coordinates), its size, its mass and the list of objects or groups to which it belongs.
NODE n

Returns information about the chosen node n: its coordinates, its mass, the list of elements to which it belongs and the list of objects or groups to which it belongs.
OBJE /LECT/

Returns information about the chosen object /LECT/: the associated elements, the associated nodes, its size and its mass.
EMIN /LECT/

Returns information (see ELEM above) about the “smallest” element among those belonging to the object specified in the following /LECT/. Use LECT tous TERM to get the smallest element in the whole mesh. As smallest element, we consider the one having the shortest (non-zero) intra-nodal distance among its nodes (and thus most likely the shortest element characteristic length as far as stability is concerned).
EMAX /LECT/

Returns information (see ELEM above) about the “largest” element among those belonging to the object specified in the following /LECT/. Use LECT tous TERM to get the largest element in the whole mesh. As largest element, we consider the one having the largest intra-nodal distance among its nodes (and thus most likely the longest element characteristic length as far as stability is concerned).
DIST <POIN> /LEC1/ <POIN> /LEC2/

Returns the minimum (intra-nodal) distance between the two objects defined in /LEC1/ and /LEC2/. Normally the two objects are interprested as a set of elements. The nodes of such elements are automatically extracted and used to compute the minimum (intra-nodal) distance. However, one may want to specify an object composed only of points (nodes). This can be done by adding the optional POIN keyword just before the /LECT/ of the concerned object(s).
MQUA ...

Introduces the commands to activate mesh quality assessment. See below for a complete description of all such commands.
TERM

Indicates the termination of measurements. This keyword is necessary so that the present directive may be used also in interactive mode.

Comments

An example of this directive (to achieve simple measurements) is as follows:

   MEASURE
     ELEM 123
     NODE 74
     ELEM 1
     OBJE LECT toto TERM
     EMIN LECT tous TERM
     EMAX LECT 1 2 4 TERM
     DIST LECT toto TERM LECT tata TERM ! min distance between two
                                        ! objects made of elements
     DIST POIN LECT p1 TERM LECT tata TERM ! min dist. between a point
                                           ! (node) and an object made
                                           ! of elements
     DIST POIN LECT p1 TERM POIN LECT p2 TERM ! distance between two
                                              ! points (two nodes)
   TERM

When used interactively, the code pauses for input after each sub-command, waiting for the next sub-command. To exit from the MEAS directive, give the final TERM command.

11.10.1  Mesh Quality assessment


Syntax:

        MEAS ... MQUA nmq
             ( $[ ASPE ; SKEW ; WARP ; TAPE ]$ < /LECT/ >
                < EROS eros > < PRIN > )
               < EVAL /CTIM/ >


MQUA nmq

Introduces the commands to activate mesh quality assessment. The nmq quantity is the number of mesh quality assessment criteria that will be defined next.
ASPE

Compute aspect ratio of the elements.
SKEW

Compute skewness of the elements.
WARP

Compute warping of the elements.
TAPE

Compute tapering of the elements.
/LECT/

Optional list of all elements for which the current quality criterion must be evaluated. By default (if omitted), the evaluation is done for all elements in the mesh (when applicable).
EROS eros

Optional keyword that produces the following effect: if the computed criterion exceeds the given value eros for an element, then the element is eroded (removed from the computation). If this keyword is omitted for a criterion, then no elements are eroded according to that criterion.
PRIN

Printout the evaluated criterion values on the listing each time they are evaluated. By default, i.e. without specifying the PRIN optional keyword, the evaluated values are not printed. Beware that the list of values may be long, since there is one value for each element in the mesh.
EVAL /CTIM/

Reading procedure (see page INT.57) of the chosen time steps or time instants at which the evaluation of the above defined mesh quality criteria should be performed. If omitted, the evaluation is performed at every time step. However, note that this may be very expensive so that in large applications it is strongly advised to perform the evaluation (and the optional element erosion) only at a certain chosen frequency in time.

Comments

The parentheses ( ... ) in the above syntax signify that more than one criterion can be chosen at the same time, by simply repeating the parenthesized context. The total number of declared criteria must be equal to the number nmq declared just after the MQUA keyword.

The results of the chosen quality criteria evaluations become available for visualization at the time steps or time instants specified in the /CTIM/ directive.

Each time an MQUA directive is entered (either in the input data set or from the command line, in case of interactive execution), any pre-existing mesh quality assessment criteria are wiped out and are replaced by the newly declared criteria.

An example of this directive is as follows:

   MEAS MQUA 3
        ASPE LECT plate TERM EROS 2.5
        WARP EROS 5.0 ! Erode if warping angle > 5 degrees
        SKEW
        EVAL TFRE 1.0E-3 NUPA LECT 5000 7500 TERM
   TERM

This means that the following three quality criteria will be evaluated:

The above mentioned evaluations (and the associated element erosions, if any) are performed every millisecond of physical time and, in addition, also at steps 5000 and 7500. At any of these chosen time instants the user will be able to visualize the computed quality criterion fields (one field for each active criterion).

11.11  SAVING FILE FOR SUCCESSIVE RESTART

G.110


Object:


This keyword creates a saving file and, in conjunction with the keyword REPR (to be used in a subsequent run), allows splitting a computation in two or more parts.


This directive replaces the old (deprecated and obsolescent) directive SAUV (group A, see page SR.20).


The results are saved on a file (saving file) at times specified by the user. Each saving corresponds to a number or position on the file (1, 2, 3 etc.), from which a restart of the computation can be carried out in a successive run (see directive REPR on page SR.30).


Syntax:

    FICH  SAUV <ndsauv>  <PROT 'maclef'>  <LAST>  </CTIM/>
nbansav

Number of the saving file or name of the file in quotes. If completely omitted, the code will assume the default file name <basename>.sau where <basename> is the root of the input file name (i.e. without extension .epx).
PROT

Keyword entering a protection on the saving file.
’maclef’

Key of up to 8 characters, enclosed in apostrophes. In order to restart the computation from that file, the instruction REPR must contain the keyword PROT with an identical key.
LAST

This keyword indicates that the saving file should contain just one saving station, corresponding to the last saved time station in the present calculation. In other words, each new saving station replaces the former one, if any. This allows to obtain a saving file of the smallest possible size. However, restarting from an intermediate time is obviously not possible in this case: the only possibility to restart the calculation will be REPR ... POSI 1 (see page SR.30).
/CTIM/

The /CTIM/ procedure (see page INT.57) is used to specify the saving times via a step frequency (FREQ), a time frequency (TFRE), a list of steps (NUPA) or a list of times (TIME). If NUPA or TIME are used, do not forget to dimension accordingly using MTTI or MNTI, respectively, see page A.100. Note that the code always saves the last step of the calculation (if the run is terminated normally), irrespective of the frequency chosen. Therefore, if one is only interested in getting the possibility to continue the calculation further on, simply omit the /CTIM/ procedure.

Comments:


The keyword PROT is not compulsory. If it is not used, there is no protection (this is equivalent to a key of 8 blanks).


If a unit number is used for nbansav, the saving file and its number must have been defined before on the control cards.


A first saving station (position number 1) containing some header data is always produced at the initial time (step 0 of the calculation). Of course, it is normally meaningless to restart from this time station, unless the LAST keyword has been specified (see above), because it would be the same as starting the calculation anew from the initial time. On the contrary, if LAST has been specified, the only possibility for restart is to use the first time station which, in this case, will contain the data of the last saving performed (not the first one in general).


Examples:


Assume a calculation performs 4994 time steps to arrive at its final time. The following saving directives are accepted:


Previous Up Next