Previous Up Next

12  GROUP H—OPTIONS

H.10


Object:


These keywords give the additional options of the computation. They can be grouped as:



Syntax:

    "OPTION"

OPTION

Announces that one or several options will be specified.

Comments:


The keyword "OPTION" may appear more than once in the EUROPLEXUS data.


The following sub-instructions may appear in any order.


The different options are described on the following pages.

12.1  OPTIONS RELATED TO THE TIME-STEP

H.20


Object:


Additional options are given to provide optimum time stepping.


Syntax:
     < |[ "PAS" |[ "UTILISATEUR" ; "AUTOMATIQUE" ]| ;
          "PARTITION" $["PLIN" ; "PNOL"]$ <PLOG> ]| >
     < "DTVAR"  dtvar      >
     < |[ "NOTEST" ; "TEST" ]| >
     < "STABILITE"           >    < "STEL" >
    (< "NOCRITIC" < $ "UPTO" t ; "TRIG" $ > /LECTURE/ >)
     < "CSTAB"      cstab    >
     < "PASMINI"    pasmi    >
     < "DTFORCE"    dtfor    >
     < |[ "STEP" "IO" ; "STEP" "IOT" ; "STEP" "LIBR" ]| >
     < "TION"       tionor   >
     < "DTML"                >
     < "DTBE"       kdtbe    >
     < "DIVG"       divg     >
     < "DTDR"       dtdrop   >
     < "CMDF"  <"NPAS"  npas > <  "CPUT"  cput > >


PAS UTILISATEUR

The time step is prescribed by the user (see also keyword CALCUL). Note that this option cannot be chosen in the case of impacts (the time increment may be limited by the program in case of an impact).
PAS AUTOMATIQUE

The time-step is determined by the program (see also keyword CALCUL). This is the default, i.e. if neither PAS UTIL nor PAR are specified the time step is automatically computed by the code.
PARTITION

The computation step is partitioned automatically in space (and the step also varies with time), according to the stability step of each element (see also keyword CALCUL).
PLIN

In the space partitioning procedure, dofs subjected to any links are treated according to the lowest level among the ones that are linked together. This works only with the LINK directive, while conditions imposed by the LIAI directive are not treated. The option has no effect in cases without space partitioning.
PNOL

In the space partitioning procedure, dofs subjected to any liaisons or any links (but only of the permanent type) are put in the lowest partition level. This is the default, so this option should not be used, except for changing back from a previously issued OPTI PLIN. The option has no effect in cases without space partitioning.
PLOG

In case of space partitioning, a special log file is written <basename>.plog. This file contains an output line for each sub-cycle, in contrast to the normal log file, which contains one line for each macro step. The extra information may be quite long but is sometimes useful for debugging. By default no such log file is written.
dtvar

Maximum growth factor of the time step among two subsequent steps in PAS AUTO. Default is 2.0.
NOTEST

The energy check and related information is not printed at each step, but only when general printouts are required (see ECRI).
TEST

The energy check and related information is printed at each step. This is the default.
STABILITE

The energy check and related informations is printed only if EUROPLEXUS reduces the time step.
STEL

At each step for which a printout is produced, the stability steps for all elements are printed out.
NOCRITIC

The elements defined in the following /LECTURE/ will not be considered in the calculation of the critical time step by EUROPLEXUS. In practice, they will be assigned a very large critical step. Optionally (see next keywords) this behaviour can be imposed only until a certain time or event. Note that the NOCR keyword (with its optional sub-keywords) can be repeated as many times as needed to set different criticality limits for the various elements in the mesh, if needed. Each element retains the last criticality limit that has been set for it (if any).
UPTO t

The above mentioned elements are not considered in the calculation of the critical step only until time t is reached. Thereafter, they are treated just like any other elements.
TRIG

The above mentioned elements are not considered in the calculation of the critical step only until a trigger is activated. The trigger refers to the TRIG keyword which activates mesh refinement in some adaptivity models, see OPTI ADAP TRIG on Page H.180. Thereafter, they are treated just like any other elements.
cstab

Safety coefficient assumed over the estimated stability (i.e., critical) time step for each element. Default value is 0.8. It is only effective for PAS AUTO or PART. See also the comments below.
PASMINI

The calculation will stop if the time increment becomes less than dtmax × pasmi.
DTFORCE

The stability step of the more stringent elements is forced to assume tha value dtfor by increasing their mass. This option is dangerous: see the comments below.
STEP IO

During the computation, the time step will be adjusted to exactly fit chosen times for output events such as printouts (see ECRI), storage of data for post-processing (FICH ALIC but not FICH TPLO nor FICH ALIC TEMP nor FICH TABL!), or storage of data for restart (FICH SAUV). Note that TPLOT, ALICE TEMPS and TABL data storages are not included (use STEP IOT instead). This choice is justified by the fact that TPLOT, ALICE TEMPS and TABL storage times are usually much more numerous than (normal) ALICE storages, but include only a limited number of nodes and elements. Note that this option has only effect in PAS AUTO or PART, but obviously it has no effect in PAS UTIL.
STEP IOT

Same as STEP IO, but now output events considered for time step adjustment include also TPLOT, ALICE TEMPS and TABL storages. Note that this option has only effect in PAS AUTO or PART, but obviously it has no effect in PAS UTIL.

STEP LIBR

During the computation, the step will be varied only according to stability limits. No adjusting to output times for printing, etc., will be performed. In this case, if the user chooses a given printout or storage time, the program will perform the action at the first step in which the time is equal or greater that the specified value. In general, the error on time is small since it is of the order of one time increment. This is the default (as opposed to STEP IO).
tionor

Important: to be effective, this option must be specified before the ECRI directive. This quantity represents the value of time units used for the normalization of selected times and time frequencies for printing and storage (in particular see the ECRI directive and its sub-directives for the different types of output files). It is only relevant to the STEP IO or STEP IOT options described above. The default value is 1 picosecond (1.D-12 s). Since at least 18 digits are available in an INTEGER(8), the final time of a calculation can be up to 1.D6 s with the standard value of tionor. Be aware that the normalization process may only take place if time values are less than 1.E18*tionor. An error is produced otherwise. This precision should be largely sufficient in practical cases. In fact, this allows to specify a precision of e.g. 1.E-6 times the typical time step, for a computation with up to 1.E12 steps.
DTML

This option chooses a different rule from the standard one to estimate the critical time step of JRC’s FLxx fluid elements. The standard rule for FLxx, originating from EURDYN, was quite complex and was documented in the report "Implementation of Compressible Fluid Models in PLEXIS-3C", Technical Note No. I.93.86. This rule was found to be inaccurate in some cases. The new rule activated with the present option uses the minimum intra-nodal distance as the characteristic length and the sound speed plus the maximum nodal (wv) value (mesh velocity minus fluid velocity) as the characteristic speed. This is in accordance with the rule used in CEA’s fluid elements. The DTML option can also be invoked to use the minimum intra-nodal distance for calculation of the stability of C27 elements in 3D (by default these elements use an estimation of the element’s stretch and shear to compute the element’s characteristic length).
DTBE

This option chooses a different rule from the standard one to estimate the critical time step for the POUT element. Three different values can be chosen: kdtbe = 0 indicates the default version (CEA’s formula); kdtbe = 1 uses an optimized time step (formula for ED01 elements); kdtbe = 2 considers only the length of the element and disregards the cross section. The default time step used for the POUT element seems to be very conservative. Larger time steps result using the formula for ED01 elements, which is as follows. If the element length L is larger than √(3)h, where h is the element thickness, then the normal expression is used: Δ t=L/c, where c is the sound speed. Otherwise, the element length is corrected: Lcorr=L2/√3h and then Δ t=Lcorr/c.
divg

This options give the possibility to define a value that the energy balance can not exceed. The default is 0.
dtdrop

Define the coefficient dtdrop. A warning message is printed on the listing each time the stability is imposed by a finite element and the ratio Δ t2 / Δ t1 is smaller than dtdrop. The default is 0.3. Some special materials (such as e.g. the JWLS material) used to represent very violent explosions and wave propagations may abruptly reduce the time step in order to preserve stability. In such cases, it may be useful to re-define dtdrop to values smaller than the default (e.g., 0.005) in order to avoid too many warning messages on the listing.
npas

Define the number of time steps after which the existence of the command file "command.epx" is checked.
cput

Define the CPU time after which the existence of the command file "command.epx" is checked. More information about the command file can be found in 17.

Comments:


Options by default : PAS AUTOMATIQUE TEST STEP LIBR.


The calculation stops if the time step becomes too small. The limit value is proportional to dtmax (directive CALCUL). By default, pasmi=0.001, i.e. the calculation will stop whenever the time step becomes less than 0.001 × dtmax. This option is only active when the old syntax of the CALCUL directive is used. With the new syntax, pasmin is redundant because DTMIN directly gives the minimum step (see I.20).


The energy check deals with the energy balance. The value of the stability time step is also printed.


The option PARTITION is especially useful when the mesh contains a few very small elements among a large number of bigger ones. In this case, the small elements are paid more attention, without carrying out useless computations on the big ones. This option could be inefficient if used when all elements have nearly the same size, or if there are only a few large elements in the mesh.


Like all explicit programs, EUROPLEXUS requires a sufficiently small time increment in order to ensure the stability of calculations. By default, EUROPLEXUS uses the CFL time step (Courant-Friedrichs-Lévy condition), multiplied by a safety coefficient CSTAB = 0.8. However, for very fast phenomena this condition may be insufficient. It is then possible to ensure stability by assuming for CSTAB a value smaller than 0.8.


The option DTFORCE affects only Lagrangian elements. In an ALE calculation, only the Lagrangian elements (if any) will be considered, and the others will be ignored. Since the mass of elements is modified, it is necessary yo check that such modifications do not affect too much the physics of the problem.


To this end, some indications are available on the listing:

12.2  OPTIONS RELATED TO THE DAMPINGS

H.30


Object:

To enter the dampings.


Syntax :

     |[   "QUASI" "STATIQUE"  fsys  beta <"FROM" t1> <"UPTO" t2> ;
          "AMORT" "LINE"  betal                                 ;
          "AMORT" "AXIA"  betal                                 ;
          "AMORT" "QUAD"  a2                                    ;
        $[ "HOURG" "VISC"  hvis ; "NOHOURG" ]$                  ]|
QUASI STATIQUE

Quasi static computation. A linear damping with a given cut-off frequency is applied.
fsys

Frequency f of the first system mode to be cut off.
beta

Reduced damping coefficient β.
t1

Initial time t1 at wich the quasi-static option starts to operate. By default, this coincides with the initial time of the calculation. See comments below for the use of t1 and t2 to define a closed interval or two open intervals.
t2

Final time t2 until wich the quasi-static option operates. By default, this coincides with the final time of the calculation. See comments below for the use of t1 and t2 to define a closed interval or two open intervals.
AMORT LINE

Computation with linear damping of high frequencies (artificial viscosity). This damping is advisable in FE calculations (CEA model: CAR1, CUBE etc.) involving a liquid, but it can also safely be added in calculations involving gases. The value to be used is betwen 0.05 and 0.20 in general. Note that this damping has no effect on calculations with cell-centred finite volumes (VFCC). In fact, the scheme with limiters used in that case is built in such a way that it does not need any damping. Note also that linear damping in FE models for fluids from JRC (FLxx elements) is activated by the keyword CL of the FLUT material, see Page C.520.
AMORT AXIA

Computation with linear damping of high frequencies, but only for the elements on the symmetry axis (for 2D axisymmetric problems only).
betal

Reduced damping coefficient βl for linear damping (of type LINE or AXIA).
AMORT QUAD

Computation with quadratic damping (artificial viscosity). This damping is advisable in FE calculations (CEA model: CAR1, CUBE etc.) involving a gas, but it can also safely be added in FE calculations involving liquids. The value to be used is betwen 2.0 and 4.0 in general. Note that this damping has no effect on calculations with cell-centred finite volumes (VFCC). In fact, the scheme with limiters used in that case is built in such a way that it does not need any damping. Note also that quadratic damping in FE models for fluids from JRC (FLxx elements) is activated by the keyword CQ of the FLUT material, see Page C.520.
a2

Coefficient a2 for the quadratic damping (shock waves).
HOURG VISC

Anti-hourglass damping on viscous terms.
hvis

Reduced damping for anti-hourglass hvis (hvis=0.5 is suggested).
NOHOURG

Allows to eliminate the anti-hourglass damping.

Comments :

In the case of the QUASI STATIQUE option, β=1 corresponds to the critical damping for the frequency f. In fact, one adds an external force FiQS proportional to the mass Mi and to the particle velocity vi for each degree of freedom i:

FiQS = − 4 π β f Mi vi = −2βω Mi vi

where ω=2π f.


In practice, only the product β f is relevant.


Linear damping of high frequencies is only possible for elements of type CAR1, CAR4, TRIA, TUBE, FUN2 and FUN3. This damping allows to eliminate the high-frequency oscillations related to the finite element discretization. In order to obtain the critical damping of a free-free oscillation for each element, take βl = 1.


When t1 is less than t2 (be these values specified or not) the quasi-static damping acts in the closed time interval t1tt2, i.e. in the central part of the transient calculation. However, it is also possible to specify t1 greater than t2: in this case the critical damping acts in the open time interval tt2 (i.e. at the beginning of the calculation) and in the open time interval t1t (i.e. at the end of the calculation). This second form of the directive may be useful when one wants to model a structure initially subjected only to gravity loads (with quasi static option so as to rapidly reach the initial static deformed configuration), followed by a dynamic event such as an explosion (without quasi static option), and finally by a stabilization phase (again with quasi static option) so as to rapidly compute the final static deformation. Thus this form of the directive allows to perform the complete analysis of the three phases in just one run of the code, instead of running three separate calculations (each one starting from the results of the previous one) via e.g. the directive INIT ALIC (see page E.140).


For the quadratic damping, it is suggested to take a2 = 4.


Quadratic damping is only possible for elements of types CAR1, CAR4, CUBE, PRIS, TRIA and TUBE.


The present linear and quadratic damping models are distinct from the selective damping model (AMOR) described on page C.106, which applies to selected dofs and nodes of a zone specified by the user.


The anti-hourglass damping is currently available only for the elements CAR1 et CUBE. By default, an anti-hourglass damping with hvis = 0.5 is affected to a calculation. If the user wants to do a calculation without anti-hourglass damping, he must use the option NOHOURG.


Warnings :

In case of restart, the QUASI STATIQUE damping remains active; to eliminate it, one must specify β = 0.


Linear damping should be used with care, since it may considerably perturbate the solution. It is advisable not to exceed the value βl = 0.05. In case of axisymmetric linear damping, since the concerned elements are usually a few and with a small mass, on may go up to βl = 0.5.

12.3  OPTIONS FOR FINITE ELEMENTS AND GEOMETRIC ISSUES

H.40


Object:

To introduce optional parameters related to finite elements and geometric issues.


Syntax:

     <   "DECENT"  |[       "TOTAL" ; "CALC"       ;
                            "IMPOSE" "DCEN" de "DCMA" dm  ]|  >
     <   "ROLIM"  rholim                               >
     <   "JAUMAN"                                      >
     <   "CODG" < "REFE" zbar >   <SMAL>               >
     <   "EDSS"                                        >
     <   "LFUN"                                        >
     <   "P2X2"                                        >
     <   $ "NF34" ; "OF34" $                           >
     <   "MOMT" kmtran                                 >
     <   "TOLC" tolc                                   >
     <   "HGQ4" hgq4ro                                 >
     <   "CLMT" < "FARF" farf> < " ABSI" absi>         >
     <   "LMST"                                        >
DECENT CALC

A.L.E. only. Upwinding computed by EUROPLEXUS according to the volume covered in one time step with respect to the total volume.
DECENT TOTAL

A.L.E. only. Total upwinding for the mass.
DECENT IMPOSE

A.L.E. only. Prescribed upwinding.
de

Upwinding concerning transport terms.
dm

Upwinding concerning mass fluxes.
ROLIM rholim

ALE/Eulerian only: if the donor element has a density less than rholim, the mass and energy fluxes are not considered for this element.
JAUMAN

Large strain computation with JAUMAN’s stress tensor.
CODG

Introduces options for calculations with degenerated shell elements (CQDx).
zbar

Parameter defining the position of the reference surface for degenerated shell elements: -1 indicates the lower element surface, 0 the mean surface, +1 the upper surface. By default, zbar = 0.
SMAL

Specifies that a small strain model of membrane deformation has to be used for degenerated shell elements, so the thickness of these elements stays constant. By default, a large membrane deformation is assumed and the element thickness is varied accordingly. This option is only useful to compare a solution with an old run done by JRC’s SHELL3D.
EDSS

Specifies that certain elements (ED01, FUN2, FUN3) will adopt a small strain, large displacements, large rotations formulation instead of the large strain formulation that is used by default.
LFUN

Specifies that certain elements (FUN2, FUN3) will adopt a fully linear, small strain model: element cross section stays constant and also length stays constant for the calculation of critical time step (which is therefore constant). This option should only be used for debugging purposes and for the study of time integration algorithms (to compare analytical and simplified numerical solutions).
P2X2

This option activates a spatial integration rule for pressure forces in CEA’s fluid elements (CUBE, PRIS, TETR) which is equivalent to a 2x2x2 Gauss rule, and is therefore exact also for distorted geometry (e.g. non-planar faces). The standard rule uses a single-point scheme which is under-integrating the function in the presence of distortions. The resulting inaccuracy of pressure force computation leads to the effect that fluid nodes internal to the fluid domain and completely surrounded by a fluid at uniform pressure are not in perfect equilibrium when the surrounding mesh is irregular. Spurious resultant pressure forces cause spurious velocities in the fluid which are non-physical. Although these velocities were usually found to remain relatively small with respect to physical ones in typical applications (explosions etc.), it is generally preferable to avoid them altogether by using the present option, although it is of course slightly more computationally expensive. The standard rule (single-point) is left as a default for compatibility with old input files and applications.
NF34

Use new (2007) implementation for FL34 JRC’s tetrahedral 4-node fluid element. The new implementation is described in reference [235]. From April 2014 this is the default, so it should be rarely necessary to specify this option.
OF34

Use old (before 2007) implementation for FL34 JRC’s tetrahedral 4-node fluid element.
MOMT

This option allows choosing the degree of precision for the spatial integration rule used in the computation of momentum transport forces in Eulerian or ALE calculations using JRC’s FL3x fluid elements. The kmtran parameter may assume the values 0 (no momentum transport forces at all), 1 (corresponding to single-point integration), 2 (for 2x2x2 spatial integration) or 3 (3x3x3 spatial integration). For distorted geometries only the 3x3x3 rule is exact. The default rule (as used in EURDYN) is the single-point one which is of course the most economical, but unfortunately may lead to spurious mechanisms (appearance of spurious fluid velocities) in some cases, typically when the geometry of the elements is irregular or distorted (e.g., non-planar faces). The mechanisms may rapidly grow and in some cases they completely destroy the numerical computation. In all practical cases investigated so far it was found that a 2x2x2 rule (MOMT 2) is accurate enough and sufficient to prevent the appearance of mechanisms. The cost of this is of the order of 20% to 30% overhead compared with the default, (MOMT 1) option. The MOMT 3 option is exact, but may cause a 100% overhead in computer time. Finally, note that the MOMT 0 option is only to be used for debugging purposes, since computations without momentum transport forces are of course largely inaccurate.
TOLC

This option allows to change the tolerance tolc that is used to automatically search for node correspondence, see page C.92. The default behaviour (no OPTI TOLC) is that two nodes are considered to match if their initial positions differ, along each one of the global coordinate axes, by less than 1.E-4 times the “mean” size of the mesh. This mean size is defined as the sum of the sizes of the mesh along each one of the global axes, divided by the space dimension. If tolc is explicitly specified, it is retained as the maximum distance between two coincident nodes along the global axes. In this case therefore, the above mentioned mean mesh size is not computed: tolc is used directly. Note that, in order to be effective, this option must be specified before the directives that might use it, in particular before the LIAI FSA directive.
hgq4ro

Adjusting coefficient for the anti-hourglass rotation stiffness of the Q4GR shell element. The default value of hgq4ro is 0.018.
CLMT

This keyword introduces options for the treatment of momentum transport forces in fluid Finite Elements (JRC formulation, i.e. FLxx family of elements). It applies to the CL22, CL2S, CL3I, CL3Q and CL3S element types, associated with either a FLUT material (for far-field conditions) or an IMPE ABSI material (for absorbing boundary conditions).
FARF farf

Use FARF 1 to activate momentum transport forces in CLxx due to far-field conditions, or FARF 0 to de-activate them. The default is 0, i.e. no momentum transport forces.
ABSI absi

Use ABSI 1 to activate momentum transport forces in CLxx due to absorbing (IMPE ABSI) conditions, or ABSI 0 to de-activate them. The default is 0, i.e. no momentum transport forces.
LMST

The LMST option (for Large Membrane STrains) is used to activate the update of the thickness of some shell elements (from CEA) due to large membrane strains. The affected elements are Q4GS and T3GS. Note, however, that the thickness update is activated only if such elements possess a non-linear material (i.e. other than LINE or GLRC). By default, the thickness of such elements is not updated even if large membrane strains occur. Note also that the thickness of other shell elements from CEA (namely Q4GR, QPPS, DST3, DKT3, T3MC) is also never updated and the present option will have no effect on such shell elements.

Comments:

A large strain calculation with the JAUMAN tensor is only possible at the moment with elements "CAR1", "CAR4" and "TRIA".


The upwinding is only effective for a computation with a non-Lagrangian formulation (keyword "ALE" or "EULER" in the type of problem to deal with , see page A.30).


By default, EUROPLEXUS uses the total upwinding (dm = 1 and de = 0).

12.4  OPTIONS FOR FLYING DEBRIS

H.45


Object:

To introduce optional parameters related to the flying debris model.


Syntax:

     < "DEBR" <"NTRA" ntra> <STTR> >
DEBR

Starts the specification of debris-related options.
NTRA ntra

Number of points ntra for flying debris trajectories. The points are equi-spaced in time betwee the initial time and the final time of the calculation given in the CALC directive. The actual number of points will be ntra + 1, since also the initial position (initial time) is stored. The default value of ntra is 100 points (i.e., 101, if one counts also the initial point).
STTR

Store the flying debris trajectories on the ALIC file. This will allow visualizing the trajectories when reading back the results (RESU). If this option is not set, the trajectories are not stored in the ALIC file (because these data may be huge, if there are many particles), and in this case the trajectories can only be visualized during the main calculation (not when reading back the results).

12.5  OUTPUT OPTIONS

H.50


Object:

These options enable the output format to be chosen.


Syntax:

     < $[ "NOPR" ;
          "PRIN" < "PMESH" > < "PCAST" > < "PCOMP" >
                 < "PGRID" > < "PLOAD" > < "PLINK" >
                 < "PRESU" > < "PLAW"  > < "PMED"  > ]$ >
     <   "DPMA"              >
     < $[ "NWAL" ; "WALI" ]$ >
     < $[ "NWSA" ; "WSAU" ]$ >
     < $[ "NWTP" ; "WTPL" ]$ >
     < $[ "NWXP" ; "WXPL" ]$ >
     < $[ "NWAT" ; "WATP" ]$ >
     < $[ "NWK2" ; "WK20" ]$ >
     < $[ "NWST" ; "WSTB" ]$ >
     < $[ "NOEC" ; "ECHO" ]$ >
     <   "LOG" nlog          >
     <   "K2FB" k2fibe       >
     < $[ "K2CH" ; "K2GP" ]$ >
     <   "K2MS" |[ "MANU" ; "READ" ]| >
     <   "DYMS" nobj*("OBJE" /LECT/) >
     <   "PRGR" >
NOPR/PRIN

This option allows to suppress or re-activate a part of the printouts of the following directives.

If one of the keywords PRIN/NOPR is followed by one or more parameters, only the corresponding parts of the listing are activated (or deactivated)

"PMESH" : mesh (nodal coordinates and elements topology)
"PCAST" : detail of the CASTEM objects
"PCOMP" : geometrical complements
"PGRID" : parameters of the ALE rezoning
"PLOAD" : details of the charges
"PLINK" : details of the liaisons/links
"PRESU" : details of the results files
"PLAW" : details of the material laws
"PMED" : detail of the MED objects
See also the comments below.

"DPMA"

Prints nodal and element masses with each general printout. This can be useful to check masses in problems where the mass varies, such as ALE calculations.
NWAL

No printout on the listing of information about each storage of data for ALICE (see "FICH ALIC").
WALI

A line of information containing the time, step number, etc. will be printed on the output listing at each storage of data on the ALICE file (see "FICH ALIC"). This is the default option.
NWSA

No printout on the listing of information about each storage of data for restart (see "SAUV").
WSAU

A line of information containing the time, step number, etc. will be printed on the output listing at each storage of data on the restart file (see "SAUV"). This is the default option.
NWTP

No printout on the listing of information about each storage of data for TPLOT (see "FICH TPLO"). This is the default option, since usually many storages are requested for TPLOT.
WTPL

A line of information containing the time, step number, etc. will be printed on the output listing at each storage of data on the TPLOT file (see "FICH TPLO").
NWXP

No printout on the listing of information about each storage of data for XPLOT (see "FICH XPLO").
WXPL

A line of information containing the time, step number, etc. will be printed on the output listing at each storage of data on the XPLOT file (see "FICH XPLO"). This is the default option.
NWAT

No printout on the listing of information about each storage of data for ALICE TEMPS (see "FICH ALIC TEMPS"). This is the default option, since usually many storages are requested for ALICE TEMPS.
WATP

A line of information containing the time, step number, etc. will be printed on the output listing at each storage of data on the ALICE TEMPS file (see "FICH ALIC TEMPS").
NWK2

No printout on the listing of information about each storage of data for K2000 (see "FICH K2000").
WK20

A line of information containing the time, step number, etc. will be printed on the output listing at each storage of data on the K2000 file (see "FICH K2000"). This is the default option.
NWST

No printout on the listing of information about each storage of data for SUPERTAB (see "FICH SPTAB").
WSTB

A line of information containing the time, step number, etc. will be printed on the output listing at each storage of data on the SUPERTAB file (see "FICH SPTAB"). This is the default option.
NOEC/ECHO

This option allows to suppress or re-activate input data echo in the EUROPLEXUS window.
LOG

Causes a one-line information to be written to standard error file each ’nlog’ time steps. The information includes current step number, time, CPU time, critical step, critical element, energy check and mass check. This is useful e.g. to monitor the execution of very long and CPU-intensive runs. Usually, the standard error information will be redirected to a file, e.g. with the Unix command ’2>file’. The colums of the log files (S standard calculation, P calculation using partitioning) are described in the table below.
 DescriptionSP
STEPTime step number (main step for Partitioning)XX
TIMETimeXX
CPU(S)CPU time usedXX
DTCRITCritical time step usedX 
ELCRElement with the smallest time stepX 
DELMINTime step of the smallest substep X
MINSMinimum level factor X
DE/EEnergy balance per elementXX
DM/M(NOD)Mass balance per nodeXX
DM/M(ELE)Mass balance per elementXX
DTMXMaximum time stepX 
ELElement of the maximum time stepX 
DELMAXTime step of the main step X
MAXSMaximum level factor X
VITMAXMaximum velocityXX
NODENode of the maximum velocityXX
ISUBTOTotal number of substeps X
MAXSTOTotal number of substeps X
ELSTEPNumber of callings of element routinesXX
K2FB

Indicates the index of the Gauss Point, along each fiber, for which variables are stored for subsequent K2000 postprocessing. For example, if there are 5 GPs along fibers in the shell elements used in a calculation, then k2fibe=1 indicates the GPs closest to one face of the structure, k2fibe=5 indicates the GPs closest to the opposite face of the structure, k2fibe=3 indicates the GPs on the midsurface of the strucure, and so on. Note that this parameter has only effect for shell elements of types ED01, ED41, COQI and CQDx. The default value is k2fibe=1.
K2CH

With this option, the output chamelems for K2000 will be defined for each element at the element nodes, rather than at the element barycenter (default) or at the Gauss points (K2GP option). Note, however, that the computation of values is crude: an average on all GPs is computed, and this value is affected to all nodes of the element (although the contributions to the same node from different elements may be different). The default (without the K2CH option) is to compute an average on all GPs and affect this value to the barycenter of the element.
K2GP

With this option, the output chamelems for K2000 will be defined for each element at the Gauss points, rather than at the element barycenter (default) or at the element nodes (K2CH option). The exact value is affected at each GPs of the element. In case of multilayer plates (CEA-plates: DKT3, Q4GS...) an average on the GPs in the thickness is computed, and each of these values is affected to the corresponding GP on the surface of the element. The default (without the K2GP option) is to compute an average on all GPs and affect this value to the barycenter of the element.
K2MS

With this option, the code will produce a file containing a series of GIBIANE instructions that, when processed by CASTEM2000, will produce the current mesh in CASTEM2000 format. This option is only useful when the mesh has been produced by a pre-processor different from CASTEM2000 (see also comments below).
MANU

The CASTEM2000 mesh generation commands will use the CASTEM2000 operator MANU. The name of the generated file is pxtok200.dgibi on the current directory
READ

The data for CASTEM2000 will be written on file pxtok200.inp on the current directory. These data are suitable to be read by CASTEM2000 via the READ operator (see also comments below)
DYMS

With this option, the code will produce an input file for LS-DYNA. For each of the nobj objects defined by the OBJE keyword (which must be repeated exactly nobj times), the nodes and elements are written in this file. No material and load definitions are exported.
PRGR

Print named element and node groups on the listing in a format that can be directly included in a .EPX file (on 72 columns and using LECT ... PAS ... TERM syntax). This printout is made in addition to the normal printout of named groups on the listing. To find the group of lines search for COMP GROU and for COMP NGRO in the listing. Note that in order to be effective, this option must be set before the definition of the named groups.

Comments:

The presence of OPTI NOPR immediately after the dimensioning in the input file minimizes the listing file. On the contrary, OPTI PRIN maximizes the listing file. It is possible to activate or deactivate the various printouts selectively. For example:

        OPTI  NOPR  PMESH  PCAST  PLINK

will deactivate the printouts relative to the mesh, the CASTEM objects and the liaisons/links. This allows to avoid repeating the commands NOPR and PRIN within the input file.


In case of re-reading the results file (file ALICE or ALICE TEMPS) the option NOPR is taken by default. To have complete printouts, it is sufficient to add OPTI PRIN after the keyword TERM of directive DIME.


The K2MS option can be very useful in the case that an input file for EUROPLEXUS uses a mesh defined in a format different from CASTEM2000, but the user wants to do the post-processing of the calculation by CASTEM2000. This option will produce a file containing data that can be used by CASTEM2000 to generate the desired mesh.


Typically, in such cases one would perform the following steps:


1. - Run the EUROPLEXUS input file with the non-CASTEM mesh, including option K2MS. The calculation can be stopped at step 0 (use VERI or CONV TEKT and then the stop interactive command). This will produce a file of data for CASTEM2000 in either file pxtok200.dgibi or file pxtok200.inp on the current directory.


2. - Run CASTEM2000 on the above mentioned file, to produce a mesh in CASTEM2000 format. See below for examples and details.


3. - Finally, run again EUROPLEXUS by specifying that the input geometrical data are from CASTEM2000 (CASTEM directive). Now, a CASTEM2000 post-processing file can be produced by EUROPLEXUS, because the input is indeed in CASTEM2000 format.


Note, however, that the CASTEM2000 mesh produced by this method will be somewhat special, in that no meaningful subobjects will be generated. Only the global mesh will be accessible as object "mesh".


When the K2MS MANU option is used, the file produced (pxtok200.dgibi) will contain a line for each node, of the form:

        Pxxxxx = xcoor ycoor [zcoor];


where xxxxx is the node number (e.g., 00025 for node 25), xcoor, ycoor (and zcoor in 3D) are its coordinates.


For example:

        P00332 =   1.000000000000D+01  1.000000000000D+01 ;

Then, for each element there will be a line of the form:

        Eyyyyy = manu elem node1 node2 ... ;


where yyyyy is the element number, elem is the element type according to CASTEM2000 (e.g., QUA4 for 4-node quadrilaterals) and node1, node2 etc. are its nodes. For example:

        E00002=manu QUA4 P00004 P00006 P00005 P00003;


The global object will be called mesh. If you need to define sub-objects, use appropriate GIBIANE instructions.


A typical CASTEM2000 command file using pxtok200.dgibi is as follows:

        (pxtok200.dgibi as produced by EUROPLEXUS) ...

        mesh3 = mesh ELEM 'TRI3';
        mesh4 = mesh ELEM 'QUA4';
        ...
        opti sauv 'file';
        sauv mesh;


Unfortunately, it has been noted that CASTEM2000 changes the numbering of elements in a mesh generated in this way. The other method (using the READ option) can be used in cases this could cause trouble (which is typically the case if other input directives in the EUROPLEXUS input file use element numbers). Or, alternatively, try using the SORT operator instead of the SAUV operator to save the mesh, as detailed below.


When the K2MS READ option is used, the file produced (pxtok200.inp) contains a simple list of nodal coordinates and element topology (by zones). These data can be read by CASTEM2000 using the READ operator developed at JRC.


To this end, use a command file of the form:

        ...
        mesh = READ 'pxtok200.inp' MESH ELEM;
        mesh3 = mesh ELEM 'TRI3';
        mesh4 = mesh ELEM 'QUA4';
        ...
        opti sauv 'file';
        sauv mesh;


From the tests performed, it seems that CASTEM2000 maintained the element numbering in this case, but only up to version 9 of the SAUV operator included. For higher versions of the SAUV operator, numbering is generally changed.


In order to try to avoid renumbering, use the CASTEM operator SORT instead of SAUV to save the mesh. The SORT operator is more limited than SAUV (it may only save meshes, for example), but has the advantage that it apparently does not change mesh numbering, and its implementation is somewhat “frozen” in the code, unlike the SAUV operator which evolves constantly.


Recall that a mesh saved with SORT must be read in EUROPLEXUS by the GIBI directive, not by the CAST directive (see page A.30), and that SORT files are formatted by default.


The command file will be in this case of the form:

        ...
        mesh = READ 'pxtok200.inp' MESH ELEM;
        mesh3 = mesh ELEM 'TRI3';
        mesh4 = mesh ELEM 'QUA4';
        ...
        opti sort 'file';
        sort mesh;


In EUROPLEXUS, the mesh will be read as follows:

        ...
        GIBI 'file' mesh
        ...

12.6  RETURNING TO DEFAULT OPTIONS

H.60


Object:


To set the options relative to a standart computation back to their default values.


Syntax:
     <   "ZERO"                           >


ZERO

Discards any previous options, returning to default values.

Comments:


All the options which have been defined previously are discarded, and the options by default are assumed again.

12.7  OPTIONS FOR AN ADVECTION-DIFFUSION COMPUTATION

H.70


Object:


To provide options for an advection-diffusion computation.


Syntax:
     <   "ADDF" < "GRAV" gravi  > < "PSYS" psyst  >
                < "ELEM" ielref > < "SORD" nsord  >
                < "NGAU" ngau   > < "ITER" nitef  >
                < "ITEP" niter  > < "TOLER" titer >
                < "ADTI" adtime > < "ERRO" errix  >
                < "NIMA" nimax  >                     >


gravi

Acceleration of gravity (default=0.0).
psyst

System pressure, used to remove the singularity of the pressure field solution matrix (default=0.0).
ielref

Index of element in which the pressure is equal to psyst. (default=1)
nsord

When 2, 3 or 4, a Taylor-Galerkin method is used of order 2, 3 or 4, respectively (default=2). When nsord=5, a Least-square, space-time method is used. When nsord=6, a Least-square, Crank-Nicolson method is used.
ngau

Number of Gauss points in each direction for the integration of advection terms, can be 1 or 2 (default=1).
nitef

Number of iterations in the factorization of the consistent mass matrix during the advection phase, can be 1 to 9. (default=3)
niter

Maximum number of iterations for the solution of the system of equations for the pressure phase. If set to null, a direct solution is performed (default=0).
titer

Convergence tolerance for the iterative solution of pressure phase equations (default=0.01).
adtime

Time step fraction.
errix

Tolerance of implicit resolution. Is only used with Least-square method (see nsord above).
nimax

Maximum number of iterations for implicit resolution. Is only used with Least-square method (see nsord above).

12.8  OPTIONS FOR ALE CALCULATIONS IN STRUCTURES

H.80


Object:


To provide options for an ALE calculation in structures.


Syntax:
     <   "ALES"  |[ "KINT" kintm ; "UPWM" upwm ; "UPWS" upws ]| >


kintm

Integration type for momentum transport: 0 means 1x1 (not available for the moment!), 1 means 2x2 (exact for plane problems), 2 means 3x3 (exact for axisymmetric problems). Default is 1.
upwm

Upwind parameter for momentum transport, can be chosen between 0 and 1 (default is 1.0).
upws

Upwind parameter for stress transport, can be chosen between 0 and 1 (default is 1.0).

12.9  OPTIONS FOR DEBUGGING

H.90


Object:


To provide options to help in debugging the program (for developers only).


Syntax:
     < $[ "DUMP" ; "NODU" ]$              >
     <   "DPAS" /LECTURE/                 >
     <   "DPEL" /LECTURE/                 >
     <   "DPEM"                           >
     <   "VIDA" /LECTURE/                 >
     <   "DPGR"                           >
     <   "OLDS"                           >
     <   "DPCA"                           >
     <   "DPLE"                           >
     <   "DPLM"                           >
     <   "DPSD"                           >
     <   "DPAR"                           >
     <   "DPAX"                           >


"DUMP"

Prints dump of variables as long as they are initialised in the various routines before starting time integration. Of course, this option tends to produce extremely large output files and is only useful for very small test cases, for program development.
"NODU"

Turns off dumping option.
"DPAS"

The following list enumerates the integration time steps for which extensive information has to be dumped out. A maximum of 200 step indexes can be specified (this dimension is fixed).
"DPEL"

The following list enumerates the elements for which extensive information has to be dumped out. A maximum of 20 element indexes can be specified (this dimension is fixed).
"DPEM"

Prints (on the log file!) tables of available elements and materials in a format suitable for rapid inclusion in this user’s manual.
"VIDA"

The following list indicates the indexes of the variables to be dumped (these can range from 1 to the total number of variables, see include MAPORGA), a value of 0 indicates that the contents of the commons has also to be dumped. Note that the commons are dumped at the moment when the directive ’OPTI VIDA LECT 0 TERM’ is encountered in the input file, therefore it is suggested to place this directive just before the ’CALC’ directive, which starts the time-marching calculation.
DPGR

Prints a table containing the list of all nodes with their grid motion attributes: L for Lagrangian, E for Eulerian, AA for ALE, manually rezoned, AM for ALE, automatically rezoned, AS for ALE, rezoned by "FSS ALE", AZ for ALE, rezoned by "MEAN". The dump is performed after complete processing of the input, immediately before starting the time loop. This allows to check possible changes applied by the program to conditions imposed by the user through the "GRILLE" directive. This option is only active for Eulerian or ALE calculations.
"OLDS"

Specifies that an old model for the VM23 material has to be used in place of the most recent model. The old model was slightly less accurate in elastoplastic cases and was used in the EURDYN programs. This option should only be used for debugging purposes, if a very precise comparison with an old EURDYN calculation is desired.
"DPCA"

Prints on the listing tables of element and material characteristics. For the elements, the NCEL variables are listed in tabular form, for the materials the MATALE and LGEP variables are listed.
"DPLE"

Prints on the listing a table of element characteristics in LATEX input format. This may then e.g. be edited for inclusion in the present User’s Manual.
"DPLM"

Prints on the listing a table of material characteristics in LATEX input format. This may then e.g. be edited for inclusion in the present User’s Manual.
"DPSD"

In multi-domain calculations, dumps out extra information on the listing file. Furthermore, for each sub-domain a separate log file is produced that reports, at every time station, a line collecting information relevant to the sub-domain. The name of such files is <base_name>_xxx.log, where xxx is the index of the sub-domain (e.g. 012 for the twelfth sub-domain), and base_name is the base name of the test case (without the extension .epx). By examining these log files, one is able to follow precisely the time integration history of each sub-domain. At most 10 such log files are produced, therefore if the number of sub-domains is larger only the first 10 sub-domains will be dumped out.
"DPAR"

In calculations with space partitioning, dumps out extra information on the listing. All cycles, in addition to macro steps, are printed out.
"DPAX"

Dump out on the listing a list of all nodes on the axis of revolution i.e. nodes with x=0. This option has only effect in 2D axisymmetric calculations, and must be issued before the GEOM directive.

Comments:


Another useful debugging tool is the "ECHO" "VERI" directive (see page A.20) that causes, among other things, the memory allocated to each variable to be printed out.


Concerning the "DPSD" option, note that the per-domain log files are automatically opened under the Windows platform. On non-windows platforms (e.g. Unix), it may be necessary to explicitly open these files by including in the input file appropriate OPNF directives (see page A.28). Here is an example:

  (on non-Windows platform)

  OPNF FORMAT 51 '/disk1/fauvin/SD_001.LOG'
  OPNF FORMAT 52 '/disk1/fauvin/SD_002.LOG'
  . . .
  OPTI DPSD
  . . .
  STRUCTURE 2
   DOMA LECT ZON1 TERM
   DOMA LECT ZON2 TERM
  . . .

In this example there are 2 sub-domains. Note that the unit numbers to be used are 51, 52, etc. up to 60 (max. 10 sub-domains). The names associated with the files are arbitrary, and the files are formatted. On some platforms, full-path names only are accepted as in the above example.

12.10  PHANTOM OPTION (Element erosion by time)

H.100


Object:


Elements are eroded when the time exceeds a given value.


Syntax:
        "FANTOME"    t_fant  /LECTURE/


t_fan

Time starting from which the elements become eroded.
/LECTURE/

List of the concerned elements.

Comments:


This option may appear at most once. However, it is possible to declare as many sequences t_fant, /LECTURE/ as needed.


In order to use this option, do not forget to specify the EROS keyword in the problem type, see GBA_0030. The value of ldam after EROS must be also given, but it has no effect on the present option.

12.11  CLASS (For a post-treatment with the directive REGION)

H.105


Object:


This directive allows to create classes of elements within a list of elements. Each element of the list of elements may belong to one and only one class.


Syntax:
        "CLASSE"    /LECTURE/
                    nb_classes*(/LECTURE/)


/LECTURE/

List of elements.
nb_classes

Number of classes.
/LECTURE/

List of elements of each of the classes.

Comments:


This option may appear at most once.


This option must be associated with the directive REGION defined on the list of elements to obtain informations on the classes (see G.100).

12.12  SHOCK AND IMPACT OPTIONS

H.110


Object:


This option alows to define the energy restitution coefficients for the shocks and the impacts.


Syntax:
        "CHOC"       coechoc


coechoc

Energy restitution coefficient for shocks and impacts.

Comments:


The restitution coefficient is between 0 (plastic shock) and 1 (perfectly elastic shock).


The default value (when the present option is not activated) is 0.5.

12.13  OPTIONS FOR FSA/FSR

H.120


Object:


To provide options for fluid-structure interactions of the ALE type for an either deformable (FSA) or rigid (FSR) structure.


Syntax:
     < "FSA" "ALF0" alf0 >
     < $[ "NFSC" ; "FSCR" < "INCL" /LEC1/ > < "EXCL" /LEC2/ > ]$  >
     < "FSR" "MFSR" >


alf0

Maximum angle, in degrees, between two element faces for which a unique normal is computed. If the actual angle exceeds this value, then two distinct normals are generated. By default, alf0 = 60 degrees.
NFSC

Do NOT correct geometrically computed normals for the FSA and FSR fluid-structure interaction conditions. This is the default.
FSCR

After computing geometrically the normals for the FSA and FSR fluid-structure interaction conditions, apply a correction based on the direction of fictitious internal forces resulting from a uniform pressure field p =1. This correction can be useful e.g. in 3D cases when the element faces are warped (non-planar), or when the integration of the element’s internal forces is done with an integration rule that does not exactly match the estimation of the normal to the surface computed by purely geometrical considerations from the surface data.
INCL /LEC1/

An optional list of nodes to which the FSCR option is applied. By default, the option is applied to all FSA and FSR nodes.
EXCL /LEC2/

An optional list of nodes to which the FSCR option is not applied. By default, the option is applied to all FSA and FSR nodes.
MFSR

Allow a manually rezoned (i.e., moving) node to be declared FSR at the same time. These two conditions are normally incompatible and therefore an error message is normally issued and the code stops. However, there are cases when this is not an error (but only the user can judge on this, it cannot be done automatically). An example is a node on a rigid plane which at the same time must be moved by some manual rezoning to avoid mesh entanglement. The node can be at the same time manually rezoned (along the plane) and FSR because the link coefficients stay constant even though the node moves. The option deactivates the error message: only one warning message is issued, for the first node concerned. Note that obviously, if this option is specified, it must be inserted in the input file before the LIAI FSR or the LINK FSR directive.

Remarks


In some special cases it may be useful to exclude some FSA or FSR nodes from the FSCR correction. For example, in the transition zone of a pipeline mesh between a 3D representation and a 1D representation by means of the TUYM (deformable structure) or TUBM (rigid structure) junction: all fluid nodes in the external circumference of the 3D pipe mesh shall be declared FSA or FSR, but we want to make sure that no FSCR correction is applied to them (while it may be desirable for the other nodes). So we may explicitly exclude them by means of the EXCL /LEC2/ directive.

12.14  OPTIONS FOR NODE-CENTERED FINITE VOLUMES

H.130


Object:


To provide options for node-centered Finite Volumes (multicomponent fluid flows).


Syntax:

     <  MC <ORDR ordr>
           <NUFL $[ ROE ; VANL ; STWA ]$ >
           <WBC>
           <SYNC sync>
     >
ORDR

Introduces the order ordr of the numerical integration scheme. May be 1 (first order) or 2 (second order). By default, it is taken ordr = 2.
NUFL

Introduces the type of flux calculation in the bulk fluid; may be ROE (Roe flux), VANL (Van Leer flux) or STWA (Steger-Warming flux). It is only accepted in purely Eulerian calculations. Recall that the far-field flux type is chosen (independently from the bulk flux type) by directive BDFO in material MCFF. By default, it is taken NUFL ROE (Roe flux).
WBC

If specified, the boundary conditions are treated according to a weak formulation. It is only accepted in purely Eulerian calculations. In this case external forces at the boundaries are evaluated by imposing zero momentum flux across the solid boundaries, while in the default case (no WBC specified) these forces are evaluated by the method of Lagrange multipliers.
SYNC

Introduces the type of synchronization sync for the MC variables: 0 (the default) is the old procedure; 1 is the new procedure.

Remarks

The “new” synchronization algorithm (SYNC 1), introduced in April 2010, should be used systematically for new calculations. The old algorithm is left only for compatibility with old input files.

12.15  OPTIONS FOR MULTIPHASE MULTICOMPONENT FLUIDS

H.140


Object:


To provide options for multiphase multicomponent fluid flows.


Syntax:
     <   "FLMP"  < "EPS1" eps1 > < "EPS2" eps2 > < "EPS3" eps3 >
                 < "EPS4" eps4 > < "NIMA" nima > < "DUMP" dump >  >

     < $[ "DPLG"   ;
          "VOFIRE" < "VSWP" > < "CORR" > < "RFCR" >
                              < "NOCR" > < "NORC" >
                   < "SKIP" /LECTURE/ >             ]$ >


eps1

Tolerance for the determination of number of effective components (a component is effectively present if its mass fraction is >= eps1mp). Default is 1.E-7.
eps2

Tolerance for the convergence of Newton-Raphson iterations. Default is 1.E-6.
eps3

Relative density variation to determine initial conditions in FLMPPR (case LIQ + GAS). Default is 1.E-5.
eps4

Tolerance to find the cut-off density for liquids in FLMPRP. Default is 1.E-12.
nima

Max. number of iterations in the above mentioned procedures
dump

Dump (1) or do not dump (0) informations on N-R iterations.
DPLG

Activates Despres-Lagoutiere anti-dissipative algorithm for multi-component flows on structured mesh (see comment below).
VOFIRE

Activates VOFIRE anti-dissipative algorithm for multi-component flows on unstructured mesh (see comment below).
VSWP

If present, exact advected volume is computed for each element face. If not, volume is approximated through the sweep formula.
CORR

Enables the use of CEA improved version of the VOFIRE algorithm.
RFCR

Enables the use of improved algorithm for mixture’s density.
NOCR

Disables the use of CEA improved version of the VOFIRE algorithm.
NORC

Disables the use of improved algorithm for mixture’s density.
SKIP

Deactivates VOFIRE for the given fluid elements.

Comments:


Despres-Lagoutiere anti-dissipative algorithm and its extension to unstructured meshes called VOFIRE are used to prevent numerical spreading of the mixing zone of physically non-miscible components. This is still a development in progress and is only available when multi-component material ADCR is used for the fluid in the model.


Improved algorithms for geometric reconstruction and computation of mixture’s density on elements faces are currently disabled by default.

12.16  OPTIONS FOR AUTOMATIC REZONING IN ALE COMPUTATIONS

H.150


Object:


To provide options for automatic rezoning algorithms in ALE computations.


Syntax:

    < REZO < SPLI |[ GIUL ; MODI ; BOTH ]| >
           < MVRE |[ NONE ; MODU <VFAC vfac>; MOPR <GAM0 gam0> ]| >
           < MEAN |[ POSI ; DEPL ]| >
           < DIRE RMAX rmaxrz >
           < NSTE rznste > < CSHE cshear > < CSTR cstret >
           < YOUN rezyo NU reznu RHO rezro >
           $[ VFLU ; LIAI ]$  >
SPLI

Use the splitting algorithm specified next in order to split up the mesh elements around each node and to form the node’s influence domain. The available possibilities are: GIUL for Giuliani’s original splitting rule, MODI for the modified rule, or BOTH to use a superposition of both methods. The default value is GIUL. This parameter applies only to Giuliani’s (AUTO) rezoning model and to the mean (MEAN) rezoning model. For the former, this parameter applies only to 2D quadrilateral ALE finite elements and finite volumes. For the latter, it applies to all elements (2D and 3D), but with a slightly different meaning: the GIUL option considers as neighbours of the node under consideration only the nodes that are connected to it by a face side; the other two options (MODI or BOTH) are equivalent and consider as neighbours all nodes belonging to neighbour elements.
MVRE

Use the mesh velocity restriction algorithm specified next in order to limit the ’raw’ optimal mesh rezoning velocity computed by a rezoning algorithm. As shown in the preceding Sections, since all implemented algorithms are explicit, they are unstable unless some limitation is introduced. The available possibilities are: NONE for no restriction (as said, this is likely to be unstable), MODU for the modulus-based rule, or MOPR to use the standard modulus plus projection rule that was adopted in the original Giuliani algorithm. The default value is MOPR. This parameter applies to all rezoning methods described above.
VFAC

The velocity factor to be used in conjunction with the MVRE MODU option. By default it is 2.0. This parameter applies to all rezoning methods described above.
GAM0

The velocity factor to be used in conjunction with the MVRE MOPR option. By default it is 0.2. The obsolete specification of this parameter in the GRIL directive should be avoided from now on. This parameter applies to all rezoning methods described above.
MEAN

Use the mean algorithm variant specified next. The available possibilities are: POSI for an algorithm based on (current) nodal positions, or DEPL for an algorithm based on (current) nodal displacements. The default value is POSI. This parameter applies to all ALE element types.
RMAX

The maximum aspect ratio to be used in conjunction with the DIRE rezoning algorithm. By default it is 5.0. Note, however, that this parameter applies only to 2D quadrilateral ALE finite elements and finite volumes.
NSTE

The number of steps in which rezoning is applied (repartition parameter). By default it is 1.0. This parameter applies to all rezoning methods described above.
CSHE

The shear weight coefficient. By default it is 1.0. Note, however, that this parameter applies only to: a) any elements rezoned by Giuliani’s method (AUTO); b) 2D triangles and quadrilaterals rezoned by the SPEC method; c) 2D quadrilaterals rezoned by the QUAD method; d) 2D quadrilaterals rezoned by the MECA method.
CSTR

The stretch weight coefficient. By default it is 1.0. Note, however, that this parameter applies only to: a) any elements rezoned by Giuliani’s method (AUTO); b) 2D triangles and quadrilaterals rezoned by the SPEC method; c) 2D quadrilaterals rezoned by the QUAD method; d) 2D quadrilaterals rezoned by the MECA method.
YOUN

The fictitious material Young’s modulus to be used in conjunction with the MECA rezoning algorithm. By default it is 1.0. Note, however, that this parameter applies only to 2D quadrilateral ALE finite elements and finite volumes.
NU

The fictitious material Poisson’s coefficient to be used in conjunction with the MECA rezoning algorithm,. By default it is 0.0. Note, however, that this parameter applies only to 2D quadrilateral ALE finite elements and finite volumes.
RHO

The fictitious material density to be used in conjunction with the MECA rezoning algorithm. By default it is 1.0. Note, however, that this parameter applies only to 2D quadrilateral ALE finite elements and finite volumes.
VFLU

Choose the ’old’ method of dealing with rezoning of nodes that are subjected to liaisons,. The imposed direction(s) are determined indirectly, from the fluid velocity components. As discussed, in 3D cases this method may be too restrictive and prevent the rezoning algorithm from fulfilling its tasks.
LIAI

Choose the ’new’ method of dealing with rezoning of nodes that are subjected to liaisons. The imposed direction(s) are determined directly from inspection of the liaison coefficients.

12.17  OPTIONS FOR CELL-CENTRED FINITE VOLUMES

H.155


Object:


To provide options for Cell-Centred Finite Volume (VFCC) computations.


Syntax:

    < VFCC <DUMP>
           <FCON fcon>  <VISC visc>
           <ORDR ordr>
         $ <OTPS otps> ; ERK2 $
           <RECO reco>
           <LMAS lmas>  <LQDM lqdm>  <LENE lene>  <LALP lalp>
           <LVEL lvel>  <LPRE lpre>  <LLAG llag>
           <KMAS kmas>  <KQDM kqdm>  <KENE kene>  <KBAR kbar>
           <RVIT rvit>
           <CENE>       <NTIL>
           <M0   m0>    <VINF vinf>
           <NCFS /LECT/>
           <FLSW flsw>
           <TGRA tgra>
           <PAS0 pas0>
    >
VFCC

Introduces the options for Cell-Centred Finite Volume computations.
DUMP

Dumps out on listing the data structures FACE_VFCC and SOLUTION_VFCC (only for debugging).
fcon

Solver for the calculation of numerical fluxes at interfaces between volumes. One of the following solvers can be chosen (by default the code uses the HLLC solver, number 6 in the following list):
  1. Rusanov
  2. Flux-centred with viscosity (see VISC below)
  3. HLLE
  4. Exact Riemann for perfect gas
  5. Zha-Bilgen (Flux Vector Splitting)
  6. HLLC This is the default.
  7. Dominant Wave-Capturing
  8. AUSM+ (Flux Vector Splitting)
  9. Zha-Bilgen modified
  10. LDFSS-2 (Flux Vector Splitting)
  11. AUSM+ Low-Mach
  12. AUSM+ -up- Low-Mach
  13. HLLC Low-Mach
visc

Defines the viscosity for use with the Flux-centered solver (FCON 2). By default there is no viscosity.
ordr

Order in space. Either first or second order is possible. The default is ORDR 2 which, however, corresponds to real second order in space only if a so-called reconstruction (see RECO below for an explanation) is chosen (RECO >0). Since by default RECO is 0 (see below), the default scheme (obtained by specifying neither ORDR nor RECO) is first-order in practice. An old (obsolescent) implementation of first order in space scheme is also available in the code, but is still accepted only for backward compatibility and should not be used in new calculations since it will be removed soon. This is activated by choosing ORDR 1 and no reconstruction (thus RECO is 0). However, be warned that the explicit choice of ORDR 1 is incompatible with use of the FLSW fluid-structure interaction model. See the comments at the end of this page for examples of use of the ORDR and RECO keywords.
otps

Order in time. Only first or second order (Van Leer-Hancock predictor-corrector scheme) is possible. The default is first order in time. In order to achieve second-order time integration in calculations with materials other than CDEM, use OTPS 2. For calculations with CDEM, use the special keyword ERK2, see below.
ERK2

This keyword (in alternative to OTPS), chooses a Runge-Kutta explicit second-order time integration scheme. This is the second-order time integration scheme to be preferably used for calculations with the CDEM material (instead of OTPS 2).
reco

Activates the so-called reconstruction of the variables at the inter-volume interfaces starting from the values at the centroids and from the (spatial) gradients at the centroids. Since the spatial gradients are only computed when second-order in space is activated (ORDR 2), reconstruction only makes sense in this case. The default value is 0 (no reconstruction). Option RECO 1 stays for Green-Gauss reconstruction of the conservative variables (density, momentum and total energy per unit volume). Option RECO 2 stays for Green-Gauss reconstruction of the primitive variables (density, velocity, internal energy per unit mass, mass fraction). Option RECO 3 is only available for the CDEM or DEMS materials and stays for Green-Gauss reconstruction of the primitive variables, which in this case involves the pressure instead of the internal energy per unit mass.
lmas, lqdm, lene, lalp, lvel, lpre, llag

Limitation for the reconstruction (RECO >0) of the various quantities: lmas for the density, lqdm for the momentum, lene for the total energy per unit volume, lalp for the volume fraction (only for CDEM or DEMS material), lvel for the velocity, lpre for the pressure, llag for the Lagrangian variables, i.e. the mass fractions prior to chemical reaction (only for CDEM material). A limiter typically is a number between 0.0 and 1.0, which multiplies the value of the gradient in order to ensure that the reconstructed values at the interfaces do not violate some conditions. The value of the limiter is automatically computed by the code in each Finite Volume (and typically varies from volume to volume, and also in time). The available types of limiter are: 0 indicates no limitation (limiter equal to 1.0), 1 indicates a first-order limitation (this corresponds to limiter equal to 0.0 and in practice vanifies the effects of the reconstruction), 2 indicates the limitation of Barth and Jesperson, and 3 indicates the limitation of Dubois. By default the code assumes the limitation of Dubois.
kmas, kqdm, kene

Parameter for the limitation of Dubois for the density (LMAS 3), for the momentum (LQDM 3) or for the total energy per unit volume (LENE 3). This parameter should be between 0.0 and 1.0. The default value is 0.5.
kbar

Parameter for the limitation of Barth and Jesperson, all variables (e.g. LMAS 2). The value 0 indicates the standard one (this is the default), while 1 indicates a modified one which is more robust for the calculation of shock waves. The value kbar 1 produces the strongest possible limitation.
rvit

Type of reconstruction of the fluid velocity field at VFCC nodes, starting from the velocity field at the VFCC volume centres. This is used to compute the automatic rezoning (mesh velocity) of ALE VFCC fluid nodes and the motion of Lagrangian VFCC fluid nodes. A value of 0 indicates no reconstruction, 1 (default) indicates the arithmetic mean of the neighboring volumes, 2 is the mean weighted by the element volumes, 3 is the mean weighted by the element masses, 4 is the mean weighted by the inverse of the element volumes, 5 is the mean weighted according to Roe.
CENE

This option adds a correction of the gradients such that the internal energy is always positive. This affects only second-order in space calculations with RECO 1 or 2, but not 3.
m0

Cut-off value for the Mach number for use with low-Mach solvers (i.e. FCON 11, 12 or 13). For the other solvers, it is ignored. By default it is 0.5.
vinf

Reference velocity for use with low-Mach solvers (i.e. FCON 11, 12 or 13). For the other solvers, it is ignored. By default it is 0.0.
NTIL

No “tilt” in the calculation (i.e. suppress error message and subsequent stop if the internal energy becomes negative). The default is to stop (tilt) if the internal energy becomes negative. This option has no effect on calculations with the CDEM or DEMS materials.
NCFS

Announces that a (nodally) non-conforming fluid-structure interaction exists between a structure (typically meshed by shell elements) and a fluid meshed by VFCC. The following /LECT/ lists all fluid nodes (which must belong to the VFCC domain) which are located along the non-conforming F-S interface. The code automatically searches the facing structural element, which must be “superposed” (within a small tolerance) to the fluid volume face (such an element must exist, else an error message is issued).
flsw

This option allows to choose the type of FLSW algorithm to be used for fluid-structure interaction modeling in conjunction with cell-centred finite volumes. The value 0 means that all numerical fluxes across interfaces near the structure are set to zero, except those related to momentum (which are the pressure forces). The value 1 is the default and means that all numerical fluxes across interfaces near the structure are computed by introducing fictitious “ghost” states corresponding to a rigid wall moving with the same speed as the structure.
tgra

By specifying TGRA i with i>0 one activates the non-regression test for the gradient limiter for the perfect gas in the CDEM model: the gradient of the i-th variable is stored in the ECR table. By default (i=0) no gradient is stored.
pas0

The initial time step is imposed to be pas0. The default is 0.0, which means that the code computes it automatically.

Comments:


Below are some examples of use of the ORDR and RECO keywords. The effect of RECO >1 is similar to RECO 1, only the type of reconstruction is different.

ORDRRECOResult
nonenoneFirst-order in space (default)
none0First-order in space (default)
none1Second-order in space
2noneFirst-order in space (default)
20First-order in space (default)
21Second-order in space
1noneOlder version of first-order in space: FLSW not available!
10Older version of first-order in space: FLSW not available!
11Input error: this combination is not available!

12.18  OPTIONS FOR CONNECTIONS ("LIAISONS"/LINKS)

H.160


Object:


To provide options for the connections in general, for the LIAISON CONTACT directive and for the pinball impact model (either standard or generalized), see Section D.


Syntax:

    < LIAJ >
    < CONT |[ CONS ; VARI ]| >
    < GLIS < NORM |[ ELEM ; NOEU ]|>
           < GAP  |[ ELEM ; NOEU ]|> >
    < PINS < DUMP > < STAT > < VIDE > < DTPB < CSPB cspb > > < UPDR >
           < EQVL > < EQVD > < EQVF > < NEQV >
           < $[ FACE ; FACI ]$ < FNOR >                             >
           < CNOR < $[ MIDP ; NCOL < RCEL < $[ MASL ; MAS2 ]$ > > ]$ > >
           < SNOR > < ASN > < NPSF >
           < $[ REB1 ; REB2 ; NORB ]$ >
           < $[ NOGR ; GRID <DGRI> <SORT>
                      $[ HGRI hgri ; NMAX nmax ; DPIN dpin ]$
                      < PACK ipac > ]$ > >
    < GPNS < DUMP > < STAT > < DTPB < CSPB cspb > >
           < $[ PROT ; REEN ]$ >
           < $[ REB1 ; REB2 ; NORB ]$ >
           < $[ NOGR ; GRID <DGRI> <SORT>
                      $[ HGRI hgri ; NMAX nmax ; DPIN dpin ]$
                      < PACK ipac > ]$ > >
    < LNKS < STAT > < STAD > < DIAG > < DUMP > < VISU >
           < RIGI <DISP> <CMID> >               >
    < FLS <CUB8 c8> >
LIAJ

This option causes all constraints on velocities to be imposed on the velocity at time n+1, rather than at time n+3/2, which is the default (note that in this notation the current configuration is indicated by n+1). The first form was used for example in PLEXIS-3C. Therefore, this option is mainly useful in order to perform fine grain comparisons between results of PLEXIS-3C and EUROPLEXUS, for debugging purposes.
CONT

Introduces options related to geometric bilateral restraints (LIAISON CONTACT, see Page D.40 and following ones).
CONS

Constant coefficients will be used in the LIAI CONT directives of type SPHE, CYLI, CONE and TORE.
VARI

Variable coefficients will be used in the LIAI CONT directives of type SPHE, CYLI, CONE and TORE. Remember to dimension adequately by the DIME VCON directive.
GLIS

Introduces options to the LIAI or LINK GLIS (sliding surfaces) model.
NORM

Options to control the face normal computation.
ELEM

Exact face normals are computed.
NOEU

Nodal normals are first computed as weighted mean values from the faces surrounding each node. Face normals are then deduced by averaging the nodal normals at the centre of each face. This is the default method (see comment below).
GAP

Options to control the way of considering the gap for contact between shell structures.
ELEM

Gap is considered on the master side, which means that the master facet is translated by the gap value in its normal direction before contact detection.
NOEU

Gap is considered on the slave side, which means that the slave node is translated by the opposite of the gap value in the direction normal to the master facet before contact detection. This is the default method (see comment below).
PINS

Introduces options related to the LIAI or LINK PINB (pinball contact) model (see page D.480).
DUMP

Dumps out extensive pinballs information on the listing. Note that even further pinball-related dumps take place by activating the generic option OPTI DUMP in conjunction with the present pinball-specific option. Note also that this option should be activated before declaring the pinballs, i.e. before the LINK PINB directive, in order to get on the listing a detailed information on pinballs.
STAT

Dumps out statistics relative to pinballs on a special file <basename>.pin. At each time step are printed: the number of “raw” detected pinball contacts, the number of contacts remaining after the CNOR algorithm, the number after the NCOL algorithm, the number after the RCEL algorithm and the (final) number of contacts after the a priori rebound algorithm.
VIDE

Visualize all descendent pinballs generated by the hierarchic splitting process. This option should only be used for debugging purposes. When activated, all the descendent pinballs (of the highest level) generated during the splitting process are considered in contact, so that they may be visualized interactively e.g. by the TRAC PINC command (see pages A.25 and O.10). This allows to visualize the result of the splitting process. Beware that in complex cases a very large number of such pinballs may be generated. When the option is activated, pinball links are not generated, however, since the retained contacts are unphysical. In addition, the calculation is automatically stopped after time step 0, and the PINS DUMP (see above) option is automatically activated.
DTPB

Activate automatic limitation of the time increment Δ t to account for contacts modelled by pinballs (irrespective of the specific model used, i.e. liaisons, coupled links, or uncoupled penalty). This option is ignored if the user pilots the time increment e.g. by specifying PAS UTIL. By default, i.e. without the present option, pinball contacts have no effect on time increments.
CSPB

Introduces the reading of the “stability” coefficient cspb to be used in conjunction with the DTPB option for the limitation of the time increment Δ t due to pinballs. By default the code assumes cspb=cstab i.e. the same value as the stability coefficient used for the elements’ stability (see OPTI CSTA on page H.20). This quantity should be less than 1.0, like for CSTA.
UPDR

Update the radius of parent (0-level) pinballs at every step. By default, the radius is computed only at the initial time. This option may be useful in problems with very large deformations.
EQVL

The radius of parent pinballs (i.e. at the 0-level) is computed in such a way that the pinball volume equals the initial volume of the associated element. By default, the radius is computed so as to encompass all element nodes in the initial configuration.
EQVD

Same as EQVL above, but concerning the descendent pinballs generated in hierarchic methods (and this at every level of the hierarchy). The sub-pinball radius is computed in such a way that its volume equals the initial volume of the associated element portion. By default, the radius is computed so as to encompass all element portion “nodes” in the current configuration.
EQVF

Same as EQVD above, but affects only the proper descendent (i.e. of level L>0) pinballs generated in hierarchic methods at the last (final) level of the hierarchy. The parent (0-level) pinballs are not affected. The radius of a final proper sub-pinball is computed in such a way that its volume equals the initial volume of the associated element portion. By default, the radius is computed so as to encompass all element portion “nodes” in the current configuration. This option should be preferably used in most cases: the other options (EQVL, EQVD or NEQV) are in fact probably useful only in special cases, or for debugging purposes.
NEQV

No equivalent volume calculations. The radius of parent pinballs is computed so as to encompass all element nodes in the initial configuration. The radius of any proper descendent pinballs is computed so as to encompass all element portion “nodes” in the current configuration. This is currently the default. It may be used to restore the default behaviour after one of the other options (EQVL, EQVD or NEQV) has been specified.
FACE

The velocity constraint for a contact between parent pinballs is written at the centroids of the faces crossed by the line joining the pinball centers (it involves only the face nodes). By default, the velocity constraint is written at the pinball centers (which for 0-level pinballs corresponds with the element centroid) and thus involves all the nodes of the element. This option has no effect on contacts between sub-pinballs.
FACI

The velocity constraint for a contact between parent pinballs is written at the intersections of the faces crossed by the line joining the pinball centers (it involves only the face nodes). By default, the velocity constraint is written at the pinball centers (which for 0-level pinballs corresponds with the element centroid) and thus involves all the nodes of the element. This option has no effect on contacts between sub-pinballs.
FNOR

The velocity constraint for a contact between parent pinballs is written along a “mean” of the two face normals n = (nAnB). Note that this requires that either OPTI PINS FACE or OPTI PINS FACI be specified as well. By default, the velocity constraint is written along the direction of the line that joins the pinball centers.
CNOR

The velocity constraint for a contact between sub-pinballs is written along a “common” normal. One such normal is determined for each couple of contacting element faces. When multiple contacts between sub-pinballs occur (pinballs hierarchy at level > 0) in case of flat (face to face) contact, this common normal is an approximation of the normal to the contacting faces.
MIDP

The velocity constraint for a contact between sub-pinballs is written at “midpoints” along the lines that join the retained contacting sub-pinballs. This option is part of the common normal algorithm and therefore it requires that the CNOR option be specified as well (see above). This option is incompatible with the NCOL option described below. Note that this option has effect only on constraints between sub-pinballs that are part of a “sequence” of two or more contacts between the same couple of ancestors. Single or “isolated” contacts between two ancestors (to which the concept of common normal does not apply) sre not affected, and in such cases the constraint is written at the sub-pinball centers.
NCOL

Collapse onto the nearest node of the parent element the center of those descendent pinballs located at “corners”. In addition, for the remaining (non-corner) descendent pinballs, collapse their center onto the element side or face. Note that the above mentioned collapse is performed only as far as the application point of contact reaction forces is concerned, i.e. when writing down the constraints, and it does not affect the position (center, radius) of the descendent pinball itself. By this option the form of the resulting constraints is simpler because they involve less dofs, and the constraints are more independent from one another. This option has only effect on contacts between sub-pinballs (not for contact between parent pinballs) and is incompatible with the MIDP option described above. It requires the CNOR option.
RCEL

Eliminate repeated constraints for contacts between sub-pinballs that may result after collapse (see option NCOL above). This option may help removing a priori from the system repeated constraints that occur e.g. in flat contact between adjacent elements. It requires that the NCOL option (and thus also the CNOR option) be specified as well. Normally to obtain the maximum benefits a user would specify the three options CNOR NCOL RCEL.
MASL

Apply master/slave rule in order to further simplify constraints in case of multiple flat contact between bodies. Constraints of type NP (node-to-point) whose associated node belongs to the “hardest” one of the two contacting bodies are rejected. Body “hardness’ is specified optionally in the PINB BODY HARD directive, see Page D.480. This option requires that HARD has actually been specified for both contacting bodies, and that the RCEL option described above has been specified as well. The result should be similar to the more traditional sliding lines (slave node / master surface) algorithm, and might lead to slight under-constraining (spurious penetration) in some cases (if this happens, try using the MAS2 option below instead).
MAS2

Apply master/slave rule in order to further simplify constraints in case of multiple flat contact between bodies. Multiple constraints of type NP (node-to-point) whose associated node belongs to the “hardest” one of the two contacting bodies are rejected. Body “hardness’ is specified optionally in the PINB BODY HARD directive, see Page D.480. This option requires that HARD has actually been specified for both contacting bodies, and that the RCEL option described above has been specified as well. The result should be intermediate between a purely pinballs-based algorithm and the more traditional sliding lines (slave node / master surface) algorithm. It might lead to slight over-constraining (contact locking) in some cases (if this happens, try using the MASL option above instead).
SNOR

When a single contact occurs between sub-pinballs belonging to the same couple of element faces, and only one of the two sub-pinballs is a face sub-pinball, then the used normal is the normal to that face. This option may be used alone or combined with the CNOR option (which acts only upon multiple contacts).
ASN

The so-called “assembled surface normal” (ASN) algorithm of Belytschko and Law (1985) is used to compute a unique (normalized) normal to each external node of the mesh portion subjected to contact, and a unique (normalized) normal to each pinball (parent or descendent). The penetration direction between contacting pinballs is then computed using the ASNs of the two pinballs according to a set of rules. This ameliorates the treatment of flat contact, especially in conjunction with a penalty formulation to compute the contact forces. This option cannot be used together with (is an alternative to) options FNOR, CNOR (and its sub-options), or SNOR.
NPSF

Add a scaling force factor for pseudo-nodal pinballs at an adaptivity level L>1. If this option is specified, then the penalty force for newly created pseudo-nodal pinballs (i.e., pinballs associated with to a mass-less PMAT element attached at element nodes) are scaled down by multiplying the penalty force normally computed by a factor:
φ = 1 / (2L−1))     (23)
where L is the hierarchy level in adaptivity of the node to which the pseudo-nodal pinball is attached (via the PMAT element). If the keyword is not specified, then φ = 1.0 and the penalty force is not scaled. If specified, the option has effect only on pseudo-nodal pinballs using the PENA (penalty) method, it has no effect on element-based pinballs nor on pseudo-nodal pinballs using the Lagrange multipliers method.
REB1

The so-called a priori pinball contact rebound detection algorithm is used. This is the default contact rebound detection algorithm and therefore specifying this keyword is usually redundant. Rebound-related options are only used in the Lagrange Multipliers version of the pinball method. The penalty formulation does not use any special rebound treatment, so these options are ignored.
REB2

The so-called a posteriori pinball contact rebound detection algorithm is used instead of the default a priori contact rebound detection algorithm. This option is only intended for internal code testing and verification, because the default algorithm is normally superior to the other one. Rebound-related options are only used in the Lagrange Multipliers version of the pinball method. The penalty formulation does not use any special rebound treatment, so these options are ignored.
NORB

Do not apply any pinball contact rebound detection algorithm. Rebound between pinballs is not treated. Rebound-related options are only used in the Lagrange Multipliers version of the pinball method. The penalty formulation does not use any special rebound treatment, so these options are ignored. This option is therefore useful only (for debugging purposes) with pinball contacts treated by Lagrange multipliers (see LINK COUP PINB).
NOGR

Do not use a grid of cells to speed up search of neighbours for contact detection. This is the default.
GRID

Use a grid of cells (as in bucket sorting) to speed up search of neighbours for contact detection. The grid encompasses all elements containing parent pinballs and is built up either automatically (if no further options are specified) in the way specified below, or according to one of the following criteria.
DGRI

Dump out initial grid on the listing (only at step 0).
SORT

Sort the list of contacts in growing order so they (should) become like in the case without grid. This option is only to be used for debugging, since it facilitates the comparison of results with and without grid.
HGRI

Specifies the size of the grid cell. Each cell has the same size in all spatial directions and is aligned with the global axes.
NMAX

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

Specifies the size of the grid cell as a multiple of the diameter of the largest parent pinball. For example, by setting DPIN 4 the size of the cell is four times the diameter of the largest parent pinball. By default, i.e. if neither HGRI, nor NMAX, nor DPIN are specified, the code takes DPIN 1.1. Normally, the cost of searching decreases as one takes smaller values of DPIN. However, the memory used tends to increase because there will be more cells. In large cases, a trade-off must be found but it is difficult to say a priori what is the optimal value for DPIN. Note that values of DPIN at or below 1.0 are unsafe. Some contacts may be overlooked (but this depends on the case). To be sure that all contacts are detected, use DPIN (slightly) larger than 1.0, say 1.001.
PACK

This optional keyword allows to specify a packing size ipac for the fast search grid. The search is then done by partially overlapping cubic (square in 2D) “macro cells” each containing ipac search cells along each spatial direction. See below for comments.
GPNS

Introduces options related to the GPIN (generalized pinball contact) model (see page D.490).
DUMP

Dumps out extensive GPINs information on the listing. Note that even further GPIN-related dumps take place by activating the generic option OPTI DUMP in conjunction with the present GPIN-specific option.
STAT

Dumps out statistics relative to GPINs on a special file <basename>.gpn. At each time step are printed: the number of “raw” detected GPIN contacts and the (final) number of contacts after the a priori rebound algorithm.
DTPB

Activate automatic limitation of the time increment Δ t to account for contacts modelled by GPINs (irrespective of the specific model used, i.e. coupled links, or uncoupled penalty). This option is ignored if the user pilots the time increment e.g. by specifying PAS UTIL. By default, i.e. without the present option, GPIN contacts have no effect on time increments.
CSPB

Introduces the reading of the “stability” coefficient cspb to be used in conjunction with the DTPB option for the limitation of the time increment Δ t due to GPINs. By default the code assumes cspb=cstab i.e. the same value as the stability coefficient used for the elements’ stability (see OPTI CSTA on page H.20). This quantity should be less than 1.0, like for CSTA.
PROT

The GPINs attached to faces of continuum elements are “protruding” from the corresponding body by half the assigned contact diameter. A penetrating entity is consider to penetrate a GPIN if it enters into the “positive” (i.e. the protruding) half of the GPIN. Penetration into the negative half of the GPIN should not be possible, if the time increment is suitably limited.
REEN

This is the default. The GPINs attached to faces of continuum elements are “reentrant” into the corresponding body by half the assigned contact diameter. A penetrating entity is consider to penetrate a GPIN if it enters into the “negative” (i.e. the reentrant) half of the GPIN. Penetration into the positive half of the GPIN is possible geometrically, but is not considered as a real penetration.
REB1

The so-called a priori GPIN contact rebound detection algorithm is used. This is the default contact rebound detection algorithm and therefore specifying this keyword is usually redundant. Rebound-related options are only used in the Lagrange Multipliers version of the generalized pinball method. The penalty formulation does not use any special rebound treatment, so these options are ignored.
REB2

The so-called a posteriori GPIN contact rebound detection algorithm is used instead of the default a priori contact rebound detection algorithm. This option is only intended for internal code testing and verification, because the default algorithm is normally superior to the other one. Rebound-related options are only used in the Lagrange Multipliers version of the pinball method. The penalty formulation does not use any special rebound treatment, so these options are ignored.
NORB

Do not apply any GPIN contact rebound detection algorithm. Rebound between pinballs is not treated. Rebound-related options are only used in the Lagrange Multipliers version of the pinball method. The penalty formulation does not use any special rebound treatment, so these options are ignored. This option is therefore useful only (for debugging purposes) with pinball contacts treated by Lagrange multipliers (see LINK COUP GPIN).
NOGR

Do not use a grid of cells to speed up search of neighbours for contact detection. This is the default.
GRID

Use a grid of cells (as in bucket sorting) to speed up search of neighbours for contact detection. The grid encompasses all elements containing GPINs and is built up either automatically (if no further options are specified) in the way specified below, or according to one of the following criteria.
DGRI

Dump out initial grid on the listing (only at step 0).
SORT

Sort the list of contacts in growing order so they (should) become like in the case without grid. This option is only to be used for debugging, since it facilitates the comparison of results with and without grid.
HGRI

Specifies the size of the grid cell. Each cell has the same size in all spatial directions and is aligned with the global axes.
NMAX

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

Specifies the size of the grid cell as a multiple of the diameter of the largest GPIN. For example, by setting DPIN 4 the size of the cell is four times the diameter of the largest GPIN. By default, i.e. if neither HGRI, nor NMAX, nor DPIN are specified, the code takes DPIN 1.1. Normally, the cost of searching decreases as one takes smaller values of DPIN. However, the memory used tends to increase because there will be more cells. In large cases, a trade-off must be found but it is difficult to say a priori what is the optimal value for DPIN. Note that values of DPIN at or below 1.0 are unsafe. Some contacts may be overlooked (but this depends on the case). To be sure that all contacts are detected, use DPIN (slightly) larger than 1.0, say 1.001.
PACK

This optional keyword allows to specify a packing size ipac for the fast search grid. The search is then done by partially overlapping cubic (square in 2D) “macro cells” each containing ipac search cells along each spatial direction. See below for comments.
LNKS

This keyword introduces options which are specific of the links model. They are ignored by the “liaisons” model.
STAT

Dumps out statistics relative to coupled links (LINK COUP) on a special file <basename>.lks. At each time step are printed: the number of link groups (N_GPS), the total number of links (N_LKS), the total number of permanent links (N_PLKS), the total number of non-permanent links (N_NPLKS) and finally the number of links of each type (e.g., BLOQ, RELA etc.).
STAD

Print similar information to the statistics for coupled links, but relative to the decoupled links (LINK DECO), on file <basename>.lkd. Attention: the programming of this feature is under development. At the moment, statistics is available only for the following types of decoupled links: PINB.
DIAG

Dumps out additional diagnostics relative to current links (both permanent and non-permanent) on the listing, together with each normal printout (see directive ECRI. The information concerns the size of the links matrix, and its “fullness” (i.e. the relative number of non-zero entries). This information can be useful in view of the choice of the most appropriate solution strategy for the links problem.
DUMP

Dumps out all current links (both permanent and non-permanent) on the listing, together with each normal printout (see directive ECRI. The generated output can be huge, therefore this option should be used with great care (and for debugging purposes only).
VISU

Activate the possibility of visualizing the links in the built-in OpenGL graphical module.
RIGI

Introduce options related to the treatment of links for rigid bodies (new JRC formulation).
DISP

Express the links for rigid bodies on the displacements rather than on the velocities.
CMID

Compute the links coefficients for rigid bodies at the new mid-step rather than at the current full step.
FLS

This keyword introduces options which are specific of the FLSR and FLSW fluid-structure interaction models.
CUB8 c8

Sets the error level for inverse mapping in 8-node cube elements. By default it is 0, meaning that any error is treated as a real error. By setting it to 1, a lack of convergence in the inverse mapping procedure is not considered an error, but simply that the point considered lies outside the 8-noded cube. By setting it to 2, both a lack of convergence and a zero determinant are considered not as errors, but as an indication that the point considered lies outside the 8-noded cube. These options should be set only in problematic cases (and until the inverse mapping for the CUB8 shape is reformulated in a more robust way). Note that this option has effects only on the FLSR and FLSW models, plus in the tracking of flying debris embedded in a fluid, but not on other model which use CUB8 inverse mapping. Note also that this option has the same effect also upon inverse mapping in 3-node triangles in 3D, but with the following meaning of the c8 parameter: 1 means that dmax<tol_vol is not considered as an error, while 2 means the above plus also abs(err)>tol_dis is not an error. Finally, this option has the same effect also upon inverse mapping in 4-node quadrilaterals in 3D (which may be warped), but with the following meaning of the c8 parameter: 1 means that performing too many iterations is not considered as an error, 2 means the above plus also that a 0 determinant is not an error, and 3 means all the above plus also the fact that the point does not lie on the quadrilateral surface is not considered an error. If you activate this optional switch, it is probably safer to use the value 2 (or 3, in the case of 3D quadrilaterals) anyway.

Comments:


Be sure to consult also the interactive commands for the visualization of pinballs and of contacts, see Pages A.25 and O.10.


As far as nodal or elementary methods are concerned to compute the facet normals for contact detection and links generation, both may present advantages and drawbacks in different situations. Nodal approach produces smoother variations of the normal along the master side and may be useful for problems such as rolling bodies. However, in the case of strongly folded structures (for example, self-contact crashed bodies), elementary approach ensures better detection of contact between folds and should be preferred.


Considering the gap on slave side is the original way that was implemented in EUROPLEXUS. It has shown recently to potentially produce instabilities for strongly folded structures. In this case, considering the gap on master side has proved to be much more robust. The former approach remains the default until the latter is fully tested and validated.


When a fast search by cells grid is specified for the macro pinballs (or for the GPINs) in contact (PINS|GPNS GRID ...) and a large 3D problem is being solved with relatively few (but largely scattered) contacts, then one may easily generate an enormous number of cells and the memory required becomes prohibitive. In such cases, it may be convenient to do the search not as a unique scan but by several scans over contiguous “packs” (i.e. rectangular patches) of cells. Each pack or “macro cell” contains a number ipac of cells along each spatial direction. In addition, an extra cell is added along each boundary since the packs must be partially superposed for the algorithm to work. Thus in 2D the size of a pack will be (ipac+2 * ipac+2) and in 3D (ipac+2 * ipac+2 * ipac+2) cells. The search by packs is slightly slower than global search because of the increased number of operations and of the more complex algorithm, but the used memory might be much smaller (the user may reduce it by using a lower ipac).

12.19  OPTIONS FOR GRAPHICAL RENDERING

H.170


Object:


To provide options for the graphical rendering (OpenGL).


Syntax:

    < REND < $[ FAST ; SAFE ]$ >
           < $[ NODU ; DUMP ]$ >
           < $[ NAVI ; NONA ]$ >
              <STAT>
              <FAC4 SPLI n TOLE eps>
              <SHAR <ANGL angl> <ABS>> >
REND

This keyword introduces the options related to rendering.
FAST

This option uses the fastest available algorithms for the in-software geometric calculations preliminary to geometric rendering operations (see TRAC REND). This is the default.
SAFE

This option uses straightforward (but inefficient) algorithms for the in-software geometric calculations preliminary to geometric rendering operations (see TRAC REND). It may be useful when one has doubts on the graphical results obtained with the fast version.
NODU

This option does not dump out data related to the in-software geometric calculations preliminary to geometric rendering operations (see TRAC REND). This is the default.
DUMP

This option dumps out on the listing data related to the in-software geometric calculations preliminary to geometric rendering operations (see TRAC REND). This may be useful for debugging purposes but it produces a big output file.
NAVI

This option declares that any changes in the following rendering operations will be due only to navigation (NAVI) around or inside a fixed (static) scene, so that use of SAVE/REUS becomes possible also in Lagrangian cases, see page O.0030. In this case the user is responsible for making sure that no geometrical data vary between a rendering and the next one(s): the mesh does not move, no elements are eroded, adaptivity does not modify the current mesh, etc. The option is useful in order to speed up preparation of an animation containing a navigation in a static scene containing Lagrangian nodes.
NONA

Disables the NAVI option set with a previous NAVI keyword so that the normal behaviour of the SAVE/REUS mechanism is restored, see page O.0030.
STAT

This option produces statistics on the allocations performed by the OpenGL graphics module on a special file <basename>.ogl. This is useful only for debugging purposes.
FAC4

This option introduces indications about how to render 4-node faces. By default each 4-node face is split into four triangles by generating an extra point at the face center. In this way the rendering of non-planar (warped) 4-node faces is best and does not depend upon face (or element) numbering. Also the representation of iso-values is best. However, a lot of memory is required. Memory can be saved, at the expense of a somewhat worse representation (and not completely numbering-independent), by splitting planar or almost planar 4-node faces into just 2 triangles, or by treating them as a single quadrilateral.
SPLI n

The number of figures into which an almost-planar 4-node face is split. By default it is 4. It may be set to 1 or 2.
TOLE eps

Tolerance є to decide whether a 4-node face is planar or not. The face is considered planar if the scalar product between the two unit normals to triangles 1-2-3 and 1-3-4 obtained from the face is greater than (1−є).
SHAR

Introduces options related to the visualization of sharp corners.
ANGL

Sets the minimum angle α0 (between two 3D faces with a common side) beyond which the side is considered to be a sharp corner. By default, this angle is 60 degrees. Let n1 and n2 be unit normals to the two faces. Then the scalar product n1 · n2 = cosα is equal to the cosine of α, the angle between the normals (which is also the angle between the faces). Thus the corner is sharp if cosα < cos60, i.e. when α < 60.
ABS

Consider the absolute value of the above scalar product instead of the signed value. This has the following effect: when two faces have a common side and opposite (or nearly opposite) normals, the side is not considered sharp (while by default it would be). This option may be useful in the presence of complex 3D shell structures, because it is not always easy (and sometimes even impossible) to orient them consistently. With this option many “spurious” sharp corners disappear. Thus with this option the rule becomes: the corner is sharp when |α| < 60.

12.20  OPTIONS FOR MESH-ADAPTIVE COMPUTATIONS

H.180


Object:


To provide options for mesh-adaptive computations.


Syntax:

    < ADAP < $[ NODU ; DUMP ]$ > <STAT> <CHEC> <RCON> <MAXL maxl> <NOPP>
           <RESE>
           < $[ PHAN CD cd <CV cv> ; DHAN < $[ DEPL ; VITE ]$ > ; WHAN ]$ >
           <PCLD $[ MODE imod ]$
                 $[ SMOO ]$>
           <TRIG |[ CONT icon ; ECRO iecr ; EPST ieps ;
                    DEPL idep ; VITE ivit ; ACCE iacc ; VCVI ivcv ]|
                    TVAL tval /LECT/>
    >
ADAP

This keyword introduces the options related to mesh-adaptive computations.
NODU

This option does not dump out data related to the mesh-adaptive computations. This is the default.
DUMP

This option dumps out on the listing data related to the mesh-adaptive computations. This may be useful for debugging purposes but it produces a big output file.
STAT

This option prints out on the listing some additional “statistical” data related to the mesh-adaptive computations. The increment in listing size is very small, but the calculation of these data requires some (small) computational effort, therefore they are not computed by default.
CHEC

This option performs some extra checks during mesh-adaptive computations. The CPU overhead is high, so the option should be used only for debugging. The checks are mainly of geometrical nature: consistency of neighbors and pseudo-neighbors, consistency of CCFV interfaces, etc. In case an inconsistency is detected, an extensive printout (dump) of the concerned data structure is made on the listing (which can become very big) and the code stops with an informative error message.
RCON

This option imposes a smooth refinement of the mesh, such that the difference in refinement level between two neighboring (or pseudo-neighboring) elements is at most 1.
MAXL

This option introduces an upper limit maxl to the level of refinemt of the adptive mesh.
NOPP

Do not propagate MAXCURV and ERRIND to descendents upon elements split (only for debugging). By default they are propagated.
RESE

Upon un-splitting of a Q41L or Q42L element with a solid material (VM23 with linear elastic characteristics), recompute SIG and ECR from parent element nodal positions instead of doing averaging on child elements.
PHAN

Use penalty (decoupled) constraints on hanging nodes rather than Lagrange multipliers (fully coupled).
CD cd

Penalty coefficient on displacements.
CV cv

Penalty coefficient on velocities. This is zero by default.
DHAN

Use decoupled Lagrange-multiplier constraints on hanging nodes rather than fully coupled Lagrange multipliers.
DEPL

The decoupled Lagrange-multiplier constraints on hanging nodes are expressed on displacements. This is the default.
VITE

The decoupled Lagrange-multiplier constraints on hanging nodes are expressed on velocities rather than on displacements.
WHAN

Use “weak” decoupled constraints on hanging nodes rather than fully coupled Lagrange multipliers.
imod

Mode for mesh refinement using PCLD indicators. 1: refinement is homogeneous within one base cell (faster mesh adaptation, more cells, this is default), 2: refinement is heterogeneous with one base cell (slower mesh adaptation, fewer cells)
SMOO

Activates a smoothing step after mesh adaptation through PCLD criteria to avoid jumps of refinement levels between neighbor cells (option close to ADAP RCON option above for PCLD).
TRIG

Introduces a “trigger” which activates any forms of “automatic” mesh adaptivity present in the calculation only when a certain variable reaches a given value at a given location. The trigger affects following types of adaptivity models: WAVE, INDI, PCLD, THRS and FLSR/FLSW. The trigger has no effect on initial mesh adaptivity (INIT ADAP) or manually piloted adaptivity (ADAP SPLI/USPL interactive commands).
CONT icon

Set the trigger on stress component icon.
ECRO iecr

Set the trigger on hardening component iecr.
EPST ieps

Set the trigger on total strain component ieps.
DEPL idep

Set the trigger on displacement component idep. If one specifies 0 for idep, then the displacement norm of the first IDIM components is used.
VITE ivit

Set the trigger on velocity component ivit. If one specifies 0 for ivit, then the velocity norm of the first IDIM components is used.
ACCE iacc

Set the trigger on acceleration component iacc. If one specifies 0 for iacc, then the acceleration norm of the first IDIM components is used.
VCVI ivcv

Set the trigger on cell-centered velocity component ivcv. If one specifies 0 for ivcv, then the cell-centered velocity norm of the first IDIM components is used.
TVAL tval

Set the value which activates the trigger. The trigger is activated when the value of the monitored quantity exceeds tval. Once activated, the trigger remains active for the rest of the computation.
/LECT/

Specify the (single) element or the (single) node at which the specified variable is monitored.

12.21  STRAIN RATE FILTERING OPTION

H.190


Object:


The strain rate filtering option allows to damp high frequency vibrations wich are not physical and therefore to obtain more physical strain rate values.


Syntax:
        "FVIT"       alpha


alpha

filter coefficient, must be of the order of the smallest element size.

Comments:



This option is still under development and testing and should therefore be used with great care. this option is available only for isotropic Von Mises material depending on strain rate (VMIS DYNA).


The default value when the present option is not activated is 1. (no filtering).

12.22  OPTIONS FOR PARALLEL COMPUTING

H.200


Object:


This section provides options for advanced parallel computing. This is still a work in progress and may be significantly modified in the future.


Syntax:
       < "DOMD" /CTIM/ >



Comments:


Using DOMD keyword toggles the update of the domain decomposition using the given frequency (MPI only). It allows to take into account strong changes in the topology of the models (large displacements, failure and fragmentation for instance), making a static domain decomposition less and less efficient as the simulation progresses.


12.23  OPTIONS FOR GRADIENT DAMAGE MODELS

H.210


Object:

This section describes various numerical parameters for the gradient damage models ENGR, see 7.6.20. In particular, several options could be provided here for the parallel linear algebra library PETSc used to solve the structural scale damage evolution equation as a bound-constrained minimization problem.


Syntax:
   < "ENGR"  < "MONI" >
             < "DEBG" >
             < "PROJ" >
             < "SAIJ" >
             < "PREC" >
             < "INIT" >
             < "EDOT" >
   >


MONI

Activate the PETSc monitor which allows the user to obtain setting and convergence information of the specified solver via an additional log file *_petsc.log. On the top of this file are summarized the global Hessian matrix information (number of rows, of non-zeros, etc.) and the solver setting (minimization method, tolerances, underlying linear solver, underlying preconditioner used, etc.). Then the log file prints at every time step following information: STEP, the current time step, ITER, number of CG iterations, FVAL, value of the objective functional (quadratic function), RNOM, norm of the residual vector, and REASON, the convergence information. At the end of this file some profiling information is given through PETSc’s log_summary command.
DEBG

This option provides various debugging information concerning for example nodes partitioning with PETSc convention.
PROJ

By default we prescribe the use of GPCG solver for such constrained minimization problems. It performs several gradient projections to identify the active (constrained by the bounds) nodes, and several subsequent conjugate gradient iterations to solve a reduced unconstrained minimization problem for all free (non-active) nodes. This method is extremely efficient.

However for comparison we also provide this option PROJ to use instead the conjugate gradient method for the unconstrained problem and then an a posteriori projection on the admissible space to satisfy irreversibility condition. Note however, that this method PROJ makes sense only when the damage constitutive law AT chosen by specifying LAW 2 is used.

SAIJ

When this option is used, only the upper triangular portion of the Hessian matrix is stored by the classical CSR format in PETSc. The memory use is reduced, however in terms of computational efficiency/cost nothing is gained through comparison with the full storage format.
PREC

This option sets the tolerance norm type of the underlying CG linear solver to be PRECONDITIONED, i.e. using the inner product defined by the preconditioner matrix. This options has virtually no influence on the computational efficiency through tests.
INIT

This option is concerned with the initial condition of damage to model for example an initial crack along some given nodes. When the option INIT is activated, all neighboring nodes of the previous ones are also prescribed by the damage value. In case of an initial crack, all the nodes of an element along this crack are thus totally damaged. (Tensile-type) wave propagation is hence prohibited across the crack.
EDOT

This option activates strain-rate effects in the damage criterion.

Previous Up Next