12 GROUP H—OPTIONS
H.10
Object:
These keywords give the additional options of the computation.
They can be grouped as:

options associated with timesteps;
 options associated with dampings;
 options for finite elements;
 output options;
 returning to default options;
 options for an advectiondiffusion computation;
 options for ALE computations in structures;
 options for debugging purposes;
 options to declare FANTOME certain elements;
 options to define classes of elements within a list of elements;
 options related to the treatment of shocks and impacts;
 options for FSA (fluidstructure interactions of the ALE type);
 options for nodecentered finite volumes;
 options for multiphase, multicomponent fluid flows;
 options for the automatic rezoning in ALE computations;
 options for cellcentred finite volumes;
 options for “LIAISONS”/LINKS (connections);
 options for graphical rendering;
 options for meshadaptive computations;
 options for strain rate filtering;
 options for parallel computing;
 computational options of the elastic gradient damage model.
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 subinstructions may appear in any order.
The different options are described on the following pages.
12.1 OPTIONS RELATED TO THE TIMESTEP
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 timestep 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 subcycle, 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 Δ t_{stab} for all elements
are printed out. The stability step is the critical
step Δ t_{crit} estimated by the code (roughly the element length
L divided by the speed of sound c in the element material)
multiplied by the safety coefficient φ (CSTA,
by default 0.8):
Δ t_{stab}=φΔ t_{crit}≈φL/c.
 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 subkeywords)
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 postprocessing
(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 subdirectives 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.D12 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.E6 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 PLEXIS3C", 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 intranodal distance
as the characteristic length and the sound speed plus
the maximum nodal (w−v) 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 intranodal
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: L_{corr}=L^{2}/√3h and then
Δ t=L_{corr}/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 t_{2} / Δ t_{1} 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 redefine 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
(CourantFriedrichsLévy 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:

The mass by zones before and after modification;
 The list of the 20 most constraining elements, with the old and
the new time step;
 A message
ATTENTION
also appears if the mass of a zone
increases more than 10 %.
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 ;
$[ "HOURG" <"ASSE"> ; "VISC" hvis ; "RIGI" hrig ; "NOHOURG" ]$ ]

QUASI STATIQUE


Quasi static computation. A linear damping with a given cutoff frequency
is applied.
 fsys


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


Reduced damping coefficient β.
 t1


Initial time t_{1} at wich the quasistatic option starts to operate.
By default, this coincides with the initial time of the calculation.
See comments below for the use of t_{1} and t_{2} to define
a closed interval or two open intervals.
 t2


Final time t_{2} until wich the quasistatic option operates.
By default, this coincides with the final time of the calculation.
See comments below for the use of t_{1} and t_{2} 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
cellcentred 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 β_{l} 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
cellcentred 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 a_{2} for the quadratic damping (shock waves).
 HOUR ASSE


Antihourglass damping for assumedstrain elements (IHOURG=3).
 VISC


Antihourglass damping on viscous terms (IHOURG=1).
 hvis


Reduced damping for antihourglass
h_{vis} (h_{vis}=0.5 is suggested).
 RIGI


Antihourglass damping based on artificial stiffness (IHOURG=2).
 hrig


Reduced damping for antihourglass.
 NOHOURG


Allows to eliminate the antihourglass 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 F_{i}^{QS} proportional to the mass M_{i} and
to the particle velocity v_{i} for each degree of freedom i:
F_{i}^{QS} = − 4 π β f M_{i} v_{i} = −2βω M_{i} v_{i}

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 highfrequency oscillations
related to the finite element discretization. In order to
obtain the critical damping of a freefree oscillation for each
element, take β_{l} = 1.
When t_{1} is less than t_{2} (be these values specified
or not) the quasistatic damping acts in the closed time interval
t_{1} ≤ t ≤ t_{2}, i.e. in the central part of the transient calculation.
However, it is also possible to specify t_{1} greater than t_{2}:
in this case the critical damping acts in the open time
interval t ≤ t_{2} (i.e. at the beginning of the calculation)
and in the open time interval t_{1} ≤ t (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 a_{2} = 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 antihourglass damping is currently available only
for the elements CAR1 et CUBE. By default, an antihourglass
damping with h_{vis} = 0.5 is affected to a calculation.
If the user wants to do a calculation without
antihourglass 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
β_{l} = 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
β_{l} = 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" >
< "NTSM" >

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. nonplanar faces).
The standard rule uses a singlepoint scheme which is
underintegrating 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 nonphysical. 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 (singlepoint) is left as a default for compatibility
with old input files and applications.
 NF34


Use new (2007) implementation for FL34 JRC’s tetrahedral 4node 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 4node
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 singlepoint 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 singlepoint
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., nonplanar
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.E4
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 antihourglass 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 farfield
conditions) or an IMPE ABSI material (for absorbing boundary conditions).
 FARF farf


Use FARF 1 to activate momentum transport forces in CLxx
due to farfield conditions, or FARF 0 to deactivate 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 deactivate 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 nonlinear 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.
 NTSM


The NTSM option deactivates the smoothing of the pressures of tetrahedrals.
Tetrahedral elements show a pressure locking in particular for nonlinear materials.
A very strong locking can be identified in impact calculations. A smoothing of the
pressures over the neighbour elements solves that problem. This option is activated
by default. The keyword NTSM deactivates that option.
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 nonLagrangian 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 debrisrelated options.
 NTRA ntra


Number of points ntra for flying debris trajectories.
The points are equispaced 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" ; "SAUV" ] >
< "DYMS" nobj*("OBJE" /LECT/) >
< "PRGR" >

NOPR/PRIN


This option allows to suppress or reactivate 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 reactivate input data
echo in the EUROPLEXUS window.
 LOG


Causes a oneline 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 CPUintensive 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.
 Description  S  P 
STEP  Time step number (main step for Partitioning)  X  X 
TIME  Time  X  X 
CPU(S)  CPU time used  X  X 
DTCRIT  Critical time step used  X  
ELCR  Element with the smallest time step  X  
DELMIN  Time step of the smallest substep   X 
MINS  Minimum level factor   X 
DE/E  Energy balance per element  X  X 
DM/M(NOD)  Mass balance per node  X  X 
DM/M(ELE)  Mass balance per element  X  X 
DTMX  Maximum time step  X  
EL  Element of the maximum time step  X  
DELMAX  Time step of the main step   X 
MAXS  Maximum level factor   X 
VITMAX  Maximum velocity  X  X 
NODE  Node of the maximum velocity  X  X 
ISUBTO  Total number of substeps   X 
MAXSTO  Total number of substeps   X 
ELSTEP  Number of callings of element routines  X  X 
 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 (CEAplates: 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 preprocessor 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).
 SAUV


With this option, the code will produce a file containing
the mesh in Cast3m’s GIBI format, similar to what would be
obtained by producing the mesh by Cast3m and saving it
with Cast3m’s SAUV command.
The file produced has the fixed name PXTOK200.SAUV.
The named element groups will be available
but no relationships (dependencies) between the
subobjects will be created.
To read back the file in Cast3m, use the commands:
OPTI REST FORM ’PXTOK200.SAUV’; REST FORM;.
 DYMS


With this option, the code will produce an input file for LSDYNA.
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 rereading 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 postprocessing
of the calculation by CASTEM2000 (or to manipulate the
mesh in CASTEM2000 before running the actual EPX calculation).
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 nonCASTEM 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 postprocessing 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.
The global mesh will be accessible as on bject named MESH.
In addition, but only if the K2MS MANU option is used,
then also all named element groups and all named node groups present
in the original EPX input file will be available in the
automatically generated CASTEM2000 mesh.
However, no other subobjects (in the sense of CASTEM2000
mesh generation building blocks) will be available.
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 4node 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 subobjects (in addition to the EPX named groups),
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;
In addition to file pxtok200.dgibi, another CASTEM2000 input
file pxrest.dgibi is also automatically produced in this case.
By running CASTEM2000 on pxtok200.dgibi first,
the CASTEM2000 mesh is produced and saved
in SAUV format. Then, by running CASTEM2000 on pxrest.dgibi,
the CASTEM2000 mesh is read back (just for checking) from the SAUV file.
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. No named element and node groups are translated into
CASTEM2000 objects in this case.
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 ADVECTIONDIFFUSION COMPUTATION
H.70
Object:
To provide options for an advectiondiffusion 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 TaylorGalerkin method is used of order
2, 3 or 4, respectively (default=2). When nsord=5, a
Leastsquare, spacetime method is used. When nsord=6,
a Leastsquare, CrankNicolson 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
Leastsquare method (see nsord above).
 nimax


Maximum number of iterations for implicit resolution.
Is only used with Leastsquare 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 timemarching 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 L^{A}T_{E}X 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 L^{A}T_{E}X input format. This may then e.g. be edited for inclusion
in the present User’s Manual.
 "DPSD"


In multidomain calculations, dumps out extra information on the
listing file. Furthermore,
for each subdomain a separate log file is produced that
reports, at every time station, a line collecting information
relevant to the subdomain. The name of such files is
<base_name>_xxx.log, where xxx is the index of the
subdomain (e.g. 012 for the twelfth subdomain), 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 subdomain. At most 10 such
log files are produced, therefore if the number of
subdomains is larger only the first 10 subdomains 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 perdomain
log files are automatically opened under the Windows platform.
On nonwindows 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 nonWindows 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 subdomains. Note that the unit numbers
to be used are 51, 52, etc. up to 60 (max. 10 subdomains). The
names associated with the files are arbitrary, and the files are
formatted. On some platforms, fullpath 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 posttreatment 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 fluidstructure 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 fluidstructure interaction conditions.
This is the default.
 FSCR


After computing geometrically the normals
for the FSA and FSR fluidstructure 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 (nonplanar), 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 NODECENTERED FINITE VOLUMES
H.130
Object:
To provide options for nodecentered 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 (StegerWarming flux). It is only
accepted in purely Eulerian calculations. Recall that the farfield
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.E7.
 eps2


Tolerance for the convergence of NewtonRaphson iterations.
Default is 1.E6.
 eps3


Relative density variation to determine initial conditions in FLMPPR (case
LIQ + GAS). Default is 1.E5.
 eps4


Tolerance to find the cutoff density for liquids in FLMPRP.
Default is 1.E12.
 nima


Max. number of iterations in the above mentioned procedures
 dump


Dump (1) or do not dump (0) informations on NR iterations.
 DPLG


Activates DespresLagoutiere antidissipative algorithm for multicomponent
flows on structured mesh (see comment below).
 VOFIRE


Activates VOFIRE antidissipative algorithm for multicomponent
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:
DespresLagoutiere antidissipative algorithm and its extension to unstructured
meshes called VOFIRE are used to prevent numerical spreading of the mixing zone
of physically nonmiscible components.
This is still a development in progress and is only available when multicomponent
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 modulusbased 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 CELLCENTRED FINITE VOLUMES
H.155
Object:
To provide options for CellCentred 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 CellCentred 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):

Rusanov
 Fluxcentred with viscosity (see VISC below)
 HLLE
 Exact Riemann for perfect gas
 ZhaBilgen (Flux Vector Splitting)
 HLLC This is the default.
 Dominant WaveCapturing
 AUSM+ (Flux Vector Splitting)
 ZhaBilgen modified
 LDFSS2 (Flux Vector Splitting)
 AUSM+ LowMach
 AUSM+ up LowMach
 HLLC LowMach
 visc


Defines the viscosity for use with the Fluxcentered 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 socalled 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 firstorder 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 fluidstructure 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 LeerHancock predictorcorrector scheme) is possible.
The default is first order in time.
In order to achieve secondorder 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
RungeKutta explicit secondorder time integration scheme.
This is the secondorder time integration scheme to be preferably
used for calculations with the CDEM material (instead of
OTPS 2).
 reco


Activates the socalled reconstruction of the variables
at the intervolume interfaces starting from the values at the
centroids and from the (spatial) gradients at the centroids.
Since the spatial gradients are only computed when secondorder 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 GreenGauss reconstruction of the
conservative variables (density, momentum and total energy per unit volume).
Option RECO 2 stays for GreenGauss 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 GreenGauss 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 firstorder 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
secondorder in space calculations with RECO 1 or 2, but not 3.
 m0


Cutoff value for the Mach number for use with lowMach 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 lowMach 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) nonconforming fluidstructure
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 nonconforming FS 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
fluidstructure interaction modeling in conjunction with cellcentred
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 nonregression test
for the gradient limiter for the perfect gas in the CDEM model:
the gradient of the ith 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.
ORDR  RECO  Result 
none  none  Firstorder in space (default) 
none  0  Firstorder in space (default) 
none  1  Secondorder in space 
2  none  Firstorder in space (default) 
2  0  Firstorder in space (default) 
2  1  Secondorder in space 
1  none  Older version of firstorder in space: FLSW not available! 
1  0  Older version of firstorder in space: FLSW not available! 
1  1  Input 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 > < ERCE >
< $[ FACE ; FACI ]$ < 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 PLEXIS3C.
Therefore, this option is mainly useful in order to perform fine
grain comparisons between results of PLEXIS3C 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 pinballrelated dumps take place by
activating the generic option OPTI DUMP in conjunction
with the present pinballspecific 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 (0level) 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 0level) 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 subpinball 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 (0level) pinballs are not affected.
The radius of a final proper subpinball 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 0level pinballs corresponds with the element centroid)
and thus involves all the nodes of the element.
This option has no effect on contacts between subpinballs.
 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 0level pinballs corresponds with the element centroid)
and thus involves all the nodes of the element.
This option has no effect on contacts between subpinballs.
 FNOR


The velocity constraint for a contact between parent pinballs
is written along a “mean” of the
two face normals n = (n_{A} − n_{B}). 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 subpinballs
is written along a “common”
normal. One such normal is determined for each couple of
contacting element faces. When multiple contacts between
subpinballs 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 subpinballs
is written at “midpoints”
along the lines that join the retained contacting subpinballs.
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 subpinballs
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 subpinball 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 (noncorner) 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 subpinballs (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 subpinballs
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
(nodetopoint) 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 underconstraining (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
(nodetopoint) 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 pinballsbased algorithm and the
more traditional sliding lines (slave node / master surface) algorithm.
It might lead to slight overconstraining (contact locking)
in some cases (if this happens, try using the MASL option above instead).
 SNOR


When a single contact occurs between subpinballs belonging
to the same couple of element faces, and only one of the
two subpinballs is a face subpinball, 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 socalled “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 suboptions), or SNOR.
 NPSF


Add a scaling force factor for pseudonodal pinballs
at an adaptivity level L>1.
If this option is specified, then the penalty force
for newly created pseudonodal pinballs (i.e., pinballs associated with
to a massless PMAT element attached at element nodes) are scaled
down by multiplying the penalty force normally computed
by a factor:
where L is the hierarchy level in adaptivity of the node
to which the pseudonodal 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 pseudonodal pinballs
using the PENA (penalty) method, it has no effect
on elementbased pinballs
nor on pseudonodal pinballs using the Lagrange multipliers method.
 REB1


The socalled 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.
Reboundrelated 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 socalled 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.
Reboundrelated 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.
Reboundrelated 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 tradeoff 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 GPINrelated dumps take place by
activating the generic option OPTI DUMP in conjunction
with the present GPINspecific 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 socalled 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.
Reboundrelated 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 socalled 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.
Reboundrelated 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.
Reboundrelated 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 tradeoff 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 nonpermanent 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 nonpermanent) 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 nonzero 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 nonpermanent) 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 builtin
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 midstep
rather than at the current full step.
 FLS


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


Sets the error level for inverse mapping in 8node 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 8noded 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 8noded 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, in the tracking of flying debris
embedded in a fluid, and in contact by pinballs,
but not on other model which use CUB8 inverse mapping.
Note also that this option has the same effect also upon inverse
mapping in 3node triangles in 3D, but with the following meaning
of the c8 parameter: 1 means that d_{max}<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 4node 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.
 ERCE


Instead of an error message for not possible inverse mapping to get the centroid shape,
the concerned element is eroded. This might be helpful to continue calculations with
highly distorted elements and pinballs.
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,
selfcontact 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 (PINSGPNS 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 insoftware
geometric calculations preliminary to geometric rendering operations
(see TRAC REND).
This is the default.
 SAFE


This option uses straightforward (but inefficient)
algorithms for the insoftware
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 insoftware
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 insoftware
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 4node
faces. By default
each 4node face is split into four triangles
by generating an extra point at the face center. In this way
the rendering of nonplanar (warped) 4node faces is best and does not depend
upon face (or element) numbering. Also the representation of
isovalues is best. However, a lot of memory is required.
Memory can be saved, at the expense of a somewhat worse
representation (and not completely numberingindependent),
by treating them as a single quadrilateral.
 SPLI n


The number of figures into which an almostplanar 4node face
is split. By default
it is 4. It may be optionally set to 1. The value 2
was initially also foreseen, but it
has still to be programmed and is not currently available.
 TOLE eps


Tolerance є to decide whether a 4node face is planar or not.
The face is considered planar if the scalar product between the
two unit normals to triangles 123 and 134 obtained from the
face is greater than (1−є).
 SHAR


Introduces options related to the visualization of sharp corners.
 ANGL


Sets the minimum angle α_{0} (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 n_{1} and n_{2} be unit normals to the two
faces. Then the scalar product n_{1} · n_{2} = 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 MESHADAPTIVE COMPUTATIONS
H.180
Object:
To provide options for meshadaptive 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 meshadaptive computations.
 NODU


This option does not dump out data related to the meshadaptive
computations.
This is the default.
 DUMP


This option dumps out on the listing data related to the meshadaptive
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 meshadaptive 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
meshadaptive 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 pseudoneighbors, 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 pseudoneighboring) 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 unsplitting 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 Lagrangemultiplier constraints on hanging nodes rather than
fully coupled Lagrange multipliers.
 DEPL


The decoupled Lagrangemultiplier constraints on hanging nodes are expressed
on displacements. This is the default.
 VITE


The decoupled Lagrangemultiplier 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 cellcentered velocity component ivcv.
If one specifies 0 for ivcv, then the cellcentered 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 7.7.20. 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 boundconstrained
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 nonzeros, 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 (nonactive) 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. (Tensiletype) wave propagation is hence prohibited across the crack.
 EDOT


This option activates strainrate effects in the damage criterion.