The ECRITURE directive enables the user to specify the requested printouts and data storages during a computation (including data saving for successive restart).
The REGION directive enables to define certain “regions” of the mesh, on which the printout of results will then be performed.
The MEASURE directive enables to request the printout of various “measurements” on the current geometrical mesh.
< ECRITURE . . . /CTIM/ < NOPO ; POIN /LECTURE/ > < NOEL ; ELEM /LECTURE/ > < FICH . . . > > < REGION ( 'nom region' . . . ) > < MEASURE ... >
The keyword ECRI must only appear once in an input sequence. It allows to specify the values to be printed on the listing file, and the nodes and elements for which these values must be printed.
Furthermore, the directive allows to define which results files should be produced, in view of a subsequent post-processing.
If the keyword ECRI is absent, a printout is performed for all the time steps, all the nodes and all the elements of the mesh.
In the following subsections, first a general description of the ECRI directive is given. Then, all the optional keywords (NOPO ...) and optional sub-directives (FICH ...) are described below. Output regions created by the directive REGI are described on page G.100. Finally, the MEAS directive is described on page G.105.
The "ECRITURE" directive can be used to select specific quantities to be printed out in the output listing at user-chosen times. It allows also to choose the nodes and elements for which the quantities will be printed.
The various quantities are associated to nodes or elements as described on page G.30 and following ones.
"ECRITURE" < "COOR" > < "DEPL" > < "VITE" > < "ACCE" > < "FINT" > < "FEXT" > < "FLIA" > < "FDEC" > < "CONT" > < "EPST" > < "ECRO" > < "ENER" > < "MCVA" > < "MCVC" > < "MCVS" > < "FAIL" > < "VFCC" >
The keyword "ECRITURE" should only appear once in an input data sequence. Keywords "COOR", "DEPL", etc. should immediately follow the "ECRI" keyword.
If none of the preceding keywods is specified, nothing will be printed.
In a standard calculation (not a restart), EUROPLEXUS always prints the last computed time step.
Take care when choosing output frequencies, because the size of listing files may grow very fast.
Note that the results file of type "ALICE" allows to re-construct a listing. You may therefore choose to print out the bare minimum. Later on, if additional results need to be printed, you may do so by re-reding the "ALICE" file (which must have been specified, of course).
For each chosen node, one may ask to print:
- current coordinates;
- internal forces;
- total external forces;
- external reaction (coupled link) forces for the nodes sujected to “coupled” conditions (see LINK COUP);
- external reaction (decoupled link) forces for the nodes sujected to “decoupled” conditions (see LINK DECO);
- multi-component flow-related data (finite volumes).
For each chosen node, the code prints X,Y or R,Z o X,Y,Z.
The chosen nodes are grouped by increasing number of degrees of freedom (d.o.f.). First all the nodes with 1 d.o.f. are printed, then those with 2 d.o.f.s, etc.
For each chosen element and each integration point one may ask to print:
- the stress components (SIG);
- the deformation (EPST);
- the hardening parameters (ECR).
The stress tensor and the total deformation tensor are related to the element, and independent from the material.
The material parameters, contained in the ECR table, sre independent of the element, and are only function of the material.
The choices done in EUROPLEXUS for these two quantities are detailed in the following pages.
For a given element type, the stress components have always the same meaning, for whatever material is assigned to the element. On the contrary, the hardening values (ECR) are strictly related to the chosen material, and do not depend upon the element type.
The stress tensor is stored and printed in vector form, and is printed for each integration point of the element.
In 2D, it will be necessary to distinguish the axisymmetric case (AXIS) from the plane strain (DPLA) and plane stress (CPLA) cases.
For continuum-like elements, the stresses are written in the global reference frame, while for the other types of elements (shells, beams, bars) they are expressed in a local frame attached to the element.
Instead of computing a bending moment, one computes a “bending stress” (sigf), that may be directly compared with the membrane stresses. This bending stress is related to the bending moment as follows:
Moment = E * I * Khi Khi : curvature sigf = E * (h/2) * Khi h : thickness Hence: Moment = 2 * ( I / h ) * sigf For a shell: Moment = ( h * h / 6 ) * sigf
These elements may only work in traction and compression. There is just one stress component (scalar).
This element works in membrane and bending. There are 4 stress components per element, expressed in a local reference frame.
The first direction of the local frame is along the element from node 1 to node 2. The second, located in the mesh plane, is normal to the first. The third direction is such that the reference (u, v, w) be right-handed.
sig(1) : membrane (u) sig(3) : bending (v) sig(2) : membrane (w) sig(4) : bending (w)
Also this element works in membrane and bending. But besides the 4 preceding stress components, there is a fifth one for the shear, which is treated elastically.
sig(1) : membrane (u) sig(3) : bending (v) sig(2) : membrane (w) sig(4) : bending (w) sig(5) : shear
The stress components are expressed in the global frame. For a calculation in plane stress, there are three stresses expressed in the (x, y) frame. For an axisymmetric calculation or a plane strain calculation there are 4 stress components, expressed in the frame (x, y, z). The z direction is the normal to the mesh plane, and such that (x, y, z) be right-handed.
1) CPLA: ( SIG(1) SIG(3) ) (sig) = ( ) ( SIG(3) SIG(2) ) 2) AXIS or DPLA: ( SIG(1) SIG(3) 0 ) ( ) (sig) = ( SIG(3) SIG(2) 0 ) ( ) ( 0 0 SIG(4) )
Like for the BARR and PONC elements in 2D, these elements may only work in traction and compression. The stress tensor has just one component.
This element works in traction, torsion and bending. There are always 4 stresses per Gauss point, expressed in the local frame.
The first direction of the local frame (u) is along the element, from node 1 to node 2. The second (v) is in the plane defined by u and the local vector V, on the same side as V. The third one (w) is deduced from the others.
Here, due to beam assumptions, the bending stresses are expressed in the frames (u, v) and (u, w):
sig(1) : traction (u) sig(3) : bending (u,v) sig(2) : torsion (u) sig(4) : bending (u,w)
In order to determine the local state of the beam, only the moments and the deformation have a sense! It is therefore mandatory to estimate the moments starting from the stresses, by the following relation:
|M = σ|
The value of σ is read on the listing, I and h are specified in the input data set (see Chapter C1). The deformations are read directly from the listing.
For an elastic calculation ONLY, it is then possible to compute the stresses in any point of the cross-section.
These elements work in membrane and bending. There are always 6 stress components per Gauss point, expressed in a local frame.
For the triangular elements COQ3, the first direction of the local frame (u) is along the first side of the element, from node 1 to node 2. The second (v) lies on the element plane, such that node 3 is on the positive side.
Because of shell hypotheses, the stresses are expressed in the (u, v) frame.
The quadrangular elements COQ4 are composed by 4 triangles:
1-2-3 3-4-1 1-2-4 3-4-2
Each of these triangles has a local reference frame as defined above. If the quadrangle is a parallelogram, the 4 local frames are identical.
The 4 Gauss points of element COQ4 are at the centers of the triangles mentioned above. If the element has an irregular shape, the stresses at the various Gauss points will not be directly comparable.
sig(1) : membrane (u) sig(4) : bending (u) sig(2) : membrane (v) sig(5) : bending (v) sig(3) : membrane (uv) sig(6) : bending (uv)
The stresses are expressed in the global frame (x, y, z).
( SIG(1) SIG(4) SIG(6) ) ( ) (sig) = ( SIG(4) SIG(2) SIG(5) ) ( ) ( SIG(6) SIG(5) SIG(3) )
The tensor of total deformations is the dual of the stress tensor. Its structure is therefore the same as that of the stresses (see the previous Section).
All internal variables pertaining to the different materials are stored in the ECR table. Initially reserved only for the hardening parameters, this table has been considerably enlarged, as more complex materials have been implemented in EUROPLEXUS.
Only the simplest materials use just the first hardening quantities. For the others, the meaning of the ECR components are described within each material law description (see page C.100 and following ones).
ECR | shells | continua (solids) | continua (fluids) --------+-------------------+-------------------+------------------ ECR(1) | V.M. membrane | Pressure | Pressure ECR(2) | V.M. memb. + bend.| Von Mises | Density ECR(3) | plast. deform. | plast. deform. | -
The equivalent plastic deformation (ECR(3)) is only printed for elasto-plastic calculations.
The Von Mises criterion for the shells is expressed as:
sig(*) = SQRT( sig(m)*sig(m) + (alpha**2)*sig(f)*sig(f))
sig(f) Von Mises stresses
in membrane and bending
alpha = 2/3 by default.
The Von Mises criterion for the beams is expresses as:
sig(*) = SQRT( ap * press*press + am * sig(1)*sig(1) + at * sig(2)*sig(2) + af * (sig(3)*sig(3) + sig(4)*sig(4)) )
sig(i) are defined above, and
press is the
internal pressure, if the beam is a pipe. The coefficients
af (bending) are computed by EUROPLEXUS
according to the type of beam, of the existence or not of
a curvature, etc.
The /CTIME/ procedure, described in the introduction (see page INT.57) is used to specify when printouts should take place during a computation.
If nothing is specified, the printouts are performed for all time steps.
If the keyword "NUPA" is used, do not forget to dimension adequately by means of the word "MNTI" as described on page A.100.
If the keyword "TIME" is used, do not forget to dimension adequately by means of the word "MTTI" as described on page A.100.
Be aware that printout times specified via "TFRE" or "TIME" are rounded to the closest time unit, that can be chosen via the "OPTI TION" directive.
Be careful in the choice of your printouts if you do not want to produce unnecessarily large listings. In general, it is advisable to use graphics post-processing in order to analyse the results, instead of reading values on a listing.
It is useful to know that the output file of the results ( "FICH" "ALICE" ), enables to print selected results on a listing after completion of a calculation. Therefore it is advisable to print only the bare minimum, although it will be necessary to read the results file again, in order to output interesting things after a calculation has been completed.
The user can choose the nodes and/or elements where he wants to print the results.
$["NOPOINT" ; "POINT" /LECTURE/ ]$ $["NOELEM" ; "ELEM" /LECTURE/ ]$
The two options "POINT" and "NOPOINT" are mutually exclusive, and the same is true for the two options "ELEMENT" and "NOELEM".
If none of the two options is specified, the results are printed for all nodes and for all elements.
G.70 - Feb 13
This directive is aimed at creating files for the post-processing of the computation results or a saving file to restart the calculation. The following file types are available:
- SAUVER file (saving file for successive restart) - ALICE file (postprocessor: EUROPLEXUS) - ALIT (ALICE TEMP) file (postprocessor: EUROPLEXUS) - PVTK file (postprocessor: PARAVIEW VTK format) - TABL file (a simple formatted table) - POCH file (for Pochhammer-Chree post-treatment by EPX) - MAPB file (for storing a blast wave to a later mapping) - MED file (compatible with many softwares)
The following file types are available but not developed further:
- SPTAB file (postpr.: SUPERTAB (old I-DEAS interface)) - TPLOT file (postprocessor: TPLOT) - XPLOT file (postprocessor: TPLOT) - K2000 file (postprocessor: CAST3M) - AVS file (postprocessor: AVS and old ParaView) - PLOT-MTV file (postprocessor: PLOT-MTV) - UNIV file (postprocessor: I-DEAS)
The SAUVER file is used to restart the calculation. It is described in detail on GBG_0110.
CAST3M is the product of CEA (Cf. http://www-cast3m.cea.fr), SUPERTAB is a commercial software by SDRC, TPLOT is a software by JRC, AVS is a commercial product by Advanced Visual Systems, PLOT-MTV is a public utility (2D plotting only), I-DEAS is a commercial software by SDRC. The MED format is a format co-developed by the CEA and EDF which is compatible with many softwares. PARAVIEW is an open-source multi-platform application designed to visualize data sets of size varying from small to very large (see http://www.paraview.org).
Note that, besides the I-DEAS interface (UNIV keyword) described hereafter, another version is available, that had been independently developed by the CESI (formerly ENEL) group, and which is described on GBG_0072.
< FICHIER |[ "SAUV" <ndsauv> <"PROT" 'maclef'> <"LAST"> </CTIME/> ; "ALICE" <"FORMAT"> <"SPLIT"> <ndgrap> /CTIME/ ; "ALIT" <"FORMAT"> <ndalic> /CTIME/ ... ... < "POINT" /LECTURE/ > ... ... < "ELEM" /LECTURE/ > ; "PVTK" < $["FORM" ; "FOLD"]$ > <ndpara> /CTIME/ <"PINB"> <"MPI"> <"FLSW"> <"GROU" |[ "AUTO" ; nobj*("OBJE" <'groupname'> $[ "GAUS" ngaus ; "GAUZ" ngauz ]$ /LECT/) ]| > <"VARI" <"DEPL"> <"VITE"> <"ACCE"> <"FEXT"> <"FINT"> <"FLIA"> <"MCXX"> <"SIGN"> <"ECRN"> <"RISK"> <"FAIL"> <"VCVI"> <"CONT"> <"EPST"> <"ECRO"> <"XLVL"> <"DTST"> <"EPAI"> > <"SHEL" vx vy vz /LECTURE/ > ; "TABL" <ndtabl> /CTIME/ "VARI" nv * ( |[ "COOR" "COMP" ic "NOEU" /LECT/ ; "DEPL" "COMP" ic "NOEU" /LECT/ ; "VITE" "COMP" ic "NOEU" /LECT/ ; "ACCE" "COMP" ic "NOEU" /LECT/ ; "FINT" "COMP" ic "NOEU" /LECT/ ; "FEXT" "COMP" ic "NOEU" /LECT/ ; "CONT" "COMP" ic "GAUS" gp "ELEM" /LECT/ ; "ECRO" "COMP" ic "GAUS" gp "ELEM" /LECT/ ; "EPST" "COMP" ic "GAUS" gp "ELEM" /LECT/ ; "FONC" ifon ]| ) ; "POCH" <"FORMAT"> <"SPLIT"> <ndpoch> /CTIME/ ... ... "NLIN" nl * ( /LECT/ ) ... ... "VARI" $[ "DEPL" ;"VITE" ; "ACCE" ]$ ; "MAPB" | "MSPA" ; "MTIM" | "DIPR" dipr "PCHE" pche /CTIME/ "SPTAB" <ndspta> /CTIME/ ; "TPLOT" <"FORMAT"> <ndtplo> /CTIME/ ... ... "DESC" 'dddddd' ... ... < "POINT" /LECTURE/ > ... ... < "ELEM" /LECTURE/ > ; "XPLOT" <"FORMAT"> <ndxplo> /CTIME/ ... ... "DESC" 'dddddd' ... ... < "POINT" /LECTURE/ > ; "K2000" < $[ "FORM" ; "XDR" ; "BINA" ]$ > <"SPLIT"> ... ... <ndcast> /CTIME/ ... ... < "POINT" /LECTURE/ > ... ... < "ELEM" /LECTURE/ > ... ... <"SHEL" vx vy vz /LECTURE/ > <"CHAMELEM"> <"VARI" < "DEPL"> <"VITE"> <"FEXT"> <"ACCE"> <"MCXX"> <"SIGN"> <"ECRN"> <"CONT"> <"EPST"> <"ECRO"> <"ECRC" /LECT/> > ; "AVS" "FORMAT" <"PRVW"> <ndavs> /CTIME/ <"VARI" <"DEPL"> <"VITE"> <"FEXT"> <"ACCE"> <"MCXX"> <"CONT"> <"EPST"> <"ECRO"> <"XLVL"> <"ECRC"> > ; "PMTV" "FORMAT" <npmtv> /CTIME/ <"VARI" < "DEPL"> <"VITE"> <"SIGN"> <"ECRN"> > ; "UNIV" <FORMAT> $["CURR" ; "OBSO"]$ <nuniv> /CTIME/ ; "MED" /CTIME/ < "POINT" /LECTURE/ > < "ELEM" /LECTURE/ > ; ]| >
.vtufiles). This is the VTK format, compatible with the newer versions of ParaView. By default, use is made of the library LIB_VTK_IO, written by Stefano Zaghi (see http://stefano.zaghi.googlepages.com/lib_vtk_io), which allows to produce either ASCII or binary output formats. However, if the (obsolete) keyword FOLD is specified in place of FORM, then formatted output is produced without making use of the LIB_VTK_IO library (note that in this case only ASCII format, not binary format, is possible).
.ALI. For the special case of split ALICE files, see comments below.
.K20. For the special case of split CAST3M files, see comments below.
.AVS. Split files are generated for this type of output. See comments below.
.pvd. This file contains links to files with the data (vtu-format, extension .vtu). See comments below.
.MTV. See comments below.
The keyword FICHIER is not compulsory. If it is used, the last step is systematically saved.
Do not forget to define the logical unit(s) of the file(s), on the control cards. As an alternative, EUROPLEXUS accepts the name of the file enclosed in quotes.
If one does not pay attention, result files may become very bulky, because the total number of computed time steps is often very large. It is then advisable to estimate the total number of steps from the stability step computed by the program, and then choose a reasonable number of storages on the ALICE file. It is also possible to obtain a smaller results file by using the ALICE TEMPS (ALIT) directive: in this case only the variables relative to the nodes and elements given in directives POIN and ELEM will be stored.
It is rare that one needs more than a dozen of time stations to plot the deformed shapes of the mesh — in this case the ALICE directive will be used. It is also infrequent that one needs more than a few hundred points to plot curves as a function of time — it is suggested to use the directive ALIT which allows to obtain a file reduced to just the selected points. Therefore it is possible to specify a much larger number of saving stations on an ALIT file than on an ALIC one.
For ALICE, the SPLI option allows to split the results into many small files, one for each stored time instant, rather than producing just one big file. This option is useful for very large computations and/or for producing animations, which typically require many saved instants. In this case, ndgrap is just the base name of the output files. The single file names are automatically given progressive numbers (_0001, _0002, etc.) appended to the name, which identify the storage index. A file with suffix _0000 is also produced, which contains the initial mesh topology.
In order to post-treat these split results with EUROPLEXUS, proceed exactly as if the results would be in a single file, but remember to specify the SPLIT keyword in the RESU ALIC directive, see page ED.20.
XPLOT storage is intended to perform pseudo-1D visualization of data in a 2D or 3D run. A curvilinear abscissa is built up passing through the nodes defined in POIN /LECT/. Then, nodal and element quantities are stored as a function of this abscissa. By using the TPLOT program, the relevant quantities can then be plotted along the curvilinear abscissa (either initial or current). Note that nodal quantities (displacements, velocities, etc.) are stored without modification at the specified nodes. Element quantities, however, (such as stresses and hardening parameters), that are usually defined only at points internal to the elements, are first extrapolated to the nodes, then stored. Currently, the extrapolation consists of simply: 1/ averaging each quantity over each element (by using the values at the different Gauss points), 2/ averaging all neighbour element contributions to obtain nodal values. Neighbour elements to a node are those elements that contain that node.
Note also that, in the extrapolation process, only certain types of elements are considered. For example, shell or beam elements are rejected, because the mean value of the stress components on all the Gauss points is likely to be meaningless for such elements. Only the following element types are considered: TRIA( 2), CAR1( 8), CAR4( 9), CUBE(11), CUB6(13), PR6 (20), TETR(21), PRIS(27), FLU1(52), FLU3(53), FL23(64), FL24(65), FL34(66), FL35(67), FL36(68), FL38(69), Q41 (71), Q42 (72), Q41N(73), Q42N(74).
In order to read with CAST3M a file written by EUROPLEXUS, use the following CAST3M commands:
1/ Formatted file:
OPTI REST FORM 'file'; REST FORM; . . . (post-treatment commands)
2/ Unformatted file:
OPTI REST BINA 'file'; REST BINA; . . . (post-treatment commands)
3/ XDR file:
OPTI REST 'file'; REST ; . . . (post-treatment commands)
For K2000, note that two syntaxes are possible. With the ‘old’ syntax (the keyword VARI does not appear), all nodal quantities are always stored. Furthermore, all element quantities are stored if CHAM appears. The components of the ECR table which are stored depends in this case from the material: they are the same components of ECR that are printed on the listing.
With the new syntax (the keyword VARI appears) only the specified nodal quantities, element quantities and ECR table components are actually stored.
Note that, strictly speaking, it is only possible to produce an output file for K2000 when the input mesh has also been produced (and read into EUROPLEXUS) in this format. However, if this is not the case but you still desire to postprocess your EUROPLEXUS calculation with K2000, consider transforming your mesh in K2000 by the option K2MS (see Section H, output options). Beware, however, that this may require some manual intervention and in any case the obtained mesh will be less flexible to use than a “real” K2000 mesh.
In the case of standard AVS storage, a set of files is written, one for each stored variable. The files basename is given by ndavs. If ndavs as given by the user contains the extension .avs or .AVS, this extension is removed by the program. An extension of the form .VARI.N.inp is then automatically provided by EUROPLEXUS. Here VARI is the variable type (DEPL, VITE , ...) and N an integer counter which is automatically incremented by 1 at each successive storage in time.
Recall that AVS storage can also be requested interactively, i.e. during an interactive execution of EUROPLEXUS (See Group A, Interactive (Foreground) Execution).
In the case of AVS storage modified for usage with PARAVIEW, elements are split into groups with same element topology and same material law. One file is stored for each group of elements at each successive storage in time. This file contains geometry and both nodal fields and elemental fields required by the user. It is named from the name given by ndavs, with its extension removed. An extension of the form _N1_N2.inp is is then added to the name. N1 is the number of the element group and N2 is an integer counter as for standard AVS files. If ndavs is not defined, the base of the EUROPLEXUS input file name is used to build AVS-PARAVIEW file names.
If a directory name is provided for AVS-PARAVIEW files with the OPNF directive, files are written in this directory, excepted if ndavs represents a name with full path. In this latter case, the above given directory is ignored.
The AVS-PARAVIEW format is only readable with older versions of PARAVIEW (less than 2.9). For newer versions of PARAVIEW, the PARAVIEW output (see PVTK) with a
files is recommended.
Automatic group definition for PARAVIEW output (with keyword GROU AUTO) consists in the same splitting of elements as described above for the AVS-PARAVIEW output.
The PLOT-MTV output is only available in 2D and for spectral elements. the program will only include spectral elements and nodes in these files. A separate file with the extension .mtv is produced for each nodal quantity and at each selected storage time.
The SIGN keyword produces storage of 4 nodal stress (6 in 3D) components (SGXX, SGYY, SGZZ, SGXY, SGYZ, SGZX). The ECRN keyword produces storage of 2 nodal hardening quantities: the hydrostatic stress (HYDR) and the Von Mises stress (VMIS).
When using SPTAB output format, a file named sptab.param must exist in the current directory, containing the following key-words useful to declare the variables to print out: DISP, VELO, ACCE, INTF, EXTF, MCVAR, MCVEL, MCMFR, FLVAR, SCUB8, ECOQI.
For CAST3M , the SPLI option allows to split the results into many small files, one for each stored time instant, rather than producing just one big file. In this case, the chosen output type MUST be formatted (FORM). This option is useful for very large computations and/or for producing animations, which typically require many saved instants. In this case, ndcast is just the base name of the output files. The single file names are automatically given progressive numbers (_0001, _0002, etc.) appended to the name, which identify the storage index. A file with suffix _0000 is also produced, which contains the initial mesh topology.
In order to post-treat one of these split results with CAST3M, proceed as follows: choose the instant to be treated, say number 3 i.e. the third storage performed; then, produce a file by concatenating the ‘zero’ file (_0000) and the file for the chosen instant; finally, read and post-process the resulting file with CAST3M. In this example:
cat mytest_0000.k20 mytest_0003.k20 >out.k20 K2000 opti rest form 'out.k20'; rest form; ...
Be careful: output files may become very large, because the total number of the time steps computed is often large. Therefore it is better to estimate that number from the stability step computed by the program. Then, the user can choose a reasonable number of writings on the output files.
The user seldom needs more than a dozen storage stations (‘cases’) to draw deformed structures and no more than fifty points to draw time functions.
This is aimed at creating files for the post-processing of computation results by I-DEAS master series.
This model is part of the models developed by the CESI team (formerly at ENEL, Milano) in collaboration with JRC.
I-DEAS is a commercial software by SDRC.
< "FICHIER" <FORMAT> "IDEA" ndidea /CTIME/ ... < "POINT" /LECTURE/ > ... ... < "ELEM" /LECTURE/ > ... < "VARI" < "DEPL" "VITE" "FEXT" "ACCE" "MCXX" > < "CONT" "MESH" "MCVA" "MCVE" "MCMF" > < "FLVA" "ECOQ" > > >
The general comments of page G.70 apply to the I-DEAS results file as well.
When using "IDEA" output format, the default options for the selection of the results are: whole geometry (i.e. all nodes/elements are treated if "POIN", "ELEM" are omitted), no variable (i.e. only the variables specified in the "VARI" option are stored).
Element output in I-deas universal file format is only available for FLxx, MCxx, CUB8, COQI, CQD3, CQD4 elements at the moment.
This directive enables the printing of physical values within a given region.
A region is defined by the list of the elements which compose it. The region could correspond to a GIBI object.
"REGION" ( 'nom region' $[ "RMAS" ; "VOLU" ; "BARY" ; "DIMX" ; "DIMN" ; "DMOY" ; "VEMX" ; "VEMN" ; "VMOY" ; "ACMX" ; "ACMN" ; "AMOY" ; "IMPU" ; "ECIN" ; "WINT" ; "WEXT" ; "PDV" ; "WINJ" ; "RESU" ; "IRES" ; "ECRG" ; "ECRM" ; "EMAS" ; "FLIR" ; "RISK" ; "EROD" ; "ENDO" ; "CLAS' ; "EPSM" ; "TOUT" ]$ < "DIRX" rx "DIRY" ry "DIRZ" rz > |[ /LECTURE/ ; "POIN" /LECTURE/ ]| )
If the slider direction is vertical, the local x-axis is collinear with the sliding direction, the y-axis is collinear with Y-axis, and z-axis completes the direct orthogonal axis system.
Only the following quantities can be written in this frame: MASS, ECIN, AMOY, ACMX, ACMN, VMOY, VEMX, VEMN, DMOY, DIMX, DIMN, BARY, IMPU, QMVT, RESU, ECRG, FLIR
The computation takes place within the elements.
It is possible to have elements which belong to several regions.
If the region is only known by its nodes (it has not been defined in the directive "GEOM"), the only possible balances are WEXT, RESU and IRES. In this case, it is mandatory to use the keyword "POIN" before the /LECTURE/ procedure, to avoid confusion between nodes and elements.
If the region is nothing else but the whole structure, the values of WINT and ECIN are the same as those printed in the energy balance.
The physical values of the regions are computed during the printing.
There is no problem if the computed quantity does not depend on masses (WINT). If the physical values are dependant on the masses (ECIN BARY VMOY IMPU RMAS VOL PDV), the computation will be correct only if the masses are constant during the EUROPLEXUS computation. In fact, in order to lighten the file of the results (FICHIER ALICE), only the initial masses are copied out. There is no problem concerning a Langrangian computation. For an Eulerian or A.L.E computation, the masses change. Therefore, the physical values will not be correct.
All this happens during a restart; if the physical values are computed during a normal (non restart) EUROPLEXUS run, all the results are correct.
This directive enables the printing of various types of “measurements” on the current geometrical mesh.
Normally, it is called from the input file and the requested measurements are then printed on the listing. However, the same directive (same syntax) is available also from the command line during an interactive execution (see pages A.25 and O.10). For this reason, the present directive must be terminated by the keyword TERM, as shown below in the syntax. In case of interactive use, the requested measurements are printed on the console window, not on the listing.
MEASURE $[ ELEM e ; NODE n ; OBJE /LECT/ ; EMIN /LECT/ ; EMAX /LECT/ ; DIST <POIN> /LEC1/ <POIN> /LEC2/ ]$ TERM
An example of this directive is as follows:
MEASURE ELEM 123 NODE 74 ELEM 1 OBJE LECT toto TERM EMIN LECT tous TERM EMAX LECT 1 2 4 TERM DIST LECT toto TERM LECT tata TERM ! min distance between two ! objects made of elements DIST POIN LECT p1 TERM LECT tata TERM ! min dist. between a point ! (node) and an object made ! of elements DIST POIN LECT p1 TERM POIN LECT p2 TERM ! distance between two ! points (two nodes) TERM
When used interactively, the code pauses for input after each sub-command, waiting for the next sub-command. To exit from the MEAS directive, give the final TERM command.
This keyword creates a saving file and, in conjunction with the keyword REPR (to be used in a subsequent run), allows splitting a computation in two or more parts.
This directive replaces the old (deprecated and obsolescent) directive SAUV (group A, see page SR.20).
The results are saved on a file (saving file) at times specified by the user. Each saving corresponds to a number or position on the file (1, 2, 3 etc.), from which a restart of the computation can be carried out in a successive run (see directive REPR on page SR.30).
FICH SAUV <ndsauv> <PROT 'maclef'> <LAST> </CTIM/>
The keyword PROT is not compulsory. If it is not used, there is no protection (this is equivalent to a key of 8 blanks).
If a unit number is used for nbansav, the saving file and its number must have been defined before on the control cards.
A first saving station (position number 1) containing some header data is always produced at the initial time (step 0 of the calculation). Of course, it is normally meaningless to restart from this time station, unless the LAST keyword has been specified (see above), because it would be the same as starting the calculation anew from the initial time. On the contrary, if LAST has been specified, the only possibility for restart is to use the first time station which, in this case, will contain the data of the last saving performed (not the first one in general).
Assume a calculation performs 4994 time steps to arrive at its final time. The following saving directives are accepted: