D3PLOT 22.1

The "Complete State" (.ptf) File (Also .rlf and d3eigv Files)

The "complete state" (.ptf) file. (Also .rlf and d3eigv files.)

Defining output parameters in Ansys LS-DYNA

The following Ansys LS-DYNA control cards control output of this file:

*DATABASE_BINARY_D3PLOT Is mandatory. Controls output frequency.
*DATABASE_EXTENT_BINARY Is optional. This card allows switching of certain parts of the file's contents on/off. These are discussed in Controllable contents of the complete state file below.

The generic contents of the complete state file


Control information:
Number of nodes
Number of each type of element

Number of materials

Amount of data written for each element type
Basic geometry & topology:
Undeformed nodal coordinates
Element topology

Arbitrary numbering tables

Complete state: (Repeated for all times dumped)
Time
Global data: energies, velocities, masses, stonewall forces
Nodal coordinates
Temperatures at nodes
Nodal velocities
Nodal accelerations
Solid element stresses and plastic strain
Thick shell stresses and plastic strains
Beam forces
Thin shell stresses, strains & related data
Deleted element tables

Controllable contents of the complete state file.

The options on the *DATABASE_EXTENT_BINARY card in the Ansys LS-DYNA input deck allow you to control the following contents of the complete state file.


NEIPH "Extra" data components for solid elements. Default None .

Some material models generate more information for solids than can be written in the standard formats. For these "extra" variables may be written. They are <neiph> scalar values that follow the normal data. They:

  • Are written for every solid element, regardless of material model.
  • Have no explicitly defined component names associated with them: this will depend on the material model.
    • NEIPS "Extra" data components for shells and thick shells. Default None .

    As with solids some material models write extra information for shells. They are <neips> scalar values that:
  • Are written at every "surface" output for every shell, regardless of material model used.
  • Have no explicitly defined components associated with them: this will depend on the material model.
    • MAXINT Number of "surfaces" written for shell and thick shell elements. Default 3 .

    The default value of 3 writes data at neutral axis, innermost and outermost integration points for shells and thick shells. Values other than 3 write results for the first <maxint> integration points: read Section 13.8.2.2 before using them.
    STRFLG Write directional strain tensors for solids, shells & thick shells. Default Off .

    By default no strain tensors are written for any elements, (although effective plastic strain is). Turning this flag on causes the strain tensors for solids, shells and thick shells to be written. Note that:
  • A single tensor at the element centre is written for solids.
  • Tensors at innermost and outermost integration points only are written for shells and thick shells, regardless of the <maxint> value.

    • The following flags can be used to reduce database size by controlling the output for shells and thick shells. By default they are all On .

    NOTE: None of the following four flags influences the output for solid elements.
    SIGFLG Controls the output of the stress tensors for shells and thick shells.

    The symmetric stress tensor (6 values) is written at <maxint> "surfaces" for every shell and thick shell, so turning this off usually saves 18 values per shell. You will, of course, then not be able to post-process any stresses.
    EPSFLG Controls the output of effective plastic strain for shells and thick shells.

    The effective plastic strain (1 value) is written at <maxint> surfaces for every shell and thick shell. Turning this off will usually save 3 values per shell.
    RLTFLG Controls the output of force and moment resultants for shells.

    Force and moment resultants (8 values) are written for every shell (but not for thick shells). Turning this off will save 8 values per shell.
    ENGFLG Controls the output of thickness and strain energy density for shells.

    Thickness, strain energy density and two other (unused) values are written for shells (but not for thick shells). Turning this off will save 4 values per shell.

    CMPFLG Composite material stress output in local axes. Default Off .

    By default all stress tensors are written in the global coordinate system. Turning this flag on causes those from composite materials to be written in the material local axis system(s).
    WARNING: There is no way for D3PLOT to tell from the database that these stress tensors are in the local system. It assumes that ALL STRESS TENSORS ARE IN THE GLOBAL SYSTEM.

    If you use this facility IT IS YOUR RESPONSIBILITY to interpret your results correctly: they will be reported in D3PLOT as global stresses.

    BEAMIP Number of "extra" data values written for beam elements. Default None .

    All beam elements write 6 basic forces and moments, but certain element and material formulations can generate extra data:

    Resultant formulation (Belytschko-Schwer) beams can generate a further 15 "plastic" values, depending upon the material model used.

    Integrated (Hughes-Liu) beams can generate 5 "extra" stress and strain values at each integration point.

    There is no way of telling from the database whether "extra" beam results contain "Integrated" stress/strain data, or "Resultant" plastic data.

    LS-970 and earlier: inconsistent beam sign conventions.


    There is an inconsistency of sign convention in beam output from versions of Ansys LS-DYNA prior to release 971.

  • "Resultant" (typically Belytschko-Schwer) elements use one sign convention
  • "Integrated" (typically Hughes-Liu) elements use the opposite sign convention for 4 of the 6 output components.


    • The following table shows the status quo up to and including Ansys LS-DYNA release 970 :

    Component Matching?
    Fx Same
    Fy Opposite
    Fz Opposite
    Mxx Opposite
    Myy Opposite
    Mzz Same

    Which is right?

    Sadly there is no "right" for beam output, as different users have different conventions. The confusion arises because of the different ways in which the beam types work: integrated beams have integration points at their centre, whereas resultant beams have (potential) hinges at their ends. The former reports force in the beam, and the latter reactions at the supports.

    This has serious implications when plotting beam data and when extracting cut section forces and moments through beam structures (see FORCES Computing Forces and Moments on the Cutting Plane )

    LS-971 onwards: beam sign conventions corrected.

    At some stage during the development of Ansys LS-DYNA 971this bug was corrected, and the output from resultant and integrated beams now match. The sign convention that has been adopted is the "integrated" one.

    D3PLOT handling of Beam sign convention problems.

    Unfortunately it is not possible to determine the analysis code version accurately from a database file (at the time of writing, September 2008, output databases from Ansys LS-DYNA 971 still report their version number as 970). Therefore D3PLOT adopts the following approach:

    • Contour plots of beam data are always shown "as is". This tends not to matter since it is usually easy enough to see what plots mean.

    • However when computing cut-section forces through beams the sign convention is vital, therefore D3PLOT will prompt you for the sign convention to be used.

    Update : From approximately 2009 onwards output from Ansys LS-DYNA 971 reports its version number correctly in output files, and D3PLOT is thus able to determine that the sign convention problem described above has been fixed.

    IT IS YOUR RESPONSIBILITY to interpret your beam results correctly.

    DCOMP Data compression flag. Default 1.

    The default value of "1" means that database compression is turned off and a full set of data values is written to the database for each rigid element in the model. If this option is set to "2" data values will not be output for rigid elements. This option can significantly reduce the size of the binary files written by Ansys LS-DYNA if the model contains a large proportion of rigid elements.

    The following output options are currently not supported by D3PLOT, and should not be changed from their default (off) states:

    SHGE Output of shell hourglass energy.
    STSSZ Output of shell element time steps.


    Previous | Next