Data for post processing is provided within
text files and read with command Load post data. The file must contain node or element IDs and node respectively
element related values for a single or for multiple load cases.

A type ID in the first line of the file
differentiates between following types of data:

ktyp =
0: 1 scalar value is given for each node

=
1: 3 vector components are given for each node

=
2: 1 scalar value is given for each element

=
3: mw scalar values are given for each element: scalar values are assigned to
the element nodes.

=
4: mw scalar values are given for each element: 1 scalar value for each surface
of volume elements

=
5: 3 vector components are given for each element

=
7: 1 vector cross is given for each element

=
8: mw scalar values are given for each node (mw load cases)

=
9: mw scalar values are given for each element (mw load cases)

=
11: mw vectors are given for each node (mw load cases)

=
12: mw vectors are given for each element (mw load cases)

=
14: mw vector crosses are given for each element (mw load cases)

=
20: mw scalar values are given for each element: 1 value for each integration
point

=
21: mw vectors are given for each element: 1 vector for each integration point

=
22: mw vector crosses are given for each integration point

=
30: 1 scalar value is given for each beam element

=
31: 2 scalar values are given for each beam element

=
32: mw scalar values are given for each beam element

=
33: 2 * mw scalar values are given for each beam element

The data files must have the following format:

First line:
7 [3] integers for ktyp, mw, lc, mip [, nl1, nl2, nl3]

ktyp
defines the type of data contained in the file.

mw is the
number of scalar or vector values belonging to each node or element. If the
number of values is not the same for all elements, the maximum number must be
given for mw and missing values for some elements or nodes have to be added as
zeros. This is for example the case when scalar values are given in integration
points and when the structure is build of quadrilateral and triangular elements
where the number of integration points is different for the two types of
elements.

lc is the
ID of a load case for separating multiple load cases.

mip is
the number of integration points for one direction (used only for ktyp = 20 –
22).

nl1 is
the number of comment lines before the first data line. For nl1 > 0 nl1
lines are skipped after the format line.

nl2 is
the number of continuous data lines. For nl3 = 0 nl2 has no effect.

nl3 is
the number of comment lines that follow each block of nl2 data lines. For nl3
> 0 nl3 lines are skipped after nl2 data lines (see demo file
„nastran2.stress).

Second
line: textual data

Given
text in this line is used as a description of this load case, which can be
plotted during graphical output. This line can be left blank.

Third line:
format

This line
specifies a FORTRAN like format for the following data lines. Leaving this line
blank causes the file to be read in a free format. Reading in free format can
only be used when all data lines contain exactly the number of values expected
by the file type, and no comment lines are contained in the input file.

The
format (I5, 5X, 3F12.0) for example will read node ID and first 3 displacement
components from the following input line which contains additional data:

8137 G -7.833E-07 -1.608E-06
0.0 0.0 0.0 -9.991E-08

If a data
set for one element or one node continues over several lines the format must
contain a / for each new line. For example using the format (I10, F15.0, 30X,
F15.0 / 25X, F15.0, 15X, F15.0) will read the ID and 1. and 4. value from the
first line and 2. and 4. value from the second line of the following data set:

1728 7.390112E-01 -1.320112E-01 -5.322112E-02 0.590112E-01 -1.053304E+01

-7.439936E-09
2.409936E-03 5.489936E-01
-7.439936E-00

The
format

(1X,I11////115X,F15.0///115X,F15.0///115X,F15.0///115X,F15.0///115X,F15.0///115X,F15.0///115X,F15.0///115X,F15.0//)

is used
to read the Von-Mises-Stresses on the 8 corner nodes of a NASTRAN element CHEXA
(see demo file „nastran2.stress)

Hint: No
FORTRAN routines are used to read the input lines, a given format is
interpreted. Only following specifications are allowed: m**I**n for integers, m**F**n.0
for real values and n**X** for fields
that should not be read; where m is an optional multiplier and n the field
width. If an error happens when reading an item no further reading is done. If
the input file contains comment line, the params nl1-nl3 must be given
appropriate.

Additional lines: data values for nodes respectively
elements

Each line
must start with a node or an element ID followed by mw scalar respectively
vector values. Node and element IDs are taken as external IDs, the data values
are assigned corresponding to these IDs. If no data values are given for some
nodes or elements, corresponding values are set to zero.

With data types 7,14 and 22 (vector crosses)
the first two data values are interpreted as length of the two orthogonal
vectors while the third data value is taken as an angle (degree) in the element
plane.

Files with data types 0-7 and 20-33 are
interpreted and saved as a single load case while files with type 8-14 are
interpreted as mw load cases. For example it’s possible to save the results of
several following steps of a nonlinear calculation or node displacements of
following time steps within a single input file.

With
ktyp = 20 –22 mip is the number of integration points for one direction.
Permissible values are mip = 2, 3, 4, 5, 6 with quadrilateral elements and mip
= 2, 3, 4 with triangular elements. The number of integration points for one
element is mip * mip with quadrilateral and 3, 7, 13 with triangular elements
when mip = 2, 3, 4. The position of the integration points is assumed to be as
with gauss integration. The ordering is shown in following picture for mip = 4
(see K. J. Bathe: Finite element methods). Integration points are only realized
for quadrilateral and triangular elements.

If scalar values are given in integration
points, the values for the nodes of the elements are calculated by
extrapolation respectively interpolation for additional nodes in the inner of
curved elements. If nodes on element edges belong to more than one element,
optionally the smallest, the largest or the mean value of the values belonging
to the different elements can be used for these nodes. If with ktyp = 3 the
number of given scalar values is less than the maximum number of element nodes,
it is assumed, that only scalar values for corner nodes of the elements are
given, the scalar values for nodes on the edges are in this case calculated by
interpolation (see the demo example “nastran2.dem”).