Post processing is required to reassemble the partitioned restart files, this is accomplished
The output of post_nsu3d can be used in tecform, a post-processor which constructs a file for input to a visualization program.
For an example of how to use the post processing tools see the tutorial.
post_nsu3d is a facility for reassembling partitioned restart files generated from parallel nsu3d runs into a single restart file which can then be used as input to other post-processors such as slice and tecform.
post_nsu3d can also be used in reverse mode, to partition an existing assembled restart file into a form suitable for use as input to a parallel nsu3d run.
Two applications of post_nsu3d can be use to convert a partitioned restart file into restart file partitioned into a different number of partitions by first assembling the existing partitioned restart file,
and then repartitioning this file.
post_nsu3d not only assembles or partitions the restart files, but also reorders the data internally in order to correspond to the architecture-optimized ordering imposed by prensu3d on the grid data.
For this reason, post_nsu3d must be invoked even for restart files resulting from non-parallel nsu3d runs.
To achieve these functions, post_nsu3d requires as input the restart directory produced by the flow solver, (or the single restart file, when using the reverse mode) and the directory of partitioned grid data produced by post_nsu3d.
In actual fact, only the order.n files from this directory are required by post_nsu3d, but it is most often simplest to supply the entire directory without separating out different files.
A sample parameter input file for post nsu3d is given below:
tecform is a post-processor which constructs a file for input to a visualization program. tecform can be used to view a grid and its associated patch system or components, to check the validity of a boundary condition (*.bcs) file applied to a particular grid, or to view a computed solution on a surface grid or in the interior volume grid.
Beginning with Version 4.3, binary output files for TECPLOT are supported. This format is specified by setting the IFORM variable for the tecform output file to 2.0. (IFORM = 1.0 produces a formatted output file.) Binary files are desirable because they are much smaller and faster to read and write. Binary TECPLOT files usually have a *.plt suffx. In order to write binary TECPLOT files, the tecutil.a library must be linked by tecform.
For cases where this library is not available, the tecform makefile provides a compile option which omits linking the library, while disabling the binary file output option. This is achieved by setting the TECIO variable in the makefile as TECIO = TECIO_OFF. When TECIO = TECIO_ON is specified, the tecutil library will be linked. In this case, the location of the library must be specified in the TECLIB make file variable.
Output files suitable for the FieldView and Ensight visualization packages is also possible as described below.
A sample input file for tecform is given below:
Line 1: A title describing the particular case. This title is written to the TECPLOT binary (only) files and appears on in the TECPLOT window when the file is read in.
Line 3: Name of grid input file, this is a *.cell file (mixed element unstructured grid cell file). Format should be 2.0 for a mixed element unstructured grid cell file (most common), or -2.0 for old obsolete tetrahedral-only cell files.
Line 5: Name of NSU3D restart file. Format should be 2.0. If only viewing grid and no solution or restart file is available, this file name can be skipped by specifying 0.0 plot variables on Line 13, and deleting lines 14 through 18.
Line 7: Name of output file to be written. Formatted (IFORM = 1.0) files and binary (IFORM = 2.0) files are supported along with Ensight (IFORM = 3.0) and Fieldview unformatted (IFORM = 4.0). The creation of binary TECPLOT files requires linking to the tecutil.a library upon compilation.
Lines 8-11: For time-dependent cases, these controls allow the user to select the range of solutions to include in the tecform output. Must be paired with the equivalent solution range when running post_nsu3d.
Line 13: For surface plot only use 1.0, for a volume plot set equal to 2.0. Surface plots are most often used due to the much smaller amount of data. Surface plots can be divided up into multiple zones, whereas volume plots are always treated as a single zone (see Line 21).
Line 16: This is the number of variables to be output for plotting in TECPLOT. There can be a maximum of 5 variables, and a minimum of 0 variables. The number of lines under the heading of Line 14 (lines 15 through 18 in this case) must be equal to the specified number of plotting variables. In the event that no plotting variables are desired, this value can be set to 0.0, and lines 14 through 18 can be omitted. In this case, no solution/restart file is read in.
Lines 18 - 21: Specify plotting variables. Number of lines must be same as stated number of variables on Line 13. IPLOT value is a dummy counter. Variable name must be selected from one of the following: density, rhou, rhov, rhow, energy, mach, cp, cptotal, entropy. The first five of these names correspond to the values in the five locations in the solution/restart file (usually conserved variables). The other variables are computed from these variables within tecform.
Line 24: Number of zones for surface plotting. For volume plotting this should be 1.0. For surface plotting, this can be any positive whole number, or -1.0, or 0.0 A value of -1.0 will automatically list each surface patch as a separate zone. No entries in the input file are required after this line in the case where the number of zones is set to -1.0. If this entry is set to 0.0, then a boundary condition (*.bcs) file must be specified on the next line (Line 22). A separate zone is then created for each boundary condition. No entries in the input file are required after the specification of the boundary condition (*.bcs) file. This option is useful for checking the correctness of a particular boundary condition file.
Lines 26-29: If the number of zones is greater than 0, then the appropriate number of zones must be defined under the heading on Line 24. IZONE is a dummy counter. ZONE_NAME is the name to be assigned to each zone.
Line 32: Zones can be defined either by patches (1.0) components (2.0) or bodies (3.0).
Lines 34 - 41: Zones are defined on these lines. IZONE refers to the zone number. All patches (or other defining entities) between BEG_NUM and END_NUM will be assigned to the zone IZONE. These entities may be listed multiple times. Their parent zone is updated at each new listing. They may also be overwritten by listing them under EXCEPTIONS starting at Line 45.
Lines 51 - 55: These lines are optional and may be deleted. They provide the possibility for computing force coefficients based on particular zones. The zone is defined by IZONE, and a reference area for force coefficients, and reference length for moment coefficients are required for each zone, as well as the location of the moment axis, and the ISPAN variable which is used to set the span-wise coordinate (see NSU3D input).