3.11. Restart and Output

3.11.1. Graphical Outputs

In this Section we will describe the various plotting capabilities available in the code. All the variables regarding graphical outputs are in the NAMELIST group grafic, with one exception that is the time interval between plots pltdt, which control the plotting frequency. This variable is in NAMELIST group xput:

pltdt Time interval (s) between successive sets of 1D profile, 2D contour, and 2D and 3D vector plots in profile.nc, if such plots are required. Default=1.

When there is only one entry in pltdt, it is treated as a scalar constant, i.e., a single time interval, but when there are multiple entries, they are associated in pairs with the odd elements representing the time interval and the even elements representing the upper time limit for that particular time interval. If the current time exceeds the last time specified in the array pltdt, the last maximum time step size will be held for the remaining simulation time up to twfin.

An example is shown here for the maximum time step, pltdt, as it is read in the NAMELIST xput:

$xput

...

; VALUE TIME

pltdt = 0.5, 10000.1,

0.6, 20000.1,

0.7, 30000.1,

0.8, 40000.1,

0.5, 50000.1,

0.6, 60000.1,

0.75, 70000.1,

1.0, 90000.0,

...

$end

For this example, the plotting time interval is held constant at 0.5 s for (0 <= time < 10000), 0.6 s for (0 <= time < 20000), and so on.

3.11.1.1. Time-History Plots

Function: Defining the locations of points used to record the time history results of the solution variables.

There are two methods for defining Time History Plot:

  1. Given a point, then calculate automatically which cell the point is located, and output ( i, j, k) values of this cell.

  2. Input the (i, j, k) of mesh cell directly.

Input Array: Time-history plots of selected solution variables can be requested with the following input array variable:

thp(1,*) i mesh index (cell number or cell face number)

thp(2,*) j mesh index (cell number or cell face number)

thp(3,*) k mesh index (cell number or cell face number)

thp(4,*) Block number (must be 1 for GASFLOW-MPI).

thp(5,*) Solution variable to be plotted. Choose one of the character strings (enclosed in single quotes) given in the following table

Symbol

Quantity to be plotted

'pn'

Pressure.

'rn'

Mixture density.

'rsn'

Species density.

'cmn'

Cell mass.

'sien'

Specific internal energy.

'un'

i- (x- or r-) velocity component.

'vn'

j- (y- or θ-) velocity component.

'wn'

k- (z-) velocity component.

'tk'

Fluid temperature, K.

'mf'

Species mass fraction.

'vf'

Species volume fraction.

'vmag'

Velocity magnitude.

'mdotx'

Mass flow rate in i- (x- or r-) direction.

'mdoty'

Mass flow rate in j- (y- or θ-) direction.

'mdotz'

Mass flow rate in k- (z-) direction.

'vdotx'

Volume flow rate in i- (x- or r-) direction.

'vdoty'

Volume flow rate in j- (y- or θ-) direction.

'vdotz'

Volume flow rate in k- (z-) direction.

'delpx'

Pressure difference in i- (x- or r-) direction.

'delpy'

Pressure difference in j- (y- or θ-) direction.

'delpz'

Pressure difference in k- (z-) direction.

'delt'

Time-step size (does not depend on spatial location).

'diffp'

Cell pressure minus an ambient or reference pressure defined by pamb0 (default = 1.01325 x 1e6 dynes/cm2) in NAMELIST group xput.

'pstag'

Stagnation pressure (ρ|u|2/2) minus pamb0.

'mu'

Effective (molecular and turbulent) viscosity.

'nu'

Effective viscosity divided by fluid density.

'tke'

Turbulent kinetic energy, only valid if tmodel has been set to 'ke'.

'eps'

Rate of dissipation of turbulent kinetic energy, only valid if tmodel has been set to 'ke'.

'tsat'

Saturation temperature, K.

'psat'

Saturation pressure, dynes/cm2.

'rh'

Percent relative humidity.

'tc'

Fluid temperature, °C.

'difft'

Fluid temperature minus the saturation temperature.

'insht'

Instrument cooling heat removal.

'pvxi'

Combustion progress variable.

'mach'

Mach number.

'presmax'

Footprint of maximum pressure

'sigmain'

Local Sigma index value in each cell (used for thp, c2d, p1d and gfd*.nc only. Do not use it for htthp …) idetchar should be greater than zero.

thp(6,*) Gas species name (symbol representing one of the species defined by mat in NAMELIST group xput) enclosed in single quotes. This variable is used only if thp(5,*) has been set to 'rsn', 'mf', or 'vf'.

The variables thp(1,*), thp(2,*), and thp(3,*) are i-, j-, and k-indices, respectively, that define the spatial location where a solution quantity is to be plotted as a function of time. The logical indices can either represent cell number or cell face number, depending on the quantity being plotted. The reason for this is that in GASFLOW-MPI components of velocity, mass flow rate, volume flow rate, and pressure gradient are defined at cell faces in the corresponding direction, while all scalar quantities such as densities, pressure, temperature, etc., are defined at cell centers for cell numbering convention.

The frequency at which time-history data are written ans subsequently plotted is controlled by the following variable:

thdt Time interval (s) at which time-history data are written to plothist.nc. Default = 1e100.

  • The user can also write the surface temperature of a solid heat structure as a function of time into plothist.nc. This is done via the following input variable:

htthp(1,*) i-index of fluid cell in contact with the heat structure.

htthp(2,*) j-index of fluid cell in contact with the heat structure.

htthp(3,*) k-index of fluid cell in contact with the heat structure.

htthp(4,*) Block number (must be 1 for GASFLOW-MPI).

htthp(5,*) Heat structure type. Choices are 'slab' for slab heat structure or 'sink' for sink heat structure or 'wall' for wall heat structure.

htthp(6,*) The side of the fluid cell which coincides with the solid surface whose temperature is to be plotted. This entry is only used if htthp(5,*) has been set to ‘slab' or 'wall', because sink structures are assumed to be distributed in the fluid cell. Choices are: 'east' (+i side of fluid cell), 'west' (-i side of fluid cell), 'north' (+j side of fluid cell) 'south' (-j side of fluid cell) 'top' (+k side of fluid cell) or 'bottom' (-k side of fluid cell).

Of course heat-transfer calculations have to be invoked (by setting ihtflag = 1 in NAMELIST group rheat) for these definitions to be effective.

  • Time dependent liquid film thickness (cm) on all GASFLOW-MPI structures can be plotted in a similar manner. This allows the user to monitor the time dependence of condensation and/or vaporization through dryout from any surface type in the form of a time-history plot. The input is located in NAMELIST rgrafic, and it is defined with the filmthp statement:

filmthp(1,*) i-index of fluid cell in contact with heat transfer structure.

filmthp(2,*) j-index of fluid cell in contact with heat transfer structure.

filmthp(3,*) k-index of fluid cell in contact with heat transfer structure.

filmthp(4,*) block number (must be 1 for GASFLOW-MPI).

filmthp(5,*) Heat structure type.

filmthp(6,*) Side of fluid cell in contact with heat transfer structure (not needed for sink heat structures).

  • Time dependent energy fluxes due to condensation/vaporization (ergs/(cm^2*s)) on all GASFLOW-MPI structures can be plotted in a similar manner. This allows the user to monitor the time dependence of phase-change heat transfer to or from any surface type in the form of a time-history plot. The input is located in NAMELIST rgrafic, and it is defined with the condfthp statement:

condfthp(1,*) i-index of fluid cell in contact with heat transfer structure.

condfthp(2,*) j-index of fluid cell in contact with heat transfer structure.

condfthp(3,*) k-index of fluid cell in contact with heat transfer structure.

condfthp(4,*) block number (must be 1 for GASFLOW-MPI).

condfthp(5,*) Heat structure type.

condfthp(6,*) Side of fluid cell in contact with heat transfer structure (not needed for sink heat structures).

  • Time dependent energy fluxes due to convective heat transfer (ergs/(cm^2*s)) on all GASFLOW-MPI structures can be plotted in a similar manner. This allows the user to monitor the time dependence of convection heat transfer to or from any surface type in the form of a time-history plot. The input is located in NAMELIST rgrafic, and it is defined with the convfthp statement:

convfthp(1,*) i-index of fluid cell in contact with heat transfer structure.

convfthp(2,*) j-index of fluid cell in contact with heat transfer structure.

convfthp(3,*) k-index of fluid cell in contact with heat transfer structure.

convfthp(4,*) block number (must be 1 for GASFLOW-MPI).

convfthp(5,*) Heat structure type.

convfthp(6,*) Side of fluid cell in contact with heat transfer structure (not needed for sink heat structures).

  • Time dependent energy fluxes due to radiation heat transfer (ergs/(cm^2*s)) on all GASFLOW-MPI structures can be plotted in a similar manner. This allows the user to monitor the time dependence of radiation heat transfer to or from any surface type in the form of a time-history plot. The input is located in NAMELIST rgrafic, and it is defined with the radfthp statement:

radfthp(1,*) i-index of fluid cell in contact with heat transfer structure.

radfthp(2,*) j-index of fluid cell in contact with heat transfer structure.

radfthp(3,*) k-index of fluid cell in contact with heat transfer structure.

radfthp(4,*) block number (must be 1 for GASFLOW-MPI).

radfthp(5,*) Heat structure type.

radfthp(6,*) Side of fluid cell in contact with heat transfer structure (not needed for sink heat structures).

Time dependent energy fluxes due to recombination heat transfer (ergs/(cm^2*s)) on all GASFLOW-MPI structures can be plotted in a similar manner. This allows the user to monitor the time dependence of recombination heat transfer to or from any surface type in the form of a time-history plot. The input is located in NAMELIST rgrafic, and it is defined with the qrecfthp statement:

qrecfthp(1,*) i-index of fluid cell in contact with heat transfer structure.

qrecfthp(2,*) j-index of fluid cell in contact with heat transfer structure.

qrecfthp(3,*) k-index of fluid cell in contact with heat transfer structure.

qrecfthp(4,*) block number (must be 1 for GASFLOW-MPI).

qrecfthp(5,*) Heat structure type.

qrecfthp(6,*) Side of fluid cell in contact with heat transfer structure (not needed for sink heat structures).

3.11.1.2. Profile Plots

To define the line along which the profile of the quantity of interest is to be plotted, GASFLOW-MPI uses the concept of points. A line parallel to any of the axes can be defined by two points with the same spatial coordinates in two directions

Points for plotting purposes can be defined with the following input variable:

pnt(1,*) i mesh index.

pnt(2,*) j mesh index.

pnt(3,*) k mesh index.

pnt(4,*) Block number (must be 1 for GASFLOW-MPI).

Once the points have been defined, the user can specify what the 1D profile plots are via the following input variable:

p1d(1,*) Identification number of the first point (the point number is the second index of the corresponding pnt definition).

p1d(2,*) Identification number of the second point (the point number is the second index of the corresponding pnt definition).

p1d(3,*) Solution variable whose 1D profile is to be plotted. Choose one of the symbols (enclosed in single quotes)

p1d(4,*) Gas species name (symbol representing one of the species defined by mat in NAMELIST group xput) enclosed in single quotes. This variable is used only if p1d(3,*) has been set to 'rsn', 'mf', or 'vf'. Instead of a character string representing the species name, a component number (based on the order in which the species is defined in the mat array) can alternatively be entered here.

Note that the first point should not have higher mesh index values than the second point, or an error will result. Consider the following input, which illustrates how to use point definitions to define 1D profile plots:

pnt(1,1) = 3, 4, 1, 1,

pnt(1,2) = 3, 4, 10, 1,

pnt(1,3) = 2, 6, 7, 1,

pnt(1,4) = 15, 6, 7, 1,

p1d(1,1) = 1, 2, 'pn', 0,

p1d(1,2) = 1, 2, 'rsn', 'h2',

p1d(1,3) = 3, 4, 'tk', 0,

Here four points are defined, with the first two and the last two points being “colinear” pairs. Therefore the two pairs of points, 1 and 2, and 3 and 4, can be used to define 1D profile plots. The first profile plot is that of the fluid pressure along the line going from point 1 to point 2. The second profile plot is that of the hydrogen species density along the same line. The third profile plot is that of the fluid temperature along the line defined by points 3 and 4.

In a similar manner, 1D profile plots for certain structural surface characteristics can also be plotted. The user can specify what the 1D surface profile plots are via the following input variable:

p1dsurf(1,*) Identification number of the first point (the point number is the second index of the corresponding pnt definition).

p1dsurf(2,*) Identification number of the second point (the point number is the second index of the corresponding pnt definition).

p1dsurf(3,*) Surface solution variable whose 1D profile is to be plotted. Choose one of the following symbols:

  • ‘condf’ Water vapour energy flux from condensation or evaporation from the given surface, ergs/(cm2*s) (see next input variable).

  • ‘convf’ Convective energy flux for a given surface, ergs/(cm2*s) (see next input variable).

  • ‘filmt’ Film of water on a given surface, cm (see next input variable).

  • ‘htcoef’ Heat transfer coefficient for a given surface, ergs/(cm2*K*s) (see next input variable).

  • ‘massf’ Water vapour mass flux condensing or evaporating from the given surface, g/(cm2*s) (see next input variable).

  • ‘qrecf’ Energy flux for a given recombiner surface, ergs/(cm2*s) (see next input variable).

  • ‘radf’Radiation energy flux for a given surface, ergs/(cm2*s) (see next input variable).

p1dsurf(4,*) Heat structure type. Choices are

  • 'slab', slab heat structure;

  • 'sink', sink heat structure;

  • 'wall', wall heat structure.

p1dsurf(5,*) The side of the fluid cell which is in contact with the heat structure whose surface profile is to be plotted. This entry is only used if p1ds(4,*) has been set to 'slab' or 'wall', because sink structures are assumed to be distributed in the fluid cell. Choices are

  • 'east',+i side of fluid cell;

  • 'west',-i side of fluid cell;

  • 'north',+j side of fluid cell;

  • 'south',-j side of fluid cell;

  • 'top',+k side of fluid cell;

  • 'bottom', -k side of fluid cell.

In problems involving heat transfer, the user can request plotting of the temperature profile in the solid heat structure via the following input variable:

ht1dp(1,*) i-index of fluid cell in contact with the heat structure.

ht1dp(2,*) j-index of fluid cell in contact with the heat structure.

ht1dp(3,*) k-index of fluid cell in contact with the heat structure.

ht1dp(4,*) Block number (must be 1 for GASFLOW-MPI).

ht1dp(5,*) Heat structure type. Choices are

  • 'slab', slab heat structure;

  • 'sink', sink heat structure;

  • 'wall', wall heat structure.

ht1dp(6,*) The side of the fluid cell which is in contact with the heat structure whose temperature profile is to be plotted. This entry is only used if ht1dp(5,*) has been set to 'slab' or 'wall', because sink structures are assumed to be distributed in the fluid cell. Choices are

  • 'east',+i side of fluid cell;

  • 'west',-i side of fluid cell;

  • 'north',+j side of fluid cell;

  • 'south',-j side of fluid cell;

  • 'top',+k side of fluid cell;

  • 'bottom', -k side of fluid cell.

3.11.1.3. 2D Contour

It is often useful to plot the contour of a solution quantity on a plane. Two-dimensional contour plots are defined in basically the same way as 1D profile plots. Two points with the same mesh index in one direction (i.e., a pair of so-called “coplanar” points) are used to define the plane where data are to be taken for the contour plot.

Contour plots can be requested via the following input variable:

c2d(1,*) Identification number of the first point (second index of the corresponding pnt definition).

c2d(2,*) Identification number of the second point (second index of the corresponding pnt definition).

c2d(3,*) Solution variable for the 2D contour plot. Choose one of the symbols (enclosed in single quotes), except 'delt'.

c2d(4,*) Gas species name (symbol representing one of the species defined by mat in NAMELIST group xput) enclosed in single quotes. This variable is used only if c2d(3,*) has been set to 'rsn', 'mf', or 'vf'.

3.11.1.4. Velocity Vector

Using the concept of points, as discussed above for profile and contour plots, the user can also specify velocity vector plots. There are two types of vector plots available. Two-dimensional velocity vector plots show the velocity magnitude and direction on a plane defined by two coplanar points. Three-dimensional velocity vector plots show the velocity magnitude and direction in a volume, which can be specified by defining two points that locate its diagonal vertices. The length of the shaft, the size of the arrowhead, and the color of the vector are made proportional to the velocity magnitude.

To specify 2D velocity vector plots, the user should define the following:

v2d(1,*) Identification number of the first point (second index of the corresponding pnt definition).

v2d(2,*) Identification number of the second point (second index of the corresponding pnt definition).

v2d(3,*) Flag for frame advance. This option (if set to 0) can be used to overlay the vector plot with the next plot for special presentation. However, it is advised that this flag be set to 1 so that the vector plot will appear by itself on a single frame.

3.11.1.5. Graphic and Tabular Particle Data Output

Warning: Lagrangian particle model is not available in current GASFLOW-MPI. Parallelization of particle model will be implemented in future release of GASFLOW-MPI.

Two kinds of graphic output are used to interpret the results of particle computations. One of these displays particles plotted in a perspective view plot of the computational domain. Any combination of particle classes may be selected for each plot. The three-dimensional volume of particles is integrated along each line of sight and plotted onto the two-dimensional plane. Another useful graphic display is the time-history plots of particle number, mass, volume fraction, mass fraction, and mass deposited in selected mesh cells. In addition, the time-history data is written on an output tape, PTHDATA, and is available for examination.

The input parameter definitions are summarized below:

ippka(np) Selects the package (i.e., particle class, size, or deposition plane) to be plotted. The input corresponds to the array mpac definition, given below. Default = 1.

ipvew(np) Viewpoint for particle plot, i.e., viewpoint 'nv' defined in viewcrds. Default = 1. (Input value corresponds with the array pplt(2,100) ).

nap(np) Number of film frame advances between particle plots 'np'. Default = 1.

npplts The number of particle packages (i.e., classes or deposition planes) to be plotted. Default = 0.

pplt(2,100) Perspective plot viewpoint, i.e., the viewpoint 'nv' defined in viewcrds. (Corresponds with ipvew and is used for perspective plots in general).

The following input is for time-history particle plots and is in the grafic NAMELIST group “xput”:

thdt Time increments between time-history data points. Default = 1e+100 s.

pthpt0 Time-history plot initial time (used for runs from restart tapes).

pthp(1,*) i-index of fluid cell.

pthp(2,*) j-index of fluid cell.

pthp(3,*) k-index of fluid cell.

pthp(4,*) Block number.

pthp(5,*) Particle data to be plotted:

pthp(6,*) Particle class (itpcl(n)):

  • =0, all classes;

  • >0, particle class number,

pthp(7,*) Particle size number (itpsz(n)):

  • =0, all sizes for class itpcl(n);

  • >0, particle size number;

pthp(8,*) Particle mass deposited on cell faces (for 'pmd' only):

  • 0, all deposited particles;

  • >0, cell faces designated in array mpac(n)

  • 11, deposited on east face of cell;

  • 21, deposited on west face of cell;

  • 12, deposited on north face of cell;

  • 22, deposited on south face of cell;

  • 13, deposited on top face of cell;

  • 23, deposited on bottom face of cell.

pthp(9,*) The number of each particle cloud monitor which is consistent with n specified in the monitor location xm(n), ym(n) and zm(n).

Procedure to set up prospective view particle plots

  1. Input the selected viewcrds.

  2. Select the number of particle plots wanted, npplts.

  3. Select the particle class number and the class size number or the cell faces with deposited particles that are to be plotted, ippka.

  4. Select the perspective view for each plot from the viewcrds input.

  5. The number of film frames advanced, nap, is typically 1, which is the default value.

Procedure to set up time-history plots

  1. Select the time interval between data points, thdt.

  2. Select the time-history plot initial time, pthpt0.

  3. Select the particle time-history data to be plotted, pthp.

3.11.1.6. Graphical Display of Criteria of FA and DDT

A methodology has been developed to evaluate the safety of ignitor implementation in complex containment geometries. The method consists of the following steps:

  1. determination of bounding H2/steam sources,

  2. high-resolution analysis of the three-dimensional transport calculation,

  3. evaluation of the detonation potential at the time of ignition,

  4. optimization of the ignitor system such that only early ignition and nonenergetic combustion occurs, and

  5. modeling of the continuous deflagration process during H2 release.

To activate this methodology, the user may define multiple rooms in several ways with the iroomdef two-dimensional array. Each room segment volume is defined by eight entries in the iroomdef input array.

iroomdef(1,*) Beginning i mesh index (cell face number).

iroomdef(2,*) Ending i mesh index (cell face number).

iroomdef(3,*) Beginning j mesh index (cell face number).

iroomdef(4,*) Ending j mesh index (cell face number).

iroomdef(5,*) Beginning k mesh index (cell face number).

iroomdef(6,*) Ending k mesh index (cell face number).

iroomdef(7,*) Block number (must be 1 for GASFLOW-MPI).

iroomdef(8,*) Actual room number:

  • >0 implies positive volume;

  • < 0 implies negative volume.

GASFLOW-MPI supports 300 definitions of iroomdef and 25 separate and distinct different rooms.

Example

The utility of the iroomdef input is best demonstrated by an example as follows:

Consider a two-dimensional computational mesh that has 9 fluid cells in the x-direction and 5 fluid cells in the y-direction Figure above. There is a complex-shaped room in this mesh shown by the obstacles.

One way to define this room is

$xput

…

mat = 'h2', 'n2', 'o2', 'h2o', 'h2ol', ; components -> HEM

mobs = 1, 2, 1, 3, 1, 2, 1, 1,

2, 4, 1, 2, 1, 2, 1, 1,

3, 5, 4, 6, 1, 2, 1, 1,

7, 8, 1, 3, 1, 2, 1, 1,

iroomdef = 1, 3, 3, 6, 1, 2, 1, +1,

4, 7, 1, 2, 1, 2, 1, +1,

2, 7, 2, 3, 1, 2, 1, +1,

8, 10, 1, 3, 1, 2, 1, +1,

3, 10, 3, 4, 1, 2, 1, +1,

5, 10, 4, 6, 1, 2, 1, +1,

...

$end

- DDT Characteristics

The Kurchatov Institute has developed a function that relates the detonation cell size to the concentrations of dry hydrogen and steam in air at temperature, T.

where A is the H_2 volume fraction, C is the steam volume fraction and T is the temperature. The coefficients a = -1.13331e+00, b = 4.59807e+01, d = 4.65429e-02, e = 3.59620e-07, f = 9.97468e-01, g = -2.66646e-02, h = 8.74995e-04, i = -4.07641e-02, j = 3.31162e+02, l = -4.18215e+02.

The user has some options concerning hydrogen limits in the iroomdef statements GASFLOW-MPI will process. The two variables in the NAMELIST group graphic are h2lowfl and h2upfl. h2lowfl is an array dimensioned 10 and h2upfl is a constant. These are respectively the lower hydrogen volume fractions and maximum hydrogen volume fraction the user is interested in processing:

h2lowfl(1:10) lower hydrogen volume fraction threshold (default: h2lowfl(1) = 0.04).

h2upfl upper hydrogen volume fraction threshold (default: h2upfl(1) = 0.75).

- Sigma Index Characteristic

Above we describe the implementation of a DDT criterion or index to examine by user defined volumes the time and space sensitivity of hydrogen mixtures to transition from a subsonic flame to a detonation. Another criterion, an index to judge the possibility of a laminar flame becoming turbulent and accelerating, through the so-called sigma criterion or index is also available. KIT has developed a 4 dimensional table, called the sigma criterion table, with the dependent variables H2, H2O, O2 and temperature T.

However, instead of interpolating this 4-dimensional table, an accurate analytic function has been developed so a direct evaluation of the sigma criteria is available. The user can activate plots of the sigma index, defined as

by specifying volumes using the iroomdef statement and

in the GASFLOW xput input stream. When idetchar > 1, the GASFLOW-MPI plothist.nc file will contain sigma index plots for the maximum hydrogen concentration in the cloud, the minimum hydrogen concentration in the cloud, and the average hydrogen concentration in the cloud, where the cloud is defined as all computational volumes in the specified room which are combustible. Cloud combustible limits are judged using the Kumar criterion.

This graph and the associated tabular values listed in the following Table are valid for lean hydrogenoxygen mixtures, i.e., when [h_2] < 2[o_2], while for rich hydrogen-oxygen mixtures, [h_2] >= 2[o_2], sigma critical is constant at 3.75.

3.11.1.7. Printed Output

In addition to graphical outputs, GASFLOW provides printed outputs for each calculation. A printed output file is cyclinfo, which lists iteration and time-step information at each computational time cycle.

The main printed output file is gfout. In the beginning of the file, the code version number and the date of the run are printed. Then the values of main input variables are listed, followed by tables showing mesh coordinates and cell spacing (edge-to-edge and center-to-center). The plotting output specifications are then echoed. Next, the calculated fluid velocity (all three components), pressure, and density at each cell are listed at selected time intervals. This time interval is defined by the following variable in NAMELIST group xput:

prtdt Time interval (s) between printing of the fluid solution field (all velocity components, pressure, and density) to the output file gfout. Default = 1000.

GASFLOW does however allow the user to dynamically specify the time interval between output, prtdt, by making use of the fact that prtdt is an array dimensioned 20.

3.11.2. Output to Terminal

Besides graphical and text file outputs, GASFLOW also writes output to a terminal. This output is intended to help the user monitor the calculation as it is being carried out. Any error messages will also be given here. After some banner messages that include identification of code version, the time-step and pressure iteration information is printed. The terminal output is printed at a selected frequency, which is defined by the following input variable in NAMELIST group xput:

cttyfreq Number of cycles between printing of time-step and pressure iteration information to the cyclinfo file. Default = 1

ittyfreq Number of cycles between printing of time-step and pressure iteration information to the terminal. Default = 20.

When calculation is finished, the code prints to the terminal the same timing information as in the output file gfout (discussed at the end of the above section). In addition, it reports the number of restart dump files written and the number of pages (or frames) generated in the plot file pgf.

3.11.3. Restart

Because GASFLOW-MPI is capable of solving complex, large problems, it may take a large amount of computer time to finish a problem. Therefore, the code provides a restart capability so that a long calculation can be divided into a series of shorter runs. A restart dump file is always produced at the end of each run. However, the user can specify that additional restart files be written at selected time intervals. This is done via the following input variable in NAMELIST group xput:

tddt Time interval (s) at which restart dump files are written. Default = 10.

GASFLOW-MPI does however allow the user to dynamically specify the time interval between restart dumps, tddt, by making use of the fact that tddt is an array dimensioned 20. When there is only one entry in tddt, it is treated as a scalar constant, i.e., a single time interval, but when there are multiple entries, they are associated in pairs with the odd elements representing the time interval for restart dump output and the even elements representing the upper time limit for that particular time interval. If the current time exceeds the last time specified in the array tddt, the last restart dump output twill be twfin.

Therefore, one restart dump file, called gfd1, will be written if the problem end time (specified by twfin in NAMELIST group xput) is less than tddt. If twfin is larger than tddt, then gfd1 will be the restart file written at time tddt. The next restart files, gfd2, gfd3, etc., will be written at times that are multiples of tddt. Hence, the restart file that contains the final solution will have the name gfdn, where n is the total number of restart files produced.

To specify that a run is to begin from the solution stored in a restart dump file, the user should define the following variable in NAMELIST group xput:

nrsdump Number that appears in the name of the restart dump file that is to be read in. For example: 0. new problem, not a restart run (default); 1. read from restart file gfd1; 2. read from restart file gfd2.

The code will check if the number of the occupied processors during restart calculation is the same as the one used in the previous calculation. To restart the calculation using various number of processors, the user should define following variable in NAMELIST group xput.

idprst Option of using different number of processors during the restart. For example: 0. using the same number of processors (default); >0. using different number of processors.

Previous3.10. Physical ModelsNext3.12. GASFLOW Parallelization

Last updated

Was this helpful?