### 13.2.4. Input and Output Data Files for Vista TF

The following sections describe the input and output files for `VistaTF.exe`.

- The Auxiliary File with the Default Name: vista_tf.fil
- Overview of Input Files
- Overview of Output Files
- Specification of the Control Data File (*.con)
- Specification of the Geometry Data File (*.geo)
- Specification of Aerodynamic Data File (*.aer)
- Specification of Correlations Data File (*.cor)
- Specification of the Real Gas Properties Data File (*.rgp)
- Specification of the Output Data File (*.out)
- Specification of the Text Data File (*.txt)
- Specification of the CFD-Post Output File (*.csv)
- Specification of Convergence History Data File (*.hst)

#### 13.2.4.1. The Auxiliary File with the Default Name: vista_tf.fil

You specify the input data and output data file names in an auxiliary data file that has the default filename `vista_tf.fil`. This auxiliary file in turn must contain the necessary filenames for the input and output files in the following order and form:

    Version number Version 3.0 or Version 4.0 (or newer)
    control datafile name             prefix.con
    geometry datafile name            prefix.geo
    aerodynamic datafile name         prefix.aer
    correlation datafile name         prefix.cor
    results output file name          prefix.out
    convergence history filename      prefix.hst
    text data output file name        prefix.txt
    Cfx-post output file name         prefix.csv
    restart datafile name             prefix.rst
    Interface output file             prefix.int
    Real gas properties data file     prefix.rgp

This auxiliary file can have another name if this name is passed to the program through a command-line argument to specify the auxiliary filename, as described in Running Vista TF from the Command Line. If no command-line argument is specified in this way, then the program assumes that the file has the name `vista_tf.fil`.

Note that the prefixes need not be identical for a given run. In fact this is not usually the case. An example of a `vista_tf.fil` file is:

    Version 4.0
    standard_control.con
    impeller_XYZa.geo
    design_point.aer
    radial_impeller.cor
    results.out
    history.hst
    impeller.txt
    cfx_post.csv
    restart.rst
    stream.int
    real_gas_CO2.rgp

Note that the program also produces and uses other files in special situations as outlined below; their names do not need to be specified separately because they are determined by the program from the names of other files in this list. The data files, results files, and the file `vista_tf.fil` are usually in the same directory, together with the VistaTF.bat file and the TECPLOT layout files. If the history (`.hst`) file already exists in the working directory before the program is run, it will be overwritten. If the restart (`.rst`) file already exists in the working directory before the program is run, it will be overwritten only if the solution has converged or reached the maximum number of iterations that you have specified. If the output (`.out`) file and the plot files (`.txt`, and `.csv`) already exist in the working directory before the program is run, they will be overwritten. The program will not prompt you for permission to overwrite these files.

#### 13.2.4.2. Overview of Input Files

Four input data files are always needed:

    Control data file (.con)
    Geometrical data file (.geo)
    Aerodynamic data file (.aer)
    Correlations data file (.cor)

A fifth input file will be used if it is available and if you specify that it should be used:

    Restart data file (.rst)

A sixth input file is needed if the calculation requires real gas properties using the Aungier-Redlich-Kwong (ARK) equation of state:

    Real Gas Property data file (.rgp)

The division of the input data into separate files provides a simple and clear way to vary or retain the annulus geometry, the aerodynamic conditions, the blade element data, or the correlations being used, without changing all the files in use. Typically during the design process, you will change the `.geo` file to examine a new geometry, and the `.aer` file to examine new operating points or boundary conditions, and you will leave the `.con` and `.cor` files untouched once you have configured their settings to meet the requirements.

The data specified in the individual files is structured to be as logical as possible, and retains the same structure even if there is a change in the input parameters. The format of the input data is organized in such a way that most of the input files retain exactly the same format with the same parameters in the same order, without the need for a change in structure when the program changes or when the computation changes. The structure may appear more complicated than necessary, but this arises from the requirement that ultimately the program should calculate all types of turbomachinery in single stage and multistage configurations, both as ductflow and as throughflow calculations. The values of the parameters defined in the control file determine the type of data required in the other files.

An attempt has been made to include a built-in “expert system” in the program. For example, the program is able to identify whether a particular blade row is a radial compressor impeller or a radial turbine inlet guide vane (from the geometry). In general many parameters may be set to zero and the program selects the value it deems appropriate. “Expert parameters” allow you to override the selections that the program would automatically make.

The functions of the six input data files are summarized next:

##### Control Data File (.con)

This is a short file giving an identifier for the file (title and headers) and control information and constants defining such choices as the number of streamline calculating planes, the convergence tolerance, the relaxation factors, the number of operating points, and the number of speed lines. Various “expert” parameters are also specified in this file. Also specified in this file are the planes and stations for which output information is required, and the level of detail requested on these planes.

To make the program easier to use, you can specify many of these parameters as 0.0, 1.0, or 0, and the program will then make a sensible choice of the value for the parameter concerned, so that typically you are only concerned with two or three parameters in this file. The control parameters that determine the selection of particular numerical models are also defined in this file, for example the type of span-wise mixing or the model for blade row choking. In general, this input file does not need to be changed from run to run, except if a different number of points or speed lines are to be calculated.

##### Geometry Data File (.geo)

The geometry data file contains the dimensions of the annulus in terms of the axial and radial coordinates of the quasi-orthogonal calculating planes at hub and casing, and information to identify the type of calculating station (such as duct, stator, or rotor). Calculating planes can represent regions of a duct or blades (leading edges, trailing edges, and internal stations) and can be curved or linear. For linear calculating planes (which, by definition, are straight in the meridional plane), details of the geometry of each calculating plane are specified at only two points and intermediate geometric values are interpolated linearly from these, whereas curved planes require more points to be specified across the span. For curved duct calculating planes, this geometry data specifies the co-ordinate points along the curved calculating plane. In blade regions, the coordinates of the calculating plane, together with information about the blade geometry at this location, must be specified (including the number of blades, blade lean angles, and blade thickness). For each blade row, additional geometrical parameters can be specified that might be relevant for the correlations (such as the throat area, the location of the throat, the location of maximum camber, the maximum thickness, the trailing edge thickness, and the tip clearance).

In general, the geometry data file will be generated automatically using a blade geometry definition program (such as ANSYS BladeEditor, or Vista GEO of PCA). A geometry conversion program is available to convert data from the BladeGen meanline `RTZT` output format into the `.geo` file format for the throughflow program and this has been tested for radial impeller rotors and stators, and axial stator and rotor blade rows (compressors and turbines); see Appendix G: The RTZTtoGEO Program. Other custom tools are available for conversion of geometrical data from specific formats into the Vista TF `.geo` file format, and others can be prepared as required.

##### Aerodynamic Data File (.aer)

The aerodynamic data file contains the definition of the fluid, boundary conditions, and operating data such as inlet conditions and rotational speed. It includes parameters related to aerodynamic models for the mean stream surface description, and the spanwise mixing coefficient.

##### Correlation Data File (.cor)

The correlation data file provides details of control parameters and empirical constants and data for the particular choice of empiricism that has been chosen. The method allows a general specification of losses, flow angle, and blockage for all calculating planes and across the span through the definition of the spanwise variation of these parameters at particular quasi-orthogonal locations and for particular blade rows. Ultimately, in many cases, if default values of zero are chosen for these parameters then the program should automatically select appropriate correlations and make its own choice of correlation parameters.

##### Restart Data File (.rst)

This restart file contains some key information from a previous calculation in a non-dimensional form. Note that the restart file can be for different flow conditions and for a different geometry but it must have the same number of quasi-orthogonal calculating stations and streamlines as the current calculation. If the restart data file has been generated from a calculation with similar geometry and flow conditions as the current calculation, it provides a much better initial estimate of the flow and the streamline positions than the first estimate generated internally within the program, promoting more rapid convergence. A restart with unchanged conditions and geometry will generally have a meridional velocity error of less than 2% and will converge almost immediately, except for choked flows where more iterations are needed. Convergence with the restart file is never immediate, even with unchanged geometry and flow conditions, because not all of the solution is saved to the restart file, and so some data needs to be regenerated over a few iterations of the solution. For small changes in flow conditions or geometry, the number of iterations when using the restart file is generally less than 50% of that required when starting from the program's own first estimate.

An existing restart file cannot be used if the number of streamlines or quasi-orthogonals is changed. The program recognizes if the number of streamlines or quasi-orthogonals has been changed and makes a new cold start in this case.

You do not have to be concerned with the content and format of the restart file because it is generated automatically at the end of a run of the program, and is automatically used if it is available. No further information is provided here with regards to the content of the restart file. In some situations where it is difficult to obtain convergence, the restart file can be used to store results for a converged operating point (at lower speed, for example) and then the required operating condition can be obtained by starting from the restart file with new flow conditions. In other cases where an un-converged solution has been stored in the restart file, it is possible that using the restart file can be disadvantageous as a starting point for a new simulation, and a cold-start may be better.

The restart file can also be used for reducing the number of computations when the program is coupled to an optimizer. In this case, an additional restart file with the name `best_restart.rst` is used and generated.

##### Real gas property data file (.rgp)

This file contains coefficients and data required to define the gas properties of a real gas using the Aungier-Redlich-Kwong cubic equation of state. Note that standard files have been prepared for the most usual gases. Note this file does not have the same format as the typical ANSYS `.rgp` real gas property data files.

#### 13.2.4.3. Overview of Output Files

The program always creates the following three output files:

- Results output file (`.out`)

- Convergence history file (`.hst`)

- Restart data file (`.rst`)

In addition, when running the program for a single calculation point at a single speed, the program can create the following output files of tabular data for plot and display purposes, depending on the value of the parameter `i_display` in the control file:

- Several comma-separated-variable output files for CFD-Post (`.csv`)

- Several text output files in a format suitable for Tecplot (`.txt`)

There is one CFD-Post output file for a calculation with no blade rows and four additional files for each blade row. There are two Tecplot output files for a calculation with no blade rows, and an additional file for each blade row.

In addition, the program can create a data file containing data in a specific format for use with other programs:

- Interface output file (`.int`)

and a file that can be produced as an alternative to the screen output:

- Screen output file (`screen.scn`)

If the program is used to calculate a performance map, the above output files are not produced, and many details of the output file are omitted and replaced by a listing of the map data.

The functions of the output data files are summarized next.

##### Results Output File (.out)

In single point calculations, this contains rudimentary details of the data used for the calculation and the results of the calculation at every plane and radial station for which output has been requested. In map predictions, this file contains the computed performance map. For more information, see Specification of the Output Data File (*.out).

##### Convergence History File (.hst)

This contains a recording of the input data, followed by details of the convergence of the main iterative procedures, and extensive details of the terms in the radial equilibrium equation for each stream tube and calculating plane. It is rare for this to be examined in any depth, but this can be useful to identify problems if the solution fails to converge. For more information, see Specification of Convergence History Data File (*.hst).

##### Restart Data File (.rst)

This restart file stores information from a converged calculation in a non-dimensional form. It provides a much better initial estimate of the flow and the streamline positions than the first estimate generated internally within the program. In most cases, it reduces the calculation time for a calculation with slightly modified geometry or changed aerodynamic data by more than 25%. If an existing restart file is available, it will be overwritten.

##### Comma Separated Variable Output Files for CFD-Post (.csv)

Depending on the value of `i_display` in the control file, the following files are produced:

- `prefix.csv`

- `global_prefix.csv`

together with four additional files produced for each blade row from 1 to n:

- `row_0n_hub_prefix.csv`

- `row_0n_mean_prefix.csv`

- `row_0n_tip_prefix.csv`

- `row_0n_loading_prefix.csv`

The first file (`prefix.csv`) contains key results of the calculation at every calculating plane and streamline in a form that can be used for setting up a meridional contour plot of the results. The second contains a summary of the global performance and reference parameters for the calculation. The additional four `.csv` files are produced for each blade row in the calculation. These contain the same information as in the row data from the `.txt` files, but separated into hub, mean, and tip streamline data, which is information along the blade calculating station from leading to trailing edge on the hub, mean, and tip streamlines. The additional file contains spanwise variation of data. This can be used to define typical blade loading diagrams and incidence plots for each blade row.

Even if no `.csv` file is required, the `prefix.csv` file must be specified in the `vista_tf.fil` file.

For more information, see Specification of the CFD-Post Output File (*.csv).

##### Text Data Output Files for Tecplot (.txt)

Depending on the value of `I_display` in the control file, the following files are produced:

- `prefix.txt`

- `test_prefix.txt`

together with one additional file produced for each blade row from 1 to n:

- `row_0n_prefix.txt`

The first file (`prefix.txt`) contains key results of the calculation at every calculating plane and streamline in a form that can be used for setting up a meridional contour plot of the results, using Tecplot software. This is an ASCII file which is formally correct for presenting the results in graphical form with the plot processing software Tecplot, but can be used by other plot systems (such as Excel) with appropriate conversion or macros. A standard layout file for Tecplot (`flowfield_2d.lay`) has been prepared for typical meridional plots from Vista TF calculations. There are no macros included in this so this may need some adjustment for a typical case (scale of axes, level of contour values, and so on). The second text file (`test_prefix.txt`) contains the grid of the initial estimate of the streamlines and quasi-orthogonals. This can be useful for debugging purposes and can be used to plot the initial grid of an un-converged calculation to identify any specific problems with this. The additional `.txt` files are produced for each blade row in the calculation (`row_0n_prefix.txt` where `n` is the number of the blade row from the inlet). These can be used to define typical blade loading diagrams and incidence plots for each blade row. The Layout files for Tecplot that have been prepared in advance assume that the `.txt` file has the prefix “`impeller`”.

Even if no `.txt` file is required, the `prefix.txt` file must be specified in the `vista_tf.fil` file.

For more information, see Specification of the Text Data File (*.txt).

##### Interface Output Files (.int)

If you request the generation of an interface file for another analysis program then the appropriate files are also generated. The first use of this has been established to allow a summary of the results to be obtained as input to an optimizing software system. An option allows the streamline locations to be printed. Even if no interface file is required, the `.int` file still must be specified in the `vista_tf.fil` file.

##### Screen Output Files (screen.scn)

In normal operation, the progress of the program can be seen on the screen. If the command line includes a parameter `-silent`, the screen results will be written to a separate file called `screen.scn` and not to the screen. If this parameter is not present, the output goes to the screen. If a name follows this parameter on the command line, the screen results are printed to a file with this name.

#### 13.2.4.4. Specification of the Control Data File (*.con)

The control data file includes lines of text that have no function other than to help you to identify the parameters defined here. Note that if values are set to 0.0 or 0 then standard values are used, so typically you do not have to worry about this input. If zero values are specified for some parameters then the values actually selected by the program are written to the output file. Standard forms of this file are available for editing to meet the specific requirements, whereby in most cases no modification of the file is necessary. An example of a control data file is given in Appendix C: Example of a Control Data File (*.con).

Section 1: Character strings identifying the control data (max 72 characters/line)

  The syntax is:

      Character string - title(1)
      Character string - title(2)
      Character string - title(3)

Section 2: Integer control parameters

  The syntax is:

      n_sl   max_it_main   max_it_mass   n_points   n_speeds   n_reserve

  Parameter | Description
  --- | ---

  `n_sl`

  Number of meridional streamlines

  Notes:

  - Must be an odd number so that there is always a mid streamline.

  - Typically n = 9 or 17. If `n_sl` = 0, then 9 will be used.

  - Maximum `n_sl` = `max_n_sl` = 29.

  - If the mixing model is being used, (`i_mix` > 0 in section 4) then there has to be a minimum of 9 streamlines.

  `max_it_main`

  Maximum number of iterations of the main streamline curvature loop in the iterative method.

  Notes:

  - Typically specified as 500 but fewer are generally needed for simple radial compressor calculations to attain convergence.

  - If `max_it_main` < 4 then `max_it_main` = 4, so that at least 4 iterations are always done as a minimum.

  - If `max_it_main` = 0 then `max_it_main` = 500.

  - If the flow reaches the convergence limit before the maximum number of iterations is reached then the calculation is automatically stopped earlier.

  `max_it_mass`

  Maximum number of iterations for internal mass flow loop at each quasi-orthogonal calculating station.

  Notes:

  - Typically 10 and if `max_it_mass` = 0, then `max_it_mass` = 10.

  - If `max_it_mass` < 5 then `max_it_mass` = 5; experience shows that this is a sensible value.

  - If `max_it_mass` > 20 then `max_it_mass` = 20.

  - If the mass flow convergence tolerance at a particular quasi-orthogonal is reached before the maximum number of iterations are completed then mass flow iteration is stopped early.

  `n_points`

  Number of points to be calculated along each speed line.

  Notes:

  - If set to 0 or 1, then a single point is calculated.

  - Maximum number of points is 11.

  - If set to a value greater than 11, then a value of 11 will be used.

  `n_speeds`

  Number of speed lines to be calculated.

  Notes:

  - If set to 0 or 1, then a single speed line is calculated.

  - Maximum number of speed lines is 11.

  - If set to a value greater than 11, then a value of 11 will be used.

  `n_reserve` | A further integer parameter not currently used but reserved for the possibility of defining additional data related to the map prediction (stagger schedule, bleed schedule, etc.).

  Note: The last three parameters were not needed or used prior to version 4.0 of the Vista TF solver (which is the internal solver version number for Vista TF as provided with Release 15.0 of ANSYS software). If the `vista_tf.fil` file being used was prepared for use with version 2 with no first line containing the version number, or was prepared for version 3 with the string “Version 3.0” in the first line, then these parameters still do not need to be specified. This allows backwards compatibility, ensuring that earlier versions will still run. These parameters will only be used if the first line of the `vista_tf.fil` file contains the string “Version 4.00” (or newer) in the first line. However, it is recommended that all files include these additional parameters even if they are not used.

Section 3: Integer control parameters that control input and output data

  The syntax is:

      i_print_plane   i_print_level   i_progress   i_display   i_restart   i_interface

  Note that setting all of these parameters to 0 gives a standard form of output.

  Parameter | Description
  --- | ---

  `i_print_plane`

  Determines the quasi-orthogonal calculating planes at which data is output into the results file.

  = 0, as `i_print_plane` = 4

  = 1, output at no planes

  = 2, data at inlet and outlet planes only

  = 3, data at leading edges and trailing edges and inlet and outlet planes only

  = 4, data at all planes

  Note:

  The extent of the data printed at each plane is determined by `i_print_level`.

  `i_print_level`

  Determines the level of output data printed into the results file at each output plane.

  = 0, standard output (as `iprint_level` = 3)

  = 1, very limited data at each plane

  = 2, generous level of data at each plane

  = 3, extensive data at each plane

  Note:

  The planes at which output is available are defined by the parameter `i_print_plane`.

  `i_progress`

  Determines the extent of intermediate data that is printed to the various files.

  - If `i_progress` = 0 then no intermediate information is printed.

  - If `i_progress` = 1 then intermediate progress of the iterations are printed to the history file.

  - If `i_progress` = 2 then data is printed to the history file and to the screen.

  `i_display`

  Determines extent of tabular data output which is prepared for displaying the results with other plot and post-processing tools:

  Notes:

  - If `i_display` = 1, then no plot files are produced.

  - If `i_display` = 0 then the output files of type .txt are produced for display of the results with Tecplot.

  - If `i_display` = 2, then a comma separated variable file with extension `.csv` is produced for display of the results with CFD-Post.

  - If `i_display` = 3, then both `i_display` = 0 and 2 above are activated.

  - Other output formats can be incorporated as requested.

  `i_restart`

  Determines whether the restart file should be used and whether the results will overwrite the restart file contents.

  Notes:

  - If `i_restart` = 0, the restart file (`prefix.rst`) will be used automatically if it is present (a warm start) and its content will be overwritten automatically at the end of a normal calculation. Note that this also overwrites the restart file even if the iterations are not converged, so that a second start with the same number of iterations starts with a better approximation. This is the normal way to use the program. The restart file includes the number of quasi-orthogonals and streamlines. If `i_restart` = 0 and this number has changed then the program makes a cold start with its own estimate of initial conditions (as in `i_restart` = 1).

  - If `i_restart` = 1 the restart file (`prefix.rst`) will not be used even if it is available and the program will set up its own initial conditions (a cold start). The content of the restart file will be overwritten as under 1 above. This is not generally recommended but can be useful in debugging difficult cases. This is equivalent to deleting the existing restart file and using option 1 above.

  - `i_restart` = 2 and 3 are special options for running the program when coupled to an automatic optimizer. In these cases the use of a good restart file reduces the number of iterations needed and brings a reduction in calculating time. Unfortunately some of the geometries being examined may be poor and so it is inadvisable to overwrite the restart file with poor results. If `i_restart` = 2 then the file runs with a restart file called `best_restart.rst` and writes the results on to `prefix.rst`. If `i_restart` = 3 then the file runs with a restart file called `best_restart.rst` and also writes the results on to the same file `best_restart.rst`. In both cases if the restart file `best_restart.rst` is not present then the internal initial estimate is used (a cold start).

  `i_interface`

  Determines the type of output interface file that is generated.

  Notes:

  - If `i_interface` = 0 then no output interface file is generated.

  - If `i_interface` = 1 then the `prefix.int` file contains a summary of the results for use in radial compressor optimization.

  - If `i_interface` = 2 then the `.int` file contains the coordinates of the streamlines of the calculation.

  - If `i_interface` = 3 then the `.int` file contains the coordinates of the streamlines of the calculation in a format suitable for the stream file of the blade-to-blade program MISES.

Section 4: Integer control parameters for various models and reference parameters

  The syntax is:

      i_expert   i_flow   i_fluid   i _inbc   i_mass   i_mix   i_ree

  Parameter | Description
  --- | ---

  `i_expert`

  Allows special calculations to be carried out making use of development features of the program. Normally you would set the value of this parameter to 0 or 1, but other expert features of the program may be modified with this control parameter. Each digit of the parameter has an influence on its effect.

  Notes:

  - The last digit controls the choke calculation mode. Using a value of zero for the last digit causes the choke mass flow limitation to be eliminated which may be more robust in difficult cases. Calculations of new cases should start in this mode.

  - Using a value of 1 for the last digit, enables the choke mass flow limitation calculation. This requires exact data for the throat areas to be specified and should only be used if this is available. It is necessary to set this value to 1 when using iteration to pressure ratio in choked stages.

  - The second-last digit controls the blending function calculation for the deviation between the blade angle and the flow angle as follows:

    0 - Turbines use departure angle at the leading and trailing edge ends, Compressors use swirl at the leading edge and departure angle at the trailing edge.

    1 - Turbines and compressors use the departure angle for the leading and trailing edges.

    2 - Turbines and compressors use departure angle at the trailing edge and relative swirl at the leading edge.

    3 - Turbines and compressors use departure angle at the trailing edge and the absolute swirl at the inlet.

    4 - Compressors use swirl at the leading edge and departure angle at the trailing edge; turbines use swirl at the outlet and departure angle at the leading edge.

    5 - Compressors use swirl at the leading edge, departure angle at the trailing edge; turbines use swirl at the trailing edge and departure angle at the leading edge.

  `i_flow`

  Determines the input definition for the reference flow parameters (which are input in `.aer` file).

  Notes:

  - `i_flow` = 0 to 4 is for a calculation with a specified mass flow. `i_flow` = 5 to 9 is for a calculation with a specified pressure ratio. See below.

  - `i_flow` = 0 then `ref_mach`, `ref_phi`, and `ref_d`, are specified, but if `ref_mach` > 3 then it is interpreted as `ref_u`, so this is equivalent to `ref_u`, `ref_phi`, and `ref_d`.

  - `i_flow` = 1 then `ref_n`, `ref_mass`, and `ref_d` are specified.

    Note: If there is more than one spool in the calculation with different rotational speeds, then this is taken into account as follows:

    - If `i_spool` = 2 and `i_flow` = 1 then `ref_n1`, `ref_n2`, `ref_mass`, and `ref_d` are specified.

    - If `i_spool` = 3 and `i_flow` = 1 then `ref_n1`, `ref_n2`, `ref_n3`, `ref_mass`, and `ref_d` are specified.

  - `i_flow` = 2 then `ref_n`, `ref_volume`, and `ref_d` are specified.

  - `i_flow` = 3 then `ref_u`, `ref_mass`, and `ref_d` are specified.

  - `i_flow` = 4 then `ref_u`, `ref_volume`, and `ref_d` are specified

  - `i_flow` = 5 then `ref_n`, `ref_mass`, and `ref_d` are specified together with the `ref_pr` (total to static pressure ratio between inlet plane and the last trailing edge on the mid-streamline). The value of `ref_mass` is a start value for mass flow in the iteration to pressure ratio and has no effect on the final solution.

  - `i_flow` = 6 then `ref_n`, `ref_mass`, and `ref_d` are specified together with `ref_pr` (total to static pressure ratio) together with `n_p_te` (the total number of trailing edges at which a guessed value of the static pressure ratio is specified, followed by the guessed pressure ratios at each trailing edge, including the last, which is also defined by `ref_pr`.

  - `i_flow` = 7 then `ref_n`, `ref_mass`, and `ref_d` are specified together with the `ref_p` (static pressure at the last trailing edge on the mid-streamline). The value of `ref_mass` is a start value for mass flow in the iteration to outlet pressure and has no effect on the final solution. This option may be useful for low speed devices where pressure ratio becomes indeterminate.

  - `i_flow` = 8 then `ref_n`, `ref_mass`, and `ref_d` are specified together with the `ref_p` (static pressure at trailing edge pane) together with `n_p_te` (the total number of trailing edges at which a guessed value of the static pressure is specified, followed by the guessed pressures at each trailing edge, including the last, which is also defined by `ref_p`.

  - `i_flow` = 9 then `ref_n`, `ref_mass`, and `ref_d` are specified together with the `ref_cu` (absolute swirl velocity at the last trailing edge on the mid-streamline). The value of `ref_mass` is a start value for mass flow in the iteration to outlet swirl and has no effect on the final solution. This option may be useful for turbine calculations where the last blade row is a turbine rotor.

  - The versions with specified static pressure and specified outlet swirl have not been fully tested.

  - Other options are available for debugging purposes but are not described here.

  - The geometry definition of Vista TF assumes clockwise rotation. This leads to a certain convention for the sign of the blade angles (see Appendix A: Sign Convention for Angles and Velocities in Vista TF). In some cases you may have a counterclockwise machine with blade angles of the opposite sign. To avoid the need to change all the angles specified in the `.geo` file, an option is provided whereby the value of `i_flow` is given a negative sign. As a more sophisticated alternative the blade speed may be defined as negative.

  `i_fluid`

  Determines the model for the equation of state of the fluid:

  - If `i_fluid` = 0 then ideal gas with constant specific heats.

  - If `i_fluid` = 1 then liquid.

  - If `i_fluid` = 2 then a real gas calculated with the Aungier-Redlich-Kwong equations.

  - If `i_fluid` = 3 then real gas calculated with the Redlich- Kwong equations.

  - If `i_fluid` = 4 then an ideal gas calculation with variable specific heats is carried out. This is done by using the real gas equations but setting the coefficients of the Aungier-Redlich-Kwong equations to the appropriate values internally in the program to reproduce an ideal gas equation.

  - If `i_fluid` = 6 or 7 a calculation is done with a real gas with a constant real gas factor and a constant isentropic exponent.

  - Steam properties can be approximated with the Aungier-Redlich-Kwong equations using the values of the coefficients to model steam.

  `i_inbc`

  Determines the type of inlet boundary conditions:

  - `i_inbc` = 0 then input values are total pressure, total temperature and swirl (`r` `x` `cu`, that is radius times circumferential component of the absolute velocity) on the input plane.

  - `i_in_bc` = 1 then input values are total pressure, total temperature, and absolute flow angle.

  - `i_in_bc` = 2 then input values are: total pressure, total temperature, and absolute circumferential flow velocity.

  See also the section on `n_inbc` in the aerodynamics file (described in Specification of Aerodynamic Data File (*.aer)) where the inlet profile across the span can be specified.

  `i_mass`

  Determines whether the mass flow is uniformly distributed across streamlines or not.

  - `i_mass` = 0 then the mass flow between each streamline is the same.

  - `i_mass` = 1 then the fractional mass between each streamline has to be input into the last line of the control file.

  - `i_mass` = 2 then the cumulative mass for each streamtube from the hub streamline is defined in the last line of the control file.

  `i_mix`

  Determines which mixing model is used:

  - `i_mix` = 0 then no mixing model.

  - `i_mix` = 1 then a spanwise mixing model based on eddy diffusion across the streamlines will be used. Note that this requires a minimum of 9 streamlines (`n_sl` => 9).

  `i_ree`

  Determines the form of the radial equilibrium equation that is used to determine the velocity gradient along the quasi-orthogonal.

  - `i_ree` = 0 then the equations as given in the paper of Casey and Roth (1984) are used, except that the dissipation term is set to zero and the blade force term is set to zero at a trailing edge and at a leading edge.

  - `i_ree` = 1 then the solution is as for `i_ree` = 0 but the dissipation term is not set to zero but the equations as given in the theory documentation are used.

  - `i_ree` = 2 then the dissipation term is not set to zero but the equations given in the paper of Casey and Roth (1984) are used.

  - `i_ree` = 3 then the velocity gradient in the radial equilibrium equation is reduced by the factor `grad_ree` given in section 5. This is useful for debugging difficult cases and the simulation becomes similar to a mean-line calculation with no gradient of meridional velocity across the span. If `grad_ree` = 1.0 then selecting `i_ree` = 3 has no effect.

Section 5: Convergence and damping factors

  The syntax is:

      damp_sc   damp_vl   cm_start   tolerance_cm   tolerance_mass   grad_ree

  The damping factor model automatically chooses the most appropriate values of these parameters based on the type of turbomachine and the grid. You then typically need to specify the following values for this section:

      0.00 0.00 0.00 0.00 0.00 1.00

  In some rare cases it may still be necessary to select these values differently.

  Parameter | Description
  --- | ---

  `damp_sc`

  Damping factor for streamline curvature terms.

  Notes:

  - The Wilkinson stability analysis for streamline curvature programs indicates that the streamline curvature damping term has to be reduced for long closely spaced quasi-orthogonals (high aspect ratio). For details, see the section on computational grid (Computational Grid).

  - If `damp_sc` = 0.0 then the program determines the value of the damping factor from the theory of Wilkinson, or uses an internally determined value that differs for each type of turbomachine — whichever is smaller.

  - Typically values of `damp_sc` between 0.05 and 0.25 are used, but lower values may be necessary for high aspect ratio quasi-orthogonals (as in end stages of steam turbines).

  - If the specified value of `damp_sc` is larger than the value predicted by the Wilkinson stability theory then the program automatically reduces the damping factor to a stable value.

  - If the program has convergence problems with an increasing error then the value is automatically reduced internally within the program during the convergence process.

  - Several different schemes for the damping are applied. The original scheme is obtained with a value of `damp_sc` between 1.0 and 1.25. New schemes which are more stable and robust in most cases can be obtained with the value of `damp_sc` between 0.0 and 0.25. A value between or 2.0 and 2.25 uses the original scheme with changed constants. A value between 3.0 and 3.25 gives a very robust scheme for highly staggered blades. The first digit then defines which scheme is used (0 - new scheme, 1 - original, 2 - modified original, 3 - new scheme for highly staggered blades) and the digits after the decimal point are the damping factor (`damp_sc`) itself.

  `damp_vl`

  Damping factor on velocity level. Note this damping factor is also used internally in the program for all parameters which are under-relaxed.

  Notes:

  - There is no stability theory to define this, and a typical value used is 0.50, indicating that 50% of the new parameter together with 50% of its original value is used.

  - If `damp_vl` = 0.0 then 0.50 is used.

  `cm_start`

  Value of meridional velocity on the mean streamline as a fraction of `u_ref`, as used in the initial conditions. This is then a sort of flow coefficient (`cx`/`u`) of the device concerned and is used as a guide to the velocity levels that can be expected.

  Notes:

  - Recommended that this should be less than the actual value when converged because this avoids choking during the early streamline curvature iterations.

  - If simulations from a cold-start (with no restart file) fail to converge, it may be useful to modify this parameter because it strongly influences the start velocities.

  - Not used if the restart initial condition is used.

  - If `cm_start` = 0.0 then 0.25 is used for all calculations except radial turbines where 0.1 is used. The value of 0.25 is probably adequate for radial compressors only.

  `tolerance_cm`

  Tolerance level on change in meridional velocity during streamline curvature iterations. The value specified is the maximum percentage change in meridional velocity for convergence. Iterations stop when all streamlines and all quasi-orthogonals have a lower value than this.

  Notes:

  - Typical value 0.01 (that is, 0.01%, which is 1 part in 10,000).

  - If `tolerance_cm` = 0.0 then 0.01% is used.

  - Note that if the meridional velocity is low at a certain point in the flow field, it may be necessary to use a higher value than this.

  - Note that the extremely low value of 0.01% does not imply that the solution is as accurate as this, but just provides confidence that convergence has really been achieved.

  `tolerance_mass`

  Tolerance level on mass flow for internal mass flow iteration. Note that because this controls the convergence of the innermost loop, it should be a factor of 2 to 10 lower than the tolerance value for the meridional velocity (above).

  Notes:

  - Typical value 0.001 (that is 0.001%, which is 1 part in 100000).

  - If `error_max` = 0.0 then 0.001% is used.

  `grad_ree` | Factor to reduce the spanwise velocity gradient from the radial equilibrium equation. Normally equal to 1.0 indicating that the gradient from the radial equilibrium equation is used without change. For calculations with `i_ree` = 3, if `grad_ree` is set to 0.0, the program takes a meridional velocity gradient of 0.0 (that is constant meridional velocity across the span) and a value between 1.0 and 0.0 reduces the spanwise gradient of meridional velocity determined by the radial equilibrium equation by this amount.

Section 6: Mass flow distribution between streamlines (n_sl - 1 values)

  The syntax is:

      f_mass_st(1), f_mass_st(2), ... f_mass_st(n_sl - 1)

  Parameter | Description
  --- | ---

  `f_mass_st`

  A list of numbers expressing the relative mass flow for each stream tube.

  Notes:

  - This line is only needed if `i_mass` = 1 or 2 on line 4 of the `.con` file, but for consistency, it is recommended to use it in all input files.

  - The number of values needed corresponds to the number of streamtubes, which is one less than the number of streamlines, so this line requires modification if the number of streamlines for the calculation is changed. The number of values and the values themselves need to change if the number of streamlines in the simulation is changed.

  - If `i_mass` = 1 then this line is interpreted as the relative mass flow for each streamtube from the hub, so the values of `1/(n_sl - 1)` would give a uniform distribution. Each value may be specified as the relative mass flow for a streamtube compared to the sum of all values, so a value of 1.0 for each streamtube also leads to a uniform mass flow distribution.

  - If `i_mass` = 2 the cumulative values from the hub are specified, so the first value is 0.0 and the last value is 1.0.

  - It is recommended that the distribution is selected such that the central streamline always splits the flow into two regions of equal mass flow. The reason for this is that some correlations operate on the mean streamline.

  - The numbers may be specified on different lines.

  Note: `f_mass_st` is not needed if `i_mass` is zero because the program will then automatically use a uniform distribution of mass flow between the streamlines. For consistency, you should use this parameter even for cases where it is not needed.

#### 13.2.4.5. Specification of the Geometry Data File (*.geo)

The geometry data file includes sections of text lines that help you to identify the parameters defined here. You should read the section on geometry in Appendix A: Sign Convention for Angles and Velocities in Vista TF to become familiar with sign conventions and angle definitions used in this file. An example of a geometry data file is given in Appendix D: Example of a Geometry Data File (*.geo) for a Radial Impeller.

Section 1: Character strings identifying the geometry data (max 72 characters/line)

  The syntax is:

      Character string - title(1)
      Character string - title(2)
      Character string - title(3)

Section 2: Number of quasi-orthogonal lines and scale factor (one line)

  The syntax is:

      n_qo   scale

  Parameter | Description
  --- | ---
  `n_qo` | `n_qo` = number of quasi-orthogonal lines from inlet to outlet of the domain. From version V1.31 onwards the maximum value of this parameter is unlimited.

  `scale`

  The scaling factor for all geometry data that is input.

  Notes:

  - Usually the geometry data is input in SI units (that is, all values are expected in m and not mm) and then this value is 1.0.

  - If the input geometry data comes from a CAD system then it may be in mm. In this case, the value of `scale` must be 0.001. Similarly the value can be adjusted to allow the geometry data to be input in other systems of units; for example, inches.

  - This scale factor only scales the data in the geometry input file and has no effect on other dimensions elsewhere; for example, it does not scale the reference diameter, which must be input with units of meters, in the aerodynamic file.

  - If you specify `scale` = 0.0, unity is used.

  For each quasi-orthogonal, the following data is required to define the flow channel for the meridional through-flow calculation and the meridional spacing of the quasi-orthogonals. Note that some of this data is also repeated in the section on the blade geometry. This duplication allows calculations to be made in a channel that is not the same as the hub and casing line of the actual blade definition (blade cropping or blade trimming).

Section 3: Definition of quasi-orthogonal types and end points (n_qo lines: i = 1 to n_qo)

  The syntax (of a single line) is:

      i   r_hub(i)   r_shr(i)   z_hub(i)   z_shr(i)   n_blade(i)   n_curve(i)   i_type(i)   i_row(i)   i_spool(i)

  Parameter | Description
  --- | ---

  `i`

  Number of a particular quasi-orthogonal line.

  Notes:

  - The actual value is not used by the program internally because it recounts the quasi-orthogonals as they are input. You can use this number to recognize a particular line of data in the input file.

  - This allows you to merge two different geometry files of, say, a rotor and stator, to a single stage geometry file without the need to renumber the quasi-orthogonals. In this case, the same number may appear more than once. In a similar way, a single quasi-orthogonal may be removed without the need for renumbering the lines.

  `r_hub(i)` | Radial coordinate at hub end of quasi-orthogonal [m].
  `r_shr(i)` | Radial coordinate at casing end of quasi-orthogonal [m].
  `z_hub(i)` | Axial co-ordinate at hub end of quasi-orthogonal [m].
  `z_shr(i)` | Axial co-ordinate at casing end of quasi-orthogonal [m].

  Notes on co-ordinates:

  - `r_hub` may not be close to zero; adapt the grid if necessary to avoid small values of `r_hub`.

  - The aspect ratio of the quasi-orthogonal lines determines the stability of the solver. The lines should not be too closely spaced.

  - The end coordinates of the leading and trailing edges of blade rows should be included in the list of coordinates.

  - The end coordinates of the leading edge of a splitter vane should be included in the list of coordinates.

  `n_blade(i)`

  Number of blades in blade row.

  Notes:

  - = 0 in duct regions.

  - The number of blades changes at a splitter blade leading edge in a compressor or at a splitter vane trailing edge in a turbine, and changes again for multiple splitters. This is the only information that the program has about the splitters, so the location of the splitter vane leading or trailing edge needs to be a quasi-orthogonal line in the input data.

  `n_curve(i)`

  Number of defining points along the `i`th quasi-orthogonal line.

  Notes:

  - = 1, a special case for duct stations. This indicates that there are 2 defining points (as for `n_curve(i)` = 2) but that no further information for this calculating station is provided in section 4 below, because it is already fully defined by the hub and casing points given in section 3.

  - = 2 for a linear calculating plane in which only the end points of the quasi-orthogonal are defined. In this case, similar information can be found in section 4.

  - > 2 for a non-linear or curved calculating plane.

  - The number of defining points can vary from station to station but `n_curve(i)` should typically be the same for all stations because streamline section data is usually available on a fixed number of spanwise sections.

  - Note that the hub and casing geometry information does not necessarily have to be the same as that defined in section 4. In this case the data in section 3 will be used to crop the blade row or to make a section through the blade information in section 4.

  `i_type(i)`

  Parameter to identify type of calculating station:

  1 - for duct region

  2 - for non-rotating blade row (stator)

  3 - for rotating blade row (rotor)

  Notes:

  - The program internally identifies which lines are leading and trailing edges from the changes of type of blade row, and which line is the leading edge of a splitter vane (by the change in blade number).

  - There must be at least two duct calculating stations upstream of the first blade row, and downstream of the last blade row.

  - A blade row must consist of at least two calculating stations (leading and trailing edge). Typically a radial impeller will have around 15 calculating stations, because this gives a 6° turn between each station and improves the calculation of the curvature terms.

  - There must be at least two blade calculating stations upstream and downstream of a splitter vane leading edge.

  - Other types of blade row may be defined at a later stage.

  `i_row(i)`

  This parameter is used to identify type of blade row and stage of the quasi-orthogonal calculating station. In fact the program can usually identify the type of blade row itself from the geometry and the context, so it is not necessary to specify these values at all and, in the first instance, this parameter may be set to zero. They are included here for special cases where the program may have difficulty with the rules that are coded to identify blade row types.

  = n11 - radial compressor inlet guide vane1

  = n12 - radial compressor inlet guide vane2

  = n13 - radial compressor impeller blade

  = n14 - radial compressor diffuser vane

  = n15 - radial compressor return channel vane

  = n16 - radial compressor axial de-swirl vane

  = n21 - axial compressor inlet guide vane1

  = n22 - axial compressor inlet guide vane2

  = n23 - axial compressor rotor blade

  = n24 - axial compressor stator vane

  = n25 - axial compressor outlet guide vane

  = n31 - radial turbine inlet guide vane1

  = n32 - radial turbine inlet guide vane2

  = n33 - radial turbine impeller blade

  = n34 - radial turbine stator vane

  = n35 - radial turbine outlet guide vane

  = n41 - axial turbine inlet guide vane1

  = n42 - axial turbine inlet guide vane2

  = n43 - axial turbine rotor blade

  = n44 - axial turbine stator vane,

  = n45 - axial turbine outlet guide vane

  Notes:

  The value of n determines which stage is being considered, such that a multistage axial compressor with an IGV would begin with values of 121 for the inlet guide vane, continue with values of 123 for the rotor, and 124 for the downstream stator, so that the next rotor would be 223, and so on. A double row of stators would be denoted as n24 and n25 for the successive blade rows.

  `i_spool`

  Parameter to identify rotational speed of spool or shafts where different blade rows have different speeds.

  0 single shaft with one speed (`ref_n`)

  1 (or 0) first shaft with speed (`ref_n1`)

  2 second spool with second speed (`ref_n2`)

  3 third spool with third speed (`ref_n3`)

  Note that counter-rotating blade rows can be dealt with by specifying negative speeds for the second spool. The program determines the number of different spools (`n_spool`) from the number of different values of `i_spool(i)` found in the geometry input file. (The maximum is set to be 3.)

  Notes:

  - The data is supplied on `n_curve` lines spaced fairly evenly from hub to casing. For example, if `n_curve` = 5, there may be points at 0%, 25%, 50%, 75%, and 100% of span. If `n_curve` = 2, there will be just two points, at 0% and 100% span.

  - The blade data and quasi-orthogonal data in section 4 may extend outside of the flow channel defined by the meridional coordinates given in section 3. In a normal calculation, the data overlaps partly with that given in section 3, because the end points of the quasi-orthogonal lines are defined twice (except for duct calculating stations with `n_curve(i)` = 1; see above). The flow channel defined in section 3 is generally congruent with the blade hub and shroud defined in section 4. The blade, as defined in section 4, may extend outside of the region of the flow channel because this allows a calculation to be made in a cropped or trimmed flow channel only by changing the data in section 3; section 4 does not need to be changed.

  - The end points of the quasi-orthogonal lines, as defined by coordinates `r_hub(i)`, `r_shr(i)`, `z_hub(i)`, and `z_shr(i)`, should lie along the quasi-orthogonal lines as defined by `r_qo (j,i)` and `z_qo(j,i)` below. In many cases, the end points will be coincident with the blade data, but if this is not the case, it is not acceptable to define end points that do not lie on the blade data point.

  - All the angles are specified in degrees because this is more convenient in those cases where it may be necessary to define the geometry by hand, and also allows a simple consistency check, but internally the program converts them into radians. A further description of the angles is provided in Appendix A: Sign Convention for Angles and Velocities in Vista TF.

  The sections above define only the hub and casing walls and provide information on the type of calculating station. The detailed orientation and position of the curved quasi-orthogonal line and the details of the blade surface geometry are provided in the next section.

Section 4: Geometry of quasi-orthogonal lines and blade

  The syntax (of a single line) is:

      i   j   r-qo(j,i)   theta_qo(j,i)   z_qo(j,i)   thu_qo(j,i)   gamma_r_qo(j,i)   gamma_z_qo(j,i)

  Parameter | Description
  --- | ---
  `i` | Number of a particular quasi-orthogonal for data input (increasing from inlet to outlet). Note that this value is not read in as input data or used by the program but is simply used as orientation in the data file when examining the geometry input data.
  `j` | Number of streamline for data input (increasing from hub to shroud). Note that this value is not read in as input data but is simply used as orientation in the data file when examining the geometry input data. Note that for each `q-o (i)`, the spanwise data is entered `(j)` before continuing with the next `q-o`.
  `r_qo(j,i)` | Radial coordinate of point `j` along `q-o (i)` [m].

  `theta_qo(j,i)`

  Circumferential coordinate of blade camber line at point (`r_qo`, `z_qo`) [degrees].

  Notes:

  - The angular coordinate (theta) is taken as positive in the clockwise direction of rotation and negative in the other direction.

  - In a duct region this angle may be zero.

  - This angle is not used by the program but helps to visualize the blade shape and may be useful for plots of the blade shape.

  - In a region where there is a splitter vane this angle is the blade camber angle of the main blade and not of the splitter, or it may be defined as the mean value for both blades.

  `z_qo(j,i)` | Axial coordinate of point along quasi-orthogonal [m].

  `thu_qo(j,i)`

  Circumferential thickness of blade at point (`r_qo`, `z_qo`) [m].

  Notes:

  - In a duct region this thickness should be specified as zero.

  - In a region where there is a splitter vane this thickness is the mean thickness of the main blade and the splitter.

  - At leading and trailing edges the value supplied is not used by the program, but the calculating station is taken to be at the limit of the chord with zero thickness.

  - The thickness is not the thickness normal to the camber line.

  `gamma_r_qo(j,i)` | Lean angle of the blade with a radial line [degrees] as defined in Appendix A: Sign Convention for Angles and Velocities in Vista TF.
  `gamma_z_qo(j,i)` | Lean angle of the blade with an axial line [degrees] as defined in Appendix A: Sign Convention for Angles and Velocities in Vista TF.

  Notes:

  - This geometry includes the coordinates of the blade camber surface (`r-qo(j,i)`, `theta_qo(j,i)`, `z_qo(j,i)`) so that it would theoretically be possible for the program to differentiate this information to determine the slope angles of the surface (`gamma_r_qo(j,i)`, `gamma_z_qo(j,i)`). This is not done for two reasons. Firstly, experience shows that with the crude grids typically used for throughflow calculations, this differentiation would be an unwanted source of error leading to poor estimates of the blade angles, so a system was chosen in which the blade angles are supplied. In fact the value of `theta_qo(j,i)` is not used by the program and can be specified as zero. Secondly, in many cases the slope angles of a blade row are known (inlet and outlet angles) whereas the circumferential coordinate is unknown.

  - This system of geometry with the definition of two angles is designed for radial turbomachinery applications because it allows the complex shape of three-dimensional blades to be defined by the use of the two lean angles, `gamma_r` and `gamma_z`.

  - In conventional axial turbomachinery ductflow programs, it is not usual to define the blade in much detail because often simulations are carried out with only inlet and outlet blade angles. This is also possible with Vista TF. In a ductflow calculation with only leading and trailing edges, the value of `gamma_r` can be set to `0°`. Because the leading and trailing edges are not considered to have any blade force, this has no effect on the simulation. The value of `gamma_z` defines the inlet and outlet blade angles of sections through the blade at constant radius.

  - Vista TF assumes that the geometry is always specified for a clockwise rotation (see Appendix A: Sign Convention for Angles and Velocities in Vista TF). If the geometry is correctly specified and a negative rotational speed is used, and Vista TF performs calculations assuming that the shaft is rotating in the wrong direction with all the wrong incidences, loading, and so forth. For the case where the geometry is specified for counterclockwise rotation, the value of `i_flow` in the `.con` file should be specified as a negative number, for example, -1 or -2. This causes the program to internally switch the angles from positive to negative, and vice-versa, before it proceeds to perform calculations as usual, assuming that the shaft rotates clockwise. A machine that has a geometry suited for counterclockwise rotation should have a negative value for the rotational speed in the `.aer` file.

  The next section provides additional blade-row geometry data for use in the correlations in the program.

Section 5: Additional geometry data (n_curve(i) lines for each blade row)

  The syntax is:

      j   throat   throat_pos   clearance   max_thickness   te_thickness   le_thickness   chord   delta_stagger

  Parameter | Description
  --- | ---
  `j` | Number of a particular streamline for data input (increasing from hub to shroud).

  `throat`

  Throat width of section `j` [m].

  Notes:

  - If the value of zero is input then the program estimates the throat width from the blade angles and the blade thickness, taking into account that the throat is close to the leading edge for compressors and close to the trailing edge for turbines. For radial compressors this estimate is not particularly accurate and for cases close to choke you should provide more precise data here.

  - For axial compressors it is assumed that the blade has a circular arc camber line and the program includes an estimate of the throat area based on the geometrical relationships for circular arc blades.

  - For other blade types, you should specify the value.

  `throat_pos(i)`

  Position of throat on this blade section as a fraction of the meridional length of the section (not currently used)

  Note:

  - If the value of zero is input then the program estimates the throat position from the blade angles and the blade thickness, taking into account that it is close to the leading edge for compressors and close to the trailing edge for turbines.

  - For radial compressors this estimate is not particularly accurate and for cases close to choke you should provide more precise data here.

  - For axial compressors it is assumed that the blade has a circular arc camber line and the program includes an estimate of the throat position based on the geometrical relationships for circular arc blades.

  - For other blade types, you should specify the value.

  `tip clearance`

  `hub/shroud`

  Tip clearance of hub section [m].

  Tip clearance of shroud section [m].

  Notes:

  - If the first value is non-zero, this is interpreted as the hub clearance.

  - If the last value (`n_curve(i)`) is non-zero, this is interpreted as the casing clearance.

  - In a variable stator vane with a hub clearance and a clearance gap for the shaft, it is possible to have non-zero values on both the hub and the tip and then both will be taken into account in the loss correlations.

  `max_thickness`

  Maximum normal thickness of blade section [m].

  Notes:

  - Although the circumferential thickness of the blade row is already specified in section 3, the location of the quasi-orthogonal lines may not coincide with the location of normal maximum thickness, so this value must be specified separately.

  - If a value of zero is specified then the program searches for the normal maximum thickness of the blade, as given in section 3, and uses it to calculate the blade thickness.

  `te_thickness`

  Trailing edge normal thickness of blade section [m].

  Notes:

  - Although the circumferential thickness of the blade row is already specified in section 3, this value must be specified separately.

  - If the value of zero is specified then the program estimates the trailing-edge thickness of the blade from the circumferential thickness given in section 3, and uses it.

  `le_thickness`

  Leading edge normal thickness of blade section [m].

  Notes:

  - Although the circumferential thickness of the blade row is already specified in section 3, this value must be specified separately.

  - If the value of zero is specified then the program estimates the leading-edge thickness of the blade from the circumferential thickness given in section 3, and uses it.

  `chord`

  Chord of blade row at this section [m].

  Notes:

  - Although the chord of the blade row can be estimated from the meridional geometry and the blade angles, this is not exact so it is possible to specify this separately.

  - If a value of zero is specified then the program estimates the chord of the blade from the geometrical data in section 3, the meridional geometry, and the blade angles.

  `delta_stagger`

  Change in stagger angle [°].

  Notes:

  - The blade row may be restaggered by specifying a change in the stagger angle in degrees. The change in angle only needs to be specified on the first of the streamline sections and is applied to all sections.

  - This is only valid for the restaggering of axial blade rows because it operates on the values of `gamma_z_qo` in section 4 by adding the change in stagger angle to those values.

  - A positive value increases the blade angles and the stagger, causing a more closed blade in a stator and a more open blade in a rotor (with negative `gamma_z` values).

#### 13.2.4.6. Specification of Aerodynamic Data File (*.aer)

The aerodynamic input data file includes sections of text that help you to identify the parameters defined here. Although in some areas this file may appear to be complex, a typical simulation uses only one of the many allowed options and so, once an input file with the correct format has been established for a particular type of calculation, further use of the file is less complex.

An example of an aerodynamic data file is given in Appendix E: Example of an Aerodynamic Data File (*.aer).

Section 1: Character strings identifying the aerodynamic data (max 72 characters/line)

  The syntax is:

      Character string – title(1)
      Character string – title(2)
      Character string – title(3)

  Many options are supplied for specifying the flow data for the simulation, but typically the options with `i_flow` = 1 (specified mass flow) and `i_flow` = 5 (specified pressure ratio) are used. Note that `i_flow` is specified in the control file.

Section 2: Reference aerodynamic parameters (depends on value of i_flow in .con file)

  The syntax is:

  `ref_mach ref_phi ref_d`

  if `i_flow` = 0 and `ref_mach` < 3, or

  `ref_u ref_phi ref_d`

  if `i_flow` = 0 and `ref_u` > 3, or

  `ref_n1 ref_mass ref_d`

  if `i_flow` = 1 and `n_spool` = 0 or 1, or

  `ref_n1 ref_n2 ref_mass ref_d`

  if `i_flow` = 1 and `n_spool` = 2, or

  `ref_n1 ref_n2 ref_n3 ref_mass ref_d`

  if `i_flow` = 1 and `n_spool` = 3, or

  `ref_n1 ref_volume ref_d`

  if `i_flow` = 2, or

  `ref_u ref_mass ref_d`

  if `i_flow` = 3, or

  `ref_u ref_volume ref_d`

  if `i_flow` = 4, or

  `ref_n1 ref_mass ref_d ref_pr`

  if `i_flow` = 5, or

  `ref_n1 ref_mass ref_d ref_pr n_p_te guess_pr_1 guess_pr_2 ...`

  if `i_flow` = 6, or

  `ref_n1 ref_mass ref_d ref_pd`

  if `i_flow` = 7, or

  `ref_n1 ref_mass ref_d ref_pd n_p_te guess_pd_1 ...`

  if `i_flow` = 8, or

  `ref_n1 ref_mass ref_d ref_cu`

  if `i_flow` = 9.

  Note: The very large number of possible ways of specifying the flow and speed appears, at first, to be slightly overwhelming. Generally `i_flow` = 1 is used. Note that the reference diameter is given here and not in the geometry file. This is because you may prefer to use the hub diameter, the tip diameter, the inlet diameter, or the outlet diameter, as a reference value for the aerodynamics without changing the geometry file.

  Note: The geometry definition of Vista TF assumes clockwise rotation. This leads to a certain convention for the sign of the blade angles (see Appendix A: Sign Convention for Angles and Velocities in Vista TF). Vista TF expects that the geometry is defined for a clockwise-rotating machine (viewed from the inlet along the positive axis). In some cases you may have a counterclockwise-rotating machine with blade angles of the opposite sign to that expected by Vista TF. To avoid the need to change all the angles specified in the `.geo` file, an option is provided whereby the value of `i_flow` is given a negative sign. As an alternative, the rotational speed may be specified as a negative value, which means that the blade is rotating in the counterclockwise direction.

  Parameter | Description
  --- | ---

  `i_flow`=0

  “Iteration to mass flow”

  `ref_mach` = Machine Mach number (based on inlet total conditions) [-] or reference blade speed [m/sec]. (In this document, “[-]” means dimensionless.)

  Notes:

  - If `ref_mach` < 3 then `ref_mach` is interpreted as `ref_mach`.

  - If `ref_mach` > 3 then `ref_mach` is interpreted as `ref_u`.

  `ref_phi` = Inlet flow coefficient (based on total inlet conditions) [-]. (In this document, “[-]” means dimensionless.)

  `ref_d` = Reference blade diameter for the definition of flow coefficient. [m]

  `i_flow`=1

  “Iteration to mass flow”

  `ref_n1` = Machine rotational speed [rpm]

  `ref_mass` = Mass flow [kg/sec]

  `ref_d` = Reference blade diameter [m] for the definition of flow coefficient

  If the machine has separate spools of different speeds (`i_spool(i)` > 2) then the speed of each spool can be provided up to a maximum of three different spools.

  `ref_n1` = Rotational speed of shaft 1 [rpm]

  `ref_n2` = Rotational speed of shaft 2 [rpm]

  `ref_n3` = Rotational speed of shaft 3 [rpm]

  Counter-rotating blade rows require the second blade row to be provided with a negative speed.

  `i_flow`=2 | “Iteration to mass flow” `ref_n1` = Machine rotational speed [rpm] `ref_volume` = Volume flow at inlet total conditions [m3/sec] `ref_d` = Reference blade diameter [m] for the definition of flow coefficient
  `i_flow`=3 | “Iteration to mass flow” `ref_u` = Reference blade speed [m/s] `ref_mass` = Mass flow [kg/sec] `ref_d` = Reference blade diameter [m] for the definition of the blade speed
  `i_flow`=4 | “Iteration to mass flow” `ref_u` = Reference blade speed [rpm] `ref_volume` = Volume flow at inlet total conditions [m3/sec] `ref_d` = Reference blade diameter [m] for the definition of the blade speed

  `i_flow`=5

  “Iteration to pressure ratio”

  `ref_n1` = Machine rotational speed [rpm]

  `ref_mass` = Mass flow [kg/sec] (estimate of actual mass flow but final converged mass flow is determined by the pressure ratio and this only serves as an initial guess)

  `ref_d` = Reference blade diameter [m] for the definition of flow coefficient.

  `ref_pr` = Ratio of static pressure at the trailing edge to total pressure at the inlet, with both of these pressures evaluated on the mean streamline.

  `i_flow`=6

  “Iteration to pressure ratio”

  `ref_n1` = Machine rotational speed [rpm]

  `ref_mass` = Mass flow [kg/sec] (estimate of actual mass flow)

  `ref_d` = Reference blade diameter [m] for the definition of flow coefficient.

  `ref_pr` = Ratio of static pressure at the trailing edge to total pressure at the inlet, with both of these pressures evaluated on the mean streamline.

  `n_p_te` = Number of trailing edges at which a guessed value of the pressure ratio is specified

  `guess_pr_1` = Guessed value of the pressure ratio at the first trailing edge

  `guess_pr_2` = Guessed value of the pressure ratio at the second trailing edge

  ...

  `guess_pr_n_p_te` = This continues up to and including the last trailing edge.

  Note that if the pressure ratio of the last trailing edge differs to that of `ref_pr`, then all values at all trailing edges are scaled with the value of `ref_pr`.

  `i_flow`=7

  “Iteration to pressure difference”

  `ref_n1` = Machine rotational speed [rpm]

  `ref_mass` = Mass flow [kg/sec] (estimate of actual mass flow but final converged mass flow is determined by the pressure ratio and this only serves as an initial guess)

  `ref_d` = Reference blade diameter [m] for the definition of flow coefficient.

  `ref_pd` = Static pressure at the trailing edge minus total pressure at the inlet, with both of these pressures evaluated on the mean streamline.

  `i_flow`=8

  “Iteration to pressure difference”

  `ref_n1` = Machine rotational speed [rpm]

  `ref_mass` = Mass flow [kg/sec] (estimate of actual mass flow)

  ref_d = reference blade diameter [m] for the definition of flow coefficient

  `ref_pd` = Static pressure at the trailing edge minus total pressure at the inlet, with both of these pressures evaluated on the mean streamline.

  `n_p_te` = Number of trailing edges at which a guessed value of the pressure ratio is specified

  `guess_pd_1` = Guessed value of the pressure difference at the first trailing edge

  `guess_pd _2` = Guessed value of the pressure difference at the second trailing edge

  ...

  `guess_pd_n_p_te` = This continues up to and including the last trailing edge

  `i_flow`=9 | “Iteration to outlet swirl” `ref_n1` = Machine rotational speed [rpm] `ref_mass` = Mass flow [kg/sec] (estimate of actual mass flow) `ref_d` = reference blade diameter [m] for the definition of flow coefficient. `ref_cu` = Swirl velocity on mean streamline at rotor outlet

  Note:

  - The reference blade speed, tip speed Mach number and/or the machine rotational speed are also needed for the calculation of a stator blade row. This is because these parameters are used to define various non-dimensional flow and work coefficients and the reference blade speed is also used to determine the flow velocities for the initial estimate of the flow field (together with parameter `cm_start`. See section 5 of the `.con` file specification given in Specification of the Control Data File (*.con)).

  - Iteration to a defined pressure ratio makes use of the so-called target pressure ratio method of Denton. This requires the program to make a fist guess of the pressure at each trailing edge of the machine. The algorithm currently incorporated makes a crude estimate of these, but it has been found that this may not be sufficient to secure convergence. For this reason, you can define the first guess of the pressure at each trailing edge by setting `i_flow` = 6 (instead of 5).

  - A line prepared with data for `i_flow` = 6 can formally also be used with `i_flow` = 5 or `i_flow` =1 with no change, so that a calculation can switch from “iteration to pressure ratio” to “iteration to mass flow” with no formal change to the aerodynamic input data file.

Section 3: Reynolds number or viscosity

  The syntax is:

      ref_re

  or

      ref_mue

  Parameter | Description
  --- | ---
  `ref_re` | Reynolds number based on `ref_u` ( ), `ref_D` ( ), and inlet total conditions [-]. (In this document, “[-]” means dimensionless.)
  `ref_mue` | Dynamic viscosity at the inlet plane and mean inlet total conditions.

  Note: The program identifies which of these parameters has been provided from the absolute value of the numerical input. If the value is greater than 1.0 [N s m^-2] (or equivalent value in other units), it is interpreted as a Reynolds number; if it is less than 1.0 [N s m^-2] but greater than 0.0000001 [N s m^-2], it is interpreted as the dynamic viscosity. A value of 0 causes the program to determine the dynamic viscosity from a built-in equation for the dynamic viscosity based on Sutherland’s law and the inlet total temperature. The reference Reynolds number is determined from this.

Section 4: Fluid data (depends on value of i_fluid in .con file)

  The syntax is:

      cp_gas   gamma_gas

  if `i_fluid` = 0, which indicates an ideal gas with constant specific heats, or

      cw_fluid   rho_fluid

  if `i_fluid` = 1, which indicates a liquid, or

      R_gas gamma_gas

  if `i_fluid` = 2, 3, 4, or 5, which indicates a real gas with equations, or

      cp_gas gamma_gas z_gas

  if `i_fluid` = 6, which indicates a real gas with a constant real gas factor Z, or

      R_gas gamma_gas z_gas

  if `i_fluid` = 7, which indicates a real gas with a constant real gas factor Z.

  Parameter | Description
  --- | ---
  `i_fluid` = 0 (ideal gas with constant specific heats) | `cp_gas` = Specific heat at constant pressure [J/kgK] `gamma_gas` = ratio of specific heats [-] (In this document, “[-]” means dimensionless.)
  `i_fluid` = 1 (liquid) | `cw_fluid` = Specific heat of fluid [J/kgK] `rho_fluid` = density of liquid [kg/m3]

  `i_fluid` = 2

  `i_fluid` = 3

  `i_fluid` = 4

  `i_fluid` = 5

  (real gas with equations)

  Real gas option in which full details of the gas properties are provided in the `.rgp` file. In order to avoid changing the format of this file and internal details of the calculation, these values also need to be specified here. The values given here are estimates that are then overwritten internally in the program by the values in the real gas data file (see Specification of the Real Gas Properties Data File (*.rgp)). If no values are specified then air is assumed.

  `R_gas` = Gas constant [J/kgK]

  R

  `gamma_gas` = mean ratio of specific heats [-]

  `i_fluid` = 6 (real gas with a constant real gas factor Z) | `cp_gas` = Specific heat at constant pressure [J/kgK] `gamma_gas` = ratio of specific heats [-] `Z_gas` = real gas factor Z pv = ZRT
  `i_fluid` = 7 (real gas with a constant real gas factor Z) | `R_gas` = Gas constant R [J/kgK] `gamma_gas` = ratio of specific heats [-] `Z_gas` = real gas factor Z pv = ZRT

Section 5: Number of points on the inlet boundary where flow conditions are specified

  The syntax is:

      n_inbc

  Parameter | Description
  --- | ---

  `n_inbc`

  Number of points at which the inlet flow conditions are specified across the inlet plane.

  Notes:

  - This should be less than the number of streamlines (`n_inbc` < `n_sl`).

  - if `n_inbc` = 1 then only a single value is input and this is taken to be on the mid-streamline. Note that a single value implies that the inlet conditions have a constant total pressure, constant total temperature, and constant swirl (rcu) across the span at the inlet, whereby the value of the swirl is determined from the values specified (rcu, alpha, or cu).

  - A maximum of 25 points is allowed.

Section 6: Fraction of mass flow where inlet conditions are specified (n_inbc values)

  The syntax is:

      f_mass_inbc

  Parameter | Description
  --- | ---
  `f_mass_inbc` | `n_inbc` values of the fraction of mass along the inlet boundary at which inlet boundary conditions are specified. The first value should be 0.0 and the last value should be 1.0. Note that if `n_inbc` = 1 then this has no function and a dummy value can be specified, but this should not be omitted.

Section 7: Pressure on the inlet boundary (n_inbc values that depend on i_inbc in .con file)

  The syntax is:

      pt_inbc

  if `i_inbc` = 0.

  Parameter | Description
  --- | ---
  `pt_inbc` (`i_inbc`=0) | Total pressure on the inlet boundary [Pa]. Note that if an incompressible calculation is carried out it is still necessary to specify the absolute value of the total pressure on the inlet boundary.

Section 8: Temperature on the inlet boundary (n_inbc values that depend on i_inbc in .con file)

  The syntax is:

      tt_inbc

  if `i_inbc` = 0.

  Parameter | Description
  --- | ---
  `tt_inbc` (`i_inbc` = 0) | Total temperature on the inlet boundary [K].

Section 9: Swirl or angle on the inlet boundary (n_inbc values that depend on i_inbc in .con file)

  The syntax is:

      rcu_inbc

  if `i_inbc` = 0, or

      alpha_inbc

  if `i_inbc` = 1, or

      cu_inbc

  if `i_inbc` = 2.

  Parameter | Description
  --- | ---
  `rcu_inbc` (`i_inbc` = 0) | Swirl on the inlet boundary [m2/sec]. Note that this is the product of the local radius of the streamline and the local circumferential velocity component and is positive if the swirl is in the clockwise direction of rotation.
  `alpha_inbc` (`i_inbc` = 1) | Flow angle on the inlet boundary [°]. Note that this is from the axial direction and positive in the clockwise direction of rotation. Note also that, if a single value is specified, it is used to calculate the swirl on the mean streamline of the inlet boundary, and the swirl is then kept constant across the span. If a constant flow angle across the span is required then 2 values need to be specified across the span (`n_inbc` = 2). Experience with radial turbines with high swirl at the inlet show that the specification of a single value of swirl across the span is more robust than specifying a variation of flow angle across the span.
  `cu_inbc` (`i_inbc` = 2) | Circumferential component of velocity [m/sec] on inlet boundary. Note that if a single value is specified then this is used to calculate the swirl (rcu) on the mean streamline of the inlet boundary and the swirl is kept constant across the span.

Section 10 : Aerodynamic model parameters

  The syntax is:

      eddy   f_bl_le   f_bl_te

  Parameter | Description
  --- | ---

  `eddy`

  Spanwise mixing parameter (eddy diffusivity).

  Notes:

  - Typically 0.0001 to 0.001. See Streamline Curvature Throughflow Theory.

  - This has no function if `i_mix` = 0.

  - If `i_mix` = 1 and `eddy` = 0.0 then a value of eddy = 0.0005 will be used.

  `f_bl_le` | `f_bl_le` is the meridional fraction of blade length at the leading edge where the blade is partly transparent to the flow (accounts artificially for the increased loading due to incidence). It is recommended that you specify a value of 0.0 for both `f_bl_te` and `f_bl_le`. If both `f_bl_te` and `f_bl_le` are equal to zero then the program estimates the values of these from the blade spacing using the equations given in Streamline Curvature Throughflow Theory. If you want, you can specify these values. If you specify 0.0 then the flow is congruent with the mean blade camber line at the leading edge. A typical value is roughly equal to the blade spacing or chord.
  `f_bl_te` | Fraction of blade length after which the blade is partly transparent to the flow at the trailing edge (accounts artificially for the decreased loading due to deviation as the trailing edge is approached). It is recommended that you specify a value of 0.0 for both `f_bl_te` and `f_bl_le`. If you specify 1.0 then the flow is congruent with the mean blade camber line right up to the trailing edge. If both `f_bl_te` and `f_bl_le` are equal to zero then the program estimates these from the blade spacing using the equations given in Streamline Curvature Throughflow Theory.

It is possible to calculate multiple operating points, in which case details of these operating points in terms of flow and speed are required in sections 11, 12, and 13.

Section 11: Relative flow for multiple operating points (not needed if `n_points` < 2)

  The syntax is:

      ref_point(1), ref_point(2), ref_point(3), ... ref_point(11)

  Parameter | Description
  --- | ---

  `ref_point(i)`

  Flow relative to the reference flow defined in the aerodynamic file. The value `ref_mass`, `ref_volume`, or `ref_phi` is multiplied by the value `ref_point` to determine the actual operating point.

  Notes:

  - Typically, this line consists of a list of values such as 1.15, 1.10, 1.05, 1.00, 0.95, 0.90, and 0.85, indicating 115% down to 85% of the flow at the reference point.

  - If the value of `i_flow` is 1, the seven values listed above would be interpreted as seven different mass flows to be calculated. If the value of `i_flow` is 2, the values would be interpreted as different volume flows. If the value of `i_flow` is 0, the values would be interpreted as flow coefficients.

  - The flow scales linearly with the speed, so that when operating at the 100% flow point on the 90% speed line, the flow is reduced to 90% of the reference value.

  - A maximum of 11 points is allowed.

Section 12: Relative flow for multiple speed lines (not needed if `n_speeds` < 2)

  The syntax is:

      ref_speed(1), ref_speed(2), ref_speed(3), ... ref_speed(11)

  Parameter | Description
  --- | ---

  `ref_speed(i)`

  Rotational speed relative to the reference speed defined in the aerodynamic file. The value `ref_n`, `ref_u`, or `ref_mach`, is multiplied by the value `ref_speed` to determine the actual operating speed.

  Notes:

  - Typically, this section consists of a list of values such as 1.1, 1.0, 0.9, 0.8, 0.7, 0.65, 0.5.

  - These seven values would be interpreted as seven different speed lines to be calculated at 110%, 100%, 90%, etc., of the reference speed.

  - A maximum of 11 speeds is allowed.

Section 13: Additional multiple point parameters (not needed if `n_speeds`*`n_points`<2)

  The syntax is:

      map_parameter(1), map_parameter(2), ... map_parameter(11)

  Parameter | Description
  --- | ---
  `map_parameter(i)` | Not used at the moment but included to allow rules with regard to automatic map generation to be included, such as the definition of a limit in the diffusion factor to automatically provide an estimate of the stability point.

Note on Multiple operating points:

It is possible to calculate multiple operating points, in which case details of these operating points in terms of flow and speed are required, and sections 11, 12 and 13 provide this data. These sections are not used if the multiple points are not calculated (`n_points`*`n_speeds` < 2 in the `.con` file). This option is available only for simulations with a specified mass or volume flow and not for specified pressure ratios.

#### 13.2.4.7. Specification of Correlations Data File (*.cor)

The input data file includes sections of text lines that help you to identify the parameters defined here; see the examples in Appendix F: Examples of Correlations Data Files (*.cor). This file partly changes its structure depending on the type of correlation chosen and the number of quasi-orthogonals or blade rows being calculated. This is a complex input file, but it does not need to be changed once it is set up.

The first part of the file contains control parameters that define the layout of the remainder of the input data that is needed. The file is arranged so that it always has a standard format at the beginning (first 8 lines) but may require different data towards the end depending on the type of calculation under consideration (axial compressor, radial turbine, single stage, multi-stage, and so on). Similar types of simulations always use similar formats for this file, but different types of simulations may require different formats for the latter part of this file.

The file has two different structures because the specification of the empirical data relies on two different approaches.

- User-specified approach

  Set all of `i_loss`, `i_dev`, and `i_ewb` in section 2 to a value of 1. You may specify the losses, the blockage, and deviation associated with specifically-defined quasi-orthogonals and streamlines. In the simplest and most common approach, a single value is specified on the mean streamline of the first quasi-orthogonal and this is then automatically used throughout the calculation.

  This approach is oriented around the quasi-orthogonals, enabling you to specify different local efficiency and blockage values for each quasi-orthogonal and streamline. Although deviation is only meaningful at the trailing edge, a similar approach, based on quasi-orthogonals, is used for deviation to be consistent with losses and blockage. In many cases, the specification of no value also allows a correlation to be used to determine the value (such as the Wiesner slip factor for a radial compressor). This approach is recommended for beginners. In general, it requires only a single value that may be changed to be specified in the correlations file. If different operating points are to be calculated, where it can be expected that the losses change, then you can take this into account by adjusting the specified loss value in the `.cor` file manually for each point.

- Built-in correlations for losses, deviation and blockage

  Set all of `i_loss`, `i_dev`, and `i_ewb` in section 2 to a value of 2. You provide information that enables the program to calculate the empirical data for the losses for each blade row by selecting one of the built-in correlations, which determines the losses from the local flow field and the geometry. Different operating points will then automatically have different values of the losses.

  This approach is oriented around blade rows and requires data to be specified at each blade row trailing edge (or upstream of this – see later).

  Note that the correlations used for individual blade rows can be changed from one blade row to another. You can also use the correlations for deviation from one source and the correlations for losses from another, if this is sensible; usually it is not sensible. In general, and for simplicity, you should apply the correlations such that all blade rows use the same correlations, and such that the losses, blockage, and deviation, are from the same source.

The correlations currently programmed can be obtained with the use of the different parameters for `i_loss_type`, `i_dev_type`, and `i_ewb_type` in sections 4, 6, and 8.

Note: In some cases the same correlations can be used in slightly different ways – this is related to the fact that the poor description of correlations in the literature sources sometimes leads to uncertainties in implementation. Where it is sensible different versions have been implemented. In the machine types with many different sources of correlations, the recommended correlation can be obtained using values of 100, 200, 300, 400 for `i_loss_type`, `i_dev_type`, and `i_ewb_type`.

Radial Compressor Correlations | i_loss_type / i_dev_type / i_ewb_type
--- | ---
Casey-Robinson correlation | 101 / 101 / 101

Axial Compressor Correlations | i_loss_type / i_dev_type / i_ewb_type
--- | ---
Recommended correlation (203 / 203 / 201) | 200 / 200 / 200
Miller-Wright (original implementation by PCA) | 201 / 201 / 201
Miller_Wright (1st revision, November 2007) | 202 / 202 / 202
Miller_Wright (2nd revision, April 2012) | 203 / 203 / 203

Axial Turbine Correlations | i_loss_type / i_dev_type / i_ewb_type
--- | ---
Recommended correlation (401 / 401 / 401) | 400 / 400 / 400
Kacker-Okapuu | 401 / 401 / 401
Dunham-Came | 402 / 402 / 402

If required, you can specify single values of the losses, deviation, and blockage parameters, for the first blade row or first quasi-orthogonal. These are then used throughout the domain provided that they are not changed again. In addition, it is possible to apply multiplicative and additive correction factors to the values predicted by the correlations, by the application of “fudge factors” (user-defined corrections). Generally this file does not need to be changed once it has been set up, so you might not need to understand all the intricacies of the many possibilities that it allows, and typically a standard type of correlations file can be established which can then be used for all subsequent simulations with the same set of correlations. Examples of some typical correlations data files are given in Appendix F: Examples of Correlations Data Files (*.cor), showing several specific examples for specific types of calculation.

Section 1: Character strings identifying the correlation data (max 72 characters/line)

  The syntax is:

      Character string – title(1)
      Character string – title(2)
      Character string – title(3)

Section 2: Integer control parameters for loss, deviation and blockage models (one line)

  The syntax is:

      i_loss   i_dev   i_ewb

  Parameter | Description
  --- | ---

  `i_loss`

  Determines the loss specification to be used.

  Notes:

  - `i_loss` = 0

    No losses are specified and the calculation uses constant entropy. Note, however, that in order to retain similar structures for the correlations file, the lines described in sections 3 and 4 are still needed, but have no effect. This allows you to switch off the losses if necessary.

  - If `i_loss` = 1 then a user-defined variation of efficiency, loss coefficient, or dissipation coefficient across the span is specified at the spanwise positions given in section 4. The number of positions that are defined across the span and through the domain is given in section 3. Different values of the efficiency, loss coefficient, or dissipation coefficient can be specified for different quasi-orthogonal calculating stations and spanwise positions.

  - If `i_loss` = 1, then a value on the first quasi-orthogonal is always needed. This value remains constant until changed by the next quasi-orthogonal at which the loss is defined. If only a single value is specified across the span then this is applied on the mean streamline and each streamline has the same entropy rise as on the mean streamline. If a calculation with a constant efficiency for all streamlines is required then the efficiency needs to be specified as a constant on at least two points across the span.

  - If `i_loss` = 2 then built-in loss correlations are used according to the values given in sections 3 and 4.

  `i_dev`

  Determines the method for calculation of a blade outlet flow angle (deviation or slip).

  Notes:

  - If `i_dev` = 0, the flow follows the mean blade camber line given in the `.geo` file with no deviation. This option allows a mean S2 though-flow calculation to be carried out using the mean stream surface obtained from a series of S1 blade-to-blade calculations, provided that these are then given as the geometry of the camber surface in the `.geo` file. Note that, in order to retain similar structures for the correlations file, the lines described in sections 5 and 6 are still needed but have no effect.

  - If `i_dev` = 1 then data is specified in sections 5 and 6 to predict the variation of the flow angle at the blade outlet from the mean blade camber line across the span. The information can be either in the form of a deviation angle, a specified flow outlet angle, a specified slip factor, or a modification to the cosine rule, according to the type of blade row.

  - If `i_dev` = 2 then built-in correlations are used to determine the flow angle according to the type of blade row as specified in sections 5 and 6.

  `i_ewb`

  Determines the blockage correlation for boundary layers that is to be used (ewb means “end-wall blockage”)

  Notes:

  - If `i_ewb` = 0 then no end-wall blockage is applied. Note that, in order to retain similar structures for the correlations file, the lines described in sections 7 and 8 are still needed, but have no effect.

  - If `i_ewb` = 1 then data is specified in sections 7 and 8 to predict the variation of the flow blockage for each quasi-orthogonal and for each streamline. A single value implies that a constant blockage value is applied in the whole calculation domain.

  - If `i_ewb` = 2 then builtin correlations are used to determine the blockage according to the type of blade row as specified in sections 7 and 8.

Section 3: Loss input data locations

  The syntax is:

      n_loss_sl   n_loss_qo

  or

      n_loss_bladerow   n_dummy

  If `i_loss` equals 0 or 1 then the losses for each quasi-orthogonal can be specified, and the following values are required:

  Parameter | Description
  --- | ---
  `n_loss_sl` | Number of the spanwise positions for which the loss data is supplied.
  `n_loss_qo` | Number of quasi-orthogonal calculating stations through the domain on which the loss information is specified.

  If `i_loss` equals 2 then the losses for each blade row can be specified, and the following values are required:

  Parameter | Description
  --- | ---
  `n_loss_bladerow` | Number of separate blade rows for which the loss data is supplied.
  `n_dummy` | A dummy integer value to ensure that section 3 always has two integer values. This enables you to switch between various alternatives without changing the structure of the data in the file.

  If `i_loss` equals 0 or 1, then the following version of section 4 applies:

Section 4: User-defined loss data specification (n_loss_qo * n_loss_sl lines)

  This version of section 4 is applicable when `i_loss` equals 0 or 1.

  The syntax is:

      i_qo_loss   k_loss   f_loss   loss

  Parameter | Description
  --- | ---
  `i_qo_loss` | Number of the quasi-orthogonal calculating station on which the loss, deviation, and blockage information is specified. The specified values will be applied for all blade rows and calculating stations downstream of this quasi-orthogonal until the value is changed by a subsequent section 4 with a new value of `i_qo_loss`. The first value of `i_qo_loss` must be 1. Subsequent lines may change the way in which the losses are defined.

  `k_loss`

  Parameter to define how the losses are specified.

  Notes:

  - If `k_loss` = 1 then the small-scale static to static polytropic efficiency (`eta_poly`) is specified. This is used in such a way that the entropy always increases so that, for a local accelerating flow with a decrease in static enthalpy, it defines a turbine efficiency, and for a decelerating flow, it defines a compressor efficiency. This small-scale efficiency is applied in blade rows and in ducts. Note that specifying a specific value does not lead to an efficiency of the same value for the whole domain because this is dependent on both the local small-scale efficiency and the path of the process. For this, `k_loss` must be set to 4 or 7. See below.

  - If `k_loss` = 2 then the entropy loss coefficient (`xsi`) is specified. Note that the loss coefficient is the entropy loss coefficient with respect to outlet plane dynamic head for accelerating blade rows (turbine rotors and stators) and with respect to the inlet plane dynamic head for decelerating blade rows (compressor rotors and stators). An inlet guide vane for a compressor is therefore calculated as a turbine blade row, and an outlet guide vane for a turbine as a compressor blade row. Like the deviation, this value is only used at the trailing edge of a blade row.

  - If `k_loss` = 3 then the dissipation loss coefficient (`cd`) is specified to determine the losses from an integration of the loss production following the so-called u-cubed model of Denton. This is applied in blade rows and in ducts.

  - If `k_loss` = 4 to 9 then various forms of efficiency are used to specify the losses, as follows:

    k_loss = 4 total-total polytropic efficiency

    k_loss = 5 total-static polytropic efficiency

    k_loss = 6 static-static polytropic efficiency

    k_loss = 7 total-total isentropic efficiency

    k_loss = 8 total-static isentropic efficiency

    k_loss = 9 static-static isentropic efficiency

    These are applied in blade rows and in duct regions.

  - In duct regions, these values are applied to the change from one quasi-orthogonal to the next. Clearly if the total enthalpy does not change, the use of 4 or 7, which give a total-total efficiency, is meaningless. In blade rows the full range is allowed, but options 6 and 9 are probably not very relevant. Use of 5 and 8 is not recommended because specifying a total-static efficiency that is too high may lead to a total-total efficiency that is greater than unity.

  - Option 4 or 7 is now recommended for rotor blade rows. This change forces the impeller total-total efficiency to be exactly the value that is specified. It is more robust, especially with real gas equations, because only the velocity triangle at the impeller outlet is involved in the estimate of the losses, and there is no need to use the real gas equations at each point in the stage when determining the entropy. It also has the advantage that the losses become exactly as specified, which was not the case with the option using a small-scale local polytropic efficiency.

  - If `k_loss` = 10 then the loss in a stator vane can be specified as a total pressure loss coefficient.

  - If `k_loss` = 11 then the performance of a stator vane can be specified as a static pressure rise coefficient.

  - These options have been programmed so that different blade rows may have different values of `k_loss`.

  `f_loss` | The fraction of the span at which the value of loss applies. If only a single value is given, it is applied at the mean streamline independent of the value of `f_loss`.
  `loss` | Depending on the value of `k_loss`, this is interpreted as a small-scale polytropic efficiency (`etapol`), a loss coefficient (`xsi`), a dissipation coefficient (`cd`), or other items given.

  If `i_loss` equals 2 then the following version of section 4 applies:

Section 4: Correlation-based loss data specification (n_loss_bladerow lines)

  This version of section 4 is applicable when `i_loss` equals 2.

  The syntax (of a single line) is:

      i_loss_bladerow   i_loss_type   factor1   factor2   factor3   factor4   factor5   factor6

  Parameter | Description
  --- | ---
  `i_loss_bladerow` | Number of the blade row on which the loss information is specified. The specified values will be applied for all blade rows downstream of this blade row until the value is changed by a subsequent section 4 with a new value of `i_loss_bladerow`, and then this will again be applied until changed. The first value must be 1.

  `i_loss_type`

  Parameter to define which correlations are used for the blade row losses. The current loss correlations incorporated into the method are as follows:

  - Radial Compressor Correlations

    - `i_loss_type` = 101

      Casey-Robinson correlation

  - Axial Compressor Correlations

    - `i_loss_type` = 200

      Recommended correlation (203)

    - `i_loss_type` = 201

      Miller_Wright (original implementation by PCA) 201

    - `i_loss_type` = 202

      Miller_Wright (1st revision, November 2007)

    - `i_loss_type` = 203

      Miller_Wright (2nd revision, April 2012)

  - Axial Turbine Correlations

    - `i_loss_type` = 400

      Recommended correlation (401)

    - `i_loss_type` = 401

      Kacker-Okapuu

    - `i_loss_type` = 402

      Dunham-Came

  `factor_loss` 1 to `factor_loss` 6

  User-defined multiplication or addition factors to the losses determined by the correlations. This allows the loss correlations to be modified to improve matching with experimental or CFD data. These have different functions for the different correlation systems. In the case of the Cox-Casey correlations these provide some empirical constants for the models used.

  `i_loss_type` = 11: Casey-Robinson radial compressor model.

  Factor 1: Impeller total-total efficiency at design point (eta_d)

  Factor 2: Design tip-speed Mach number (Mu2_d)

  Factor 3: Design flow coefficient (phi_d)

  Factor 4: Type of stage: 1.0 = turbocharger, -1.0 = process

  Factor 5: Type of diffuser: 1.0 = vaned, -1.0 =vaneless

  Factor 6: not in use

  `i_loss_type` = 21, 22, 23, 24, 41, and 42: Factors on losses.

  Factor 1: Multiplication factor on profile losses

  Factor 2: Multiplication factor on secondary losses

  Factor 3: Multiplication factor on tip clearance losses

  Factor 4: Multiplication of penetration of secondary losses

  Factor 5: Multiplication of penetration of tip clearance losses

  Factor 6: Not in use

  These are all generally specified as a value of 1.0.

  `i_loss_type` = 31: Cox-Casey radial turbine model.

  Factor 1: Small-scale polytropic efficiency

  Factor 2: Loss multiplier for tip clearance loss vortex

  Factor 3: Loss penetration of tip clearance vortex (fraction of span from the tip)

  Factors 4 to 6: Not in use

Section 5: Deviation input data locations

  The syntax is:

      n_dev_sl n_dev_qo

  or

      n_dev_bladerow n_dummy

  If `i_dev` equals 0 or 1 then the deviation for each quasi-orthogonal can be specified, and the following values are required:

  Parameter | Description
  --- | ---
  `n_dev_sl` | Number of spanwise positions for which the flow angle data is supplied.
  `n_dev_qo` | Number of quasi-orthogonal calculating stations on which the flow angle information is specified.

  If `i_dev` equals 2 then the deviation flow angle data can be specified for each blade row, and the following values are required:

  Parameter | Description
  --- | ---
  `n_dev_bladerow` | Number of separate blade rows for which the flow angle data is supplied.
  `n_dummy` | A dummy integer value to ensure that section 5 always has two integer values.

  If `i_dev` equals 0 or 1 then the deviation for each quasi-orthogonal can be specified, and the following version of section 6 is applicable:

Section 6: Flow angle data specification (n_dev_qo * n_dev_sl lines)

  This version of section 6 is applicable when `i_dev` equals 0 or 1.

  The syntax is:

      i_qo_dev   k_dev   f_dev   dev

  Parameter | Description
  --- | ---
  `i_qo_dev` | Number of the quasi-orthogonal calculating station on which the deviation information is specified. The specified values will be applied for all blade row trailing edges downstream of this quasi-orthogonal until the value is changed by a subsequent section 6 with a new value of `i_qo_dev`. The first value must be 1.

  `k_dev`

  Determines the type of outlet flow angle calculation, as follows:

  - If `k_dev` = 1 then the deviation angle is specified (in degrees).

  - If `k_dev` = 2 then the relative outlet flow angle is specified (in degrees).

  - If `k_dev` = 3 then a slip factor is specified and applied on the mean line (dimensionless). Note that if no value is specified then the Wiesner slip factor is used. Only recommended for radial impellers and not for mixed flow stages, which should use deviation.

  - If `k_dev` = 4 then a slip factor is applied at each radius of the trailing edge (dimensionless). Note that if no value is specified then the Wiesner slip factor is used. Only recommended for radial impellers and not for mixed flow stages, which should use deviation.

  - If `k_dev` = 5, this is analogous to `k_dev` = 3, but the slip factor correlation of Xuwen Qiu is applied on the mean-line.

  - If `k_dev` = 6, this is analogous to `k_dev` = 4, but the slip factor correlation of Xuwen Qiu is applied on each streamline separately.

  `f_dev` | The fraction of the span of at which the value of the deviation (and similar things) applies. If only a single value is given, it is applied at the mean streamline independent of its value.
  `dev` | Depending on the value of `k_dev`, this is interpreted as a deviation angle, flow angle, slip factor, or correction to the cosine rule.

  If `i_dev` equals 2 then the deviation for each blade row can be specified, and the following version of section 6 is applicable:

Section 6: Flow angle data specification (n_dev_bladerow lines)

  This version of section 6 is applicable when `i_dev` equals 2.

  The syntax is:

      i_bladerow_dev   i_dev_type   factor1   factor2   factor3   factor4   factor5   factor6

  Parameter | Description
  --- | ---
  `i_bladerow_dev` | Number of the blade row on which the deviation information is specified. The specified values will be applied for all blade row trailing edges downstream of this quasi-orthogonal until the value is changed by a subsequent section 6 with a new value of `i_bladerow_dev`. The first value must be 1.

  `i_dev_type`

  Parameter to define which correlations are used for the blade row deviations. The current deviation correlations incorporated into the method are as follows:

  - Radial Compressor Correlations

    - `i_dev_type` = 101

      Casey-Robinson correlation

  - Axial Compressor Correlations

    - `i_dev_type` = 200

      Recommended correlation (203)

    - `i_dev_type` = 201

      Miller-Wright (original implementation by PCA)

    - `i_dev_type` = 202

      Miller_Wright (1st revision, November 2007)

    - `i_dev_type` = 203

      Miller_Wright (2nd revision, April 2012)

  - Axial Turbine Correlations

    - `i_dev_type` = 400

      Recommended correlation (401)

    - `i_dev_type` = 401

      Kacker-Okapuu

    - `i_dev_type` = 402

      Dunham-Came

  - More General Correlations

    - `i_dev_type` = 501

      User defined on a blade row by blade row basis

    - `i_dev_type` = 502

      Carter’s rule

    - `i_dev_type` = 503

      Cosine rule (Taupel)

  `factor_dev` 1 to `factor_dev` 6

  User-defined coefficients or addition factors to the deviations determined by the correlations. This allows the deviation correlations to be modified to improve matching with experimental or CFD data.

  `i_dev_type` = 11: Casey-Robinson radial compressor model.

  Factor 1: Impeller slip factor for rotors. If this is specified as 0.0 then the Wiesner slip factor is used.

  Factor 1: Deviation angle for stators. If this is specified as 0.0 then Carter’s rule is used.

  Factors 2 to 6: Not in use.

  `i_dev_type` = 21, 22, 23, 24: Correction to deviation.

  Compressor deviation correlations of Miller and Wright for DCA compressor blades with modifications.

  Factor 1: Additive factor in degrees (°) on hub deviation

  Factor 2: Additive factor in degrees (°) on mean deviation

  Factor 3: Additive factor in degrees (°) on tip deviation

  Factors 4 to 6: Not in use.

  Typically values of 0.0 would be used.

  `i_loss_type` = 31: Graham Cox radial turbine model.

  Factor 1: Shroud deviation angle offset (d_s). If specified as 0.0 then 10.0° is used.

  Secondary deviation parameters for the hub:

  Factor 2: Hub related vortex swirl (half) amplitude (Amp_h). If specified as 0.0 then 3.0 is used.

  Factor 3: Hub related vortex swirl variation 1/4 wavelength (QW-h). If 0.0 is specified then 0.34 is used.

  Secondary deviation parameters for the shroud:

  Factor 4: Shroud related vortex swirl (half) amplitude (Amp_s). If 0.0 is specified then 6.0 is used.

  Factor 5: Shroud related vortex centre (VC s). If 0.0 is specified then 0.86 is used.

  Factor 6: Hub trailing edge thickness parameter. If specified as less than 0.07 then 0.26 is used, otherwise 0.16 is used.

  For details see publication of Cox. Note that values of 0.0 for all parameters is acceptable.

  `i_dev_type` = 41 or 42: Kacker-Okapuu, Dunham-Came.

  Turbine deviation using the cosine rule.

  These have different functions for the different correlation systems. In the case of the Cox-Casey correlations these provide some empirical constants for the models used. Otherwise generally as follows.

  Factor 1: Additive factor in degrees (°) on hub deviation.

  Factor 2: Additive factor in degrees (°) on mean deviation.

  Factor 3: Additive factor in degrees (°) on tip deviation.

  Factor 4: Not in use.

  Factor 5: Not in use.

  Factor 6: Not in use.

Section 7: Blockage input data locations

  The syntax is:

      n_ewb_sl   n_ewb_qo

  or

      n_ewb_bladerow   n_dummy

  If `i_ewb` equals 0 or 1 then the blockage for each quasi-orthogonal can be specified, and the following values are required:

  Parameter | Description
  --- | ---
  `n_ewb_sl` | Number of spanwise positions for which the blockage data is supplied.
  `n_ewb_qo` | Number of quasi-orthogonal calculating stations on which the blockage information is specified.

  If `i_ewb` equals 2 then the blockage correlation can be specified for each blade row, and the following values are required:

  Parameter | Description
  --- | ---
  `n_ewb_bladerow` | Number of separate blade rows for which the blockage is supplied.
  `n_dummy` | A dummy integer value to ensure that section 7 always has two integer values.

  If `i_ewb` equals 0 or 1 then the blockage for each quasi-orthogonal can be specified, and the following version of section 8 is applicable:

Section 8: End wall blockage data specification (n_dev_qo * n_dev_sl lines)

  This version of section 8 is applicable when `i_ewb` equals 0 or 1.

  The syntax is:

      i_qo_ewb   k_ewb   f_ewb   ewb

  Parameter | Description
  --- | ---
  `i_qo_ewb` | Number of the quasi-orthogonal calculating station on which the blockage information is specified. The specified values will be applied for all blade rows and calculating stations downstream of this quasi-orthogonal until the value is changed by a subsequent section 4 with a new value of `j_qo_ewb`. The first value must be 1.
  `k_ewb` | Determines the type of blockage calculation. Has no effect because the blockage is input in only one form as below.
  `f_ewb` | The spanwise location of the value of the blockage. If only a single value is given, it is applied at all streamlines.
  `ewb` | End-wall boundary layer blockage is specified. A value of 0.05 represents 5% blockage of the flow channel by the end-wall boundary layers. If zero is specified then there is no end-wall boundary layer blockage. Typically a constant value is specified across the whole span, but this parameter can be varied across the span to allow for the higher blockage in the end-walls related to blade ends with tip clearance.

  If `i_ewb` equals 2 then the blockage for each blade row can be specified, and the following version of section 8 is applicable:

Section 8: End wall blockage data specification (n_ewb_bladerow lines)

  This version of section 8 is applicable when `i_ewb` equals 2.

  The syntax is:

      i_bladerow_ewb   i_ewb_type   factor1   factor2   factor3   factor4   factor5   factor6

  Parameter | Description
  --- | ---
  `i_bladerow_ewb` | Number of the blade row on which the blockage information is specified. The specified values will be applied for all blade row trailing edges downstream of this quasi-orthogonal until the value is changed by a subsequent section 6 with a new value of `i_bladerow_ewb`. The first value must be 1.

  `i_ewb_type`

  Parameter to define which correlations are used for the blade-row blockage. Currently only axial compressor blockage correlations based on the Miller-Wright calculations are incorporated into the method as follows:

  - `i_ewb_type` = 200

    Recommended (202)

  - `i_ewb_type` = 201

    Blockage calculated using the Miller Wright method adjusted to allow the blockage to vary through the blade row. The blockage value, however, is not used.

  - `i_ewb_type` = 202

    Blockage calculated as in `i_ewb_type` = 201. The calculated values are used. The calculation leads to different values of blockage at all quasi-orthogonals and is based on a throughflow interpretation of the Miller Wright method.

  - `i_ewb_type` = 203

    Blockage calculated and not used. The value of the blockage is calculated at trailing edges only and then remains constant to the next trailing edge. This is done to be consistent with SC90C blockage calculations, which are based on a ductflow interpretation of the Miller Wright method.

  `factor_ewb` 1 to `factor_ewb` 6

  User-defined multiplication or addition factors to the blockage determined by the correlations. This allows the end-wall blockage correlations to be modified to improve matching with experimental or CFD data. These have different functions for the different correlation systems.

  Factor 1: Not in use.

  Factor 2: Not in use.

  Factor 3: Not in use.

  Factor 4: Not in use.

  Factor 5: Not in use.

  Factor 6: Not in use.

#### 13.2.4.8. Specification of the Real Gas Properties Data File (*.rgp)

The real gas property input data file includes lines of text that help you to identify the parameters defined there. The name `.rgp` is used to describe this file, but the content is different compared to the usual (ANSYS CFX) real gas property file, which has a similar name.

An example of a real gas property data file is given in Appendix H: Example of a Real Gas Property Data File (*.rgp).

Section 1: Character strings identifying the aerodynamic data (max 72 characters/line)

  The syntax is:

      Character string - title(1)
      Character string - title(2)
      Character string - title(3)

Section 2: Name of gas (72 characters)

  The syntax is:

      gas_name

  Parameter | Description
  --- | ---
  `gas_name` | Text characters defining the gas name

Section 3: Molecular mass and/or Gas constant

  The syntax is:

      MW Gas_R

  Parameter | Description
  --- | ---
  `MW` | Molecular mass of gas (kg/kmol)
  `Gas_R` | Gas constant = Universal gas constant/MW J(kg/K)

  Note that if either of these values is specified with a numerical value of less than 0.1 then it is calculated from the universal gas constant using the other value, which needs to be specified correctly.

Section 4: Critical point parameters and acentric factor

  The syntax is:

      Pc (Pa) Tc (K) Vc (m3/kg) gas_omega (-)

  Parameter | Description
  --- | ---
  `Pc` | Critical pressure (Pa)
  `Tc` | Critical temperature (K)
  `Vc` | Specific volume at critical point (m3/kg)
  `gas_omega` | Acentric factor (-)

Section 5: Temperature limits of specific heat curve polynomial

  The syntax is:

      T_min (K) T_max(K) order_T_poly (max 8)

  Parameter | Description
  --- | ---
  `T_min` | Lowest temperature in range (K)
  `T_max` | Highest temperature in range (K)
  `n_T_coeff` | number of coefficients = Order of polynomial plus 1

Section 6: Coefficients of cp polynomial (T_min < T < T_max)

  The syntax is:

      A1 A2 A3 A4 A5 A6 A7 A8

  Parameter | Description
  --- | ---
  `A1` | First coefficient in polynomial
  `A2` | Second coefficient in polynomial
  `…` | Subsequent coefficients
  `A8` | Eighth coefficient in polynomial

Note that this representation only allows a single interval dependant polynomial to be defined. If a third order polynomial is specified then only four coefficients are needed.

Note that if the value of the first coefficient specified is less than the value of the gas constant then all of the coefficients will be multiplied by the gas constant as in some databases this form of the coefficients is used.

#### 13.2.4.9. Specification of the Output Data File (*.out)

The output data file includes lines of text in ASCII format that show the results of the simulation. The file consists of several sections:

Section 1: Input data

  At the start of this file, a list of the input data files that were used is recorded in this file so that a record of the file names is available.

      INPUT DATA FILES:        Control data file: agard.con
                               Geometric data file: agard.geo
                               Aerodynamic data file: agard.aer
                               Correlation data file: agard.cor
                               Restart data file: agard.rst
      OUTPUT DATA FILES:       Results file: agard.out
                               Tecplot data file: impeller.txt
                               CFD-POST data file: agard.csv
                               Convergence history file: agard.hst
                               Interface output file: agard.int

Section 2: Reference data

  The program uses the input data to set up the values of various other parameters; for example, where the reference mass flow is specified, the reference volume flow is calculated. The values of all other parameters not included in the input specification are given in this section. In addition, the internal calculation of the damping factors is provided. Other data listed here relates to the program's own estimates of the throat area and the throat position. An example is given below.

  Example radial compressor calculation:

      Reference flow parameters
      -------------------------

      Mass flow distribution across streamlines:
       0.000 0.062 0.125 0.188 0.250 0.312 0.375 0.438 0.500 0.562
       0.625 0.688 0.750 0.812 0.875 0.938 1.000

      Inlet distribution across streamlines:
       Fraction of flow: 0.00
       Total pressure: 100000.00
       Total temperature: 293.00
       Inlet swirl: 0.00

      Ideal gas calculation

      gamma_gas gas_m r_gas cp_gas
       1.400 3.500 287.200 1005.200

      ref_pt(bar) ref_tt ref_rhot ref_soundt
         1.0000 293.00 1.1884 343.23

      Reference rotational direction: clockwise

      ref_d ref_u ref_omega ref_n
      0.2700 398.10 2948.91 28160.0

      ref_mach ref_phi ref_mass ref_volume
      1.1599 0.0667 2.3000 1.94

      ref_re ref_mue
       6963614.0 0.00001834

      ref_n1 ref_n2 ref_n3
         28160.0 0.0 0.0

      Simulation with no spanwise mixing

      Iterate to mass flow, ref_mass =        2.30000

      First approximation of streamline positions
      taken from an earlier calculation

      Estimated max. thicknesses for blade row 1
      span 0.00000 0.17343 0.34429 0.51305 0.67879 0.84126 0.97669 1.00000
      thickne 0.00351 0.00319 0.00291 0.00266 0.00241 0.00215 0.00195 0.00191

      User-input throat widths for blade row 1
      span 0.00000 0.17343 0.34429 0.51305 0.67879 0.84126 0.97669 1.00000
      throat 0.01760 0.02137 0.02460 0.02732 0.02959 0.03141 0.03257 0.03276

      Estimated throat positions for blade row 1
      span 0.00000 0.17343 0.34429 0.51305 0.67879 0.84126 0.97669 1.00000
      throat_pos 0.00969 0.02084 0.03424 0.04835 0.06224 0.07573 0.08688 0.08882

      Empirical correlation data

             User specified losses
             User specified deviation
             No blockage specified

      Relaxation factor calculation of Wilkinson
      ------------------------------------------

      Maximum aspect ratio:      6.0667
      at calculating station:    5
      damp_sc (user input):      0.2500
      damp_sc (Wilkinson):       0.0577

      Warning: damp_sc reduced by the code
               to the value suggested by Wilkinson

Section 3: Short history of the convergence

  The `.out` file contains a statement about convergence of the results. A converged calculation includes a header such as the following:

      ***********************************************
      * VistaTF          converged -it_main: 6      *
      *                                             *
      *  cm_error(%)   p_error(%)   mass_error(%)   *
      *     0.042        0.000         0.000        *
      ***********************************************
      *    Global performance                       *
      *                                             *
      *    mass (kg/s):         0.093200            *
      *    est. choke:          0.107995            *
      *                  t-t      t-s      s-s      *
      *    eta_p:        0.8453   0.7415            *
      *    eta_s:        0.8553   0.7583            *
      *    pr:           0.5800   0.5374   0.6100   *
      *    er (1/pr):    1.7243   1.8609   1.6392   *
      *    power (kW):             -5.4316          *
      ***********************************************

  A more detailed convergence history is output to the history file, which is described in Specification of Convergence History Data File (*.hst).

Section 4 : Simulation results on quasi-orthogonal planes and streamlines

  Results are provided at every quasi-orthogonal requested (see control file parameter `i_print_plane`) in the level of detail requested (parameter `i_print_level`). The data is provided across the span for each streamline. If the number of streamlines is greater than 9 then data for every second streamline is given. The structure of this data and the information provided varies depending on the type of calculation station. The example below is for a radial impeller leading edge:

      Quasi-orthogonal - i = 3
       n_blade n_curve i_type i_row i_spool
         13       6       3      0     0
      Rotor blade - leading edge
      At throat (or just upstream of throat)
      Compressor
      Radial impeller
      Throat area =   0.00274713
      Annulus choke parameters: dm_dcm = 0.79601  Mach_eff = 0.45166
      choke mass at this q_o           =    7.72100
      choke_mass of machine            =    7.72100
      choke_mass of this blade row     =    7.72100
      current_mass at this q_o         =    6.70000
      inlet mass flow                  =    6.70000
      Factor on slope of ree: grad_re = 1.00000   cm_guess_save = 152.57564
      Flow parameters - print_level=1
      streamline    1       3       5       7       9      11      13      15      17
      r [m]      0.07612 0.08753 0.09759 0.10647 0.11445 0.12176 0.12855 0.13493 0.14100
      z [m]     -0.13500-0.13500-0.13500-0.13500-0.13500-0.13500-0.13500-0.13500-0.13500
      1/rc[1/m]   -5.996   1.353   2.758   2.818   2.475   1.984   1.438   0.864   0.244
      throat mm    23.00   24.41   25.66   26.77   27.40   27.84   28.17   28.30   29.00
      f_sl [-]   0.17503 0.17777 0.18110 0.18431 0.18734 0.19021 0.19295 0.19556 0.19806
      f_qo [-]   0.00000 0.17593 0.33098 0.46775 0.59076 0.70340 0.80807 0.90652 1.00000
      f_bl [-]   0.00000 0.00000 0.00000 0.00000 0.00000 0.00000 0.00000 0.00000 0.00000
      f_thr [-]  0.02584 0.03400 0.04157 0.04823 0.05408 0.05923 0.06379 0.06785 0.07150
      gamma_in   1.00000 1.00000 1.00000 1.00000 1.00000 1.00000 1.00000 1.00000 1.00000
      gamma_out  0.00000 0.00000 0.00000 0.00000 0.00000 0.00000 0.00000 0.00000 0.00000
      cm [m/s]    146.87  142.25  145.30  149.18  152.57  155.22  157.11  158.32  158.87
      - error %  0.0001 -0.0002  0.0001  0.0001  0.0001  0.0001  0.0000 -0.0002 -0.0001
      - max       169.57  166.48  168.30  172.19  174.87  177.33  179.61  180.96  186.11
      cu [m/s]      0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      M_cm [-]     0.437   0.423   0.432   0.444   0.455   0.463   0.469   0.472   0.474
      M_crit[-]    1.000   1.000   1.000   1.000   1.000   1.000   1.000   1.000   1.000
      M_rel [-]    0.765   0.837   0.914   0.985   1.050   1.109   1.163   1.213   1.260
      beta_fl°    -55.19  -59.65  -61.79  -63.21  -64.34  -65.33  -66.23  -67.08  -67.90
      beta_bl°    -43.03  -46.77  -50.17  -52.99  -55.37  -57.46  -59.30  -60.92  -62.35
      incidence    12.16   12.88   11.62   10.22    8.98    7.86    6.93    6.16    5.55
      p [bar]     0.8706  0.8778  0.8730  0.8669  0.8614  0.8571  0.8540  0.8519  0.8510
      t [K]       282.38  283.04  282.60  282.04  281.54  281.14  280.84  280.66  280.57
      rho[kg/m3]  1.0742  1.0806  1.0764  1.0710  1.0661  1.0623  1.0595  1.0577  1.0569
      A*/A        0.9485  0.9758  0.9935  0.9998  0.9980  0.9907  0.9799  0.9666  0.9517
      m/m_max     0.8661  0.8545  0.8633  0.8664  0.8725  0.8753  0.8747  0.8749  0.8536
      m_prime      75.46   84.55   95.91  106.88  116.97  126.15  134.46  141.98  148.76
      m_pr_max     87.12   98.94  111.09  123.37  134.07  144.11  153.70  162.27  174.26
      ch_ratio    0.8662  0.8545  0.8634  0.8664  0.8725  0.8753  0.8748  0.8749  0.8537
      Flow parameters - print_level=2
      eps   [°]    12.82   14.30   12.54   10.34    8.13    6.01    4.00    2.08    0.23
      psi   [°]    77.18   75.70   77.46   79.66   81.87   83.99   86.00   87.92   89.77
      c   [m/s]   146.87  142.25  145.30  149.18  152.57  155.22  157.11  158.32  158.87
      w   [m/s]   257.28  281.50  307.34  330.98  352.35  371.83  389.80  406.55  422.31
      u   [m/s]   211.24  242.91  270.83  295.46  317.60  337.88  356.73  374.45  391.29
      wu  [m/s]  -211.24 -242.91 -270.83 -295.46 -317.60 -337.88 -356.73 -374.45 -391.29
      M_abs [-]    0.437   0.423   0.432   0.444   0.455   0.463   0.469   0.472   0.474
      alpha_fl°     0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      pt  [bar]   0.9921  0.9921  0.9921  0.9921  0.9921  0.9921  0.9921  0.9921  0.9921
      tt    [K]   293.00  293.00  293.00  293.00  293.00  293.00  293.00  293.00  293.00
      s [J/kgK]     2.29    2.29    2.29    2.29    2.29    2.29    2.29    2.29    2.29
      ds[J/kgK]     0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      ewb   [-]   0.0500  0.0500  0.0500  0.0500  0.0500  0.0500  0.0500  0.0500  0.0500
      Loading parameters - print_level=3
      w_s  [m/s]  287.34  314.82  342.24  366.60  388.17  407.50  425.12  441.51  456.87
      w_p  [m/s]  227.21  248.18  272.45  295.36  316.53  336.16  354.47  371.59  387.74
      M_ws   [-]  0.855    0.936   1.018   1.091   1.157   1.215   1.268   1.318   1.364
      M_wp   [-]  0.676    0.738   0.810   0.879   0.943   1.002   1.058   1.109   1.157
      C_btob [-]  0.234    0.237   0.227   0.215   0.203   0.192   0.181   0.172   0.164

#### 13.2.4.10. Specification of the Text Data File (*.txt)

The text data file includes lines of text in ASCII format that are intended as input for various software packages for producing plots of the converged results. The text files can be used as input data for Tecplot. Standard layout (`.lay`) files for Tecplot have been prepared which allow typical diagrams to be produced on the basis of this data. The information is structured in such a way that it can just as easily be used by Excel or some other similar program with an appropriate interface.

In fact, after running the program, several standard `.txt` files for Tecplot are produced: one covering the whole flow field and one for each blade row. The flow field data is written in the file `prefix.txt`, and the blade-row data in the files `row_01_prefix.txt`, `row_02_prefix.txt`, and so on, whereby the number of the files refers to the blade rows numbered from the start of the computational domain. You only need to provide the name of one of these files in the `vista_tf.fil` file, because the others are automatically generated and numbered by the program.

Some standard Tecplot layout files have been prepared that operate on the `.txt` files to produce typical plots that are needed during the design of a component. For example, the files used for radial compressor impellers are called: `flowfield_2d_v_2_0.lay` and `rc_impeller_row1.lay`. The first of these prepares a plot showing the 2D meridional channel with contours of constant parameters (such as meridional velocity, swirl velocity, static temperature, Mach number, `cm_error` and so on) and the second prepares blade loading plots for a typical blade row. The layout file (`.lay`) determines the format of the plot and the ASCII `.txt` file contains the data to be plotted. The format and the scales can also be changed on-line within Tecplot by clicking on the screen. Other Layout files for other cases (ac = axial compressor, hp = hydraulic pump, ht= hydraulic turbine, rt = radial turbine, at= axial turbine) are also available and these can be easily customized (scales, parameters and so on).

The standard Tecplot layout files (`.lay`) have all been written to work on the data in text files named `impeller.txt` and `row_01_impeller.txt`, and so on. The first dataset, `impeller.txt`, contains information for the contour plots showing the meridional velocity and other parameters projected on the meridional plane and the second, `row_01_impeller.txt`, contains the various blade loading parameters for an individual blade row. If the case concerned has several blade rows then there is also a file called `row_02_impeller.txt`, `row_03_impeller.txt`, and so on; there is one file for each blade row. A new layout file is needed for each blade row. The letters “impeller” in this name rely on the fact that the prefix for the `.txt` file has this name in the `vista_tf.fil` file.

Other prefixes will produce `.txt` files containing the prefix as specified in the `vista_tf.fil` file. In this case, the layout files need to be modified; the layout files can be opened in a text editor; the name of the `.txt` file is on the second line. This name can then be changed to match the name given as a prefix in the `vista_tf.fil` file. Alternatively, the same layout files can be used for several cases if all data that needs to be plotted always retains the prefix name `impeller`; the text output file from `vista_tf` always has the name `impeller.txt` in the `vista_tf.fil` file.

Generally, a good strategy is to set up the `.aero`, `.cor`, `.con`, and `.txt` files with a certain prefix in the `vista_tf` file and to let these keep the same names for all runs on a particular case because they normally do not change as the design progresses. It then remains necessary to switch the `.geo` files around to look at different impellers, or else the prefix for the `.geo` file can be retained and the cases can be distinguished by simply putting them into different directories to distinguish the different cases.

The data in the `prefix.txt` file is in approximately the following format:

    TITLE
    Flow field data for whole flow field from hub to shroud for all q-os

    Variables = '"r" "z" "cm" "cu" "cr" "cz" "p" "t" "pt" "tt" "s" "h" "q_o" "error" "choke_ratio"
    "M_rel" "M_abs" "alpha_flow" "beta_flow" "1/rc" "beta"'

    "r"                  Radius coordinate
    "z"                  Axial coordinate
    "cm"                 Meridional velocity
    "cu"                 Swirl velocity
    "cr"                 Radial velocity
    "cz"                 Axial velocity
    "p"                  Static pressure
    "t"                  Static temperature
    "pt"                 Total pressure
    "tt"                 Total temperature
    "s"                  Entropy
    "h"                  Static enthalpy
    “q_o”                an integer identifying the particular type of q-o
    “error”              Meridional velocity error in %
    "choke_ratio"        choke ratio (ratio of local mass flow to choke flow at this location)
    "M_rel"              Relative Mach number
    "M_abs"              Absolute Mach number
    "alpha_flow"         Absolute flow angle [°]
    "beta_flow"          Relative flow angle [°]
    "1/rc"               Curvature ( inverse of the radium of curvature)
    "beta”               Blade angle [°]

The data in the `row_01_prefix.txt` file is approximately in the following format:

    TITLE
    Data on hub, mean and tip streamlines for all blade rows from LE to TE
    and data along leading edge and trailing edge of all blade rows

    VARIABLES =VARIABLES = "i_type", "f_bl", "M", "M_s", "M_p", "w", "w_s", "w_p",...
    "p", "p_s", "p_p", "c_btob", "c_htos", "beta_bl", "beta_fl", "dep_angle", "gamma_in", ...
    gamma_out", "f_qo", "de_haller", "cp_ideal", "incidence", "deviation", "lambda", ...
    "df_lieblein", "zweifel" "c_lift", "c_zw"
    "f_bl"               Fraction of meridional distance along the blade
    "M"                  Mean mid-passage Mach number (relative to blade)
    "M_s"                Suction side Mach number
    "M_p"                Pressure side Mach number
    "w"                  Mean mid-passage velocity (relative to blade)
    "w_s"                Suction surface velocity
    "w_p"                Pressure surface velocity
    "p"                  Static pressure in mid-channel between two blades
    "p_s"                Suction surface static pressure
    "p_p"                Pressure surface static pressure
    "c_btob"             Blade to blade loading parameter
                         (c_btob = (w_s-w_p)/w, that is the difference between suction surface
                         and pressure surface velocities divided by the mid-channel velocity
    "c_htos"             Hub to shroud loading parameter
                         (c_htos = (cm_shroud – cm_hub)/ cm_mean, that is the difference
                         between the meridional velocity on the casing and the hub divided by
                         the mean velocity.
    "beta_bl"            Blade angle in degrees [°]
    "beta_fl"            Flow angle in degrees [°]
    "dep_angle"          Departure angle in degrees [°]
    "gamma_in"           Blending function at blade inlet
    "gamma_out"          Blending function at blade outlet
    "f_qo"               fractional distance along q-o
    "de_haller"          De Haller number
                         (de_haller = w2/w1, that is outlet/ inlet relative velocity
    "cp_ideal"           Ideal static pressure recovery coefficient
                         ( Cpideal = 1 – (de_haller)**2 )
    "incidence"          Incidence at the leading edge [°]
    "deviation"          Deviation at the trailing edge[°]
    "lambda"             Work coefficient ( lambda = (h2-h1)/u**2, that is Deltah / u squared)
    "df_lieblein"        Lieblein Diffusion Factor (see below)
    "zweifel"            Zweifel loading parameter (see below)
    "c_lift"             Lift coefficient (see below)
    "c_zw"               Lift coefficient times solidity (see below)

Note that the values of the last four parameters have been included mainly for axial blade rows. Each of them includes the blade solidity (ratio of chord to spacing) in its definition. In radial machines, the spacing and solidity change with radius along the streamline. There is no generally agreed method to calculate these parameters for radial machines, so the mean value of the spacing has been selected in the following definitions used in Vista TF. In any case, caution is suggested in the use of these parameters for radial machine blade rows because the experimental basis for limit values has generally been derived from axial machines.

Lieblein diffusion factor (df_lieblein)

Zweifel coefficient (zw)

Lift coefficient (CL)

where

Zweifel number (c_zw)

#### 13.2.4.11. Specification of the CFD-Post Output File (*.csv)

The text data files `*prefix.csv` include lines of text in ASCII Comma Separated Variable format. These files contain user surface data for CFD-Post, and are intended as input for CFD-Post for plotting purposes. For details on the user surface data format for CFD-Post, see USER SURFACE Data Format in the CFD-Post User's Guide.

In the current `.csv` files, the following data is available for each grid node:

    [Name]
    Vista-TF
    [Data]
    X [m], Y [m], Z [m], Cm [m/s], Cu [m/s], Cr [m/s], Cz [m/s], p [bar], t [K], s [J kg^-1 K^-1],
    h [J/kg], q_o [], error [], M_rel[], M_abs[], rc [m^-1]

The file `global_prefix.csv` contains a list of parameters, whereby these are specified as:

    Name 1 = value1 [units]
    Name 2 = value2 [units]

Separated by comment lines which begin with “`#`”.

In addition, there are four additional files produced for each blade row from 1 to n:

    row_0n_hub_prefix.csv
    row_0n_mean_prefix.csv
    row_0n_tip_prefix.csv
    row_0n_loading_prefix.csv

These contain essentially similar information to the `row_0n_prefix.txt` files described above, but this is split into four separate files: one for the hub, one for the mean span, one for the tip, and one for the loading parameters.

#### 13.2.4.12. Specification of Convergence History Data File (*.hst)

The convergence history data file includes lines of text in ASCII format that show the convergence of the simulation. This contains details of the convergence of the main iterative procedures, and extensive details of the terms in the radial equilibrium equation for each stream tube and calculating plane. It is rare for this to be examined in any depth, but this can be useful to identify problems if the solution fails to converge.

Section1: Input Data

  At the start of the `.hst` file, the input data is recorded. This is essentially in the same format as the input files. At the start of this file, there is a list of the names of the input data files that were used. This information can be useful if an error occurs in the input data because the `.hst` file records only the data that has been successfully read into the program.

Section 2: Convergence Data

  At every iteration, a summary of the iteration progress is provided. It looks like this:

      History of the main iteration loop
      ----------------------------------
          it_main: 1 error_cm(%): 100.000 at i_qo: 0 j_sl: 0 it_mass: 11 at i_qo: 1
          it_main: 2 error_cm(%): 38.940 at i_qo:10 j_sl:17 it_mass: 11 at i_qo: 1
          it_main: 3 error_cm(%): 30.036 at i_qo:10 j_sl:17 it_mass: 11 at i_qo: 3
          it_main: 4 error_cm(%): 24.600 at i_qo:10 j_sl:17 it_mass: 11 at i_qo: 4
          it_main: 5 error_cm(%): 20.939 at i_qo:10 j_sl:17 it_mass: 11 at i_qo: 5
          it_main: 6 error_cm(%): 18.306 at i_qo:10 j_sl:17 it_mass: 11 at i_qo: 6
          it_main: 7 error_cm(%): 16.403 at i_qo:10 j_sl:17 it_mass: 11 at i_qo: 6

      .....

          it_main: 284 error_cm(%): 0.013 at i_qo: 7 j_sl:17 it_mass: 1 at i_qo: 1
          it_main: 285 error_cm(%): 0.012 at i_qo: 7 j_sl:17 it_mass: 1 at i_qo: 1
          it_main: 286 error_cm(%): 0.011 at i_qo: 7 j_sl:17 it_mass: 1 at i_qo: 1
          it_main: 287 error_cm(%): 0.010 at i_qo: 7 j_sl:17 it_mass: 1 at i_qo: 1
          it_main: 288 error_cm(%): 0.009 at i_qo: 7 j_sl:17 it_mass: 1 at i_qo: 1

Section 3: Streamline Curvature Solution Data

  At every quasi-orthogonal, details of the terms in the radial equilibrium equation for each stream tube are provided. This can be useful in identifying errors and also helpful to determine the magnitude of the terms in the equations. “rhs” is the value of the right hand side of the radial equilibrium equation, giving the square of the gradient of the meridional velocity.

  The streamline curvature solution data looks like this:

      Quasi-orthogonal - i = 5
       n_blade n_curve i_type i_row i_spool
          9       8       3      0     0
      Radial equilibrium parameters -print_level = 4
      rhs          1049.90 1059.86  871.10  684.48  510.68  349.39  199.63   55.28
      ret             0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      ret_dh          0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      ret_tds         0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      ret_drcu        0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      sct          1049.90 1059.86  871.10  684.48  510.68  349.39  199.63   55.28
      sct_rc        641.48  681.97  558.43  431.70  315.91  211.42  118.25   34.87
      sct_dcm       408.43  377.89  312.67  252.78  194.78  137.97   81.38   20.40
      bft             0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      dft             0.00    0.00    0.00    0.00    0.00    0.00    0.00    0.00
      cm_error%    -0.0010  0.0002 -0.0003 -0.0007 -0.0007 -0.0003  0.0003  0.0010
      f_mixing      0.0000  0.0000  0.0000  0.0000  0.0000  0.0000  0.0000  0.0000
      1/rc       2.853   4.466   4.153   3.505   2.773   2.016   1.261   0.517  -0.209
      cm       137.936 145.590 152.396 157.708 161.716 164.594 166.473 167.450 167.568
      rcu        0.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000
      drcu/dm   47.323  53.336  48.562  35.419  15.376 -11.226 -43.868 -81.313-123.649
      s          1.885   1.885   1.885   1.885   1.885   1.885   1.885   1.885   1.885
      bl_block   0.0000  0.0000  0.0000  0.0000  0.0000  0.0000  0.0000  0.0000  0.0000

Release 18.2 - © ANSYS, Inc. All rights reserved.