label TOP
q1quit=t;dmpstk=f;nocomm=t;nocopy=t;nowipe=t
rset(v,0)
 
  Preliminaries :
 
  Satelite subroutine sat calls CHKINP for FORTRAN string comparison
 
namsat=chkc
 
  Set up 4 character values, and one logical.  Logical is set true
  immediately prior to satrun call, and is returned false
 
  Character strings are set to give prompts and accept data for test
 
boolean(log1)
char(cvl1,cvl2,cvl3,cvl4);cvl3='Correct!'
 
        QCOM statements are used to annotate the Q1 file, DCOM to
        process command and annotate Q1 file
 
               -----        start of tutorial :   -----
 
      write group identifiers etc to Q1 file
 
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 1. Run title and other preliminaries
qcom(  *
  display
                   WELCOME TO PIL TUTORIAL NUMBER 1
                   ********************************
 
        This tutorial starts to teach you the basic PIL commands
        and specifies a simple problem of flow in a channel
        which can then be run by PHOENICS.
 
        This tutorial defines the problem shown.
 
                              Wall
             __________________________________________
            |                                          |
            |                                          |
            |                                          |
    Inlet   |                                          | Outlet
          Y |                                          |
          ^ |                                          |
          | |                                          |
          | |__________________________________________|
             ----> X           Wall
 
CALL LOAD_96
        The tutorial is configured to expect valid PIL commands
        to be entered by you at the terminal.
 
 
        String comparison is then undertaken to ensure that you
        have entered the correct data.
 
 
        As such, it is important to note that the exact numbers
        are required to be input.
 
 
        *     YOU MUST READ the panels presented to you
        *     The form of the PIL commands and other hints are given
 
        NB: You can quit the tutorial at any time by entering "quit"
 
 
 
CALL LOAD_96
                             GRID
        X-Direction                            Y-Direction
    XLength       : 0.5                    YLength       : 0.1
    No. of regions: 1                      No. of regions: 1
    No. of cells  : 10                     No. of cells  : -20
    Power         : 1.0                    Power         : 1.4
 
    NB. Negative sign on No. of cells in Y indicates that these
        are symmetrically distributed.
 
 
 
 
CALL LOAD_96
                             VARIABLES
 
    Solved: P1, U1, V1                          Stored : ENUT
 
 
                             PROPERTIES
 
    Turbulence model           : k-epsilon
    Reference pressure (PRESS0): 1.E5
    Density            (RHO1  ): 1.22
    Viscosity          (ENUL  ): 1.4654E-4
 
                             INITIAL FIELDS
 
    KE=0.04      ;   EP=0.13
 
 
 
 
CALL LOAD_96
                             BOUNDARY CONDITIONS
 
        All PATCH LOCATIONS ARE: #1,#1,#1,#1,#1,#1,#1,#1
 
                             WALL
 
    NAME        : TOP     ; BOT
    TYPE        : NORTH   ; SOUTH
    PIL var    Coef        Value
     U1       loglaw       0.0
     KE       loglaw       loglaw
     EP       loglaw       loglaw
 
 
 
 
CALL LOAD_96
                             INLET
 
    NAME        : INLET
    TYPE        : WEST
    PIL var    Value
    P1        10.0*rho1
    U1        10
    V1        0.0
    KE        0.04
    EP        0.13
 
 
 
 
CALL LOAD_96
                             OUTLET
 
    NAME        : OUT
    TYPE        : EAST
    PIL var    Value
    P1          0.0
 
 
 
 
CALL LOAD_96
                *    Start of Tutorial 1    *
 
            * * * EXPECTED title is 'tutorial.1'
 
        Group 1 of the Q1 file is used to specify the title
        of the prediction
 
 
        The title should be a unique identifier. This is
        presented on PHOTON output, and included in results
        files.
 
        The PIL command to set the title has the syntax:
 
        TEXT(Required Text
 
        The required text in this case is the title shown above
        hence the input required at the prompt MUST be
 
                      text(Tutorial.1
cvl2=text(Tutorial.1
cvl4='Please_enter_the_TEXT_command_to_set_the_title_for_this_case'
CALL LOAD_95
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 2. Transience; time-step specification
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 3. X-direction grid specification
qcom(  *
                    regions in x = 1
            GROUP 2. Transience; time-step specification
            GROUP 3. X-direction grid specification
 
        There are several methods available within PHOENICS to
        define the computational mesh.  This Tutorial will
        exemplify the method of REGIONS and gridpower
 
        Hence, The first step in setting the mesh for this
        tutorial is to define the number of regions in the X
        direction
        These region identities are then used to control the
        mesh spacing according to other PIL commands
 
        The number of regions in each direction is given
        by a PIL command with the syntax
 
            NREGdir=integer number
        where :
        dir is T,X,Y, or Z for time,or spatial co-ordinates
        and the integer is the required number of regions
cvl4='Please_set_the_number_of_regions_in_the_x_direction_to_1'
cvl2=nregx=1
CALL LOAD_95
        * * * * * iregx 1 + grdpwr
 
        Having specified the number of regions in X,
        we now have to specify the cell spacing in each region
 
        To do this requires two operations:
 
         1) to identify the relevant region
         2) to specify the grid spacing
 
        The identification of the relevant region is via
        a PIL statement with the Syntax
 
             IREGdir=integer number
 
        where :
        dir is T,X,Y, or Z for time,or spatial co-ordinates
        the integer is the required region
cvl4='Please_enter_the_index_of_the_first_x_region_to_be_modified'
cvl2=iregx=1
CALL LOAD_95
        Cell spacing in region 1 is determined via a PIL statement
        with the syntax:
                     GRDPWR(dir,IC,LENGTH,PWR)
 
        where :
        dir is T,X,Y, or Z for time, and spatial co-ordinates
        IC is the number of cells in the region
        LENGTH is the extent of the region
        PWR is the power that is used to distribute the cells
 
        GRDPWR(x,10,100,1.4)
 
        would put 10 cells in x over 100 metres, with small cells
        at the beginning, large cells at the end.
        Negative powers will put large cells at the beginning!
 
        Negative numbers of cells symmetrically place cells
        according to the power
        reminder: xlength=0.5; no. of cells = 10; power=1.0
cvl4='Please_enter_the_distribution_of_cells_in_x_region_1'
cvl2=grdpwr(x,10,0.5,1.0)
CALL LOAD_95
do jj=1,25
mesg(
enddo
                    Congratulations,
 
        You have now set the X direction mesh distribution.
 
 
        This mesh will now be shown by use of the view statement.
 
 
        NOTE: we have only defined the mesh in X thus far.
 
 
 
        please  press "enter" to view the mesh thus far
 
        and then press "enter" again to continue the tutorial
 
 
 
CALL LOAD_96
view(k,1)
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 4. Y-direction grid specification
qcom(  *
                    regions in y = 1
            GROUP 4. Y-direction grid specification
 
        Having completed the specification of the X Mesh,
        The next task is to specify the Mesh in Y, and again
        we will use the method of REGIONS and gridpower
 
        Hence, The first step in setting the mesh in Y
        is to define the number of regions in Y
 
        These region identities are then used to control the
        mesh spacing according to other PIL commands
 
        The number of regions in each direction is given
        by a PIL command with the syntax
 
            NREGdir=integer number
        where :
        dir is T,X,Y, or Z for time, and spatial co-ordinates
        the integer is the required number of regions
cvl4='Please_set_the_number_of_regions_in_y_to_1'
cvl2=nregy=1
CALL LOAD_95
        * * * iregy 1 + grdpwr
 
        The specification in Y is analogous to that in X.
 
        Remember, To do this requires two operations:
 
            1) to identify the region.
            2) to specify the grid spacing
 
        Remember, the identification of the relevant region is
        via a PIL statement with the Syntax
             IREGdir=integer number
        And the grid spacing is specified with
             GRDPWR(dir,IC,LENGTH,PWR)
        where :
        dir is T,X,Y, or Z for time,or spatial co-ordinates
        the integer is the current region to be modified
        IC is the number of cells in the region
        LENGTH is the cartesian extent of the region
        positive/negative power expands/contracts cells
 
        reminder: ylength=0.1 ; No. of cells =-20; power=1.4
cvl4='Please_enter_the_index_of_the_y_region_to_be_modified'
cvl2=iregy=1
CALL LOAD_95
 
cvl4='Please_enter_the_distribution_of_cells_in_y_region_1'
cvl2=grdpwr(y,-20,0.1,1.4)
 
CALL LOAD_95
                     Congratulations,
 
        You have now completed the mesh specification in the
                     XY plane for the tutorial
 
        This mesh will now be shown by use of the view statement
 
 
 
 
        please  press "enter" to view the mesh
 
        and then press "enter" again to continue the tutorial
 
 
 
CALL LOAD_96
view(k,1)
 
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 5. Z-direction grid specification
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 6. Body-fitted coordinates or grid distortion
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 7. Variables stored, solved & named
qcom(  *
                    variables to be solved
    GROUP 5. Z-direction grid specification
    GROUP 6. Body-fitted coordinates or grid distortion
          GROUP 7. Variables stored, solved & named
 
        The PHOENICS code requires you to specify which
        equations are to be solved as the solution proceeds.
 
        PHOENICS solves the Navier-Stokes equations for fluid
        flow using the SIMPLEST scheme.
 
        As such, the relevant velocity component for each
        direction and the pressure are the minimum equations
        to be solved.
 
        The PIL statement has the Syntax
              SOLVE(variable list)
 
        Variables are separated by a comma, and are
            P1                 pressure
            U1                 velocity in X direction
            V1                 velocity in Y direction
cvl4='Please_enter_the_names_of_the_variables_to_be_solved'
cvl2=solve(p1,u1,v1)
CALL LOAD_95
        The solution process for the PRESSURE correction can
        be configured to be "whole field" or slabwise
 
        Slabwise solution is the default, and is more suited
        for thin shear (parabolic), or hyperbolic (supersonic)
        flows
        PIL syntax:  SOLUTN(var,Y,Y,N,N,N,N)
        where  :
        var is the variable name, and the six other parameters
        store,solve,elliptical,jacobi,explicit,harmonic
        For more information, see the encyclopaedia entry
        on SOLUTN
 
        Elliptical (whole field) pressure fields are normal
        for general engineering flows, and are essential for
        flows with recirculations/separations.
 
        This case has recirculation, and hence requires
        an elliptical pressure field.
 
            eg: SOLUTN(P1,Y,Y,Y,N,N,N)
cvl4='Change_pressure_solver_to_be_whole_field'
cvl2=solutn(p1,y,y,y,n,n,n)
CALL LOAD_95
                    other stored variables
 
        The PHOENICS code can solve/store up to 50 variables
        Some of which we have already activated.
 
        Storage of auxiliary variables and properties such as
        density are required according to which problem is being
        examined.
 
        The variables stored can then be under-relaxed if
        required to assist convergence, and are available for
        plotting within PHOTON and AUTOPLOT
 
        This case has no problems with convergence, but will
        use the k-epsilon turbulence model, and the auxiliary
        store for the turbulent viscosity (ENUT) is required
 
        The PIL statement for the storage is :
             STORE(variable list)
 
        For more information, see Encyclopaedia entry on STORE
cvl4='Please_indicate_variables_to_be_stored'
cvl2=store(enut)
CALL LOAD_95
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 8. Terms (in differential equations) & devices
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 9. Properties of the medium (or media)
qcom(  *
                    reference pressure
 
    GROUP 8. Terms (in differential equations) & devices
             GROUP 9. Properties of the medium (or media)
 
        PHOENICS can model fluids with fluid properties that
        vary,for example, density as a function of temperature
        and pressure
 
        The Auxiliary equations used for relationships quite
        often require reference values to avoid divisions by
        zero and to minimise rounding errors.
 
        For this case, we do NOT vary the density, but as a
        measure of "Good Practice" we should set a reference
        pressure.
 
        The PIL Syntax for setting a reference pressure is:
                PRESS0=required real number
 
            ( reminder ref. pressure is 1.e5 )
cvl4='Please_set_the_reference_pressure'
cvl2=press0=1.e5
CALL LOAD_95
                    fluid density
 
        PHOENICS has default values for typical variables
        such as density, laminar viscosity etc.
 
        As mentioned in the previous panel, it is possible to
        specify relationships for these parameters.
 
        For the purpose of this tutorial, the density is
        constant, and its value must be specified.
 
        The PIL statement  :
 
           RHO1=real value
 
        will specify a constant density throughout the flow
        domain.
           (Reminder density=1.22)
cvl4='Please_set_the_fluid_density'
cvl2=rho1=1.22
CALL LOAD_95
 
                    reference laminar viscosity
 
        For a similar reason, we must specify a value for the
 
                      Laminar viscosity
 
        Constant values are specified via a PIL statement:
 
           ENUL=real number
 
         (Reminder viscosity of fluid is 1.465e-5)
cvl4='Please_indicate_the_reference_laminar_viscosity'
cvl2=enul=1.465e-5
CALL LOAD_95
                    activate turbulence models
 
        PHOENICS can use several models of turbulence.
 
        The PIL statement to activate a turbulence model is:
 
           TURMOD(text)
 
        where text is:
 
           KLMODL  -  The Prandtl energy model
           KEMODL  -  The Kolmorogov k-epsilon model
                      (which solves KE and EP)
 
        Other models are available, such as
        fixed viscosity (PIL:  ENUT=required viscosity)
        Laminar         (PIL:  ENUT=0.0)
cvl4='Please_activate_the_k-epsilon_turbulence_model'
cvl2=turmod(kemodl)
CALL LOAD_95
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 10. Inter-phase-transfer processes and properties
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 11. Initialization of variable or porosity fields
qcom(  *
                    set initial fields
 
        PHOENICS uses an iterative solution process to reach
        the predicted flow.
 
        As such, some guesses to the initial fields should be
        supplied to the iterative solver.
 
        All initial fields are set to 1.e-10 by default
 
        If this value is inapropriate for any variable then
        we can set these to suit. with the PIL statement
 
             FIINIT(var)=required value
 
         eg:  FIINIT(U1)=100
 
              sets uniform U1 velocity of 100 ms-1
 
cvl4='Please_set_initial_field_value_of_0.04_for_ke'
cvl2=fiinit(ke)=0.04
CALL LOAD_95
 
 
do jj=1,25
mesg(
enddo
        It is normally good practice to set initial fields
 
        for both ke and ep to minimise convergence problems
 
cvl4='Please_set_initial_field_value_of_0.13_for_epsilon'
cvl2=fiinit(ep)=0.13
CALL LOAD_95
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  * GROUP 12. Patchwise adjustment of terms
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  * GROUP 13. Boundary conditions and special sources
qcom(  *
        Having specified the geometry and the fluid properties
        we must now indicate the locations of relevant boundaries
        and what exactly is happening at each boundary.
 
        This tutorial will introduce three types of boundary
        condition
 
        *  INLETs   where fluid will enter the domain
 
        *  OUTLETS   where fluid leaves the domain
 
        *  Wall friction
 
        There are numerous methods and types of boundary
        specification the methods demonstrated in this tutorial
        are only a small sub-set of the full range.
CALL LOAD_96
 
    GROUP 10. Inter-phase-transfer processes and properties
    GROUP 11. Initialization of variable or porosity fields
    GROUP 12. Patchwise variation of terms
            GROUP 13. Boundary conditions and special sources
 
        Boundary conditions are located within the
        computational volume by the pil statements
        with the form
 
           PATCH(name,type,ixf,ixl,iyf,iyl,izf,izl,itf,itl)
 
        where:
        name is a unique text identifier to link patches and
        the values being set on the patch.
        type is the relevant cell face area, volume etc.
        ixf, etc are region indices if prefixed by a #,
        or else CELL indices.
 
        example:
           INLET(IN,LOW,1,NX,#1,#2,1,1,#1,#1)
        sets an inlet patch on the low cell faces for all x
        cells in the first two regions in Y
        (reminder Inlet is called INLET, is on the west side
        of the first region in X, Y and Z)
cvl4='Please_set_name,_type_and_location_of_the_inlet'
cvl2=inlet(inlet,west,#1,#1,#1,#1,#1,#1,#1,#1)
CALL LOAD_95
        Having specified the patch location, we now have to
        specify what mass flows etc are present in the inlet
        patch.
 
        Mass flow rates are specified by adding a source to P1
        the pressure correction equation.
        The source within PHOENICS is linearised to have a
        coefficient and value.
        The magnitude of the coefficient is assumed for the
        INLET style of PATCH, and the value must be mass per
        unit area.
        Other variables are just set to the required value
 
           VALUE(name,variable,value)
 
        where: name is used to link value to the patch.
            Variable is the relevant equation eg. P1
            Value is the required flux
     (reminder the flow rate is 10.0*rho1; inlet velocity is 10.0)
cvl4='Please_set_mass_flow_rate_for_inlet_called_inlet'
cvl2=value(inlet,p1,10.0*rho1)
CALL LOAD_95
 
cvl4='Please_set_u_velocity_component_for_inlet_to_10.0'
cvl2=value(inlet,u1,10.0)
 
CALL LOAD_95
 
cvl4='Please_set_v_velocity_component_for_inlet_to_0.0'
cvl2=value(inlet,v1,0.0)
 
CALL LOAD_95
 
cvl4='Please_set_kinetic_energy_entrained_at_the_inlet_to_0.04'
cvl2=value(inlet,ke,0.04)
 
CALL LOAD_95
 
cvl4='Please_set_epsilon_being_entrained_at_the_inlet_to_0.13'
cvl2=value(inlet,ep,0.13)
 
CALL LOAD_95
 
                    congratulations....
        you are really quite good at this now !!
 
        Having specified the the inlet patch, we now have to
        specify the outlet patch.
 
        Regions of outflow are normally specified by regions
        of nomimally constant pressure in a manner similar to
        inlet above, but the patch name is OUTLET.
 
        example:
           OUTLET(OUT,HIGH,1,NX,#1,#2,NZ,NZ,#1,#1)
 
        sets an outlet over all x, first two regions in Y last Z
                     for the first time region
 
        (reminder outlet is called out and is on the east of the
        domain, extending over region 1 in y and z)
cvl4='Please_set_name,type_and_location_of_the_outlet'
cvl2=outlet(out,east,#1,#1,#1,#1,#1,#1,#1,#1)
CALL LOAD_95
        Again, on outlet boundaries, Mass flow rates etc are
        linearised to have a  coefficient and value.
 
        At an outlet, only the relative pressure need be set -
        all other values are internal, and hence known to EARTH.
 
        Required pressure values are set using :
 
           VALUE(name,P1,value)
 
        where:
 
        name   is used to link value to the patch.
        value  is the external pressure, relative to PRESS0
cvl4='Please_set_nominal_pressure_on_outlet_boundary_to_0.0'
cvl2=value(out,p1,0.0)
CALL LOAD_95
        Having specified the inlet and exit patches, we now have to
        specify wall friction.
 
        Regions with wall friction can be specified using a PATCH.
 
        example:
           PATCH(TOP,NWALL,1,NX,#1,#1,1,NZ,#1,#1)
 
        sets a north wall over all x, last cell in Y, all Z
        for the first time region
 
        the type is NWALL, SWALL EWALL,WWALL,HWALL or LWALL
        as required, but ONLY for wall regions.
 
        These are special names used to identify regions
        where the distance from wall to cell centre is important
 
        (reminder, wall is called TOP and is on the North
        part of the domain, extending in all x-regions)
cvl4='Please_set_name_type_and_location_of_the_top_wall'
cvl2=patch(top,nwall,#1,#1,#1,#1,#1,#1,#1,#1)
CALL LOAD_95
        The wall condition must be specified in the
        linearised form having a  coefficient and value.
 
        The magnitudes of the coefficients are NOT KNOWN for the
        formal PATCH statement, and we use COVAL statements to
        specify the required data
 
        COVAL(name,variable,COefficient,VALue)
 
        where: name is used to link value to the patch.
            Variable is the relevant equation eg. P1
        Coeffficient can be set as follows:
        Coef,        influence on prediction
        blasius           Blasius law
        loglaw           Log law
        genlaw           Generalised log law
        Value
        Velocities      Wall speed.
        ke-ep      loglaw or genlaw  Bounds the Ke and ep equations
        For this wall the log law method is to be activated.
cvl4='Please_set_the_coval_for_the_velocity_parallel_to_the_wall'
cvl2=coval(top,u1,loglaw,0.0)
CALL LOAD_95
 
cvl4='Please_set_the_coval_for_the_kinetic_energy_boundary'
cvl2=coval(top,ke,loglaw,loglaw)
 
CALL LOAD_95
 
cvl4='Please_set_the_coval_for_the_dissipation_boundary'
cvl2=coval(top,ep,loglaw,loglaw)
 
CALL LOAD_95
 
 
                    CONGRATULATIONS.
 
        You have set the three types of Boundary to be covered
 
        in this tutorial.
 
 
        All other boundaries ( one wall in this case ) are being
 
        set for you.
 
 
 
 
CALL LOAD_96
 
dcom(patch(bot,swall,#1,#1,#1,#1,#1,#1,#1,#1)
dcom(coval(bot,u1,loglaw,0.0)
dcom(coval(bot,ke,loglaw,loglaw)
dcom(coval(bot,ep,loglaw,loglaw)
 
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 14. Downstream pressure for PARAB=.TRUE.
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 15. Termination of sweeps
qcom(  *
 
    GROUP 14. Downstream pressure for PARAB=.TRUE.
                 GROUP 15. Termination of sweeps
 
        PHOENICS is an iterative code that proceeds from your
        first guess to a converged prediction.
 
        For general engineering problems, the "whole field"
        pressure is likely to be used, and the iterative
        process can be described as follows:
 
        1) A series of "sweeps" through the domain from IZ = 1
                          to IZ = NZ.
        2) Each Z "slab" is treated in turn to derive velocity
              updates to satisfy momentum, and the pressure
                   coefficients for the 3D solver
        3) The 3D pressure field is solved, and then used to
               derive velocities that satisfy continuity.
 
        For this tutorial, we are only concerned with the
        overall number of SWEEPS, with the PIL statement
 
           LSWEEP=n
        where  n is the integer number of sweeps required.
cvl4='Set_the_iteration_sweeps_to_50'
cvl2=lsweep=50
CALL LOAD_95
 
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  * GROUP 16. Termination of iterations
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 17. Under-relaxation devices
qcom(  *
dcom(real(maxv,minl,relx)
dcom(maxv=5.0
dcom(minl=0.1
dcom(relx=10.0
 
dcom(relax(p1,linrlx,0.8)
dcom(relax(u1,falsdt,minl/maxv*relx)
dcom(relax(v1,falsdt,minl/maxv*relx)
dcom(relax(ke,falsdt,minl/maxv*relx)
dcom(relax(ep,falsdt,minl/maxv*relx)
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 18. Limits on variables or increments to them
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 19. Data communicated by satellite to GROUND
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 20. Preliminary print-out
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 21. Print-out of variables
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 22. Spot-value print-out
qcom(  *
dcom(ixmon=5
dcom(iymon=5
dcom(tstswp=-1
 
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 23. Field print-out and plot control
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
qcom(  *
qcom(  *  GROUP 24. Dumps for restarts
qcom(  *
qcom(  * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
   You have now completed the tutorial.
 
   You may now end satellite and write out the Q1 file, or
   quit this tutorial.
 
   'Enter' will end the satellite and save the Q1.
 
   'Quit' will quit the tutorial.
 
    IMPORTANT!!
 
    If you are running from the satellite top menu, and you
    want to save the Q1 you have generated, you MUST select
    'Command mode', NOT 'End satellite' when you return to
    the top panel, otherwise you will lose your Q1.
 
CALL LOAD_96
 
goto DONE
 
label QUIT
CALL LOAD_97
 
label DONE
ENDMAIN
 
SUBROUTINE LOAD_95
L($095)
ENDSUB
 
SUBROUTINE LOAD_96
L($096)
ENDSUB
 
SUBROUTINE LOAD_97
L($097)
ENDSUB