Import velocity profile

Questions and remarks about code_saturne usage
Forum rules
Please read the forum usage recommendations before posting.
Robert
Posts: 26
Joined: Mon May 22, 2017 11:14 am

Import velocity profile

Post by Robert »

Hello,
Could you, please, tell me how to import a velocity profile on the inlet?
I made a simple case and I exported the velocities to a .CSV file using Paraview. I have in this file four columns: 1 for position, and 3 for each component of the velocity on x, y, z axis and now I'm trying to import them on the inlet of another geometry. I did read this post viewtopic.php?f=2&t=1693&p=8917#p8917 but I didn't understand how to do it so any help is welcome.

Regards,
Robert
Yvan Fournier
Posts: 4070
Joined: Mon Feb 20, 2012 3:25 pm

Re: Import velocity profile

Post by Yvan Fournier »

Hello,

The referenced example only mentions how to have the csv files copied automatically, not how to use them.

We do not have a fully automatic way of doing what you need here, though we might have one in a few months based on some current developments. If the data were provided under the form of a mesh (in .med format), MEDcoupling could be used (see exemple in recent Doxygen documentation).

Otherwise, you basically need to read you csv files from user subroutines (easy part) and interpolate the values to inlet faces (more complex part). We will try to make this easier in the future, but now, most users doing this write their own interpolation based on knowledge of the profile data min/max and stepping info.

Some users on this forum might have easy-to-adapt examples they might share. I do not have anything up to date on my side.

Best regards,

Yvan
Robert
Posts: 26
Joined: Mon May 22, 2017 11:14 am

Re: Import velocity profile

Post by Robert »

Hello,

Thank you for the answer. I forgot to mention that I'm using the version 5.0 for windows. So far I've found only how to couple code_saturne and salome on linux platform, is there any way to do the MEDcoupling on windows, or will it be available in the next version?

Regards,
Robert
Yvan Fournier
Posts: 4070
Joined: Mon Feb 20, 2012 3:25 pm

Re: Import velocity profile

Post by Yvan Fournier »

Hello,

No, we do not include MEDCoupling in the Windows version.

Regarding the Windows version, see this thread: viewtopic.php?f=4&t=2034. I may have a solution for the graphical part (I should test it within a month), but for the non-graphical part, the solution would be either to use the Windows subsystem for Linux (which already works well today, and in which MEDCoupling should work) or Docker (with which we have experimented but not built a complete package so far).

In any case, the use of MEDCoupling is limited in Code_Saturne version 5.0 (it is better to use 5.2 or 5.3). I might be able to write a subroutine for 5.0 that would do what you need (and work on the Windows build), but probably not before a few weeks (schedule being already very busy for this month).

Best regards,

Yvan
Robert
Posts: 26
Joined: Mon May 22, 2017 11:14 am

Re: Import velocity profile

Post by Robert »

Hello,

That would be great, thank you.

Regards,
Robert
Robert
Posts: 26
Joined: Mon May 22, 2017 11:14 am

Re: Import velocity profile

Post by Robert »

Hello,

I've got another question. Is it possible to put the equation which describes the profile and then fit the data to it? If so, could you give give me some hints about which subroutines should I modify to it?
Regards,
Robert
Yvan Fournier
Posts: 4070
Joined: Mon Feb 20, 2012 3:25 pm

Re: Import velocity profile

Post by Yvan Fournier »

Hello,

Yes, absolutely.

You can do this in cs_user_,boundary_conditions.f90 (check the Doxygen documentation for examples).

Although performance is slightly reduced, for testing you can also directly define an equation expression in the graphical interface.

Regards,

Yvan
Robert
Posts: 26
Joined: Mon May 22, 2017 11:14 am

Re: Import velocity profile

Post by Robert »

Hello,

I tried with no succes to read values from a .txt file. As you can see in the error file attached, there is a problem with the "read" command and I'm unable to fix it.
I tried to put the Values.txt in SRC and DATA folders, I tried to write the entire path in the "open" command. Unfortunataely I don't get any error files with more details, the one you will find in attachaments it's copied from that log which appear when you start a calculation.
Attached you will find the main code, the boundarycondition.f90 file, the error and the list with values. "D" is the variable I'm looking to read from Values.txt.
Regards,
Robert

Code: Select all

!-------------------------------------------------------------------------------

!                      Code_Saturne version 5.0.7
!                      --------------------------
! This file is part of Code_Saturne, a general-purpose CFD tool.
!
! Copyright (C) 1998-2018 EDF S.A.
!
! This program is free software; you can redistribute it and/or modify it under
! the terms of the GNU General Public License as published by the Free Software
! Foundation; either version 2 of the License, or (at your option) any later
! version.
!
! This program is distributed in the hope that it will be useful, but WITHOUT
! ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS
! FOR A PARTICULAR PURPOSE.  See the GNU General Public License for more
! details.
!
! You should have received a copy of the GNU General Public License along with
! this program; if not, write to the Free Software Foundation, Inc., 51 Franklin
! Street, Fifth Floor, Boston, MA 02110-1301, USA.

!-------------------------------------------------------------------------------

!===============================================================================
! Function:
! ---------

!> \file cs_user_boundary_conditions.f90
!>
!> \brief User subroutine which fills boundary conditions arrays
!> (\c icodcl, \c rcodcl) for unknown variables.
!>
!> See \subpage cs_user_boundary_conditions_examples for examples.
!>
!> \section cs_user_boundary_conditions_intro Introduction
!>
!> Here one defines boundary conditions on a per-face basis.
!>
!> Boundary faces may be selected using the \ref getfbr subroutine.
!>
!> \code getfbr(string, nelts, lstelt) \endcode
!>  - string is a user-supplied character string containing selection criteria;
!>  - nelts is set by the subroutine. It is an integer value corresponding to
!>    the number of boundary faces verifying the selection criteria;
!>  - lstelt is set by the subroutine. It is an integer array of size nelts
!>    containing the list of boundary faces verifying the selection criteria.
!>
!> string may contain:
!>  - references to colors (ex.: 1, 8, 26, ...)
!>  - references to groups (ex.: inlet, group1, ...)
!>  - geometric criteria (ex. x < 0.1, y >= 0.25, ...)
!>
!> These criteria may be combined using logical operators (\c and,\c or) and
!> parentheses.
!>
!> \par Example
!> \code 1 and (group2 or group3) and y < 1 \endcode
!> will select boundary faces
!> of color 1, belonging to groups 'group2' or 'group3' and with face center
!> coordinate y less than 1.
!>
!> Operators priority, from highest to lowest:
!>  '( )' > 'not' > 'and' > 'or' > 'xor'
!>
!> Similarly, interior faces and cells can be identified using the \ref getfac
!> and \ref getcel subroutines (respectively). Their syntax are identical to
!> \ref getfbr syntax.
!>
!> For a more thorough description of the criteria syntax, see the user guide.
!>
!>
!> \section bc_types Boundary condition types
!>
!> Boundary conditions may be assigned in two ways.
!>
!>
!> \subsection std_bcs For "standard" boundary conditions:
!>
!> One defines a code in the \c itypfb
!> array (of dimensions number of boundary faces).
!> This code will then be used by a non-user subroutine to assign the
!> following conditions.
!> The available codes are:
!>  - \c ientre: Inlet
!>  - \c isolib: Free outlet
!>  - \c isymet: Symmetry
!>  - \c iparoi: Wall (smooth)
!>  - \c iparug: Rough wall
!>
!> These integers are defined elsewhere (in paramx.f90 module).
!> Their value is greater than or equal to 1 and less than or  equal to
!> ntypmx (value fixed in paramx.h)
!>
!> In addition, some values must be defined:
!>  - Inlet (more precisely, inlet/outlet with prescribed flow, as the flow
!>           may be prescribed as an outflow):
!>    - Dirichlet conditions on variables other than pressure are mandatory
!>      if the flow is incoming, optional if the flow is outgoing (the code
!>      assigns zero flux if no Dirichlet is specified); thus,
!>      at face \c ifac, for the variable \c ivar: \c rcodcl(ifac, ivar, 1)
!>
!>
!>  - Smooth wall: (= impermeable solid, with smooth friction)
!>    - Velocity value for sliding wall if applicable:
!>                  - \c rcodcl(ifac, iu, 1) = fluid velocity in the x direction
!>                  - \c rcodcl(ifac, iv, 1) = fluid velocity in the y direction
!>                  - \c rcodcl(ifac, iw, 1) = fluid velocity in the z direction
!>    - Specific code and prescribed temperature value at wall if applicable:
!>                  - \c icodcl(ifac, ivar)    = 5
!>                  - \c rcodcl(ifac, ivar, 1) = prescribed temperature
!>    - Specific code and prescribed flux value at wall if applicable:
!>                  - \c icodcl(ifac, ivar)    = 3
!>                  - \c rcodcl(ifac, ivar, 3) = prescribed flux
!>    .
!>    Note that the default condition for scalars (other than k and epsilon)
!>    is homogeneous Neumann.
!>
!>
!>  - Rough wall: (= impermeable solid, with rough friction)
!>    - Velocity value for sliding wall if applicable:
!>                  - \c rcodcl(ifac, iu, 1) = fluid velocity in the x direction
!>                  - \c rcodcl(ifac, iv, 1) = fluid velocity in the y direction
!>                  - \c rcodcl(ifac, iw, 1) = fluid velocity in the z direction
!>    - Value of the dynamic roughness height to specify in
!>                  - \c rcodcl(ifac, iu, 3)
!>    - Value of the scalar roughness height (if required) to specify in
!>                  - \c rcodcl(ifac, iv, 3) (values for iw are not used)
!>    - Specific code and prescribed temperature value at wall if applicable:
!>                  - \c icodcl(ifac, ivar)    = 6
!>                  - \c rcodcl(ifac, ivar, 1) = prescribed temperature
!>    - Specific code and prescribed flux value at rough wall, if applicable:
!>                  - \c icodcl(ifac, ivar)    = 3
!>                  - \c rcodcl(ifac, ivar, 3) = prescribed flux
!>    .
!>    Note that the default condition for scalars (other than k and epsilon)
!>    is homogeneous Neumann.
!>
!>  - Symmetry (= slip wall):
!>    - Nothing to specify
!>
!>  - Free outlet (more precisely free inlet/outlet with prescribed pressure)
!>    - Nothing to prescribe for pressure and velocity. For scalars and
!>      turbulent values, a Dirichlet value may optionally be specified.
!>      The behavior is as follows:
!>          - pressure is always handled as a Dirichlet condition
!>          - if the mass flow is inflowing:
!>              one retains the velocity at infinity
!>              Dirichlet condition for scalars and turbulent values
!>               (or zero flux if the user has not specified a
!>                Dirichlet value)
!>          - if the mass flow is outflowing:
!>              one prescribes zero flux on the velocity, the scalars,
!>              and turbulent values
!>    .
!>    Note that the pressure will be reset to p0 on the first free outlet
!>    face found.
!>
!>
!> \subsection nonstd_bcs For "non-standard" conditions:
!>
!> Other than (inlet, free outlet, wall, symmetry), one defines
!>  - on one hand, for each face:
!>    - an admissible \c itypfb value (i.e. greater than or equal to 1 and
!>      less than or equal to \c ntypmx; see its value in paramx.h).
!>      The values predefined in paramx.h:
!>      \c ientre, \c isolib, \c isymet, \c iparoi, \c iparug are in this range,
!>      and it is preferable not to assign one of these integers to \c itypfb
!>      randomly or in an inconsiderate manner. To avoid this, one may use
!>      \c iindef if one wish to avoid checking values in paramx.h. \c iindef
!>      is an admissible value to which no predefined boundary condition
!>      is attached.
!>      Note that the \c itypfb array is reinitialized at each time step to
!>      the non-admissible value of 0. If one forgets to modify \c itypfb for
!>      a given face, the code will stop.
!>
!>  - and on the other hand, for each face and each variable:
!>    - a code
!>                      - \c icodcl(ifac, ivar)
!>    - three real values
!>                      - \c rcodcl(ifac, ivar, 1)
!>                      - \c rcodcl(ifac, ivar, 2)
!>                      - \c rcodcl(ifac, ivar, 3)
!>
!> \anchor icodcl \anchor rcodcl
!> The value of \c icodcl is taken from the following:
!>  - 1: Dirichlet      (usable for any variable)
!>  - 3: Neumann        (usable for any variable)
!>  - 4: Symmetry       (usable only for the velocity and components of
!>                       the Rij tensor)
!>  - 5: Smooth wall    (usable for any variable except for pressure)
!>  - 6: Rough wall     (usable for any variable except for pressure)
!>  - 9: Free outlet    (usable only for velocity)
!>  - 13: Dirichlet for the advection operator and
!>        Neumann for the diffusion operator
!>
!> The values of the 3 \c rcodcl components are:
!>  - \c rcodcl(ifac, ivar, 1):
!>     - Dirichlet for the variable          if \c icodcl(ifac, ivar) = 1 or 13
!>     - Wall value (sliding velocity, temp) if \c icodcl(ifac, ivar) = 5
!>     .
!>     The dimension of \c rcodcl(ifac, ivar, 1) is that of the
!>     resolved variable, for instance:
!>        - U (velocity in m/s),
!>        - T (temperature in degrees)
!>        - H (enthalpy in J/kg)
!>        - F (passive scalar in -)
!>  - \c rcodcl(ifac, ivar, 2):
!>       "exterior" exchange coefficient (between the prescribed value
!>                        and the value at the domain boundary)
!>                        rinfin = infinite by default
!>     - For velocities U,                in kg/(m2 s):
!>        \c rcodcl(ifac, ivar, 2) =          (viscl+visct) / d
!>     - For the pressure P,              in  s/m:
!>        \c rcodcl(ifac, ivar, 2) =                     dt / d
!>     - For temperatures T,              in Watt/(m2 degres):
!>        \c rcodcl(ifac, ivar, 2) = Cp*(viscls+visct/turb_schmidt) / d
!>     - For enthalpies H,                in kg /(m2 s):
!>        \c rcodcl(ifac, ivar, 2) =    (viscls+visct/turb_schmidt) / d
!>     - For other scalars F              in:
!>        \c rcodcl(ifac, ivar, 2) =    (viscls+visct/turb_schmidt) / d
!>            (d has the dimension of a distance in m)
!>
!>  - \c rcodcl(ifac, ivar, 3) if \c icodcl(ifac, ivar) = 3 or 13:
!>      Flux density (< 0 if gain, n outwards-facing normal)
!>     - For velocities U,                in kg/(m s2) = J:
!>        \c rcodcl(ifac, ivar, 3) =         -(viscl+visct) * (grad U).n
!>     - For pressure P,                  in kg/(m2 s):
!>        \c rcodcl(ifac, ivar, 3) =                    -dt * (grad P).n
!>     - For temperatures T,              in Watt/m2:
!>        \c rcodcl(ifac, ivar, 3) = -Cp*(viscls+visct/turb_schmidt) * (grad T).n
!>     - For enthalpies H,                in Watt/m2:
!>        \c rcodcl(ifac, ivar, 3) = -(viscls+visct/turb_schmidt) * (grad H).n
!>     - For other scalars F              in:
!>        \c rcodcl(ifac, ivar, 3) = -(viscls+visct/turb_schmidt) * (grad F).n
!>
!>  - \c rcodcl(ifac, ivar, 3) if \c icodcl(ifac, ivar) = 6:
!>      Roughness for the rough wall law
!>     - For velocities U, dynamic roughness
!>         \c rcodcl(ifac, iu, 3) = roughd
!>     - For other scalars, thermal roughness
!>         \c rcodcl(ifac, iv, 3) = rough
!>
!>
!> Note that if the user assigns a value to \c itypfb equal to \c ientre, \c isolib,
!> \c isymet, \c iparoi, or \c iparug and does not modify \c icodcl (zero value by
!>  default), \c itypfb will define the boundary condition type.
!>
!> To the contrary, if the user prescribes \c icodcl(ifac, ivar) (nonzero),
!> the values assigned to \c rcodcl will be used for the considered face
!> and variable (if \c rcodcl values are not set, the default values will
!> be used for the face and variable, so:
!>                          - \c rcodcl(ifac, ivar, 1) = 0.d0
!>                          - \c rcodcl(ifac, ivar, 2) = rinfin
!>                          - \c rcodcl(ifac, ivar, 3) = 0.d0)
!>
!> Especially, one may have for example:
!>  - set \c itypfb(ifac) = \c iparoi which prescribes default wall
!>    conditions for all variables at face ifac,
!>  - and define IN ADDITION for variable ivar on this face specific
!>    conditions by specifying \c icodcl(ifac, ivar) and the 3 \c rcodcl values.
!>
!> The user may also assign to \c itypfb a value not equal to \c ientre, \c isolib,
!> \c isymet, \c iparoi, \c iparug, \c iindef but greater than or equal to 1 and less
!> than or equal to ntypmx (see values in param.h) to distinguish groups
!> or colors in other subroutines which are specific to the case and in
!> which itypfb is accessible. In this case though it will be necessary
!> to prescribe boundary conditions by assigning values to icodcl and to
!> the 3 \c rcodcl fields (as the value of \c itypfb will not be predefined in
!> the code).
!>
!>
!> \subsection comp_bcs Boundary condition types for compressible flows
!>
!> For compressible flows, only predefined boundary conditions may
!> be assigned among: \c iparoi, \c isymet, \c iesicf, \c isspcf, \c isopcf, \c iephcf, \c ieqhcf
!>
!>  - \c iparoi : standard wall
!>  - \c isymet : standard symmetry
!>
!>  - \c iesicf, \c isspcf, \c isopcf, \c iephcf, \c ieqhcf : inlet/outlet
!>
!> For inlets/outlets, we can prescribe
!> a value for turbulence and passive scalars in \c rcodcl(.,.,1)
!> for the case in which the mass flux is incoming. If this is not
!> done, a zero flux condition is applied.
!>
!> - \c iesicf: prescribed inlet/outlet (for example supersonic inlet)
!>           the user prescribes the velocity and all thermodynamic variables
!> - \c isspcf: supersonic outlet
!>           the user does not prescribe anything
!> - \c isopcf: subsonic outlet with prescribed pressure
!>           the user presribes the pressure
!> - \c iephcf: mixed inlet with prescribed total pressure and enthalpy
!>           the user prescribes the total pressure and total enthalpy
!> - \c ieqhcf: subsonic inlet with prescribed mass and enthalpy flow
!>           to be implemented
!>
!>
!> \subsection cons_rul Consistency rules
!>
!> A few consistency rules between \c icodcl codes for variables with
!> non-standard boundary conditions:
!>
!>  - Codes for velocity components must be identical
!>  - Codes for Rij components must be identical
!>  - If code (velocity or Rij) = 4
!>    one must have code (velocity and Rij) = 4
!>  - If code (velocity or turbulence) = 5
!>    one must have code (velocity and turbulence) = 5
!>  - If code (velocity or turbulence) = 6
!>    one must have code (velocity and turbulence) = 6
!>  - If scalar code (except pressure or fluctuations) = 5
!>    one must have velocity code = 5
!>  - If scalar code (except pressure or fluctuations) = 6
!>    one must have velocity code = 6
!>
!>
!> \remarks
!>   - Caution: to prescribe a flux (nonzero) to Rij, the viscosity to take
!>              into account is viscl even if visct exists
!>              (visct=rho cmu k2/epsilon)
!>   - One have the ordering array for boundary faces from the previous time
!>       step (except for the fist one, where \c itrifb has not been set yet).
!>   - The array of boundary face types \c itypfb has been reset before
!>       entering the subroutine.
!>
!>
!> \subsubsection cs_user_bc_cell_id Cell values of some variables
!>
!> Cell value field ids
!>
!> - Density:                        \c irom
!> - Dynamic molecular viscosity:    \c iviscl
!> - Turbulent viscosity:            \c ivisct
!> - Specific heat:                  \c icp
!> - Diffusivity(lambda):            \c field_get_key_int(ivarfl(isca(iscal)), &
!>                                      kivisl, ...)
!>
!>
!> \subsubsection fac_id Faces identification
!>
!> - Density:                               \c field id \c ibrom
!> - Boundary mass flux (for convecting \c ivar):
!>     field id \c iflmab
!>     using \c field_get_key_int(ivarfl(ivar), kbmasf, iflmab)
!> - For other values: take as an approximation the value in the adjacent cell
!>                     i.e. as above with \c iel = ifabor(ifac).
!>
!> Please refer to the
!> <a href="../../theory.pdf#boundary"><b>boundary conditions</b></a>
!> section of the theory guide for more informations.
!-------------------------------------------------------------------------------

!-------------------------------------------------------------------------------
! Arguments
!______________________________________________________________________________.
!  mode           name          role                                           !
!______________________________________________________________________________!
!> \param[in]     nvar          total number of variables
!> \param[in]     nscal         total number of scalars
!> \param[out]    icodcl        boundary condition code:
!>                               - 1 Dirichlet
!>                               - 2 Radiative outlet
!>                               - 3 Neumann
!>                               - 4 sliding and
!>                                 \f$ \vect{u} \cdot \vect{n} = 0 \f$
!>                               - 5 smooth wall and
!>                                 \f$ \vect{u} \cdot \vect{n} = 0 \f$
!>                               - 6 rough wall and
!>                                 \f$ \vect{u} \cdot \vect{n} = 0 \f$
!>                               - 9 free inlet/outlet
!>                                 (input mass flux blocked to 0)
!>                               - 13 Dirichlet for the advection operator and
!>                                    Neumann for the diffusion operator
!> \param[in]     itrifb        indirection for boundary faces ordering
!> \param[in,out] itypfb        boundary face types
!> \param[out]    izfppp        boundary face zone number
!> \param[in]     dt            time step (per cell)
!> \param[in,out] rcodcl        boundary condition values:
!>                               - rcodcl(1) value of the dirichlet
!>                               - rcodcl(2) value of the exterior exchange
!>                                 coefficient (infinite if no exchange)
!>                               - rcodcl(3) value flux density
!>                                 (negative if gain) in w/m2 or roughness
!>                                 in m if icodcl=6
!>                                 -# for the velocity \f$ (\mu+\mu_T)
!>                                    \gradt \, \vect{u} \cdot \vect{n}  \f$
!>                                 -# for the pressure \f$ \Delta t
!>                                    \grad P \cdot \vect{n}  \f$
!>                                 -# for a scalar \f$ cp \left( K +
!>                                     \dfrac{K_T}{\sigma_T} \right)
!>                                     \grad T \cdot \vect{n} \f$
!_______________________________________________________________________________

subroutine cs_f_user_boundary_conditions &
 ( nvar   , nscal  ,                                              &
   icodcl , itrifb , itypfb , izfppp ,                            &
   dt     ,                                                       &
   rcodcl )

!===============================================================================

!===============================================================================
! Module files
!===============================================================================

use paramx
use numvar
use optcal
use cstphy
use cstnum
use entsor
use parall
use period
use ihmpre
use ppppar
use ppthch
use coincl
use cpincl
use ppincl
use ppcpfu
use atincl
use atsoil
use ctincl
use cs_fuel_incl
use mesh
use field
use turbomachinery
use iso_c_binding
use cs_c_bindings

!===============================================================================

implicit none

! Arguments

integer          nvar   , nscal

integer          icodcl(nfabor,nvar)
integer          itrifb(nfabor), itypfb(nfabor)
integer          izfppp(nfabor)
integer iel
integer ifac
integer nlelt
integer ilelt
double precision Vtan, Vax, Vrad, D
double precision dt(ncelet)
double precision rcodcl(nfabor,nvar,3)
double precision x, y, z

! Local variables

! INSERT_VARIABLE_DEFINITIONS_HERE

integer, allocatable, dimension(:) :: lstelt

!===============================================================================


!===============================================================================
! Initialization
!===============================================================================

allocate(lstelt(nfabor))  ! temporary array for boundary faces selection

! INSERT_ADDITIONAL_INITIALIZATION_CODE_HERE

!===============================================================================
! Assign boundary conditions to boundary faces here
call getfbr('Inlet',nlelt,lstelt)
! For each subset:
! - use selection criteria to filter boundary faces of a given subset
! - loop on faces from a subset
!   - set the boundary condition for each face
!===============================================================================

! INSERT_MAIN_CODE_HERE
do ilelt = 1, nlelt
ifac = lstelt(ilelt)
iel = ifabor(ifac)
x = cdgfbo(1,ifac)
y = cdgfbo(2,ifac)
z = cdgfbo(3,ifac)
!a = acos(x/sqrt(x**2+y**2))*asin(y/sqrt(x**2+y**2))/abs(asin(y/sqrt(x**2+y**2)))


open (1, file="Values.txt")

read (1,*) D

itypfb(ifac) = ientre

rcodcl(ifac,iu,1) = 0

rcodcl(ifac,iv,1) = 0
rcodcl(ifac,iw,1) = -0.7012*(D**2)+0.1144*D+0.0057

enddo
!--------
! Formats
!--------

!----
! End
!----

deallocate(lstelt)  ! temporary array for boundary faces selection

return
end subroutine cs_f_user_boundary_conditions

!> \section examples Examples
!>   Several examples are provided
!>   \ref cs_user_boundary_conditions_examples "here".

Code: Select all

---- error analysis -----


At line 493 of file E:\Robert\Test\RESU\20181120-1532\src_saturne\BoundaryCondition.f90 (unit = 1, file = 'Values.txt')

Fortran runtime error: 

End of file 












solver script exited with status -3. 

Error running the calculation. 

Check Code_Saturne log (listing) and error* files for details. 

Error in calculation stage. 



 ****************************

  Saving calculation results

 ****************************

Attachments
BoundaryCondition.f90
(21.66 KiB) Downloaded 210 times
Antech
Posts: 197
Joined: Wed Jun 10, 2015 10:02 am

Re: Import velocity profile

Post by Antech »

Robert
Hello. The error you get means that the required amount of bytes cannot be read form file because the end-of-file is reached. The other problem is that the file is opened every loop iteration. Also, I didn't find the declaration for the variable D. Try something like this:
<Declare D at the top of the subroutine>
...
open (unit=1,file="Values.txt",action='read',access='stream')
...
do ilelt = 1, nlelt
...
read (1,*) D
<use D here>
...
end do

But it assumes that "Values.txt" contents a sequence of variable values for the boundary mesh faces and the order of values in the file corresponds the order Saturne lists the BC faces. I don't think that this is what you need. I'd prefer to use my BC subroutine I posted for you in your previous topic. Or, if you need something custom (not circular profile) you may use the following algo:

1. Read in the BC file like Values.txt where you define a matrix of variable value at this BC in form
x1 y1 z1 value1
x2 y2 z2 value2
x3 y3 z3 value3
You may use the matrix like real*8 TAB(N,4). The simplest way is to hard-code the matrix and not bother with files at all. More flexible way is to use fixed-format file and just do something like read (1,*) TAB. The best way is to use flexible format reader but it will require some time to code.
...
Do it at the beginning of the subroutine and only once (use the flag with the save statement to save between calls). Don't forget to make you array for the BC data global to be saved between calls.

2. Inside the do loop, interpolate with the matrix (TAB) you read from file using current coordinates (x, y, z). The simplest way is just to find the value in nearest point.

Try to hard-code the TAB matrix first and get the interpolation to work, then add the file reader.
Robert
Posts: 26
Joined: Mon May 22, 2017 11:14 am

Re: Import velocity profile

Post by Robert »

Hello,
Thank you for the answer. Sorry, I just saw that it didn't upload the Values.txt. Anyway in this file I had a column with few values... So, D is the diameter of the pipe and in the .txt I had a column with 0*D 0.1*D ... 0.9*D 1*D. If the order of values in the file corresponds the order Saturne lists the BC faces, should I write something like:

rcodcl(ifac,iu,1) = 0
rcodcl(ifac,iv,1) = 0
rcodcl(ifac,iw,1) = -0.7012*(z**2)+0.1144*z+0.0057
where z = cdgfbo(3,ifac)

Regards,
Robert
Post Reply