Neumann condition for temperature in only one direction

[mmagain]

Hi,

I am trying to find a way to implement a Neumann boundary condition on the temperature T in the z direction only. Via the GUI, I can use the "prescribed flux (user law)" to define my function but I don't know how I can define my condition. Essentially I am trying to impose the condition dT/dz = some variable quantity that depends on the properties of the liquid inside. I suspect that doing it via the GUI is not possible, maybe by defining a user subroutine might be easier but I have no idea how to do it that way, and I didn't find any satisfactory solution in the documentation either.

Any tips are appreciated,

Best,

Michael

PS : I am using CS 7.0.6

[Yvan Fournier]

Hello,

Not only with the GUI, but with the whole of the "legacy" finite volume scheme, Neumann BC's can only be set up relative to the normal direction relative to a boundary.

Using the CDO models it is possible to define a Neumann BC using an arbitrary direction.

In your case, is the z direction normal to the boundary ?

Best regards,

Yvan

[mmagain]

Hi,

Yes the z direction is normal to my boundary.
Does that mean I can just use the prescribed flux (user law) on this boundary? Since the z-axis is normal to my boundary

Best,

Michael

[Yvan Fournier]

Hello,

Yes, you can use the prescribed flux condition in this case.

Best regards,

Yvan

[mmagain]

Great ! Thank you for your help

[mmagain]

Hello,

I am trying to use the cs_user_boundary_conditions.c user subroutine. But I am unsure if that should work, and I find the documentation very hard to read. Could you tell me if the following code should work ?

Code: Select all

/*============================================================================
 * User definition of boundary conditions.
 *============================================================================*/

/* code_saturne version 7.0 */

/*
  This file is part of Code_Saturne, a general-purpose CFD tool.

  Copyright (C) 1998-2021 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.
 */

/*----------------------------------------------------------------------------*/

#include "cs_defs.h"

/*----------------------------------------------------------------------------
 * Standard C library headers
 *----------------------------------------------------------------------------*/

#include <assert.h>
#include <stdio.h>
#include <stdlib.h>
#include <string.h>
#include <math.h>

/*----------------------------------------------------------------------------
 * Local headers
 *----------------------------------------------------------------------------*/

#include "cs_headers.h"

/*----------------------------------------------------------------------------*/

BEGIN_C_DECLS

/*=============================================================================
 * Public function definitions
 *============================================================================*/

/*----------------------------------------------------------------------------*/
/*!
 * \brief User definition of boundary conditions
 *
 * \param[in]     nvar          total number of variable BC's
 * \param[in]     bc_type       boundary face types
 * \param[in]     icodcl        boundary face code
 *                                - 1  -> Dirichlet
 *                                - 2  -> convective outlet
 *                                - 3  -> flux density
 *                                - 4  -> sliding wall and u.n=0 (velocity)
 *                                - 5  -> friction and u.n=0 (velocity)
 *                                - 6  -> roughness and u.n=0 (velocity)
 *                                - 9  -> free inlet/outlet (velocity)
 *                                inflowing possibly blocked
 * \param[in]     rcodcl        boundary condition values
 *                                rcodcl(3) = flux density value
 *                                (negative for gain) in W/m2
 */
/*----------------------------------------------------------------------------*/

void
cs_user_boundary_conditions(int         nvar,
                            int         bc_type[],
                            int         icodcl[],
                            cs_real_t   rcodcl[])
{
	const cs_zone_t* z = cs_boundary_zone_by_name("BC_1");
	const cs_field_t *f = cs_field_by_name("temperature");
  	cs_real_t *rcodcl3 = f->bc_coeffs->rcodcl3;
  	for (cs_lnum_t i = 0; i < z->n_elts; i++) {
           cs_lnum_t face_id = z->elt_ids[i];
           rcodcl3[face_id] = *my neumann condition expression*;
       }
}

/*----------------------------------------------------------------------------*/

END_C_DECLS

[Yvan Fournier]

Hello,

I did not notice any obvious mistake, so assuming you boundary zone is indeed named "BC_1", and you replace the correct expression for the flux value, it should work.

Note also that if you are using a constant flux value, you can use the GUI. Even with a more complex expression, you can define it with the "user" option in the GUI. In that case, appropriate code will be generated in a "cs_meg_boundary_..." file, in the "src" directory of a code run (RESU/<run_id>/src). This code is generated, so you should never place it in a SRC folder (as it may be overwritten), but looking at the generated code may help provide additional examples taylored to your case (though the zone is selected in a different manner, the loop should be similar).

Best regards,

Yvan

[mmagain]

Thank you for your fast reply, Yvan.

Unfortunately, I cannot use the GUI because the flux depends on values of the properties of the liquid (such as viscosity, temperature itself, etc.) and are therefore not constant.

I will try it soon.

Best,

Michael

[mmagain]

Hello,

I have tried running the simulation but bc_coeffs has no attribute rcodcl3. How do I do then to apply the Neumann boundary condition correctly ?

EDIT : After investigation, it seems I should call the attribute af or bf, but I don't know which one I should call.

Here is my code

Best regards,

Michael

cs_user_boundary_conditions.c

(8.08 KiB) Downloaded 6 times

[Yvan Fournier]

Hello,

Using v7.0, you do not have direct access to "bc_coeffs->rcodcl3[face_id]", as this was added in v8.0 for better readbility.

In v7.0, the equivalent for this is
rcodcl[2 * n_b_faces * nvar + var_id*n_b_faces + face_id] = flux;

(See last example in cs_user_boundary_conditions-notebook.c for a more complete usage example and initialization of var_id, nvar, and n_b_faces above).

I also recommend switchint to v8.0 .

Best regards,

Yvan