CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

Speeds of 100 m / s in Oven - pimpleFoam + Energy Equation

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree5Likes
  • 2 Post By alexeym
  • 1 Post By alexeym
  • 1 Post By alexeym
  • 1 Post By alexeym

Reply
 
LinkBack Thread Tools Display Modes
Old   February 22, 2014, 01:01
Default Speeds of 100 m / s in Oven - pimpleFoam + Energy Equation
  #1
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Dear, good night.
I am new to OpenFOAM and I'm simulating the air flow within a continuous furnace.
I changed the pimpleFoam by adding the energy equation, resulting in my_pimpleFoam. Is continuing with the establishment of the boundary conditions for the entry, exit, adiabatic walls (up, down, left side and right side) and burner (central tube at 1000 K). At the end, I ran the command and checked the presence of extremely high speeds, on the order of 100 m / s. What is absurd for configuring an oven, it should work in natural convection.
Could you please check the attached files? Point me any errors, wherever they are.
Attached solver my_pimpleFoam and information about the design of the oven.

Finally, it has to be air enters the furnace at room temperature and atmospheric pressure and exits with a suction pressure of 10 cmH2O.
I appreciate everyone's attention and await response.
Attached Files
File Type: gz Arquivos.tar.gz (2.7 KB, 7 views)
jrsilvio_ver is offline   Reply With Quote

Old   February 22, 2014, 01:06
Default
  #2
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Now follows the solver my_pimpleFoam.
Attached Files
File Type: gz my_pimpleFoam.tar.gz (2.5 KB, 3 views)
jrsilvio_ver is offline   Reply With Quote

Old   February 22, 2014, 03:08
Default Images I
  #3
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Attached pictures of the simulation.
Attached Images
File Type: jpg 1.jpg (41.3 KB, 21 views)
File Type: jpg 2.jpg (40.6 KB, 20 views)
File Type: jpg 3.jpg (40.9 KB, 21 views)
jrsilvio_ver is offline   Reply With Quote

Old   February 22, 2014, 03:09
Default
  #4
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Attached pictures of the simulation.
Attached Images
File Type: jpg 4.jpg (43.1 KB, 15 views)
File Type: jpg 5.jpg (43.6 KB, 12 views)
File Type: jpg 6.jpg (44.8 KB, 12 views)
jrsilvio_ver is offline   Reply With Quote

Old   February 22, 2014, 03:11
Default
  #5
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Attached pictures of the simulation..
Attached Images
File Type: jpg 7.jpg (41.5 KB, 11 views)
File Type: jpg 8.jpg (43.8 KB, 9 views)
jrsilvio_ver is offline   Reply With Quote

Old   February 22, 2014, 03:13
Default
  #6
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Mesh geometry.
Attached Images
File Type: jpg Malha1.jpg (46.0 KB, 12 views)
File Type: jpg Malha 2.jpg (47.9 KB, 11 views)
jrsilvio_ver is offline   Reply With Quote

Old   February 22, 2014, 09:48
Default
  #7
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,084
Rep Power: 18
alexeym will become famous soon enough
Hi,

1. If you'd like to simulate natural convection maybe it'll be better to start with buoyantBoussinesqPimpleFoam. The solver is more or less what you are trying to do in my_pimpleFoam but it also has buoyancy terms in pressure equation.

2. Are you sure that one nOuterCorrector step is enough for your simulation to converge? I'd increase this parameter up to 50 and add residual controls for termination of outer corrector loop. Something like this:

Code:
PIMPLE
{
    ...
    nOuterCorrectors 50;
    ...
    residualControl
    {
        "(p|U|T)"
        {
            tolerance 1e-4;
            relTol 0;
        }
    }
}
jherb and jrsilvio_ver like this.
alexeym is offline   Reply With Quote

Old   February 22, 2014, 18:06
Default
  #8
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Using buoyantFoam I have built a model of heat transfer by radiation?
jrsilvio_ver is offline   Reply With Quote

Old   February 22, 2014, 21:03
Default
  #9
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Guys, another detail.
Could anyone detail me the boundary condition "totalPressure"?
In my project, for example, I know that the inlet pressure is atmospheric and do not know the speed and output'm assuming a suction pressure of 10cmH2O, but in any case I know the speeds. How can I implement this boundary condition?
I am considering the density of air at the average temperature ((1000 +300) / 2 = 650 K) equal to 0.5356 kg / m.
Someone could solve my doubts?
jrsilvio_ver is offline   Reply With Quote

Old   February 22, 2014, 22:12
Default
  #10
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Nobody has an interest in the subject in question?
jrsilvio_ver is offline   Reply With Quote

Old   February 23, 2014, 07:13
Default
  #11
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,084
Rep Power: 18
alexeym will become famous soon enough
Quote:
Originally Posted by jrsilvio_ver View Post
Using buoyantFoam I have built a model of heat transfer by radiation?
You'd like to have radiative heat transfer in your simulation? With buoyantBoussinesqPimpleFoam you can have it.

As I can guess from your case files totalPressure BC will calculate pressure with:

Code:
    if (psiName_ == "none" && rhoName_ == "none")
    {
        operator==(p0p - 0.5*(1.0 - pos(phip))*magSqr(Up));
    }
I still wasn't able to understand your last question about boundary conditions.
jrsilvio_ver likes this.
alexeym is offline   Reply With Quote

Old   February 23, 2014, 14:44
Default
  #12
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
The buoyantBoussinesqPimpleFoam would have included heat exchange by radiation, the energy transport and the transport of momentum? I would not need to make any changes in solver?
And as the boundary conditions used in my my_pimpleFoam, correct? The issue is that I do not quite understand how to use the boundary condition totalPressure, explain to me? Preferably with an example.
I greatly appreciate your attention.
jrsilvio_ver is offline   Reply With Quote

Old   February 23, 2014, 14:46
Default
  #13
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
Another question regarding buoyantBoussinesqPimpleFoam. How could I totally remove the terms involving turbulence? In the case of turbulence model, since it will be working with laminar flow.
jrsilvio_ver is offline   Reply With Quote

Old   February 23, 2014, 14:58
Default
  #14
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,084
Rep Power: 18
alexeym will become famous soon enough
Hi,

If you just take a look at the sources in $FOAM_APP/solvers/heatTransfer/buoyantBoussinesqPimpleFoam, you will find answers to your questions (concerning equations solved by the solver and if there is radiative heat transfer). As far as I understand the problem, you do not need to modify anything.

I'd suggest you forget about totalPressure for a moment and thoroughly describe physical conditions at the inlet and outlet; maybe you need completely different set of BCs. From the previous posts I wasn't able to figure out what's happening at the inlet and outlet boundaries.

About turbulence: put laminar RASModel in constant/RASProperties. In addition you can change "turbulence on" to "turbulence off" there.
jrsilvio_ver likes this.
alexeym is offline   Reply With Quote

Old   February 23, 2014, 16:59
Default
  #15
Member
 
JuNNioR
Join Date: Feb 2014
Location: Brazil
Posts: 38
Rep Power: 3
jrsilvio_ver is on a distinguished road
After disabling the turbulence model, tried to run the command and got:

__________________________________________________ _________________________
Create time

Create mesh for time = 0


Reading g
Reading thermophysical properties

Reading field T

Reading field p_rgh

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Creating turbulence model

Selecting RAS turbulence model laminar
Reading field alphat



--> FOAM FATAL IO ERROR:
cannot find file

file: /home/silvio/Mestrado/buoyantBoussinesqPimpleFoam/hotRoom/0/alphat at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

__________________________________________________ _________________________

If the turbulence model is disabled, as it is reading the alphat?
jrsilvio_ver is offline   Reply With Quote

Old   February 24, 2014, 02:43
Default
  #16
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,084
Rep Power: 18
alexeym will become famous soon enough
Hi,

Reading code can be a source of endless insights. Here is the part of TEqn.H:

Code:
...
    alphat = turbulence->nut()/Prt;
    alphat.correctBoundaryConditions();

    volScalarField alphaEff("alphaEff", turbulence->nu()/Pr + alphat);

    fvScalarMatrix TEqn
    (
        fvm::ddt(T)
      + fvm::div(phi, T)
      - fvm::laplacian(alphaEff, T)
     ==
        radiation->ST(rhoCpRef, T)
      + fvOptions(T)
    );
...
Surely it needs alpha cause the solver was made universal (i.e. to run in laminar and turbulent cases). If you disable turbulence nut == 0 => alphat == 0, so your alphaEff is just a constant.

If you so unhappy with alphat, you can modify solver (createFields.H, TEqn.H, and buoyantBoussinesqPimpleFoam.C files) and remove any mentions of turbulence from there. Though I really doubt you really need this
jrsilvio_ver likes this.
alexeym is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Cannot run the code properly: very large time step continuity error crst15 OpenFOAM Running, Solving & CFD 9 December 14, 2014 19:17
error EOF in blockMesh Ahmed Khattab OpenFOAM Meshing & Mesh Conversion 7 May 17, 2012 00:37
error message cuteapathy CFX 14 March 20, 2012 07:45
energy equation in rhoCentralFoam nakul OpenFOAM 0 October 10, 2010 15:07
Why FVM for high-Re flows? Zhong Lei Main CFD Forum 23 May 14, 1999 13:22


All times are GMT -4. The time now is 13:35.