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

Blow of compressible solver while using K-epsilon model in openfoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 25, 2011, 07:57
Default Blow of compressible solver while using K-epsilon model in openfoam
  #1
New Member
 
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 6
Amit Mathur is on a distinguished road
Dear all,

I am trying to run a simulation for a compressible flow in a pipe by using the K-Epsilon turbulence model in the version 1.7 from OpenFOAM.
For this simulation, I use a compressible solver : rhoSimpleFoam and I have defined the following boundary conditions :
- Inlet : pressure-101325
- Outlet : pressure-98383

My problem is that, after some iterations, the epsilon start bounding for very high values like 1e70. Afterwards solver blow and stop working.
I used K-epsilon, resizable K-epsilon, RngKE but problem remain as it is.

I already have remeshed my geometry to try to get a better mesh (orthogonal cell at the walls) but the problem persists.
I already have increased the number of nNonOrthogonalCorrectors but the problem persists.
To reproduce my problem, I have meshed a straight pipe and used the same setup. With the straight pipe (hexahedra), there is no problem and with a complex geometry (hexcore mesh from Tgrid), I do not understand what happens.
I presume that there are some problems with my setup but I do not understand where.
Afterwards i applied K-Omega-SST model. That time solver produce results but i dont why K-epsilon is not running.

So my question is why K-epsilon model in compressible flow is not working with Tet mesh in openfoam?


Thanks.

Best regards,
Amit
Amit Mathur is offline   Reply With Quote

Old   January 26, 2011, 11:35
Default
  #2
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi,

It seems possible that there might be some problem with your BC.

Do you really need a fixed value of pressure at outlet? Try changing outlet pressure to zeroGradient,

What is the flow velocity and temperature?

Specify more details of your case.
nakul is offline   Reply With Quote

Old   January 27, 2011, 01:06
Default problem in rhosimplefoam using k-epsilon model
  #3
New Member
 
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 6
Amit Mathur is on a distinguished road
Hi nakul,
Thanks for reply.
Flow in the geometry is pressure driven so the inlet at higher pressure and outlet at lower pressure. The velocity bc is zero gradient at both outlet and inlet. The temperature is fixed at 293 K for both inlet and outlet. I tried the same BC for hex mesh it works properly for K-epsilon model but in Tet mesh its fail even mesh quality is good.
Amit Mathur is offline   Reply With Quote

Old   January 27, 2011, 02:30
Default
  #4
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi,

Do a checkMesh on your tet mesh and see what you get.

Try reducing Co no. and use first order schemes in fvSchemes.

See if is helps.
nakul is offline   Reply With Quote

Old   January 27, 2011, 03:28
Default problem in rhosimplefoam using k-epsilon model
  #5
New Member
 
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 6
Amit Mathur is on a distinguished road
Dear Nukul,
I am using steady compressible solver (rhoSimpleFoam), there is no need of co no.
I am sending you the cheak Mesh result. Ots seems to be Ok.
Thanks
Checking geometry...
Overall domain bounding box (-0.917934 -0.649145 0.434051) (0.147203 0.0148634 0.759144)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (-9.87366e-16 -8.81665e-17 3.83878e-17) OK.
Max cell openness = 7.52033e-16 OK.
Max aspect ratio = 38.487 OK.
Minumum face area = 9.7289e-09. Maximum face area = 0.00235134. Face area magnitudes OK.
Min volume = 2.21352e-12. Max volume = 0.000103724. Total volume = 0.0505074. Cell volumes OK.
Mesh non-orthogonality Max: 71.3198 average: 22.1898
*Number of severely non-orthogonal faces: 1.
Non-orthogonality check OK.
<<Writing 1 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 3.35511 OK.
Amit Mathur is offline   Reply With Quote

Old   January 27, 2011, 03:38
Default
  #6
Member
 
Join Date: Jun 2010
Posts: 33
Rep Power: 7
RalphS is on a distinguished road
Hi,

I tried for two months rhoSimpleFoam, wasn't easy to get a stable simulation.

Right settings in fvSchemes and fvSolution are very important.

relTol, relaxationFactors, divSchemes

In my opinion try to set:

fvSolution:

solvers
{
...
relTol 0.1;
...
}
relaxationFactors
{
p 0.01;
rho 0.01;
U 0.5;
h 0.1;
k 0.1;
epsilon 0.1;
}

When it works, you could set the factors higher.


fvSchemes:

divSchemes
{
div(phi,U) Gauss vanLeerV;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
}

I would use realizable k-Epsilon.

Are your velocity high?
Why you have fixed temperature at inlet and outlet?

Regards,

Ralph
RalphS is offline   Reply With Quote

Old   January 27, 2011, 05:36
Default problem in rhosimplefoam using k-epsilon model
  #7
New Member
 
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 6
Amit Mathur is on a distinguished road
Dear RalpS,
Thanks for replying. I adjust the system schemes, solution and relaxation factor
according to you. But the problem is same the solution stops for KE. Well resizable KE
is already running successfully but it is not converging. While using K-Omega SST model the solution is converged and max Velocity is 130m/s.
For K-Epsilon the problem is remain as its is
Thanks
__________________
It is not in the stars to hold our destiny but in ourselves
Regards
Amit Mathur
Amit Mathur is offline   Reply With Quote

Old   January 27, 2011, 06:08
Default
  #8
Member
 
Join Date: Jun 2010
Posts: 33
Rep Power: 7
RalphS is on a distinguished road
Have your tried to use a start solution for KE?

With realizable KE and K-Omega SST the simulation runs without stopping?
Why you want to use KE then?
RalphS is offline   Reply With Quote

Old   January 27, 2011, 06:14
Default problem in rhosimplefoam using k-epsilon model
  #9
New Member
 
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 6
Amit Mathur is on a distinguished road
Dear RalpS,
The solution runs successfully in Simple Foam (incompressible) but fails using
rhoSimpleFoam (compressible) while using K-epsilon.
The initial value of K-E from turbulent intensity and mixing length.
__________________
It is not in the stars to hold our destiny but in ourselves
Regards
Amit Mathur
Amit Mathur is offline   Reply With Quote

Old   January 28, 2011, 03:59
Default
  #10
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi Amit,

Since you are getting converged solutions with k-omega that means your case setup is correct.

But if you want to have solutions with k-epsilon try the following and see if you are getting any convergence:

1 Are you using the fvSchemes proposed by Ralph? If yes then make the divScheme for (phi, U) as upwind also. Use upwind scheme for all divSchemes as it is first order.

2 Run the case with turbulence switched off and solve for the flow field. Then use this converged solution as initial condition for turbulence on.

Hope this helps you. If you still face problems then upload your case and I will try to have a look if time permits.
nakul is offline   Reply With Quote

Old   January 28, 2011, 05:10
Default
  #11
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 234
Rep Power: 9
olivierG is on a distinguished road
Hello,
Did you run in parallel ? Because there is some trouble with turbulence (k-epsilon) and DILUPBiCG (see Problem using single precision in simpleFoam )
So you may try to switch to smooth solver for U, k and epsilon, and keep Gauss upwind for div(phi,k) and div(phi,epsilon)
Also try Gauss linearUpwind cellLimited Gauss linear 1; for div(phi,U)

Regards,
olivier
olivierG is offline   Reply With Quote

Old   January 28, 2011, 06:29
Default problem in rhosimplefoam using k-epsilon model
  #12
New Member
 
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 6
Amit Mathur is on a distinguished road
Hi Nukul,
Thanks for replying. I made changes what so ever you suggested to me. But the problem is remain as it is. The solution blow of after some iterations.
It runs good while making turbulence off and starts converging. I solve the flow field
without turbulence model. Its runs and converged up to 10e-3. And then "on" the turbulence model. But again solution is blow after 9 or 10 iterations.
Thanks
__________________
It is not in the stars to hold our destiny but in ourselves
Regards
Amit Mathur
Amit Mathur is offline   Reply With Quote

Old   January 28, 2011, 06:34
Default
  #13
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 234
Rep Power: 9
olivierG is on a distinguished road
Hello,
OpenFoam is sensitive to initial values, specialy with turbulence one.
Show your k and epsilon file in 0/ dir.
What is your initial conditions ?

Regards,
olivier
olivierG is offline   Reply With Quote

Old   January 28, 2011, 06:59
Default problem in rhosimplefoam using k-epsilon model
  #14
New Member
 
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 6
Amit Mathur is on a distinguished road
Hi OlivierG,
Thanks for reply. I runs solver in parallel. But in series the problem of blowing is not solved. I changed the solver and schemes settings as you suggest to me but the problem as its is.
Here below i am showing my k and epsilon file.
K-
FoamFile
{
version 2.0;
format binary;
class volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [ 0 2 -2 0 0 0 0 ];

internalField uniform 1;

boundaryField
{
wall
{
type compressible::kqRWallFunction;
value uniform 1;
}
inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.01;
value uniform 1;
}
outlet
{
type inletOutlet;
inletValue uniform 1;
value uniform 1;
}
symplane
{
type symmetryPlane;
}
}
and Epsilon-

dimensions [0 2 -3 0 0 0 0];

internalField uniform 1;

boundaryField
{
inlet
{
type fixedValue;
value uniform 1;
}
outlet
{
type fixedValue;
value uniform 1;
}
symplane
{
type symmetryPlane;

}
wall
{
type compressible::epsilonWallFunction;
value uniform 1;
}

}
__________________
It is not in the stars to hold our destiny but in ourselves
Regards
Amit Mathur
Amit Mathur is offline   Reply With Quote

Old   January 28, 2011, 07:15
Default
  #15
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 234
Rep Power: 9
olivierG is on a distinguished road
Hello,
1) for outlet, try zeroGradient for k and epsilon
2) for inlet, k is ok, but for epsilon you can use "turbulentMixingLengthDissipationRateInlet"
In any case, for k/epsilon, you may also try fixedValue at inlet
3) You use initial value 1 for k and 1 for epsilon: are you sure this is a correcte estimation ? (i think no)
check http://www.openfoam.com/docs/user/ca...#x5-290002.1.7 at chap2.1.8.1

Regards,
Olivier
olivierG is offline   Reply With Quote

Old   January 29, 2011, 03:46
Default problem in rhosimplefoam using k-epsilon model
  #16
New Member
 
Amit Mathur
Join Date: Dec 2010
Location: India, New Delhi
Posts: 10
Rep Power: 6
Amit Mathur is on a distinguished road
Dear OlivierG,
Thanks for reply.
I made the k and epsilon boundary condition to zero gradient at outlet and for inlet epsilon
turbulentMixingLengthDissipationRateInlet is used. The mixing length is 0.00821.
It is difficult to predict the correct value of k-epsilon for boundaries because the flow is pressure driven.
Inlet-101325
outlet-98383
But on the basis of successful simulation of model using K-omegaSST model which is previously done. The max velocity is 130m/s. As reference of that velocity 130m/s and using intensity 1% i calculate k=2.535 and epsilon=4.368.
But the things are not working, the solution is just blow off after 5 iterations.
thanks
__________________
It is not in the stars to hold our destiny but in ourselves
Regards
Amit Mathur
Amit Mathur is offline   Reply With Quote

Old   October 6, 2013, 11:09
Default
  #17
Member
 
Martin Novák
Join Date: Dec 2012
Location: Prague
Posts: 56
Rep Power: 4
novakm is on a distinguished road
Quote:
Originally Posted by Amit Mathur View Post
Dear OlivierG,
Thanks for reply.
I made the k and epsilon boundary condition to zero gradient at outlet and for inlet epsilon
turbulentMixingLengthDissipationRateInlet is used. The mixing length is 0.00821.
It is difficult to predict the correct value of k-epsilon for boundaries because the flow is pressure driven.
Inlet-101325
outlet-98383
But on the basis of successful simulation of model using K-omegaSST model which is previously done. The max velocity is 130m/s. As reference of that velocity 130m/s and using intensity 1% i calculate k=2.535 and epsilon=4.368.
But the things are not working, the solution is just blow off after 5 iterations.
thanks
Hi amit.

I am facing same issue. Did you find out a reasonable solution for such a setting?

Best regards

Martin
novakm 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
compressible flow calculation error using rhoSimpleFoam solver student4326 OpenFOAM 6 February 10, 2012 10:36
bounding epsilon blow up jiez OpenFOAM Running, Solving & CFD 4 January 16, 2011 18:14
Epsilon boundary condition for walls in LamBremhorst LowRe model maruthamuthu_venkatraman OpenFOAM 0 March 16, 2010 04:27
Weller combustion model - engineFoam solver. ghindi OpenFOAM Running, Solving & CFD 0 February 22, 2010 05:02
Compressible magnetohydrodynamics solver thekay OpenFOAM 0 January 27, 2010 09:04


All times are GMT -4. The time now is 05:00.