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

Problem in 3D Navier stokes solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 25, 2013, 03:36
Default Problem in 3D Navier stokes solver
  #1
New Member
 
suhasjain
Join Date: Aug 2012
Location: Paderborn,Germany
Posts: 27
Rep Power: 4
suhas jain is on a distinguished road
Hi everyone,

I am solving unsteady 3D Navier stokes equations on staggered cartesian grid. The solver is converging but the results are not matching with the Literature. What might be the reason? I have attached the profile obtained for Re Number 1000.


Thanks in advance.

suhas
Attached Images
File Type: jpg 3d navier staokes.jpg (38.3 KB, 24 views)
__________________
Suhas Jain
suhas.jain2000@gmail.com
suhas jain is offline   Reply With Quote

Old   October 25, 2013, 04:12
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,189
Rep Power: 16
FMDenaro will become famous soon enough
check if you really reached a steady solution, then check if the divergence-free constraint is satisfied cell-by-cell. The BC is correctly imposed?
Furthermore, you case is a 3D lid-driven, what database are you using to compare your solution?
FMDenaro is offline   Reply With Quote

Old   October 25, 2013, 05:41
Default
  #3
New Member
 
suhasjain
Join Date: Aug 2012
Location: Paderborn,Germany
Posts: 27
Rep Power: 4
suhas jain is on a distinguished road
Hi,


Thank you for the reply.

1. It is reaching steady state.
2. It is divergence-free with residual 10e-10
3. I am doubtful about the boundary condition applied. I am using explicit BC method i.e I am updating the value of ghost cell after the iteration. Is this right?
4. I ran the same solution in OpenFOAM to compare it with mine and referred Feldman paper to match 3D results.


And the more important thing is I am using first order upwind which should be more diffusive. But I am getting a bigger secondary vortex as can be seen in the above attachment. How can this occur?
__________________
Suhas Jain
suhas.jain2000@gmail.com
suhas jain is offline   Reply With Quote

Old   October 25, 2013, 06:01
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,189
Rep Power: 16
FMDenaro will become famous soon enough
Quote:
Originally Posted by suhas jain View Post
Hi,


Thank you for the reply.

1. It is reaching steady state.
2. It is divergence-free with residual 10e-10
3. I am doubtful about the boundary condition applied. I am using explicit BC method i.e I am updating the value of ghost cell after the iteration. Is this right?
4. I ran the same solution in OpenFOAM to compare it with mine and referred Feldman paper to match 3D results.


And the more important thing is I am using first order upwind which should be more diffusive. But I am getting a bigger secondary vortex as can be seen in the above attachment. How can this occur?
1. is reaching or reached?
2. cell-by-cell?
3. are you using a first order extrapolation?
4. I don't know that paper, I suggest to check for a more quantitative variable than the snapshot of streamlines. It is also advisable to check if a 2D solver provides the well known solution at Re=1000.

First order upwind can increase the tangential stress, more energy can be transferred to secondary vortices and they can become bigger.
FMDenaro is offline   Reply With Quote

Old   October 25, 2013, 08:36
Default
  #5
New Member
 
suhasjain
Join Date: Aug 2012
Location: Paderborn,Germany
Posts: 27
Rep Power: 4
suhas jain is on a distinguished road
1. It has already reached steady state.
2. I am checking divergence free for every cell and the max value of residual is 10e-10.
3. What exactly do you mean by extrapolation(Is it richardson extrapolation?).
4. I have plotted the centre line value of Ux velocity and tried to match with Ghia's result, but there is small difference due to the presence of that vortex which cuts that centre line.
__________________
Suhas Jain
suhas.jain2000@gmail.com
suhas jain is offline   Reply With Quote

Old   October 25, 2013, 08:54
Default
  #6
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,189
Rep Power: 16
FMDenaro will become famous soon enough
you can not compare your 3D driven cavity with the Ghia's solution that is 2D... have you tested the 2D OpenFoam solver?
FMDenaro is offline   Reply With Quote

Old   October 25, 2013, 09:00
Default
  #7
New Member
 
suhasjain
Join Date: Aug 2012
Location: Paderborn,Germany
Posts: 27
Rep Power: 4
suhas jain is on a distinguished road
No I ran a 3D OpenFOAM problem. And one more difference is the solution in OpenFOAM was highly unsteady for that Reynolds Number. But for my case it was less fluctuating and reached steady state earlier than OpenFOAM's result.
__________________
Suhas Jain
suhas.jain2000@gmail.com
suhas jain is offline   Reply With Quote

Old   October 25, 2013, 09:05
Default
  #8
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,189
Rep Power: 16
FMDenaro will become famous soon enough
Quote:
Originally Posted by suhas jain View Post
No I ran a 3D OpenFOAM problem. And one more difference is the solution in OpenFOAM was highly unsteady for that Reynolds Number. But for my case it was less fluctuating and reached steady state earlier than OpenFOAM's result.
it has no sense in comparing 3D and 2D solutions due to the strong effect of the lateral walls.... you have to do a 2D run..
A possible chance is to run a lower Re case (Re=400) using the 3D solver but setting periodic condition in the spanwise direction (z).
FMDenaro is offline   Reply With Quote

Old   October 25, 2013, 09:11
Default
  #9
New Member
 
suhasjain
Join Date: Aug 2012
Location: Paderborn,Germany
Posts: 27
Rep Power: 4
suhas jain is on a distinguished road
No I actually ran 3D OpenFOAM code to match it with my solver which is also 3D.
__________________
Suhas Jain
suhas.jain2000@gmail.com
suhas jain is offline   Reply With Quote

Old   October 26, 2013, 11:36
Default
  #10
Member
 
M. Nabi
Join Date: Jun 2009
Posts: 41
Rep Power: 7
mnabi is on a distinguished road
It is probably because of first order upwinding. Try, for example, Quick Scheme and then compare the results.
mnabi is offline   Reply With Quote

Old   October 26, 2013, 14:19
Default
  #11
New Member
 
suhasjain
Join Date: Aug 2012
Location: Paderborn,Germany
Posts: 27
Rep Power: 4
suhas jain is on a distinguished road
Yes I am changing that first order upwind now to deferred correction by giving blending between UDS and CDS.
__________________
Suhas Jain
suhas.jain2000@gmail.com
suhas jain is offline   Reply With Quote

Old   October 26, 2013, 14:32
Default
  #12
Member
 
M. Nabi
Join Date: Jun 2009
Posts: 41
Rep Power: 7
mnabi is on a distinguished road
You also can try central differentiating. If you use pressure correction, no wiggles will usually happen, as the pressure correction acts as stabilizer for the momentum. You can try, and see either your model works without wiggles for your applied Re number.
mnabi 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
thobois class engineTopoChangerMesh error Peter_600 OpenFOAM 4 August 2, 2014 09:52
solver compilation problem, /bin/linux64GccDPOpt directory empty arnaud6 OpenFOAM Running, Solving & CFD 0 July 25, 2013 10:48
Solver problem in Oscillating Plate tutorial vovogoal CFX 1 November 22, 2011 09:54
Coupled solver energy equation problem lucioantonio FLUENT 0 April 3, 2009 10:21
Can I use coupled solver for this problem Frank FLUENT 0 April 11, 2006 06:28


All times are GMT -4. The time now is 20:14.