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

Cannot get similiar result with fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 7, 2011, 11:30
Default Thermal Stratification Cannot get similiar result with fluent
  #1
New Member
 
Joe
Join Date: Aug 2011
Posts: 14
Rep Power: 5
qsx4881 is on a distinguished road
Dear all,
I am simulating thermal stratification in pipe.
In piping systems where hot and cold fluids flow in, two fluid layers can be formed due to the difference in fluid density (or temperature). Such a phenomenon is called thermal stratification. When this is the case, the cold (denser) fluid occupies the lower position of the pipe while the hot fluid occupies the upper space.
In my computational domain, cold water(denser) enters through the left inlet with a velocity of 15.852m/s, while hot water enters through the up inlet with a velocity of 0.0175m/s,0Pa at the outlet. See the figure. I use k-epsilon model. In order to simulate the phenomena of thermal stratification, gravity need to be considered. So I select the buoyancy model.
The question is CFX computational results does not meet the actual physical laws. But I can get a good result with Fluent. The interface of cold water and hot water should be approximate horizontal. See the following pictures. The above picture is the result of CFX ,bottom Fluent. I do not know why I get the wrong results whth CFX, there is something wrong in my setting? I have uploaded the ccl file. Please help!
Thanks in advance!
Attached Images
File Type: png 1.png (20.9 KB, 28 views)
File Type: png contrast.png (76.2 KB, 29 views)
File Type: jpg contrast1.jpg (40.4 KB, 28 views)
File Type: jpg contrast2.jpg (40.5 KB, 27 views)
Attached Files
File Type: txt thermal stratification.txt (27.8 KB, 28 views)

Last edited by qsx4881; November 8, 2011 at 21:03.
qsx4881 is offline   Reply With Quote

Old   November 7, 2011, 13:23
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I am also facing same problem. My CFX results are good for turbo-machinery cases, therefore I have decided to shift to CFX and remain with Fluent for all other cases.
Far is offline   Reply With Quote

Old   November 8, 2011, 05:27
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You have too much diffusion in your CFX simulation. Are you using upwinding? You should be using high-res, or even better hybrid with a blend factor of 1.0. Also second order time stepping if transient. And make sure you have converged tight enough.

Is it the same mesh in the two runs? This can also be caused by coarse meshes, or even poor quality meshes.
ghorrocks is offline   Reply With Quote

Old   November 8, 2011, 07:34
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
But glenn, isn't it true that at some point CFX is more stronger than Fluent and Vice versa?
Far is offline   Reply With Quote

Old   November 8, 2011, 08:04
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by CCL file
SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution

END
Seems to be using the high order scheme for momentum and turbulence model. So this is not the problem
Quote:
Originally Posted by CCL file
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 100000
Minimum Number of Iterations = 1
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END
Try to use the timescale factor = 0.5 and lets see what happens!

Quote:
Originally Posted by CCL file
CONVERGENCE CRITERIA:
Conservation Target = 0.01
Residual Target = 1e-06
Residual Type = RMS
END
Quote:
Originally Posted by Glenn
And make sure you have converged tight enough
Although conservation target = 0.01 may be ok for design iteration and not for type of study you are making i.e. comparing two codes. Lets see what happens if you change it to 0.001 otherwise delete this line and do not use this option at all. I guess this is what Glenn referring to!!! And are you sure that you touch the residual criteria of 1e-06 for all equations?

For your understanding I am quoting one of the Glenn's post regarding the convergence criteria setting in CFX pre for some different type of usage

Quote:
Originally Posted by Glenn
Turn the imbalances convergence criteria on in the output tab and set the criteria to 0.01. Note that this will apply the imbalance criteria to all equations, not just the H-energy equation. define a convergence criteria in CFX-Pre
Far is offline   Reply With Quote

Old   November 8, 2011, 11:03
Default
  #6
New Member
 
Joe
Join Date: Aug 2011
Posts: 14
Rep Power: 5
qsx4881 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You have too much diffusion in your CFX simulation. Are you using upwinding? You should be using high-res, or even better hybrid with a blend factor of 1.0. Also second order time stepping if transient. And make sure you have converged tight enough.

Is it the same mesh in the two runs? This can also be caused by coarse meshes, or even poor quality meshes.
@ghorrocks

Thanks for your suggestion!
1. The mesh were generated with icemcfd and imported as .cfx5 and .msh files for cfx and fluent. So the mesh number and quality are similar.
2. I have used High Resolution for Advection Scheme and Tumberlance Numerics.
As you say, whether steady or transient simulation the result is similar and the diffusion is serious.
I will try hybrid with a blend factor of 1.0, and upload my result soon.
Thanks again.
qsx4881 is offline   Reply With Quote

Old   November 8, 2011, 11:15
Default
  #7
New Member
 
Joe
Join Date: Aug 2011
Posts: 14
Rep Power: 5
qsx4881 is on a distinguished road
Quote:
Originally Posted by Far View Post
Seems to be using the high order scheme for momentum and turbulence model. So this is not the problem

Try to use the timescale factor = 0.5 and lets see what happens!





Although conservation target = 0.01 may be ok for design iteration and not for type of study you are making i.e. comparing two codes. Lets see what happens if you change it to 0.001 otherwise delete this line and do not use this option at all. I guess this is what Glenn referring to!!! And are you sure that you touch the residual criteria of 1e-06 for all equations?

For your understanding I am quoting one of the Glenn's post regarding the convergence criteria setting in CFX pre for some different type of usage
@Far
Thank you for your reply.
I do donot reach the residual criteria of 1e-06. I set the residual target as 1e-6 just want to keep the computation going until it reach steady. When I changed the analysis type to trensient, the residual was changed to 1e-4 as well.
I will also try your suggestion for change the conservation target from 0.01 to 0.001 or remove the limit.
Thank you again!
qsx4881 is offline   Reply With Quote

Old   November 8, 2011, 17:43
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you are looking for the steady state result then I would expect the hot and cold water to diffuse the temperature between them. How do you know the fluent result is correct? How much diffusion of the interface is correct?
ghorrocks is offline   Reply With Quote

Old   November 8, 2011, 22:00
Default
  #9
New Member
 
Joe
Join Date: Aug 2011
Posts: 14
Rep Power: 5
qsx4881 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
If you are looking for the steady state result then I would expect the hot and cold water to diffuse the temperature between them. How do you know the fluent result is correct? How much diffusion of the interface is correct?
To be honest, I am not sure the fluent results are entirely correct. But the fluent result seems more reasonalbe. Because thermal stratification is caused by different density, the thermal interface reflects the density interface, so the interface should be horizontal. But the interface of cfx result is slope. See the following pictures(the density contour of wall).
I am trying your and Far's suggestion and will upload the results soon.
Attached Images
File Type: png stratified interface.png (57.0 KB, 12 views)
File Type: png density1.png (70.0 KB, 14 views)
File Type: jpg density2.jpg (40.1 KB, 17 views)
File Type: jpg density3.jpg (40.5 KB, 13 views)
qsx4881 is offline   Reply With Quote

Old   November 8, 2011, 23:19
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The CFX result is stratified, it is just that a lot of diffusion has meant the temperature front ends up being a diagonal line rather than a horizontal line. This can be physically correct so do not write it off as wrong unless you know what the true flow really is.

It may be that Fluent does not have enough diffusion and the CFX result is correct.
ghorrocks is offline   Reply With Quote

Old   November 9, 2011, 05:39
Default
  #11
New Member
 
Joe
Join Date: Aug 2011
Posts: 14
Rep Power: 5
qsx4881 is on a distinguished road
I checked my residuals.
Unfortunately,the energy residual of steady state simulation is high. But does it has a such big impact on the results? Should I use a smaller physical time step(I have used autotime scale)? Refine the mesh,or what should I do?
Attached Images
File Type: png residual1.png (12.4 KB, 11 views)
File Type: png residual2.png (11.4 KB, 10 views)
File Type: png residual3.png (11.4 KB, 10 views)
File Type: png residual4.png (17.5 KB, 14 views)
qsx4881 is offline   Reply With Quote

Old   November 9, 2011, 05:49
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
What is the maximum yplus?

1. change time scale factor = 0.5 if problem persist then
2. rerun with SST model,
3. if residuals are still at the similar level then it might be the mesh problem, but it is too early to jump onto to conclusions
Far is offline   Reply With Quote

Old   November 9, 2011, 06:19
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
There is an FAQ describing exactly what you should do:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is offline   Reply With Quote

Old   November 9, 2011, 11:22
Post
  #14
New Member
 
Joe
Join Date: Aug 2011
Posts: 14
Rep Power: 5
qsx4881 is on a distinguished road
I have tried hybrid with a blend factor of 1.0, the residual of all equation remained high. The results seems not correct, so Ichanged the blend factor to 0.75. I have also tried changed the time scale factor in to 5, it did not work well.
I have uploaded the tin, block and ccl files. I am honored that if you have a try!
Many thanks!
Attached Files
File Type: zip tin block and ccl.zip (23.0 KB, 6 views)
qsx4881 is offline   Reply With Quote

Old   November 9, 2011, 11:24
Default
  #15
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by qsx4881 View Post
I have also tried changed the time scale factor in to 5, it did not work well.
Many thanks!
It is 0.5 not 5 and also SST model
Far is offline   Reply With Quote

Old   November 9, 2011, 19:08
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Please have a look at the FAQ I posted. It describes in some detail what you should do.
ghorrocks is offline   Reply With Quote

Old   November 10, 2011, 02:40
Default
  #17
New Member
 
Joe
Join Date: Aug 2011
Posts: 14
Rep Power: 5
qsx4881 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Please have a look at the FAQ I posted. It describes in some detail what you should do.
Thanks, I am reading the wiki page of you recommend and the cfx guide.
qsx4881 is offline   Reply With Quote

Old   November 10, 2011, 02:44
Default
  #18
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,916
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Checked your mesh and got determinant = 0.2-0.3 at the 90 deg band in small long pipe. increase the quality = 0.3 or higher.
Far is offline   Reply With Quote

Old   November 10, 2011, 05:24
Default
  #19
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,831
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Bad mesh quality increases diffusion and makes convergence harder. Improving mesh quality is always worthwhile.
ghorrocks is offline   Reply With Quote

Old   November 10, 2011, 11:20
Default
  #20
New Member
 
Joe
Join Date: Aug 2011
Posts: 14
Rep Power: 5
qsx4881 is on a distinguished road
Quote:
Originally Posted by Far View Post
Checked your mesh and got determinant = 0.2-0.3 at the 90 deg band in small long pipe. increase the quality = 0.3 or higher.
Mesh quality statistics:
determinant 2*2*2>0.5
degree>36
qsx4881 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
How to start Fluent with Matlab?? Jay Hu FLUENT 5 October 9, 2013 14:20
Abaqus - Fluent Coupling WITHOUT MPCCI s.mishra FLUENT 0 May 1, 2011 09:45
Fluent Vs Star CCM firda Main CFD Forum 3 February 26, 2011 03:51
few quesions on ANSYS ICEMCFD and FLUENT Prakash.Paudel ANSYS 0 August 12, 2010 12:07
Fluent 6.3.26 vs 12.1 and partition method Anorky FLUENT 0 April 27, 2010 10:55


All times are GMT -4. The time now is 20:39.