Cannot get similiar result with fluent

qsx4881 · November 7, 2011, 10:30

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!

Far · November 7, 2011, 12:23

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.

ghorrocks · November 8, 2011, 04:27

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.

Far · November 8, 2011, 06:34

But glenn, isn't it true that at some point CFX is more stronger than Fluent and Vice versa?

Far · November 8, 2011, 07:04

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. http://www.cfd-online.com/Forums/cfx...a-cfx-pre.html

qsx4881 · November 8, 2011, 10:03

Quote:

Originally Posted by ghorrocks

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 · November 8, 2011, 10:15

Quote:

Originally Posted by Far

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!

ghorrocks · November 8, 2011, 16:43

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?

qsx4881 · November 8, 2011, 21:00

Quote:

Originally Posted by ghorrocks

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.

ghorrocks · November 8, 2011, 22:19

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.

qsx4881 · November 9, 2011, 04:39

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?

Far · November 9, 2011, 04:49

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

ghorrocks · November 9, 2011, 05:19

There is an FAQ describing exactly what you should do:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

qsx4881 · November 9, 2011, 10:22

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!

Far · November 9, 2011, 10:24

Quote:

Originally Posted by qsx4881

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

ghorrocks · November 9, 2011, 18:08

Please have a look at the FAQ I posted. It describes in some detail what you should do.

qsx4881 · November 10, 2011, 01:40

Quote:

Originally Posted by ghorrocks

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.

Far · November 10, 2011, 01:44

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.

ghorrocks · November 10, 2011, 04:24

Bad mesh quality increases diffusion and makes convergence harder. Improving mesh quality is always worthwhile.

qsx4881 · November 10, 2011, 10:20

Quote:

Originally Posted by 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.

Mesh quality statistics:
determinant 2*2*2>0.5
degree>36

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
How to start Fluent with Matlab??	Jay Hu	FLUENT	8	November 9, 2022 06:30
Abaqus - Fluent Coupling WITHOUT MPCCI	s.mishra	FLUENT	1	April 5, 2016 06:47
Fluent Vs Star CCM	firda	Main CFD Forum	3	February 26, 2011 02:51
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

November 7, 2011, 12:23		#2
Far Super Moderator Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,553 Blog Entries: 6 Rep Power: 54	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.

November 8, 2011, 04:27		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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.

November 8, 2011, 06:34		#4
Far Super Moderator Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,553 Blog Entries: 6 Rep Power: 54	But glenn, isn't it true that at some point CFX is more stronger than Fluent and Vice versa?

November 8, 2011, 16:43		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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?

November 8, 2011, 22:19		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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.

November 9, 2011, 04:49		#12
Far Super Moderator Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,553 Blog Entries: 6 Rep Power: 54	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

November 9, 2011, 05:19		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	There is an FAQ describing exactly what you should do: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

November 9, 2011, 18:08		#16
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Please have a look at the FAQ I posted. It describes in some detail what you should do.

November 10, 2011, 01:44		#18
Far Super Moderator Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,553 Blog Entries: 6 Rep Power: 54	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.

November 10, 2011, 04:24		#19
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Bad mesh quality increases diffusion and makes convergence harder. Improving mesh quality is always worthwhile.