CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Cannot get similiar result with fluent (http://www.cfd-online.com/Forums/cfx/94145-cannot-get-similiar-result-fluent.html)

qsx4881 November 7, 2011 11:30

Thermal Stratification Cannot get similiar result with fluent
 
5 Attachment(s)
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 13:23

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 05:27

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 07:34

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

Far November 8, 2011 08:04

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 11:03

Quote:

Originally Posted by ghorrocks (Post 331160)
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.:p

qsx4881 November 8, 2011 11:15

Quote:

Originally Posted by Far (Post 331184)
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 17:43

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 22:00

4 Attachment(s)
Quote:

Originally Posted by ghorrocks (Post 331273)
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 23:19

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 05:39

4 Attachment(s)
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 05:49

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 06:19

There is an FAQ describing exactly what you should do:

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

qsx4881 November 9, 2011 11:22

1 Attachment(s)
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 11:24

Quote:

Originally Posted by qsx4881 (Post 331384)
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 19:08

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

qsx4881 November 10, 2011 02:40

Quote:

Originally Posted by ghorrocks (Post 331439)
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 02:44

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 05:24

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

qsx4881 November 10, 2011 11:20

Quote:

Originally Posted by Far (Post 331473)
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


All times are GMT -4. The time now is 17:36.