CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Natural Convection - cavity - problem

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

Like Tree3Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 6, 2021, 05:51
Default
  #21
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
Hi,

I simulated natural convection in a square cavity using OpenFOAM7, installed on ubuntu 18.04LTS. The numerical simulation results were compared against experimental data of Ampofo F. and Karayiannis T.,2003.
The correspondence of the vertical velocity profile at the mid-height of the cavity with the experiment is good. However, the average temperature profile is under-predicted than the corresponding experimental data. When calculating using different versions of the OpenFOAM package(OF5, OF6, OF8), the average temperature profiles are small compared to the experiment. I will be happy if someone can help to solve this issue.
Kerim
Share case setup if possible. It's difficult to suggest anything on this information.
sadsid is offline   Reply With Quote

Old   May 6, 2021, 09:01
Default
  #22
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
Share case setup if possible. It's difficult to suggest anything on this information.
Dear Sadsid,


I used upwind scheme. Maybe that is a reason of under prediction of T.
Kerim
Attached Files
File Type: zip aa.zip (156.6 KB, 10 views)
kerim is offline   Reply With Quote

Old   May 6, 2021, 11:35
Default
  #23
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
Dear Sadsid,


I used upwind scheme. Maybe that is a reason of under prediction of T.
Kerim
Pl. share the "constant" folder as well. I want to test the case by running it.
sadsid is offline   Reply With Quote

Old   May 7, 2021, 02:07
Default
  #24
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
Dear Sadsid,


I used upwind scheme. Maybe that is a reason of under prediction of T.
Kerim
No need to share constant folder. If possible share the data with which you are trying to get a comparision.
sadsid is offline   Reply With Quote

Old   May 7, 2021, 07:00
Default
  #25
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
No need to share constant folder. If possible share the data with which you are trying to get a comparision.
Vertical velocity profile at mid-height in the cavity was digitized from this article:
https://www.researchgate.net/publica..._square_cavity
kerim is offline   Reply With Quote

Old   May 7, 2021, 07:02
Default
  #26
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
No need to share constant folder. If possible share the data with which you are trying to get a comparision.
The vertical velocity profile was attached.
Attached Files
File Type: txt Fig.2.txt (1.6 KB, 8 views)
kerim is offline   Reply With Quote

Old   May 8, 2021, 03:20
Default
  #27
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
The vertical velocity profile was attached.

My observations are:
1) your mesh coarser and it can be a reason for the wrong profile. Use stretching normal to the surface (I would prefer on the left and right walls as temperature gradients are expected to be steeper at these surfaces).
2) your solution is not statistically converged and ultimately giving wrong results.
3) Instead of 2D, you can test 3D (a more appropriate way to handle turbulent flow). The results you are trying to retrieve are for a cavity with dimensions .75x.75x1.5. So try 3D.

Good Luck!
sadsid is offline   Reply With Quote

Old   May 16, 2021, 20:09
Default
  #28
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
The vertical velocity profile was attached.
A better result!
Attached Images
File Type: jpg Figure_1.jpg (39.0 KB, 27 views)
sadsid is offline   Reply With Quote

Old   May 17, 2021, 23:50
Default
  #29
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
A better result!
Thank you FYI. Would you like to give more info about it?
I struggling with two equations models but have small success with LLR and SGG ones.
Attached Images
File Type: jpg LRR-SSG-LIC.jpg (89.6 KB, 19 views)
kerim is offline   Reply With Quote

Old   May 18, 2021, 00:27
Default
  #30
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
Thank you FYI. Would you like to give more info about it?
I struggling with two equations models but have small success with LLR and SGG ones.
I formulated 3D-LES model and used 90x80x180 number of cells. I think, a little more dense mesh will give me more closer results. Your boundary conditions are correct. I think you should increase the number of cells.
sadsid is offline   Reply With Quote

Old   May 18, 2021, 03:34
Default
  #31
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
I formulated 3D-LES model and used 90x80x180 number of cells. I think, a little more dense mesh will give me more closer results. Your boundary conditions are correct. I think you should increase the number of cells.

At first, I thought about LES modelling. However, as a first step, the RANS model turned out to be easier for me. As a first approximation, the simulation was for 2D. Increasing the number of nodes up to 500 in each direction RANS does not give an acceptable result. Both models for large Reynolds numbers and models for low numbers were used. The numerical results in both cases are approximately equally underpredicted.


PS. I came to this problem because of buoyantCavity tutorial:
Please see: OpenFOAM 7 buoyantCavity tutorial-ERCOFTAC test case 79
p { margin-bottom: 0.1in; line-height: 115% }a:link { so-language: zxx }
kerim is offline   Reply With Quote

Old   May 18, 2021, 10:09
Default
  #32
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
At first, I thought about LES modelling. However, as a first step, the RANS model turned out to be easier for me. As a first approximation, the simulation was for 2D. Increasing the number of nodes up to 500 in each direction RANS does not give an acceptable result. Both models for large Reynolds numbers and models for low numbers were used. The numerical results in both cases are approximately equally underpredicted.


PS. I came to this problem because of buoyantCavity tutorial:
Please see: OpenFOAM 7 buoyantCavity tutorial-ERCOFTAC test case 79
p { margin-bottom: 0.1in; line-height: 115% }a:link { so-language: zxx }
If you want I can share my mesh so that you can test your case on a mesh with stretching introduced on side walls. I think you are struggling because of mesh!
sadsid is offline   Reply With Quote

Old   May 19, 2021, 08:11
Default
  #33
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
If you want I can share my mesh so that you can test your case on a mesh with stretching introduced on side walls. I think you are struggling because of mesh!
If you can share with your mesh that will be great for me.
kerim is offline   Reply With Quote

Old   May 19, 2021, 19:53
Default
  #34
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
My observations are:
1) your mesh coarser and it can be a reason for the wrong profile. Use stretching normal to the surface (I would prefer on the left and right walls as temperature gradients are expected to be steeper at these surfaces).
2) your solution is not statistically converged and ultimately giving wrong results.
3) Instead of 2D, you can test 3D (a more appropriate way to handle turbulent flow). The results you are trying to retrieve are for a cavity with dimensions .75x.75x1.5. So try 3D.

Good Luck!
Hi,


You were right about 3D. I used graded mesh in the OX and OY directions, and uniform mesh in the OZ direction. And got better kOmegaSST results. May be I should take more finer 3D mesh.


Going ahead, I faced with the next error during LES modelling:



--> FOAM FATAL ERROR:

[U[0 1 -2 0 0 0 0] ] == [-grad(p)[1 -2 -2 0 0 0 0] ]


I never used LES but I know the problem is concerned with dimensions.

Could you help me to resolve this issue?
Attached Images
File Type: png residuals.png (9.0 KB, 14 views)
File Type: jpg T-profile.jpg (99.4 KB, 11 views)
kerim is offline   Reply With Quote

Old   May 19, 2021, 22:10
Default
  #35
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
Hi,


You were right about 3D. I used graded mesh in the OX and OY directions, and uniform mesh in the OZ direction. And got better kOmegaSST results. May be I should take more finer 3D mesh.


Going ahead, I faced with the next error during LES modelling:



--> FOAM FATAL ERROR:

[U[0 1 -2 0 0 0 0] ] == [-grad(p)[1 -2 -2 0 0 0 0] ]


I never used LES but I know the problem is concerned with dimensions.

Could you help me to resolve this issue?

Your dimensions for pressure are wrong. I think it should be: dimensions [0 2 -2 0 0 0 0]. I think you need to correct it in 0 folder. Regarding mesh, it is not possible to upload here due to its size. I can share over email. Let me how can I share!
sadsid is offline   Reply With Quote

Old   May 20, 2021, 01:47
Default
  #36
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
Your dimensions for pressure are wrong. I think it should be: dimensions [0 2 -2 0 0 0 0]. I think you need to correct it in 0 folder. Regarding mesh, it is not possible to upload here due to its size. I can share over email. Let me how can I share!
Please see the attached picture for all changes I have made for LES modeling. I don't understand why should I change the dimension of the pressure in this case? I switched the turbulence model from kOmegaSST into LES and I have made minor appropriate changes in controlDict, fvScheme, fvSolution files.
Where I have made mistakes?
My email. is: abdikerimkurbanaliev@gmail.com
Attached Files
File Type: docx files.docx (13.3 KB, 9 views)
kerim is offline   Reply With Quote

Old   May 20, 2021, 01:50
Default
  #37
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by kerim View Post
Please see the attached picture for all changes I have made for LES modeling. I don't understand why should I change the dimension of the pressure in this case? I switched the turbulence model from kOmegaSST into LES and I have made minor appropriate changes in controlDict, fvScheme, fvSolution files.
Where I have made mistakes?
My email. is: abdikerimkurbanaliev@gmail.com
Sorry I forgot to attach a picture
Attached Images
File Type: jpg changed_from_kOmegaSST_into_LES.jpg (72.1 KB, 22 views)
kerim is offline   Reply With Quote

Old   May 24, 2021, 18:07
Default
  #38
Senior Member
 
abdikerim kurbanaliev
Join Date: Jun 2010
Location: Kyrgyzstan, Osh
Posts: 109
Rep Power: 14
kerim is on a distinguished road
Quote:
Originally Posted by sadsid View Post
Your dimensions for pressure are wrong. I think it should be: dimensions [0 2 -2 0 0 0 0]. I think you need to correct it in 0 folder. Regarding mesh, it is not possible to upload here due to its size. I can share over email. Let me how can I share!
I solved this issue.
kerim is offline   Reply With Quote

Old   May 24, 2021, 18:17
Default
  #39
Member
 
Join Date: Jan 2017
Posts: 68
Rep Power: 8
sadsid is on a distinguished road
Quote:
Originally Posted by kerim View Post
I solved this issue.
Good Luck!
sadsid is offline   Reply With Quote

Old   May 31, 2021, 08:28
Default
  #40
gu1
Senior Member
 
Guilherme
Join Date: Apr 2017
Posts: 184
Rep Power: 7
gu1 is on a distinguished road
Quote:
Originally Posted by kerim View Post
At first, I thought about LES modelling. However, as a first step, the RANS model turned out to be easier for me. As a first approximation, the simulation was for 2D. Increasing the number of nodes up to 500 in each direction RANS does not give an acceptable result. Both models for large Reynolds numbers and models for low numbers were used. The numerical results in both cases are approximately equally underpredicted.


PS. I came to this problem because of buoyantCavity tutorial:
Please see: OpenFOAM 7 buoyantCavity tutorial-ERCOFTAC test case 79
p { margin-bottom: 0.1in; line-height: 115% }a:link { so-language: zxx }
''After a small correction of buoyantCavity and using buoyantKE model of turbulence I had an acceptable agreement with ERCOFTAC test case 79. Please see the attached pictures'' (from ur post).

Can u share this corrections?

Best.
gu1 is offline   Reply With Quote

Reply

Tags
buoyantboussinesqsimple, natural convection

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Natural convection regime in a small cavity AntonioDesah FLUENT 7 May 5, 2020 08:48
Natural convection regime in a small cavity AntonioDesah Main CFD Forum 1 April 29, 2020 14:45
SU2-7.0.1 on ubuntu 18.04 hyunko SU2 Installation 7 March 16, 2020 05:37
UDF for body force for rotating cavity with natural convection s.jaiswal FLUENT 0 February 18, 2014 03:01
Natural Convection Problem Eduardo FLUENT 0 October 21, 2006 15:04


All times are GMT -4. The time now is 21:08.