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

Cd not matches with literature-How to improve simulation-frustrated-OF-user

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 20, 2016, 20:37
Default Cd not matches with literature-How to improve simulation-frustrated-OF-user
  #1
Member
 
Ran
Join Date: Aug 2016
Posts: 32
Rep Power: 5
random_ran is on a distinguished road
Dear O.F.er:

I am struggling with the benchmark problem: flow around circular cylinder at Reynolds number 3900. I am really appreciated it if anyone can give me some suggestions.

The blue line is my drag history. Mean drag gives me 1.30 averaged from 20 periods. Strouhal number matches with other people, but I am struggling with drag coefficient.

Result - Copy.png
The mesh is good. It was generated from ICEM in 2D and extended it in Z direction for 32 and 64 nodes (pi/2*D and pi*D) following YOUTUBE video. I tested the y+ number is smaller than 1 using ANSYS/FLUENT 17.0. The mesh configuration frequently shows up on the literature. Courant number is smaller than 0.2 during the simulation. The total number of control volume is 5 million for 32 nodes and 10 million for 64 nodes. The computational domain is 30D*20D, 10D from Inlet 20D from Outlet.
Grid2.JPG
Y+.JPG
As far as boundary conditions are concerned, I tried symmetry boundary condition for the front, back, up and down are wall; velocity inlet at INLET B.C. and zero pressure at OUTLET; noSlip at cylinder. I also tested periodic B.C. at front, back, up and down B.C., but there is no too much difference.

For time step, I choose 10^(-4) seconds. The solver is pisoFOAM. A geometric agglomerated algebraic multigrid solver (GAMG) with the Gauss-Seidel smooth method iteratively solve the linear algebraic system with a local accuracy of 10-6 for the pressure and 10-7 for the rest of variables at each time step.

In terms of turbulent model, I have tried SpalartAllmarasDDES LES model. I wanted to try dynOneEqEddy but fail with the O.F. coding.
Finally, I use OpenFOAM v4.1. The hardware and O.S. are as follows:
24 cores/node, Memory per node 32 G, infiniband connection, AMD @2.1GHz CPU, Centos 6.8. Most jobs are done using 144 cores parallel computing.
The 0, constant and control directory are lists in the following section.

Do you have any suggestion?

controlDict.txt
turbulenceProperties.txt

Last edited by random_ran; December 21, 2016 at 22:19.
random_ran is offline   Reply With Quote

Old   December 20, 2016, 20:40
Default
  #2
Member
 
Ran
Join Date: Aug 2016
Posts: 32
Rep Power: 5
random_ran is on a distinguished road
fvSchemes.txt

fvSolution.txt

k.txt

nut.txt

nuTilda.txt
random_ran is offline   Reply With Quote

Old   December 20, 2016, 20:41
Default
  #3
Member
 
Ran
Join Date: Aug 2016
Posts: 32
Rep Power: 5
random_ran is on a distinguished road
p.txt

U.txt
random_ran is offline   Reply With Quote

Old   December 21, 2016, 22:24
Default
  #4
Member
 
Ran
Join Date: Aug 2016
Posts: 32
Rep Power: 5
random_ran is on a distinguished road
Anyone? No suggestions? also the comment "stupid questions cannot expect great answer" would be useful !
random_ran is offline   Reply With Quote

Old   December 22, 2016, 05:19
Default
  #5
Senior Member
 
Join Date: Jun 2012
Location: Germany, Bochum
Posts: 220
Rep Power: 11
Bazinga is on a distinguished road
Well, I am also not certain why it is not working but here are some suggestions that might help:

Maybe try to improve the mesh in the wake flow. You have a nice transition from the o-grid to the upstream part of the domain and to the top and to the bottom. But there is a jump in cell dimensions downstream.

You might want to consider not using the LUST scheme for the convective term. Maybe try linear interpolation - I had better results with it.

How did you calculate the forces? I have not seen the functionObject for it in the controlDict file.

How long did you initiate your simulation, or did you average the forces from the beginning?

Have you checked the pressure distribution on the surface - where are we failing to calculate the correct pressure? Probably in the wake?

Have you checked if the RAS and LES regions for the turbulence model are correct?

Maybe try to use the Smagorinsky LES model and see the influence.

Best regards
Bazinga is offline   Reply With Quote

Old   December 22, 2016, 14:39
Default
  #6
Member
 
Ran
Join Date: Aug 2016
Posts: 32
Rep Power: 5
random_ran is on a distinguished road
Thanks for your suggestions.

1. I will resolve that jump transiation.

2. The convective term you refer to is div(phi, U), which one exactly? Gauss linear or Gauss limitedLinear 1?

3. The force is included in another file. Attached please find that file.

4. I start calculate the drag forces start from 6 seconds; the Cd pattern indicates the convergency.

5. I am downloading the file right now, and I will check the pressure distribution at wake region.

6. I am not clear with this suggestion. The turbulent model I choose is LES. Why I need to check RAS? Can you give me some guidences to check correction of turbulence model?

7. I will try different LES models to see the difference.

Thanks for your suggestion.

Bazinga,
forceCoeffsIncompressible.txt
random_ran is offline   Reply With Quote

Old   December 22, 2016, 15:26
Default
  #7
Senior Member
 
Join Date: Jun 2012
Location: Germany, Bochum
Posts: 220
Rep Power: 11
Bazinga is on a distinguished road
2. Gauss linear but maybe try the other one too.

3. Good.

4. Not sure but this might not be enough. In my experience (maybe other have better recommendations) 150 Tu for initialization and 400 Tu for averaging should be fine. Here Tu is T*U/D. T time, U velocity, D diameter.

6. You are using the SA DDES turbulence model which is a hybrid model that uses the RANS and LES approach.
One pure LES model is the Smagorinksy turbulence model. There should be a tutorial using it.

Is the value k according to the other experiments used for validation?

Good luck
Bazinga is offline   Reply With Quote

Old   December 22, 2016, 16:21
Default
  #8
Member
 
Join Date: Mar 2014
Posts: 53
Rep Power: 7
mzzmrt is on a distinguished road
I have not used the DDES model before but what if,

nut= 1.67e-05, nuTilda= 8.35e-05 and "nutLowReWallFunction" instead of "nutUSpaldingWallFunction" on the cylinder?

Regards,
mzzmrt is offline   Reply With Quote

Old   December 23, 2016, 04:10
Default
  #9
Senior Member
 
Join Date: Jun 2012
Location: Germany, Bochum
Posts: 220
Rep Power: 11
Bazinga is on a distinguished road
Spalding's law can also be used for very small y+ values. The lowRe Boundary conditions is used for y+ around 5 IIRC. I read it here somewhere on the board but never tried it myself.
Bazinga is offline   Reply With Quote

Old   December 23, 2016, 18:56
Default
  #10
Member
 
Ran
Join Date: Aug 2016
Posts: 32
Rep Power: 5
random_ran is on a distinguished road
Thanks Bazinga! Give me some time to figure it why. I will put the result here ASAP.
random_ran is offline   Reply With Quote

Old   December 23, 2016, 19:02
Default
  #11
Member
 
Ran
Join Date: Aug 2016
Posts: 32
Rep Power: 5
random_ran is on a distinguished road
Thanks for sharing your experience mzzmrt.

What is the difference between "nutLowReWallFunction" and "nutUSpaldingWallFunction" according to your experience?

Anyway, I will try it and see what is the result.
random_ran is offline   Reply With Quote

Old   December 24, 2016, 05:30
Default
  #12
Member
 
Join Date: Mar 2014
Posts: 53
Rep Power: 7
mzzmrt is on a distinguished road
After Bazinga's reply, I made a fast comparison with 3 (2D external, mildly separated flow) case files and SA turbulence model;

1. lowRE mesh on highRe flow (Re 1,6e06) with average yPlus=0,48 and max yPlus=1,55
2. lowRe mesh on lowRe flow (Re 3,5e05) with average yPlus=0,38 and max yPlus=2,11
3. lowRe mesh on lowRe flow (Re 1,0e05) with average yPlus=0,124 and max yPlus=0,79

Compared the two wall functions: nutLowReWallFunction and nutUSpaldingWallFunction for all cases.

As a result I have learned that Spalding's law works as expected and both wall conditions produced almost the same results for the forces and the convergence behaviour with these cases at least.

So, for the random_ran; forget about the wall function change. On the other hand intial nut and nuTilda boundary conditions have significant effects on the solution results...
mzzmrt is offline   Reply With Quote

Old   December 24, 2016, 06:09
Default
  #13
Senior Member
 
Join Date: Jun 2012
Location: Germany, Bochum
Posts: 220
Rep Power: 11
Bazinga is on a distinguished road
Really cool! Thanks for the update.
Bazinga is offline   Reply With Quote

Old   December 24, 2016, 22:13
Default
  #14
Member
 
Ran
Join Date: Aug 2016
Posts: 32
Rep Power: 5
random_ran is on a distinguished road
Thanks for your clarification. I am too eager to play with them. Please keep an eye on this thread. I will try my best.
random_ran is offline   Reply With Quote

Reply

Tags
re3900;drag;openfoam;

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
literature data for simulation coal combustion darookie CFX 1 April 29, 2014 09:50
Does using Parallel simulation improve Physics peter.pan Main CFD Forum 4 March 14, 2014 06:29
Boundary condition setting regarding turbine simulation using CFX Lacerlacer CFX 11 March 12, 2012 10:32
Improve Mesh quality - airfoil simulation Lukas84 STAR-CCM+ 4 July 6, 2010 11:07
Improve accuracy on air foil blade simulation? Bian CFX 4 December 12, 2006 12:29


All times are GMT -4. The time now is 00:16.