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

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

 December 20, 2016, 20:37 Cd not matches with literature-How to improve simulation-frustrated-OF-user #1 Member   Ran Join Date: Aug 2016 Posts: 32 Rep Power: 5 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.

 December 20, 2016, 20:40 #2 Member   Ran Join Date: Aug 2016 Posts: 32 Rep Power: 5

 December 20, 2016, 20:41 #3 Member   Ran Join Date: Aug 2016 Posts: 32 Rep Power: 5

 December 21, 2016, 22:24 #4 Member   Ran Join Date: Aug 2016 Posts: 32 Rep Power: 5 Anyone? No suggestions? also the comment "stupid questions cannot expect great answer" would be useful !

 December 22, 2016, 05:19 #5 Senior Member   Join Date: Jun 2012 Location: Germany, Bochum Posts: 220 Rep Power: 11 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

 December 22, 2016, 14:39 #6 Member   Ran Join Date: Aug 2016 Posts: 32 Rep Power: 5 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

 December 22, 2016, 15:26 #7 Senior Member   Join Date: Jun 2012 Location: Germany, Bochum Posts: 220 Rep Power: 11 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

 December 22, 2016, 16:21 #8 Member   Join Date: Mar 2014 Posts: 53 Rep Power: 7 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,

 December 23, 2016, 04:10 #9 Senior Member   Join Date: Jun 2012 Location: Germany, Bochum Posts: 220 Rep Power: 11 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.

 December 23, 2016, 18:56 #10 Member   Ran Join Date: Aug 2016 Posts: 32 Rep Power: 5 Thanks Bazinga! Give me some time to figure it why. I will put the result here ASAP.

 December 23, 2016, 19:02 #11 Member   Ran Join Date: Aug 2016 Posts: 32 Rep Power: 5 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.

 December 24, 2016, 05:30 #12 Member   Join Date: Mar 2014 Posts: 53 Rep Power: 7 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...

 December 24, 2016, 06:09 #13 Senior Member   Join Date: Jun 2012 Location: Germany, Bochum Posts: 220 Rep Power: 11 Really cool! Thanks for the update.

 December 24, 2016, 22:13 #14 Member   Ran Join Date: Aug 2016 Posts: 32 Rep Power: 5 Thanks for your clarification. I am too eager to play with them. Please keep an eye on this thread. I will try my best.

 Tags re3900;drag;openfoam;