
[Sponsors] 
Cfd simulation on a smooth cylinder (drag coefficient) 

LinkBack  Thread Tools  Search this Thread  Display Modes 
October 12, 2016, 21:03 
Cfd simulation on a smooth cylinder (drag coefficient)

#1 
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Hi to everyone!
Now I will explain my problem: Software: STARCM+ Goal: find the right value of drag coefficient on my cilinder Details: u=45.9 m/s, D=1 m, Re=2.9*10^6  2D Domain: 10D over the cylinder, 10D belowe the cylinder, 10D at the left of the cylinder, 20D to the right od the cylinder Boundary conditions: top and bottom planes are symmetry planes, the right plane is pressure outlet, the left plane is velocity inlet I can't find the right value of the drag coefficient on my cylinder!! I am getting crazy since the beginning of Semptember! I have tried both (steady) kepsilon and komega model, but nothing, I have always oscillations (small or large) on the drag coefficients, around 0.4 (that is the right value if I would have a Reynolds of 1*10^6), but I need a value around 0.7 , 0.8 ... Can anyone help me, please?! 

October 13, 2016, 02:52 

#2 
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46 
Oscillations in a steadystate solution can be a sign that the flow has an unsteadiness that can not be captured correctly by the steadystate approach. In this case this is definitely true.
Consequently, at least an unsteady RANS approach would be necessary to get a converged solution. But even then you will not get the correct value for the drag coefficient without tweaking the turbulence model. The correct approach here is a LES. 

October 13, 2016, 03:43 

#3 
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Thank you for your answer!
After having seen a lot of scientific articles, I know for sure that the only good available methods are the URANS and the LES.. And I need to make a comparison between these two method for my master thesis.. I know that by the Strohual number I am able to decide the suitable timestep for my unsteady simulations, so right now I am performing my first unsteady simulation.. do you know how much I have to wai until I get my statistically steady result? Do you have any suggestion to make some improvements on my simulation? I have already a very fine mesh: 20 prism layers, 1E6 first prism layer to the wall, 0.01 m total thickness prism layer, a wally+ between 0.01 and 0.22, a mesh refinement around the cylinder and on its wake. Maybe something on the initial condition? I don't know, I am desperate.. Thank you very much for your patience! 

October 13, 2016, 05:20 

#4 
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46 
Let me throw in a few thoughts:
Last edited by flotus1; October 13, 2016 at 09:12. 

October 13, 2016, 10:31 

#5 
Senior Member
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17 
Are you using the force coefficient report to get cd?


October 13, 2016, 11:14 

#6 
Super Moderator

Check these videos. May be useful to you... I will discuss more in detail after you watch these videos...
https://www.youtube.com/watch?v=anTkWfMyEPM https://www.youtube.com/watch?v=TFQ_0HaBXXM 

October 13, 2016, 12:13 

#7  
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Quote:
Here I atached some pictures of my general mesh, then the detail about the cylinder and the result about the drag coefficient (it is about 0.38.. and I would need a greater value!) I have used kepsilon method, with implicit unsteady of 2nd order in time, and a timestep of 0.001 s. I think that I have kept a low volume jump in the transition regionbetween the layers and the general mesh, as you can see.. I wait for your answer, thank you very much again! 

October 13, 2016, 12:15 

#8  
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Quote:
As soon as I can, I will see these videos! 

October 13, 2016, 12:19 

#9 
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Yes, why?
Here I atached some pictures of my general mesh, then the detail about the cylinder and the result about the drag coefficient (it is about 0.38.. and I would need a greater value!) I have used kepsilon method, with implicit unsteady of 2nd order in time, and a timestep of 0.001 s. I think that I have kept a low volume jump in the transition regionbetween the layers and the general mesh, as you can see.. After having seen a lot of scientific articles, I know for sure that the only good available methods are the URANS and the LES.. And I need to make a comparison between these two method for my master thesis.. I know that by the Strohual number I am able to decide the suitable timestep for my unsteady simulations, so right now I am performing my first unsteady simulation.. do you know how much I have to wai until I get my statistically steady result? Do you have any suggestion to make some improvements on my simulation? I have already a very fine mesh: 20 prism layers, 1E6 first prism layer to the wall, 0.01 m total thickness prism layer, a wally+ between 0.01 and 0.22, a mesh refinement around the cylinder and on its wake. Maybe something on the initial condition? I don't know, I am desperate.. Thank you very much for your patience! 

October 13, 2016, 12:30 

#10 
Senior Member
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17 
I have run into issues with this before. There is a bug, or as CDAdapco would call it a philosophical difference that they won't resolve, related to how the issue of unit depth is handled. The coefficient report is a 3D tool. For 2D analysis it assumes you have a depth of 1 m regardless of unit system so the reference area you input needs to reflect this to get the 'correct' coefficient back out of it.
Now that being said, it sounds like you are already in SI units so this may not be the issue you are experiencing. However, given that this bug exists I always shy away from using the coefficient reports and extract force data directly to calculate my own coefficients. It is easier to track down why a coefficient is wrong if you can look and/or control all of the inputs directly. Try calculating Cd yourself from the drag force and see what you get. There is a good chance you will get a different and possibly better answer. 

October 13, 2016, 12:40 

#11 
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Yes, I know what you are talking about and I have tried few days ago to calculate the drag coefficient like you said, but I've obtained the same result..


October 13, 2016, 15:20 

#12  
Super Moderator

Quote:
what reference values you are using for the Cd? how did you decide this time step? in how many time steps you are resolving one vortex shedding frequency?? keep Yplus at 0.50.8... 

October 13, 2016, 16:21 

#13  
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Quote:
Since the Strohual number should be around 0.25, reexpressing the formula I obtain the inverse of the frequency, that is the period one vortex, and that will be the maximum timestep! However, I resolve in 20, 30 times one vortex shedding.. I will stop the simulation when the solution become statistically steady.. Honestly, I have the y+ quite low (<0.2).. 

October 13, 2016, 17:05 

#14  
Super Moderator

Quote:
Quote:


October 13, 2016, 17:23 

#15 
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 

October 13, 2016, 18:42 

#16  
Super Moderator

Quote:
Quote:
Quote:
Let say for each cycle, you have 20 time steps. so for 5 cycles it is 100 time steps and 100 values for Cd. Just sum all values of Cd and divide sum by 100. that is your time mean drag. For Cl, practice is different. Normally people quote the root mean square value, because simple mean will give you zero Cl for symmetric bodies such as cylinder. 

October 13, 2016, 20:56 

#17  
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Quote:
However, I will try to apply your advices and I will let you know 

October 14, 2016, 04:16 

#18 
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46 
The residuals are too high? This means that the results we are discussing here are not converged? Run more iterations per time step.
You should also have a look at these resources: http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F http://www.cfdonline.com/Forums/flu...nvergence.html 

October 14, 2016, 05:25 

#19 
Super Moderator

or alternatively reduce the time step by order of magnitude (means divide your current time step by 10, two orders means divide by 100 and so on...)
Example : current time step Delta T = 0.05 order of magnitude reduction = 0.05 / 10 = 0.005 Two orders of magnitude reduction = 0.05 / 100 = 0.0005 

October 14, 2016, 19:14 

#20  
New Member
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9 
Quote:
Now I have almost finished my timestep independence study and the residuals are periodically converged, and the same for my drag coefficient.. what I'm worried about is the fact that, smaller the timestep is, smaller the drag coefficient.. I know that I have to do the space gridindepence study yet, but it is not so comforting.. I would desire my drag coefficient to grow up towards the right value.. XD 

Tags 
cfd, cylinder, drag coefficient 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Flow past a 2D cylinder  High Re (1E+05)  Cd too high  Pervispasco  OpenFOAM Running, Solving & CFD  4  March 14, 2022 03:19 
Flow past a cylinder at Re 1e05 using LES, drag force coefficient is to low  Scabbard  Main CFD Forum  21  June 19, 2018 14:58 
2D cylinder drag coefficient  miku11  OpenFOAM Running, Solving & CFD  0  June 28, 2016 08:36 
Pump's Torque in CFD simulation is higher than experience.  ngoc_tran_bao  CFX  6  June 7, 2016 00:00 
Forces Acting on a Rotating Cylinder (Moving Mesh)  dreamchaser  CFX  5  April 25, 2015 07:01 