
[Sponsors] 
Various questions and doubts about simulating Drag Coefficient of Cylinder 

LinkBack  Thread Tools  Display Modes 
September 9, 2016, 11:32 
Various questions and doubts about simulating Drag Coefficient of Cylinder

#1 
New Member
Join Date: Aug 2016
Posts: 9
Rep Power: 3 
Hello all,
I have been attempting to calculate Cd for a cylinder in sea water using a 2D case. Diameter = 5mI'm using SimpleFoam solver with Realisable ke as the turbulence model. In the documentation I am using for comparison/validation, the value of Cd listed for a smooth cylinder is 0.65 in steadystate flow situation. The value I calculated for Cd were 0.159 and 0.113 for time steps of 1e2 and 1e3, respectively. Both of which are far lower than they should be. My questions: 1. My mesh is limited to 100k nodes, is this too coarse to generate an accurate result? (see attached) 2. Why is the result seemingly independent of the fluid density? (it is never required as an input) 3. Why is there lift measured for the smaller of the two time steps? My requests: 1. General advice on calculation of drag coefficients for high Re 2. Any helpful advice would be greatly appreciated Attached are pictures of my mesh, and residuals & results for each run. mesh.PNG fcoeffs_biggerDELt_1e02.PNGfcoeffs_littlerDELt_1e03.PNG resids_biggerDELt_1e02.PNG resids_littlerDELt_1e03.PNG I hope someone can help  I feel like this is a simple problem but I am really struggling with it. Thank you very much! 

September 9, 2016, 11:38 

#2 
New Member
Join Date: Aug 2016
Posts: 9
Rep Power: 3 
For clarity, these were formed using SimFlow  a GUI for OpenFOAM. I hope this is an appropriate place to post this as there is currently no SimFlow specific sub.


September 9, 2016, 11:41 
Case Summary

#3 
New Member
Join Date: Aug 2016
Posts: 9
Rep Power: 3 
Here is the case summary:
case summary.JPG 

September 12, 2016, 08:01 
Aref // lref

#4 
New Member
Join Date: Aug 2016
Posts: 9
Rep Power: 3 
Bonus question (for extra points): What is the use of Aref/lref in 2D simulation?
I am at the end of my tether with this. Please demystify these issues and I will be eternally grateful. 

September 13, 2016, 05:07 

#5  
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,912
Blog Entries: 6
Rep Power: 32 
Hello Angus,
first of all, a very clear thread with a lot of information. I highly appreciate that. Based on the fact that I did similar simulations during my master, I think I can help you (but it is a few years ago). Quote:
Quote:
Quote:
Quote:
Quote:
Quote:
Did you ever check your simulation results? Like, how does the velocity and pressure field look like and change during the iterations. You have some jump in the residual plot. Do you know where this behavior come from? I would first check the simulation results in paraview to get an idea about the flow field (it should be smooth and should not jump during the iterations). If you have some jumps, it could be based on the setup you did (more than one solution allowed). In addition, at the end you have some unsteady behavior of your simulation. Maybe your mesh is too fine and you really resolve some vortexes but this can be analyzed by using paraview. One way would be, to reduce your relaxation factors to be more stable. Quote:
Quote:
I hope I could help you a bit. Good luck.
__________________
Keep foaming, Tobias Holzmann 

September 13, 2016, 05:49 

#6 
New Member
Join Date: Aug 2016
Posts: 9
Rep Power: 3 
Extremely helpful, thank you.
How can one measure a value for Δz in a 2D simulation? As I understand it, OpenFOAM doesn't truly model in 2D? Is Δz therefore the cell size in z direction? Secondly, I can't make sense of why Cd should be so dependent on Area? I understand that it is intrinsically connected to the Force but cannot seem get round this circular relationship. Linear relationship between value of Cd and variance in Area? Lastly, changing "lref" seems to have no effect on the solution at all? Sorry to be a burden, thanks for all the help so far. 

September 13, 2016, 06:35 

#7  
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,912
Blog Entries: 6
Rep Power: 32 
Quote:
Quote:
Code:
// lift, drag and moment coeffs[0] = (totForce & liftDir_)/(Aref_*pDyn); coeffs[1] = (totForce & dragDir_)/(Aref_*pDyn); coeffs[2] = (totMoment & pitchAxis_)/(Aref_*lRef_*pDyn); scalar Cl = sum(coeffs[0]); scalar Cd = sum(coeffs[1]); scalar Cm = sum(coeffs[2]); scalar Clf = Cl/2.0 + Cm; scalar Clr = Cl/2.0  Cm; This value will not change your drag and lift coefficient, it will only influence your moment (cm) as you can see in the C++ code above.
__________________
Keep foaming, Tobias Holzmann 

September 13, 2016, 07:10 

#8 
New Member
Join Date: Aug 2016
Posts: 9
Rep Power: 3 
Brilliant, thank you.
That is what I had initially thought, I think my confusion stemmed from a tutorial video produced by SimFlow themselves: https://www.youtube.com/watch?v=wASYUxQ9LMc at ~10:00 they set the values of lref and Aref. For the latter he sets it to be equal to dcyl^2 . Any idea why this may have been done? It is a similar case, in that it is 2D and of a cylinder in crossflow. All the best, Angus 

September 13, 2016, 11:40 
As it stands...

#9 
New Member
Join Date: Aug 2016
Posts: 9
Rep Power: 3 
Recap / Overview:
Attempting to calculate drag coefficients for a smooth cylinder in crossflow using 2D steady state, incompressible case. The expected value from literature (http://www.germanlloyd.org/pdf/DNVOSJ101_201405.pdf) is Cd = 0.65 for steady flow.Diameter = D = 5m Current state: After refining the mesh as much as possible within the 100k node limit and resetting the discussed parameters (Δt, lref, Aref, relaxation) the case converged in 5,118 iterations. The calculated value was found to be Cd = 2.66712 which is far larger than the expected. (Somewhat humorously, it is nearly equidistant from the expected solution as my initial calculation) Case Details: Mesh: See attached. Solver: SimpleFoam Turbulence Model: Realizable kε Model with full defaults on constants. Discretisation: Steadystate. Using LUST scheme for U, k and ε convection. Boundary Conditions: Inlet: Velocity inlet, of type "Surface Normal Fixed Value" (=U=1m/s) Initial Conditions: U=1m/s Monitor Reference Values: lref = D = 5 Questions: {{ Expected: Cd=0.65 // Calculated: Cd=2.66712 }}
Pictures: Mesh: Mesh_l8stgr8st.PNG Mesh_l8stgr8st_zoom.PNG Residuals & Case Summary: Residuals_l8stgr8st.PNG case summary_l8stgr8st.PNG Any guidance at this point (specific or otherwise) would be greatly appreciated. Kind regards, Angus 

September 13, 2016, 14:06 

#10 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,912
Blog Entries: 6
Rep Power: 32 
Hi,
my time is very limited but I uploaded my project work onto my web space (unfortunately it is in German). Nonetheless, maybe it will help you. You will find it here: http://www.holzmanncfd.de/index.php...karmanstrasse I am wondering why your projected area is equal to 5  and if you say it is the diameter, the unit would be [m] and not [mē]. I can not belive that you extrude the mesh in z  direction to 1m.
__________________
Keep foaming, Tobias Holzmann 

Tags 
drag coefficient, help needed 
Thread Tools  
Display Modes  

