# Why strouhal number decreases as time step decrease?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 September 20, 2016, 17:03 Why strouhal number decreases as time step decrease? #1 New Member   Ran Join Date: Aug 2016 Posts: 11 Rep Power: 2 Hi CFDers: I am doing simulation of flow over a cylinder. Reynolds number is 100 in my case. Following is the descrition of my simulation: a. computation domain diameter of cylinder: d = 0.0889 m. 2016-09-04_140735.jpg b. mesh detail: (Grid 1) Over sizing: Max face size 0.015m First layer thickness 2.2225e-3 m Inflation layer around cylinder: 40 Growth rate: 2.5 b'. mesh detail: (Grid 2) First layer thickness: 0.001 m (Grid 1 is 0.002 m) number of inflation layers: 80 (Grid 1 is 40) Over sizing of max face size: 0.075 m (Grid 1 is 0.015 m) Mesh.jpg c. solver : pressure base, transient d. material: air density 1.225 kg/m3, viscosity 1.7894 kg/m-s e. model: laminar f. boundary condition: cylinder: no slip wall: specified shear(X-Component 0, Y-Component 0) inlet: velocity 0.01643 m/s g. reference value Area: 0.0889 m2 h. solution method: Pressure-velocity coupling: SIMPLE scheme Spatial Discretization: Gradient: least squares cell based Pressure: Second order Momentum: Second order Upwind Transient Formulation Second order Implicit i. solution Initialization: Hyper Initialization Result: 0.05.jpg Following is the summary of my result: Capture1.JPG Capture2.JPG My question is why strouhal number decreases as I decrease time step and why drag is bigger than experimental data? Can someone gives me some suggestions what I can do to improve my simulation? Thank you, Ran

 September 21, 2016, 07:11 #2 Member   Join Date: May 2014 Posts: 30 Rep Power: 4 Interesting, I don't really know tbh. My only thought was that you have too high CD and too low St, so maybe overly dissipative numerical viscosity causes that, hence it could be a mesh-thing and give feedback on time-step sensitivity.. But then again, your CD vaule doesn't change from grid1 to grid2, neither does the separation point, and your schemes are 2nd order... Sorry that I can't help really just thought it may give you ideas if I comment anyway. would like to know the solution, good luck

 September 21, 2016, 09:33 #3 New Member   Ran Join Date: Aug 2016 Posts: 11 Rep Power: 2 Hi mome: Thanks for your reply. My intuition is the mesh. I will definitely try to use some other types of mesh to compare the result. I have also try time step 0.001s and Fluent gave me useless result (Cd=10+), my convergence criteria is 10e-3. Is this a potential problem? Ran

October 10, 2016, 10:28
#4
New Member

Ran
Join Date: Aug 2016
Posts: 11
Rep Power: 2
Quote:
 Originally Posted by mome Interesting, I don't really know tbh. My only thought was that you have too high CD and too low St, so maybe overly dissipative numerical viscosity causes that, hence it could be a mesh-thing and give feedback on time-step sensitivity.. But then again, your CD vaule doesn't change from grid1 to grid2, neither does the separation point, and your schemes are 2nd order... Sorry that I can't help really just thought it may give you ideas if I comment anyway. would like to know the solution, good luck

Problem solved!

I changed residual to 10-6, then shedding frequency mathces with literatural very well. It showed that this number is extremely sensitivity to residual.

October 11, 2016, 15:30
#5
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,571
Rep Power: 22
Quote:
 Originally Posted by random_ran Problem solved! I changed residual to 10-6, then shedding frequency mathces with literatural very well. It showed that this number is extremely sensitivity to residual.
This is just my rant but this is why you should not rely on residuals, because residuals are not convergence monitors. You need to be monitoring solution values to establish whether you have achieved inter-timestep convergence. It is a big problem and many editorials have been written on it. Patrick Roache devoted a section in his book to bash residuals. Too many people have been fooled into thinking their simulation has converged by setting convergence monitors based on residuals that are too lax. More strict residual criteria certainly does help (because it generally results in more iterations per time-step) but that is not an excuse to not check to make sure your solution is correct! The onus of proof is on the author.

 Tags flow over a cylinder, fluent 16.0, re=100

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post almir OpenFOAM Running, Solving & CFD 69 January 20, 2017 08:28 gooya_kabir OpenFOAM Running, Solving & CFD 2 November 2, 2013 14:58 sharonyue OpenFOAM Running, Solving & CFD 6 June 10, 2013 09:34 sharonyue OpenFOAM Running, Solving & CFD 13 January 2, 2013 23:40 liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07

All times are GMT -4. The time now is 16:39.

 Contact Us - CFD Online - Top