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

Why strouhal number decreases as time step decrease?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 20, 2016, 17:03
Default Why strouhal number decreases as time step decrease?
  #1
New Member
 
Ran
Join Date: Aug 2016
Posts: 11
Rep Power: 2
random_ran is on a distinguished road
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
random_ran is online now   Reply With Quote

Old   September 21, 2016, 07:11
Default
  #2
Member
 
Join Date: May 2014
Posts: 30
Rep Power: 4
mome is on a distinguished road
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
mome is offline   Reply With Quote

Old   September 21, 2016, 09:33
Default
  #3
New Member
 
Ran
Join Date: Aug 2016
Posts: 11
Rep Power: 2
random_ran is on a distinguished road
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
random_ran is online now   Reply With Quote

Old   October 10, 2016, 10:28
Default
  #4
New Member
 
Ran
Join Date: Aug 2016
Posts: 11
Rep Power: 2
random_ran is on a distinguished road
Quote:
Originally Posted by mome View Post
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.
random_ran is online now   Reply With Quote

Old   October 11, 2016, 15:30
Default
  #5
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,571
Rep Power: 22
LuckyTran will become famous soon enough
Quote:
Originally Posted by random_ran View Post
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.
LuckyTran is online now   Reply With Quote

Reply

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

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Foam::error::PrintStack almir OpenFOAM Running, Solving & CFD 69 January 20, 2017 08:28
Micro Scale Pore, icoFoam gooya_kabir OpenFOAM Running, Solving & CFD 2 November 2, 2013 14:58
mixerVesselAMI2D's mass is not balancing sharonyue OpenFOAM Running, Solving & CFD 6 June 10, 2013 09:34
same geometry,structured and unstructured mesh,different behaviour. sharonyue OpenFOAM Running, Solving & CFD 13 January 2, 2013 23:40
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07


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