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

Initial drag for cylinder in cross-flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 28, 2012, 15:26
Default Initial drag for cylinder in cross-flow
  #1
New Member
 
Orxan Shibliyev
Join Date: Aug 2011
Posts: 17
Rep Power: 5
orxan.shibli is on a distinguished road
Hi everyone!

I am simulating flow over cylinder at Re=100 with my own code. Setting time step to dt=1s, I monitor initial values of drag coef. and it solves it without problem. But when I set it to say dt=0.001 then initially drag coef. rises to very high values (hundreds) and then it becomes negative even. It is not important whether it will be better as time passes since I am also trying to understand why decreasing time step causes this kind of problem.

Other specifications:
  • Unsteady
  • Fully Implicit, 1st order Euler temporal discre.
  • 2nd order upwind spatial discre.
  • Max. Inner Iterations = 10
  • 2D, laminar
  • Initially velocity and pressure field is zero

Any idea?
orxan.shibli is offline   Reply With Quote

Old   May 28, 2012, 19:46
Default
  #2
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
You are starting the flow from a standstill, so that takes a big pressure drop to accomplish. That is one reason for the high drag. Also, you are only doing 10 inner iterations, which probably means it is not converging within each time step. In that case, the initial results don't mean much anyways.
cdegroot is offline   Reply With Quote

Old   May 29, 2012, 05:44
Default
  #3
New Member
 
Orxan Shibliyev
Join Date: Aug 2011
Posts: 17
Rep Power: 5
orxan.shibli is on a distinguished road
Dear Chris

OK but this should be true for both time steps. That is why I decreased time step however it became worse unexpectedly. Also I tried to make inner iterations 100 but that only caused to reach high values faster.

Last edited by orxan.shibli; June 3, 2012 at 17:45.
orxan.shibli is offline   Reply With Quote

Old   May 29, 2012, 10:06
Default
  #4
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
Well, your small timestep is 1000 times smaller than your large time step, so I would guess that the large time step just "steps over" a lot of the initial transient stuff.

Also, imagine in reality having completely still fluid and then instantly accelerating it to whatever value you have specified at the inlet. Not going to happen. It will take some (maybe small) amount of time to accelerate. In your simulation that time to accelerate is your first time step. Thus, I believe a smaller timestep will imply a larger initial pressure drop and also drag forces. In any case, these initial transients will die out eventually.
cdegroot is offline   Reply With Quote

Old   June 3, 2012, 17:43
Default
  #5
New Member
 
Orxan Shibliyev
Join Date: Aug 2011
Posts: 17
Rep Power: 5
orxan.shibli is on a distinguished road
I found the problem. It was due to time-step dependency of original Rhie and Chow MIM. Hence, it is better to use modified version:

"Discussion on Momentum Interpolation Method for Collocated Grids of Incompressible Flow", Yu et al.
orxan.shibli is offline   Reply With Quote

Old   June 4, 2012, 01:10
Default
  #6
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
Quote:
Originally Posted by orxan.shibli View Post
I found the problem. It was due to time-step dependency of original Rhie and Chow MIM. Hence, it is better to use modified version:

"Discussion on Momentum Interpolation Method for Collocated Grids of Incompressible Flow", Yu et al.
Very interesting. Thanks for sharing.
cdegroot is offline   Reply With Quote

Reply

Tags
cross, cylinder, drag, flow

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
Interfoam blows on parallel run danvica OpenFOAM Running, Solving & CFD 16 December 22, 2012 03:09
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM 6 April 12, 2011 11:24
Negative value of k causing simulation to stop velan OpenFOAM Running, Solving & CFD 1 October 17, 2008 05:36
Unknown error sivakumar OpenFOAM Pre-Processing 9 September 9, 2008 12:53
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 17:57.