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

Lack of Recirculation for Lid Driven Cavity Flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 17, 2011, 19:30
Default Lack of Recirculation for Lid Driven Cavity Flow
  #1
klw
New Member
 
Kristina
Join Date: May 2011
Location: Seattle, WA
Posts: 7
Rep Power: 6
klw is on a distinguished road
Hi there,

I've been working on a Lid-Driven Cavity flow code in Fortran, and the results I'm getting have me stumped. I would greatly appreciate any help!

I'm using a staggered mesh on the Projection Method, with a CFL of 1.0, Re = 100, and grid of 100x100. I'm getting no recirculation in the lower corners, and the streamlines seem to be "squished" in the y-direction. I don't know if this is characteristic of having bad boundary conditions, a bad algorithm, or not running to the correct timestep.

Boundary conditions implemented are u = 0, v = 0 for all four sides (u = 1.0 for the top wall), and dp/dx = 0 for the side walls and dp/dy = 0 for the top and bottom walls, with p = 0 pinned in the center of the top boundary.

I've attached a picture of my x-velocity (u) with streamlines to show what I'm talking about.

Thank you!

-K
Attached Images
File Type: jpg Screen shot 2011-05-17 at 4.28.32 PM.jpg (72.3 KB, 44 views)
klw is offline   Reply With Quote

Old   May 18, 2011, 17:23
Default
  #2
New Member
 
lemee.thomas@gmail.com
Join Date: Apr 2011
Posts: 9
Rep Power: 6
Thomas_L is on a distinguished road
Hello,

It seems you have a perfect Stockes Flow without convection. (v.grad(v))
What is your criteria for stopping your calculation? How long do you run your code?


About the no recirculation in the corner, I can notice you use Tecplot, isn't it?
So you use the streamtraces tool. How did you use it?
Because if you use the icon "Add a single or a rake of streamtraces" in the bottom corner, the recirculation will appear.

Thomas
Thomas_L is offline   Reply With Quote

Old   May 18, 2011, 17:40
Default
  #3
klw
New Member
 
Kristina
Join Date: May 2011
Location: Seattle, WA
Posts: 7
Rep Power: 6
klw is on a distinguished road
Hi Thomas,

Thanks for your reply! Yes, I am using TecPlot...I'm very new to it, so I'm still figuring out how to use its features. I just clicked "streamtraces" to add, and drew a line covering the whole plot (it seemed to me that the line dictated where you wanted streamlines to appear, but I could be very wrong). My criteria for stopping the flow is when my residual < 1E-4, where my residual is:

R = max(|u^{n+1}-u^{n}|, |v^{n+1}-v^{n}|)

For my non-dimensionalized time, it's running to t = .225, with a CFL of 1.0, Re = 100, lid velocity U = 1, and box with side dimensions L = 1, and a 150x150 grid.

-K
klw is offline   Reply With Quote

Old   May 19, 2011, 10:03
Default
  #4
Senior Member
 
Andrew
Join Date: Mar 2009
Location: Washington, DC
Posts: 194
Rep Power: 8
mettler is on a distinguished road
have you tried jumping your mesh size up?..or increasing the Re?
mettler is offline   Reply With Quote

Old   May 19, 2011, 10:55
Default
  #5
klw
New Member
 
Kristina
Join Date: May 2011
Location: Seattle, WA
Posts: 7
Rep Power: 6
klw is on a distinguished road
I've tried jumping the mesh up, but I've seen examples with meshes more coarse than 150x150. I also wanted to match Re to the cases I've seen, so I kept it at 100...however, I have tried to jump Re up, and it doesn't look much different.
klw is offline   Reply With Quote

Old   May 19, 2011, 11:12
Default
  #6
Senior Member
 
Andrew
Join Date: Mar 2009
Location: Washington, DC
Posts: 194
Rep Power: 8
mettler is on a distinguished road
I got mine to work using the steam function-vorticity. What are your boundary conditions for the corners? One thing I forgot, if I remember correctly (I did this a while ago) was the negative when computing the velocities from the stream function. Another thing you can try is make more stream lines (more dense)..i.e. have a stream line for every .01 change, so you get a whole bunch of them. I am not sure how you do that in your program.
mettler is offline   Reply With Quote

Old   May 20, 2011, 03:34
Default
  #7
klw
New Member
 
Kristina
Join Date: May 2011
Location: Seattle, WA
Posts: 7
Rep Power: 6
klw is on a distinguished road
So after some investigation, it appears as if my method for checking tolerance is insufficient. I forced the algorithm to run for 10x more time steps (despite having no changes in the residuals), and the solution continues to develop! Very odd. Thank you to those who replied with help!
klw is offline   Reply With Quote

Old   May 20, 2011, 17:43
Default
  #8
Member
 
vicarious's Avatar
 
Pedram Mojtabavi
Join Date: Apr 2011
Location: Iran
Posts: 66
Rep Power: 6
vicarious is on a distinguished road
Send a message via Yahoo to vicarious
hello,

As one of the guys mentioned try to add more streamline in TECPLOT because at small Re the vortices are tiny.
Also try to increase your mesh up to 250*250 to capture all vortices. I had the same problem with my code which I used vorticity-stream function and at Re=10 & Re=100 there were no vortices at corners while at Re=1000 they were clearly captured.if you simulate caivty in FLUENT you see the vortices in corners at Re=100 are too small if you even use SIMPLEC!

Vicarious
vicarious is offline   Reply With Quote

Old   May 21, 2011, 04:57
Default
  #9
New Member
 
Pål Grøthe Sandnes
Join Date: Oct 2010
Posts: 12
Rep Power: 6
palgroth is on a distinguished road
I had the exact same problem a couple of weeks ago. As you, I used projection method. In my case, the problem was related to the advectivce term. First, the advective term was expressed strictly conservative.

d/dx_j (u_i*u_j)

For some reason, I ended up with something similar to your result. Then I changed the expression to a less conservative one, and everything worked just fine.

u_j d/dx_j (u_i)

Pål
palgroth is offline   Reply With Quote

Reply

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
Urgent: Unsteady 3-D supersonic cavity flow Min-Sung Kang FLUENT 3 April 6, 2014 09:50
Supersonic Flow over a Cavity (coodles): Maximum Iterations Exceeded sushant OpenFOAM Running, Solving & CFD 0 April 9, 2009 02:52
lid driven cavity ani Main CFD Forum 3 April 2, 2006 13:27
The 2-D Driven Cavity Problem debiao Main CFD Forum 2 January 11, 2006 14:14
boundary condition of wall driven cavity flow ramin shams Main CFD Forum 2 June 2, 2004 04:01


All times are GMT -4. The time now is 04:30.