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

Poiseuille!

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 23, 2000, 05:46
Default Poiseuille!
  #1
Luca
Guest
 
Posts: n/a
Hi everyone. I'm testing Fluent on the Poiseuille problem (long straight tube, Newtonian fluid, parabolic inlet velocity profile, zero pressure outlet) both with bricks and tetrahedral elements. I have been told that Fluent works fine with tetra elements, but when I check the pressure loss between the inlet and the outlet, with bricks I get a value that is close to the analitic solution even with coarse grids and a thin boundary layer, while with tetras I get a pressure loss that is near to double than the correct one, even with grids that are more than double finer that the one made of bricks. I'm trying to change convergence, solution methods, to change outlet pressure value, but with no result. I also tried to check the pressure loss between two internal surfaces, to avoid boundary effects, but I coulnd't find the correct values. Can anyone who knows give me a hint? Thanks a lot

Luca
  Reply With Quote

Old   November 23, 2000, 06:48
Default Re: Poiseuille!
  #2
Volker Pawlik
Guest
 
Posts: n/a
Did you use 2nd oder discretisation? And did you also resolve the boundary layer in the tetrahedral case?

Volker
  Reply With Quote

Old   November 23, 2000, 08:08
Default Re: Poiseuille!
  #3
Luca
Guest
 
Posts: n/a
Thanks a lot, I'm working on discretization order and boundary layer for tetrahedreal case, and also on upwinding scheme, and things are getting better, even if not yet precisely correct. I am looking forward to get the right numbers!
  Reply With Quote

Old   November 23, 2000, 13:18
Default Re: Poiseuille!
  #4
John C. Chien
Guest
 
Posts: n/a
(1). I am glad that someone is doing this test. (2). There is no question that the brick mesh is more accurate than the tet mesh. (3). If you Change the stream-wise mesh size distribution, you can observe the change in stream-wise wall skin friction distribution. Run a few meshes with different stream-wise mesh distributions, this will give you some ideas about the results. (4). I think, the readers here would be very interested in your results related to the mesh size, distributions, and the accuracy.
  Reply With Quote

Old   November 23, 2000, 19:53
Default Re: Poiseuille!
  #5
chris
Guest
 
Posts: n/a
It's also nice to check this simple case with the equations of momentum. You have the pressures, the velocities and all the forces at the tube. Are there differences between the different cell-types ?
  Reply With Quote

Old   November 24, 2000, 05:59
Default Re: Poiseuille!
  #6
Luca
Guest
 
Posts: n/a
I'm using a cilynder of L=10*D. Tetrahedral mesh size is dependent on how many nodes I use to discretize the two edges on the bases of the cilynder. So far I used three different interval counts, of 20, 35, 50. Boundary layer was set to have a first row of D/33 or D/50 (depends on the case), a growth factor of 1.25 and a number of rows so that the most interior element is nearly squared (e.g. 4 for the 50 case, and 6 for the 20 case). So far I have noticed that even with the finest mesh (base mesh interval count of 50, resulting in 41133 nodes), if I don't include a boundary layer the pressure drop is overestimated by a 25% in respect to the analytical results. With the 20 case, the error is only 2% with previously described boundary layer (resulting in 11320 nodes), while 40% without boundary layer (3313 nodes). (I realize that these results are messed up, but I'm going to put some order). All the simulations were performed with segregated approach, second order discretization and upwinding, and SIMPLE coupling algorithm. Parabolic velocity inlet profile and zero pressure outlet. My question is: how can I change stream-wise mesh distribution without changing the overall mesh distribution? The number of triangles on the wall is implicitly set with the discretization of the base edges. Thank you all for your attention!

Luca
  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
Validation of OpenFOAM for Poiseuille and Womersley Solution nobound OpenFOAM 1 September 12, 2011 09:53
Boundary condition and Poiseuille flow simulation Cyp OpenFOAM 6 March 11, 2011 15:53
Poiseuille boundary condition cosine CFX 2 May 18, 2010 07:47
Spectral methods need help - Poiseuille flow vetnav Main CFD Forum 0 February 5, 2010 14:51
Simple Poiseuille flow Maggie CFX 0 May 27, 2004 10:58


All times are GMT -4. The time now is 16:13.