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

on unconvincing results for channel flow simulatio

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 19, 2001, 11:06
Default on unconvincing results for channel flow simulatio
  #1
yf yap
Guest
 
Posts: n/a
i am doing a simulation on steady, viscous, incompressible flow through a curved channel. the NS equations are parabolized. the solution is marched in the streamwise (from station n to n+1) direction using the ADI method. after imposing the required boundary conditions, and the solution for the n=2,3,4,.. plane are obtained. the boundary conditions are: 1) uniform inlet velocity (streamwise) 2) tranverse velocity =0 (inlet)(r and z, cylindrical coordinate system is used, n being the streamwise direction) 3) at the channel wall, u=v=w=0 (u in r direction, v in z direction and w in the streamwise direction,n) however, the results that i obtained is not convincing at all. for a given plane(n>=2), the streamwise velocity that i obtained for any grid point immediately adjacent to the wall is almost equal, and sometime, even larger than the inlet velocity, that is the streamwise velocity is impulsively increased form zero at the wall to almost equal to the inlet velocity, which is not true. below is one of the results that i obtained.(lower left corner of the channel) the streamwise inlet velocity=1.0

magnitude of the streamwise velocity 0 0.974201 0.975 0.975 0.975 0.975 0 0.974201 0.975 0.975 0.975 0.975 0 0.974201 0.975 0.975 0.975 0.975 0 0.974201 0.975 0.975 0.975 0.975 0 0.974201 0.975 0.975 0.975 0.975 0 0.974201 0.975 0.975 0.975 0.975 0 0.974201 0.975 0.975 0.975 0.975 0 0.974201 0.975 0.975 0.975 0.975 0 0.974201 0.975 0.975 0.975 0.975 0 0.973805 0.974599 0.974595 0.97459 0.974586 0 0 0 0 0 0

A z | +------->

r

Questions: 1)what would possibly cause this kind of results? 2)in discretizing the transformed NS(non-orthogonal boundary fitted coordinate, the velocities are not transformed into this coordinate), i just use taylor series approximation for all the derivatives(normal finite difference method), and i did not adopt a staggered grid system, can this be the problem? please advise. thanks.

  Reply With Quote

Old   January 19, 2001, 15:28
Default Re: on unconvincing results for channel flow simul
  #2
John C. Chien
Guest
 
Posts: n/a
(1). You need to state the Reynolds number of your problem. (2). What is your mesh distribution? (3). Try a fully-developed smooth inlet velocity distribution first. (or any smooth profile you like) (4). The uniform inlet velocity is always very tricky. There you have zero boundary layer thickness. (5). If you still have problem. Try a fully-developed 2-D channel flow.
  Reply With Quote

Old   January 20, 2001, 13:54
Default Re: on unconvincing results for channel flow simul
  #3
yf yap
Guest
 
Posts: n/a
thanks a lot for your kindness and willingness to spend you precious time helping me. the following result was obtained for Re=1000(characteristic length is based on hidraulic diameter of the channel). mesh size=0.04 (50x50) for a computational plane of 2 units x 2 units inlet velocity(streamwise)=1.0

magnitude of the streamwise velocity(lower left corner of the channel) 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720512 1.04102 1.10091 1.11213 1.11424 1.11464 1.11472 1.11473 0 0.720511 1.04102 1.10091 1.11213 1.11424 1.11464 1.11471 1.11473 0 0.720506 1.04101 1.1009 1.11212 1.11423 1.11463 1.11471 1.11472 0 0.720481 1.04098 1.10086 1.11208 1.11419 1.11459 1.11466 1.11468 0 0.720348 1.04078 1.10065 1.11187 1.11397 1.11437 1.11444 1.11445 0 0.719634 1.03974 1.09954 1.11073 1.11282 1.1132 1.11326 1.11326 0 0.715815 1.03417 1.0936 1.10468 1.10671 1.10704 1.10705 1.10699 0 0.695368 1.00447 1.06202 1.07262 1.07441 1.07456 1.0744 1.07417 0 0.585913 0.845959 0.894004 0.902493 0.90358 0.903278 0.902717 0.902107 0 0 0 0 0 0 0 0 0

A z | +------->

r

this result is for the second station (n=2). it is obvious that there is an impulsive increase in the streamwise velocity immediately adjacent to the channel wall. by right, it should possesses a semi-paraboloid profile. Questions: 1)as mentioned earlier, i did not adopt a staggered grid for a incompressible flow, can this be the main problem? 2)i have tried a fully-developed smooth inlet velocity distribution, as suggested, the same problem remains(an impulsive increase in the streamwise velocity immediately adjacent to the channel wall). with the same mesh size.

inlet streamwise velocity(lower left corner of the channel) 0.32 0.3592 0.3968 0.4328 0.4672 0.5 0.2952 0.3344 0.372 0.408 0.4424 0.4752 0.2688 0.308 0.3456 0.3816 0.416 0.4488 0.2408 0.28 0.3176 0.3536 0.388 0.4208 0.2112 0.2504 0.288 0.324 0.3584 0.3912 0.18 0.2192 0.2568 0.2928 0.3272 0.36 0.1472 0.1864 0.224 0.26 0.2944 0.3272 0.1128 0.152 0.1896 0.2256 0.26 0.2928 0.0768 0.116 0.1536 0.1896 0.224 0.2568 0.0392 0.0784 0.116 0.152 0.1864 0.2192

streamwise velocity(second station, n=2)(lower left corner of the channel) 0 0.241684 0.46766 0.57633 0.640955 0.688283 0 0.23484 0.456614 0.567086 0.633843 0.682756 0 0.229557 0.447118 0.559565 0.628581 0.679111 0 0.226088 0.439544 0.554231 0.625693 0.677895 0 0.223991 0.433379 0.550662 0.624875 0.678893 0 0.221079 0.425588 0.545652 0.623012 0.679153 0 0.2116 0.407318 0.528942 0.60936 0.667868 0 0.183983 0.35846 0.474999 0.555234 0.61454 0 0.119979 0.241377 0.330239 0.395187 0.444938 0 0 0 0 0 0

A z | +------->

r

3) can you suggest any method to deal with this problem, that's is capturing the entry flow properly instead of having these results? 4) since i use parabolized NS equations, as stated by John C. Tannehill, Dale A. Anderson and Richard H. Pletcher in "Computational Fluid Mechanics and Heat Transfer", pp. 559-562, the mesh size must be larger than a given value for sake of stability. for stability concern, the mesh size is much greater that what i used in obtaining the above results. That's why i can only obtain the solution for second station(n=2) for such fine mesh. (stability remains if delta >=.67)(30x30 grid points) so, can i still capture the entry flow properly with the given mesh size constraint? please advise. thanks.
  Reply With Quote

Old   January 20, 2001, 16:46
Default Re: on unconvincing results for channel flow simul
  #4
John C. Chien
Guest
 
Posts: n/a
(1). Reduce the mesh size in the marching direction. (2). Check the overall mass conservation. (3). If the overall mass is not conserved, then it is all right. (3). If the mass is not conserved, then you will have to check your program again. To reduce the wall effect or accuracy related to it, also reduce the mesh size to a much smaller value near the wall. Basically, with the uniform flow, there is a sort of singularity at the leading edge. (4). You will have to squeez 10~20 points into this initial boundary layer region. (5). Take a look at the book "Boundary Layer Theory" by Schlichting,there is a chapter on the exact solution of boundary layer equation, and especially, there is a velocity distribution for laminar flow in the inlet section of a channel. "ENLARGE THAT PICTURE AND STUDY THE VELOCITY PROFILES CAREFULLY FROM THE WALL TO THE CENTERLINE", even though it is a 2-D problem. (6). I would strongly suggest that you try this 2-D problem first (using symmetry condition in 3-D code), to see if you can duplicate the solution, if the probelm does not go away. good luck.
  Reply With Quote

Old   January 20, 2001, 16:49
Default Error: (3)if mass is conserved, it's all right.
  #5
John C. Chien
Guest
 
Posts: n/a
(3) should read "(3). If the overall mass is conserved, then it is all right. Sorry.
  Reply With Quote

Old   January 29, 2001, 23:30
Default Re: Error: (3)if mass is conserved, it's all right
  #6
yf yap
Guest
 
Posts: n/a
dear John, i would like to thank your for the advice. i re-checked the formulation, reynolds number and i tried to reduce the mesh size(2+ times smaller in the all the directions), and the velocity profile in the boundary is captured, as what you mentioned, it is confined to a very thin layer very near the boundary. regards, yfyap
  Reply With Quote

Old   January 30, 2001, 00:18
Default Re: Error: (3)if mass is conserved, it's all right
  #7
John C. Chien
Guest
 
Posts: n/a
(1). I am glad that you are making progress. (2). The important fact is that the mesh has to be consistent with the solution in the first place. (3). But you will probably ask, you need a mesh to obtain a solution. Without a mesh, there is no way to get a solution to evaluate the mesh. (4). This is the fundamental process in CFD. It is the process to obtain a mesh, a solution in a loop. (5). And the experience about the solution (test results or analytical solutions) all will aid you in reaching your goal.
  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
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 105 November 20, 2009 05:19
target flow rate: varying results Ryan FLUENT 3 January 9, 2008 14:54
Flow Over Airfoil With Simple Flap Results fez FLUENT 3 February 23, 2005 11:56
CFD Modeling of Two-phase Flow in Small Dia.Tubes Eric Poindexter Main CFD Forum 2 September 22, 2000 09:21
computation about flow around a yawed cone Tylor Xie Main CFD Forum 0 June 9, 1999 07:33


All times are GMT -4. The time now is 07:00.