CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Main CFD Forum (https://www.cfd-online.com/Forums/main/)
-   -   on unconvincing results for channel flow simulatio (https://www.cfd-online.com/Forums/main/3033-unconvincing-results-channel-flow-simulatio.html)

yf yap January 19, 2001 11:06

on unconvincing results for channel flow simulatio
 
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.


John C. Chien January 19, 2001 15:28

Re: on unconvincing results for channel flow simul
 
(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.

yf yap January 20, 2001 13:54

Re: on unconvincing results for channel flow simul
 
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.

John C. Chien January 20, 2001 16:46

Re: on unconvincing results for channel flow simul
 
(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.

John C. Chien January 20, 2001 16:49

Error: (3)if mass is conserved, it's all right.
 
(3) should read "(3). If the overall mass is conserved, then it is all right. Sorry.

yf yap January 29, 2001 23:30

Re: Error: (3)if mass is conserved, it's all right
 
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

John C. Chien January 30, 2001 00:18

Re: Error: (3)if mass is conserved, it's all right
 
(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.


All times are GMT -4. The time now is 10:00.