I'm attempting to validate simulations of a swirling air flow in a straight pipe, because I'm going to study the swirling flow in a engine cylinder. I've an experimental set of data that I obtained using a straight plexiglass pipe (diameter 94[mm], lenght 2[m])with a simple inlet geometry (a tangential, straight rectangular pipe - 20[mm]X 40[mm]). massflow was measured by means of a von karman vortex transducer, and swirl intensity was obtained by means of a paddle-wheel swirl meter. I'm using a thetraedral, unstructured mesh (220,000 cells), pressure B.C at inlet, pressure B.C. at outlet. My simulations are running on a parallel 2-processors system winNt-based.

1) using the k-e model I obtained a tangential velocity profile that is underestimated (40% less than expected - 50<Y+<500 near the walls); 2) using the RNG model (swirl-dominated flow) and the standard walls treatment I have severe convergence problems. the central core is charactherized by a couter-rotating, reversed swirl flow.

Has anyone any idea to address this problem? Thanks in advance

1) It is well known in the literature that the ke model does not have the capability to deal with swirling flows. Using this model you will not obtain the correct velocity profile.

I would suggest to you to change to the RSM model which should work a lot better.

2) What discretization are you using? This also has a large impact on the accuarcy of your results. I would suggest to you to use Second Order Upwind for all variables. SIMPLE for pressure-velocity coupling.

Hope this helps

dear Tom sorry, but my original message was truncated (maybe it was too long)! I've already tried to obtaing the convergence starting from a k-e model then switching to RMS model and 2nd order discretization for all variables, but I couldn't address convergence problems and velocity profile underestimation (about 40%). Now I'm trying to obtain better results using an hexaedral mesh (280.000 cells, walls BL), but the results don't seems to be satisfactory. Thanks again, Ugo

Ugo, what URFs are you using? Changing these could help your convergence problems.

Hi, Johnny B, what is the mean of URF?

Dear Ugo, I am also working on the same kind of problem (Swirling flow simulations) in curved tubes, for that i am using Second order upwind scheme and the URF which i am using for my solution are

pressure is 0.3; velocity is 0.5; body force is 0.8.

u just try with this parameters i think your results will converge, cause my results are coming and matched with the experimental results.

Hi, Johnny; I tried to increase pressure URF (from 0.3 to 0.5) and decrease momentum URF (to approx 0.6), and the simulation converged. The result are still unsatisfying., because velocyty profile is underestimated compared to experimental data.

The URFs are the Under Relaxation Factors, and they have a strong influence on the convergence of a simulation. You can find a lot of information about URFs in your User Manual. Bye

Dear Vimal, Thanks for your suggestion. I obtained a convergent solution with a RNS simulation with standard URFs and first-order discretization scheme, but velocity profile doesn't match the experimental data (simulated swirl ratio is 40% less than the measured one...) I will try to change the discretization method and I will use your URFs. bye P.S.: how about the wall treatment? I'm using standard wall functions, and my mesh have no BL cells

Thanks, Ugo. These days I am adjusting the URFs to make my simulation convergence. And I find that only making all the URFs to be 0.1 can make my simu.convergence(that the residuals are under the limit).But there still some(about 15000) cell's turbulence viscosity ratio go beyond the limit of 10^5 and some reverse flow exist,and the velocity and pressure field are both weird and the absolute pressure is far less than 0. What i am simulating is a incompressible flow, and there is three pressure inlets, one velocity inlet and one pressure outlet. the discretization for pressure is body force weighted, and piso for v-o coupling.as to the others I use first windup. would you so kind enough to tell me what leads to the abnormities in my simulation? Thanks in advance

Hi richard; I'm trying to guess what is going wrong with your simulations; first of all I would like to know what kind of mesh are you using (tet, hex...) and if it is coarse or fine (n° of cells); furthermore you should check y+ values near walls, and adjust mesh size in conformity with the BL threatment you choose (for standard BL you should have 30<y+<200). bye

(for standard BL you should have 30<y+<300) hope this helps bye

Hi Ugo, Thanks a lot.About my simulation, I use the hex mesh, and Fluent saids this:

Domain Extents:

x-coordinate: min (m) = 0.000000e+00, max (m) = 3.511800e+02

y-coordinate: min (m) = -8.399000e+01, max (m) = 1.350000e+01

z-coordinate: min (m) = -2.000000e+00, max (m) = 6.500000e+00 Volume statistics:

minimum volume (m3): 9.983918e-07

maximum volume (m3): 1.998029e+00

total volume (m3): 3.087065e+04 Face area statistics:

minimum face area (m2): 9.981380e-05

maximum face area (m2): 2.058751e+00 Checking number of nodes per cell. Checking number of faces per cell. Checking thread pointers. Checking number of cells per face. Checking face cells. Checking bridge faces. Checking right-handed cells. Checking face handedness. Checking element type consistency. Checking boundary types: Checking face pairs. Checking periodic boundaries. Checking node count. Checking nosolve cell count. Checking nosolve face count. Checking face children. Checking cell children. Checking storage. Done.

and i don't know if it is fine or coarse,is there any criteria for this ? as to Y* and Y+, I have checked them and Y+ is between 30 and 300, fitting the condition of using standard wall function. and what's your means of BL treatment? is that the wall function?

Dear richard, The info you sent me are relative to mesh cheking, and they are not useful to determine if the grid is fine or coarse. A good way to do that is to perform a "first guess", using a robust viscous, BL law & discretization choice -for example: k-e + standard BL law + I order discretization-, then to check if an adaption of the grid is necessary. To do that you should apply the "10% rule" to gradient adaption: compute max&min values of (for example) pressure gradient, then set your coarsening Threshold to 110% of min value, and refinement Threshold to 10% of max value. try and let me know!! bye

Can you please explain this 10% rule to me please.

BOB

Hi Bob; The "10% rule" is just a practical method: it's not an hard or straight foward rule for gradient-based adapting, but it gives you a good first-guess principle. For example, if you have min. PressureGradient=0.1 and max. PressureGradient=5, you should set refinement threshold to 0.5 and coarsening threshold to 0.11 (see previous post for details). Hope this helps, bye

i would like to suggest u

1. make the grid independency study 2. when u r using the rsm , ur near wall mesh should be be very fine 3. use k-epsilon with rng and enable swirl dominate flow and also switch on the non-equilibruim wall funtins

hope this will work

[dporfirev]

Hi everyone
I have same problem. I'm attempting to simulate a swirling compressible air flow in a pipe (diameter 39mm, lenght 60mm) with a combination of tangential inlet (4 square pipes, 10mm) and axial inlet (circular hole in the pipe end, diameter 12mm). I'm using a thetraedral, unstructured mesh (~2.700.000 cells), pressure BC at inlet, pressure BC at outlet.
I've used various turbulence models and a laminar model. In all cases I've obtained a wrong profile for tangential velocity. It has been significantly underestimated.
I've used as 1st and 2nd order discretization for all variables and I haven't had problems with convergence.
Hope for your help.

[Trev]

Basically a quick run through of what you need is if you haven't already got it setup is:

RSM turbulence model (Quadratic pressure strain if you can get convergence with it although depending on gradients in the flow the linear pressure strain model should be fine)
PRESTO pressure discretisation
QUICK discretisation for momentum
Either 2nd order/Quick for the rest.

Also I would use a 2nd order scheme for the time step.

Although if the mesh is fully unstructured you might as well replace QUICK with 2nd order. Obviously run 1st order first before moving to higher discretisation methods.

Also I would use a 2nd order scheme for the time step.

I'm surprised you have had no problems with convergence either as alot of swirling flows can be trouble to deal with especially with getting residuals down to an decent level.

If you want a more accurate tangential profile I would suggest using a structured mesh because despite the time involved in building it you are less likely to encounter convergence issues when using higher order schemes. It also produces less numerical diffusion as the cells are aligned with the flow giving you a more accurate solution.

One last thing would be to determine where the transition between solid body rotation and the free vortex. So you can make sure you have sufficient radial mesh resolution to properly resolve the radial profiles.

Neil

[Ali.nabavi]

Originally Posted by richard
;109659

Hi, Johnny B, what is the mean of URF?

under relaxation factor