Could you please give some more details on the problem/outcomes you're interested in? Furthermore, it would be nice to know which issues you're observing - "None of them gave very good results" is not expressive...

First of all, I would like to tell you that your problem statement is not clear, so please describe your problems in an appropriate way. However, in my understanding by went through model assembly, I guess your are trying to model the water flow across the assembly. If its the same then what are the results your are looking for and what is the problem ??

I actually am modelling a vortex tube in Ansys Fluent but Iam not able to acheive appreciable temperature difference in the CFD model. Attached is the model of the file. I tried meshing it using workbench meshing. But after having a very fine mesh also I was not able to obtain the Temperature difference. And the reversible flow also was not be seen. I would like to know what might be the problem 

I have also attached the setup data file. Please suggest any changes to be made in them to acquire proper results.

Thank you 

I'm still not sure how your system operates, but based on the attached file with the boundary conditions I recommend checking the following:

1.) The ideal gas law for air material properties is defined, where the density is calculated from dens=p*M/R/T. Therefore, I would check the proper defintion of the operation conditions, where you can specify the 'operation pressure', which is used for the above density calculation (according to Fluent's theory guide).

2.) Pressure inlet and outlet conditions are specified for your inlets and exits. Based on the given information I cannot estimate the turbulence level in your system and if this justifies the use of turbulence models (instead of calculating laminar flow). However, the standard k-epsilon model is well-known to generally underestimate turbulence, which may be a driving force for heat transfer in your system. Thus, if the turbulence is underestimated this may give you false temperature profiles; but:

3.) Based on the boundary conditions, I cannot see where any temperature difference in your model should come from, because a temperature of 300 K is defined for each of the walls as well as for the entering/leaving materials. In addition, no heat fluxes are defined. So, where do you expect higher/lower temperatures?

4.) Check if the standard wall function is meaningful for your case. If you use very fine grids near the wall, the defintion of alternative wall functions could make sense.

Last but not list a small hint: you have a lot of different walls, which perhaps could be combined with others. To do so, select all walls with identical boundary conditions (in the Meshing tool of the ANSYS workbench) and insert a "named selection" for the selected walls by using right-click option. You also can define a name for this selection, other than the default Fluent names, which makes it easier to identify it during the Fluent setup process. In your case, all walls with names "wall-29" to "wall-39" may be combined with other boundaries.

I hope that these ideas help you to solve problem.

With best regards,

Stephan Kaiser

Hi Stephan,

Thanks for your quick reply. 

Regarding Temperature difference: Actually in a vortex tube the temperature difference is obtained due to transfer of heat between the inner(slower) vortex and Outer(faster) vortex. 

The problem in my case is the inner vortex is not forming at all. Please refer the image to understand how it works. 

I don't understand the term alternative functions in the point 4)

Can you tell me why one would choose "Ideal Gas" in Density?

How to estimate the turbulence level of a system?

Regards

Sankeerth

https://www.google.co.in/url?sa=i&rct=j&q=&esrc=s&source=images&cd=&cad=rja&uact=8&ved=0CAcQjRw&url=http%3A%2F%2Fwww.overclockers.com%2Fforums%2Farchive%2Findex.php%2Ft-485837.html&ei=O-Q0Ve_5AYeyuASM-oGwCA&psig=AFQjCNFNVMxd_2-AlubSBOYvAGKma5azTQ&ust=1429616019462628

Hi Sankeerth,

Now I took some time to read about vortex tubes in general - so I hope to understand the issue better - apologize that I didn't had enough time to do this earlier. But let's start with the generals:

As to Point 4: wall functions are used to calculate/approximate the velocity profile near the wall. If we consider the flow in a linear tube, you will get a parabolic velocity profile over the complete diameter and thus the near wall region is also well-defined (assuming non-slip walls, i.e. v=zero). This is not the case for turbulent flows, where the flow away from the wall is superimposed by a laminar subregion near the wall; numerical details for Fluent are given here: https://www.sharcnet.ca/Software/Fluent6/html/ug/node512.htm

The density of ideal gases can be calculated via dens=p*M/R/T, which is universal and depends on the operation parameters (temperature, pressure) and the type of gas (molecular weight) - i.e. known parameters. Alternatively, you could specify the relationship between density and temperature via user-defined functions (similar to the example 2.3.19.4 in http://www.arc.vt.edu/ansys_help/flu_udf/flu_udf_sec_define_property.html).

In your case, I would approximate the level of turbulence in the vortex tube assuming it to be a simple pipe. You should know your (average) total mass flow rate of air flowing through your tube and you then can calculate a mean flow velocity through the pipe. Via the general Reynolds equation (Re=w*d*rho/mu) you can calculate the pipe Reynolds number, which should be well above 2000 if the flow is turbulent. If this is not the case, you may calculate assuming laminar conditions (which makes the simulation easier and more stable).However, based on what I read so far, I expect the flow to be turbulent. Thus, using a turbulence model should be necessary, but if the standard k-epsilon model is suitable for your issue is another question...

I'm not sure if a steady state (time-independent) solver in conjunction with a two-equation turbulence model is capable of simulating such complex flows, which may have many turbulent eddies of different scales. Hence, more sophisticated turbulence modelling (such as LES) may be required.

Nevertheless, in my opinion, the issue with the temperatures remains: if your vortex is obtained by differently temperatured gases, you should at least specify different inlet and outlet temperatures respectively. The cold gas leaves through the small tube outlet, the warmer gas leaves through the large tube oulet, right? However, the temperature boundary conditions are identical for all walls (in your setup data file).

Again I hope this is helpful for you.

Regards,

Stephan

Hi Stephan,

Issue regarding temperature: The formation of an inner vortex and outer vortex results in the difference in temperature that we are able to see. This is the information i know from what I have read. 

Why would you say that the problem might not be a steady one? 

Why would you say that k-eps model may not be suitable? Can you explain! 

Thanks 

Regards,

Sankeerth

HI Sankeerth, 

As to the temperature again: I understand that the temperature difference is a result of the vortex formation - it was unclear to me in the beginning of the discussion but I've read the same information in the meanwhile. However, this phenomenon is not reflected by your boundary conditions. If the colder gas leaves the tube through another exit than the warmer gas then the temperatures at both exits should be different - but, according to your data file, all temperatues were identical (300 K). 

The (standard) k-eps turbulence model is know to fail predicting turbulence in swirl flows, as well as in flows with adverse pressure gradients, streamline curvature and seperations. Furthermore, the calculated turbulent diffusion (eddy viscosity) only depends on a single turbulence length scale, whereas in reality all scales of motion will contribute to the turbulent diffusion. Last but not least, the model assumes isotropic turbulence, which may not be the case in your system. You will find several excellent papers about the weaknesses of the k-eps turbulence model published.

Interestingly, in a quick search on modelling of vortex tubes, I found the following article: http://www.arpapress.com/Volumes/Vol6Issue1/IJRRAS_6_1_07.pdf. Despite the disadvantages, the authors used the k-eps turbulence model and they provide many details on their boundary conditions. A similar model has been used in the article "Parametric and internal study of the vortex tube using a CFD model" (doi:10.1016/j.ijrefrig.2004.04.004). 

Hope this helps.

Regards, 

Stephan

Stephan C. Kaiser

hello Dr, i have a problem when i used fluent flow to simulate the vortex hilsch tube. this steps for my project, can you check and tell me whats wrong?

Hello Ahlam,

Since I don't know what the expected outcome is, it is difficult to tell you what's wrong with your simulation. In general, the residuals don't look good and the turbulent viscosity was limited for a significant number of cells by the system. This indicates that the settings for the turbulence boundary conditions are not otpimal, but I cannot say what you have to change without more background knowledge (and I don't have any capacity to do research on this right now). However, I recommend to use a first-order upwind solver first and to refine the solution with the second-oder solver later. This should improve the convergence.

Hope this helps.

Regards,

Stephan

Stephan C. Kaiser thanks a lot doctor . later , i already used the first upwind but i still have the same problem .if the mesh is not fine .

Is it possible to be the reason?

" the size element equal 1 mm "

If I used specification method " intensity and viscosity ratio " by default ,is this wrong?