Turbulence model in a simulation with wide spatial range of Reynolds numbers
 

Hi,

In my computational domain fluid(water) enters through a large inlet and flows through slot nozzle of small width before flowing out through a large outlet. It is a steady state problem.

a)For the case with highest flow rate, the Reynold number (Re) at inlet is ~4000 and at nozzle is ~800. I use k-epsilon model. With the default timescale factor of 1, the simulation fails with fatal overflow in linear solver. But the case converges by reducing the timescale factor to 0.1. How is the k-epsilon model able to work for this simulation? Although the Re at inlet is high, it is <1000 at nozzle and the CFX manual says that for Re<1000, laminar flow assumption has to be used? Does CFX switch internally to laminar flow model in regions of low Re?

b) For the case with lowest flow rate, Re at inlet is ~600 and at nozzle is ~110. For this case if I use laminar model, simulation does not converge (convergence stalls), even with low timescale factor. However, if I use k-epsilon model with timescale factror 0.1, simulation converges ! In this case Re is <1000 at both inlet and at nozzle. So why doesn't the laminar model work while k-epsilon works?

Thanks for your inputs!
Best,
Chander

No it does not. If you use the k-e model in a laminar flow it will give you more dissipation then is really there, so is a significant source of error. The SST and related models are better here because they degenerate to (almost) laminar flow at low turbulence energies.

As discussed above, the k-e model is putting additional dissipation (ie viscosity) into the flow and that is stabilising it. When this artificial dissipation is removed the flow might be probably becoming transient - or it might not yet be converging properly.

Some tips are here:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

@ghorrocks

Thanks for your reply. Your argument that k-e model gives more dissipation in laminar flow seems very plausible. If I look at the flow field of the unconverged laminar model solution (momentum residuals in the range of 1e-3), it shows a lot of swirling while i don't see that in the converged solution using k-e model.
k-e model is based on the eddy viscosity assumption. Why does this lead to high viscosity at low flow Re?


And when you say "SST and related models", do u mean the k-omega models ? I already tried with the basic k-omega model which did not converge. I am using a fine uniform mesh for all three models: laminar, kepsilon and komega. I have not bothered to check for the y+ of my mesh due to the 'automatic' wall treatment in case of komega and 'scalable' wall functions in case of k-e model as used in CFX. Since komega did not converge, do u still suggest going for SST? I had earlier tired to use SST for a similar problem where Re was varying a lot spatially and SST model did not help there while komega converged with large reduction in timescale factor for that problem.

The eddy viscosity in the k-e model is proportional to k^2/e (http://www.cfd-online.com/Wiki/Standard_k-epsilon_model). Epsilon gets small in laminar flows so the eddy viscosity does not degenerate to zero eddy viscosity as k tends to zero.

The k-w model (and SST is similar) has eddy viscosity proportional to k/w (http://www.cfd-online.com/Wiki/Wilcox%27s_k-omega_model). Omega remains finite in laminar flows so the eddy viscosity correctly tends to zero as k tends to zero.

This is the fundamental reason why k-w based models are better for low Re flows than the baseline k-e model.

Yes, this is the model I would recommend. It will not have the artifical dissipation that k-e has so will be a little harder to converge but at least it will be more correct.

But for your flow as very low Re I would consider not using a turbulence model at all and just using a laminar model.

@ghorrocks
Thanks for your reply.

As far as the use of laminar model for the low inlet Re case (case (b) above) is concerned, i have tried it but not been able to get convergence with it. Actually in my simulation, water flows through a slot nozzle into a porous medium before flowing out through another duct and out of the domain. Re number at entry to the nozzle is 110 but Re based on pore size is > 1 (around 10) and so flow through the porous medium is non-Darcy and has a second non-linear term . I guess this is the reason that since inertia effects in my porous medium are significant, I have to use some turbulence model there. For this low Re case, I tried with k-epsilon, komega and SST. I have been able to get convergence with all three models !

At the other extreme of operating parameters with inlet Re ~4000 (case (a) above) and Re at nozzle ~800, Re based on pore size is ~75. For this also, I tried to use all the three turbulence models : k-epsilon, k-omega and SST.
k-epsilon model again converged but both k-omega and SST did not converge.

So in essence, kepsilon works at both the highest and lowest Re while k-omega and SST work at the lowest but not at highest Re. Is it again because of differences in estimated viscosity by both class of models? Any suggestions to get convergence with SST? I have been trying with different timescale factors and also tried with better initial conditions (converged k-epsilon solution) by following the directions at http://www.cfd-online.com/Wiki/Ansys...gence_criteria.

This flow is definitely laminar and therefore you should be using the laminar flow model. If you cannot get this to converge then fix it rather than using a turbulence model. As previously mentioned the laminar model has less dissipation than a turbulence model so it is expected that convergence is harder.

I think your problem is more fundamental than choice of turbulence model. Can you post an image of your geometry and the CCL?

@ghorrocks

Hi Glen,

Thanks for your reply.

I am posting images of my geometry showing the boundary conditions and various domains in my simulation. in the first figure Full_geometry.png, the unmarked boundaries are walls : side and top walls are adiabatic and bottom wall has input heat fluxes.

Thanks. Have you read the documentation about "Obtaining Convergence"? Also some more tips are here: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Note that based on your previous comments it appears this flow is not steady state, so you are going to have to go to a transient flow to get correct results.

@ghorrocks

And here is the CCL file for my case (inside the .zip file).
Referring to my other thread ( http://www.cfd-online.com/Forums/cfx...on-komega.html ) , the situation is summarized again in the attached figure 'summary.png'

@ ghorrocks

Thanks for the tip regarding transient flow.
However, before I give trasinet simulation a try, I have also uploaded my CCL file and a summary of the situation above. Kindly have a look at that too.

Some comments:

I see you have specified water properties in some detail. If you want accurate water properties then just use the built-in IAPWS water properties. This is the best source for water properties.

Other than that, you need to go to a transient solution. But I have said that before :)

@ghorrocks

Hi Glen,

I am going to start the transient simulation for my set-up. I have two quick queries on that:

1) You already said that for the low Re case, I need to do a laminar transient simulation. Do you suspect transient behavior for the high Re case also where k-omega and SST models are not converging (refer table above)? If I apply the test for whether a flow is steady or transient ( as mentioned in 'Obtaining convergence'), I cannot clearly decide if changing the timescale factor for the steady state simulation really keeps the period residual oscillations constant at both the high and low Re operating conditions.

2) For steady state simulations, CFX introduces a pseudo transient term to evolve the steady state solution. Then doesn't a steady state simulation in CFX use same solution methodology as a transient simulation? Why is the convergence behavior different ?

1) I suspect both cases (low and high Re) are transient from what you have said.

2) The steady state simulation eliminates many of the terms which come about in the transient Navier Stokes which do not affect the final steady state result. Additionally, there are options to advance difference equations at different time scales and different sections of the domain at different time scales. That means the flow is not evolving in a time accurate manner, but it should converge to the steady state result.

In short CFX uses a psuedo-transient approach to numerical stability to obtain convergence, but this approach is not time accurate and does not include all transient effects.

@ghorrocks

Thanks a lot for the clear and precise explanation.
Your understanding and explanations regarding both the CFD theory and software usage is admirable.
Although I have had CFD courses earlier but I was not aware of this subtle difference in solution methodologies for steady state with pseudo-transient term and transient solution.
Did you read any particular text for understanding of details like the one you explained here? Can you suggest me the same for going through further details?

I learnt all that stuff on the forum years ago. There was a guy called "Robin" who posted some very informative posts here years ago, if you do a search you might find some of his posts from years back. And now I am attempting to pass the information onto today's users.

@ghorrocks

Thanks Glen for that info. I have tried but could not find much with this name on the forum. May be the posts have been removed.

There are a host of other queries that are still puzzling me. May I ask them here ?
1.a)Why is k-epsilon model giving seemingly incorrect boundary layer development at high Re (~4200) case also for my problem. This is a very commonly used model in academia and industry.
1.b)Also, at low Re, you had explained that this model imposes artificially high viscosity. Then shouldn't it show a thicker boundary layer as compared to k-omega while what I see is exactly opposite (figures in thread http://www.cfd-online.com/Forums/cfx...on-komega.html)
1.c) How do you approach a turbulence simulation in CFX? Do you take any special care in meshing such as y+ etc.?

2) Another thing that creates doubt is whether the way I define my Re is correct or not. To define the inlet Re, I just calculate the hydraulic diameter for my inlet rectangular duct (2*width*height/(width+height)).
However the number that I get is quite different from what CFX reports in .out file under 'Average scale information'. For example, I calculate my lowest Re as ~600 but .out file reports an Re of ~1000 for inlet duct.
I could not find any detail on how this Re is calculated by CFX in the manual. I had asked CFX support also sometime back but they also could not tell me much except for saying "the average scale information in the out file for the Reynolds Number is just an assumption and does NOT influence the simulation!"

The forum still has posts from 10 years back. It is just a little hard to find things with so many posts.

1a) The default k-e model only works for mid to high turbulence. It is not good at low turbulence. Refer to a turbulence textbook for more details.
1b) The boundary layer is set by the wall functions. The extra dissipation is in the internal regions. I cannot recall what a k-e wall function does in low turbulence, it could be anything. So if it generates artificially thin boundary layers I would not be surprised.
1c) I first of all determine whether a turbulence model is appropriate. In your case it is not. But if it is a turbulent flow then my default option is SST and I would only choose anything else if I had a specific reason to do so - eg anisotropic, bluff body etc. And yes, meshing is very important. The mesh is tailored to the boundary layer I expect to generate.

2) The average scale is simply a length scale from the cube root of the volume of the domain, and similarly a gross average velocity, density and viscosity scale. It is almost meaningless so ignore it. Your calculation is much more meaningful as you know wha the important length scales are.

@ghorrocks

Thanks Glen for the info again.
I am now trying with transient simulations.
Lets see how this goes.
Regarding your comment that you tailor your mesh according to the expected boundary layer, can you give more details on it. I usually stick to uniform mesh for turbulent flows but keep it making finer for grid independence. I know that one can make mesh coarser away from walls but in my geometry, i see a lot of vortices in mid regions due to fluid recirculation. Since I cant keep trying to make fine mesh in all regions of high shear I stick to uniform mesh till now. And while making finer meshing near walls I don't care for y+ due to the way CFX handles near wall treatment (scalable and automatic treatment). Is my approach correct?
Any specific directions in meshing will be greatly helpful !

And you mentioned that SST is default model for you for turbulent flows. Any specific situations, where you chose to use models other than SST ?

Depends on what you are modelling. There are no simple answers in CFD. If you are modelling a flow where boundary layer effects are not very important then this sounds fine. Also if you are in the regime where you will be using a wall function approach and this is appropriate then OK. But if you need accurate boundary layer development then this approach will not be accurate.

Anisotropic turbulence = Reynolds stress models.
Bluff body with large scale vortex shedding = LES style models (including DES and SAS).
Low and transitional Re = Laminar

@ghorrocks

Thanks Glen again for the info.
My simulations involve conjugate heat transfer. So I guess, I should be a bit more careful with the mesh near walls??
CFX manual has some guidelines liking keeping y+=1 or 2 for 'accurate boundary layer simulations in turbulent flow. There aren't any particular guidelines for laminar flow but I think mesh resolution near wall for laminar flow can be decided based on grid convergence studies. May be I should follow these guidelines more closely when using turbulence models for more correct results although I doubt this alone will have any effect on convergence behavior.


One update from my side. I mentioned before that am using porous media model in my simulations. For the lowest inlet Reynolds number, I just tried with one case by replacing the porous media with a simple fluid domain. The simulation converged easily with laminar model! (If the porous media is present, laminar model does not converge). Can porous media be a major contributor to non-convergence? Fluid flows from inlet duct to this porous medium through a domain interface. Similarly it flows out from this porous medium to outlet duct through another domain interface. Conservation of mass and momentum across the interfaces is enabled by default. Can a sudden change from fluid domain to a low porosity porous media across the interface have some contribution to non-convergence?