[Jade M]

I have not received a consistent answer and am hoping to get come clarification from this forum.

I am simulating air flow through a duct. The air flows through a constant-area duct, then through a series of fins and then through a constant-area duct similar to the upstream section. By a standard Reynolds number calcuation with hydraulic diameter, the flow upstream and downstream would be turbulent and the flow between the fins would be laminar. The duct is 1.5" wide by 0.35" tall. Perhaps the shape of the duct has something to do with the stability of the flow.

I have several questions with regard to CFX's treatment of this flow. I am new to CFX and also to turbulence, so please feel free to provide as basic an answer as necessary, as if explaining to a beginning mechanical engineering student. Please feel free to answer all or any part of my questions, as I am asking a lot!

How does CFX treat this problem if the flow is actually turbulent but the laminar option is specified?

How does CFX treat this problem if the flow is actually laminar but the turbulent option is specified?

What happens if part of the flow is laminar and part is turbulent?

An ANSYS CFX consultant says that the Reynolds number calculation is based on the cubed root of the volume, that CFX does not calculate some instability in the flow to determine whether the flow is laminar or turbulent, and that the warning message is purely based on this Reynolds number which may not be meaningful. This consultant's advice seemed the most reasonable to me compared with everything else that I have been told. However, this would not explain one thing -- it seemed that as the mesh became finer, the warning that the flow may be turbulent when the laminar option was set. Any explanation? I thought that the solution may have detected the the flow never becomes unsteady or turbulent with the finer mesh but apparently CFX does not try to calculate this.

Also, a colleague of mine asks:
We know the flow is (or rapidly becomes) laminar in the fin section based on a Reynolds for that region of 1000. The fin section is where we are interested in determining heat transfer (and pressure drop). How does a solution setting of turbulent capture the fact that the flow is laminar? Will it converge? How accurate will it be compared to a laminar setting? Wouldn’t we come closer to what we are seeking by using a laminar setting? Further, the correlations we are comparing to are based on laminar flow.

Thank you very much for any information! Help would be most gratefully appreciated.

[ghorrocks]

How does CFX treat this problem if the flow is actually turbulent but the laminar option is specified?

Then it will attempt to model the vorticities which make up the turbulence, providing you have a numerical scheme accurate enough to capture this. If you run steady state you will not get convergence. If you run transient you will notice small perturbations in the fields at low Re, which increase to large vorticies at high Re.

How does CFX treat this problem if the flow is actually laminar but the turbulent option is specified?

For a k-e based model you will just get rubbish as this model does not handle low k well. For a k-omega (inc SST) based model it will handle small k well and should give a similar result to a laminar simulation. But any turbulence model will add some dissipation (that's what turbulence models do!) so it will not be quite as well resolved as a laminar model.

The comments by the CFX consultant is correct. The reported Re is just a guide and is only useful to check you are in the ball park. If you want a more representative Re you should calculate it yourself using an appropriate length, velocity, viscosity and density scale.

Finer meshes have reduced numerical dissipation and therefore capture more fow features. This means a simulation on a coarse grid with a laminar model may be steady, but with grid refinement goes unsteady. This was not "detected" by CFX, it is just a fact that the numerical dissipation has reduced sufficiently that the transient features are not damped out.

We know the flow is (or rapidly becomes) laminar in the fin section based...How does a solution setting of turbulent capture the fact that the flow is laminar?

If you are using k-e turbulence model your results will be rubbish. If you are using k-omega or SST it should be much improved. But if your flow is only just turbulent and becoming laminar I would probably run it laminar.

Will it converge?

Turbulence models add dissipation and so it should be easier to converge.

[Jade M]

I appreciate your detailed comments. This really helps!

[wxmoore]

Based on my experience with Fluent the k-omega SST model at least exhibits better convergence behavior for cases in which there is both fully laminar and turbulent flow in the same fluid domain, provided that there is sufficient resolution of the boundary layer and appropriate y-plus values.
Howver this does not necessarily mean that the k-omega SST model is more accurate than the k-epsilon models unless verified by test data.

One option worth trying would be to beraek the fluid domain into separate zones (laminar and turbulent) and use a turbulence model but specify a laminar flow model for the fluid zone which is known to be laminar.

One peculiarity we have observed is that when we apply a mass flow inlet with a secondary species defined, the k-omega model gives a huge mass imbalance for the secondary species after a few hundred iterations, which does not occur when we use the k-epsilon models. Has anyone else observed this behavior with k-omega model?

[ghorrocks]

If you have turbulence transition in a model then that sounds like a case for the turbulence transition model. Then there is no need for defining different domains, and then linking them together somehow (I do not know how you would do this - it sounds very dodgy to me).

[wxmoore]

Excellent point! The k-omega model works very well but our species mass balance was totally wrong for some reason. We are currently using the k-epsilon realizable model with enhanced wall treatment and refined boundary mesh. It is converging well after 50 iterations but due to the size of the model (16 million cells) it will take sevral hundred or more iterations. I wish I knew why the secondary species mass balance was so far out of balance for the k-omega model and not the other turbulence models.

[wxmoore]

Having done some more testing we discovered that we were using the wrong type of boundary condition to model the trace secondary species input into the flow domain. Rather than using a fixed mass flow inlet we chose to use volumetric mass generation as a source term by creating a separate volume next to the large fluid domain. Now when we use k-omega SST model the trace secondary species mass convergence is completely satisfied. This also required using a boundary layer mesh with a wall y plus very close to 1. The k-omega model appears to be predicting the correct flow pattern and velocity vector profile even though our model contains both fully turbulent and laminar flow.

William

[Ana Jakanica]

Originally Posted by ghorrocks

If you have turbulence transition in a model then that sounds like a case for the turbulence transition model. Then there is no need for defining different domains, and then linking them together somehow (I do not know how you would do this - it sounds very dodgy to me).

Dear Glenn,

Could you help me - what is the conclusion from this thread: should we use the turbulence transition model (which one exactly?) or k-omega tubulence model when we have the case of flow regime change from turbulent to laminar (or vice versa) in the same flow domain?
Can you also recommend a model for this case but for swirling flows?

Thanks!

[ghorrocks]

I thought the post #5 is pretty clear.

You can use any transition model you like, but the gamma theta model is probably the most general. But the transition model only works with the SST turbulence model. You cannot change the turbulence model.

Note that CFX does not have a relaminarisation model. It can be approximated by low turbulence levels, but this approximation will not necessarily be accurate depending on the application.

For swirling flows activate the streamline curvature model in the SST model, but be aware that the turbulence transition model does not have a curvature model.

[Ana Jakanica]

Originally Posted by ghorrocks

I thought the post #5 is pretty clear.

You can use any transition model you like, but the gamma theta model is probably the most general. But the transition model only works with the SST turbulence model. You cannot change the turbulence model.

Note that CFX does not have a relaminarisation model. It can be approximated by low turbulence levels, but this approximation will not necessarily be accurate depending on the application.

For swirling flows activate the streamline curvature model in the SST model, but be aware that the turbulence transition model does not have a curvature model.

Thanks for the explanation!

[ghorrocks]

I might add that the gamma theta model was developed in rotating machine blade applications, and it works pretty well there. But it has not been tuned for other applications. Use of the model in other applications (such as turbulence with lots of streamline curvature) it will be up to the user to determine if the model is appropriate or not.

[Ana Jakanica]

Glenn, could you,please, recommend the suitable literature where I can see that 'For a k-e based model you just get rubbish as this model does not handle low k well'?
Thanks!

[ghorrocks]

It comes from the equations. As a turbulent flow goes laminar then k and epsilon go to zero.

The eddy viscosity equation has a k^2/epsilon term, this is undefined with epsilon equal to zero and goes bezerk as epsilon gets small.

https://en.wikipedia.org/wiki/K-epsi...rbulence_model

The k-omega model on the other hand has the eddy viscosity defined as k/omega where omega does not go to zero as turbulence goes to zero. It nicely goes to eddy viscosity = 0 as k=0 and the flow goes laminar.

[marcel_jay]

I am really confused by the question what to set for the turbulence intensity option.

In my CHT simulation, (rotating tool in open domain with atmospheric pressure), I set the intensity to 0% (laminar), 5% (SST) and 10%(SST) and get results with pretty equal flow fields as well as same temperatures in my solids. The conclusion must be, there is no turbulence at all? Hard to believe since I have a solid rotating with 1600 rpm and 80mm diameter, with relative fluid velocities of up to 12 m/s.

I would love to continue with the laminar assumption since my CPU time for solving is cut into half.

[leasken]

Originally Posted by marcel_jay

I am really confused by the question what to set for the turbulence intensity option.

In my CHT simulation, (rotating tool in open domain with atmospheric pressure), I set the intensity to 0% (laminar), 5% (SST) and 10%(SST) and get results with pretty equal flow fields as well as same temperatures in my solids. The conclusion must be, there is no turbulence at all? Hard to believe since I have a solid rotating with 1600 rpm and 80mm diameter, with relative fluid velocities of up to 12 m/s.

I would love to continue with the laminar assumption since my CPU time for solving is cut into half.

If different turbulence intensities at the inlet have little effect on your flow field, then the conclusion I draw is that turbulence created in the domain is larger than turbulence conditions at the inlet. So no, you cannot say that the flow is laminar only by investigating the inlet turbulence conditions.

[walakaka]

Originally Posted by ghorrocks

For a k-e based model you will just get rubbish as this model does not handle low k well. For a k-omega (inc SST) based model it will handle small k well and should give a similar result to a laminar simulation. But any turbulence model will add some dissipation (that's what turbulence models do!) so it will not be quite as well resolved as a laminar model.

When you mention the the results will be rubbish, will it be possible that the mass is not conservered? Is this what people mean when they say non-physical results?

Regards
Shafik

[ghorrocks]

I suspect if you used a k-e model on a flow which is actually laminar it will converge fine and mass will be conserved. However the turbulence model will have put far too much dissipation into the simulation so the flow will be unrealistically viscous.

I have checked the SST model against laminar flow results and at least for the flows I checked the difference was very small. So I have confirmed the SST model degenerates to a good approximation of a laminar flow in the cases I looked at.

[rzsd1374]

Originally Posted by ghorrocks

Then it will attempt to model the vorticities which make up the turbulence, providing you have a numerical scheme accurate enough to capture this. If you run steady state you will not get convergence. If you run transient you will notice small perturbations in the fields at low Re, which increase to large vorticies at high Re.



For a k-e based model you will just get rubbish as this model does not handle low k well. For a k-omega (inc SST) based model it will handle small k well and should give a similar result to a laminar simulation. But any turbulence model will add some dissipation (that's what turbulence models do!) so it will not be quite as well resolved as a laminar model.

The comments by the CFX consultant is correct. The reported Re is just a guide and is only useful to check you are in the ball park. If you want a more representative Re you should calculate it yourself using an appropriate length, velocity, viscosity and density scale.

Finer meshes have reduced numerical dissipation and therefore capture more fow features. This means a simulation on a coarse grid with a laminar model may be steady, but with grid refinement goes unsteady. This was not "detected" by CFX, it is just a fact that the numerical dissipation has reduced sufficiently that the transient features are not damped out.



If you are using k-e turbulence model your results will be rubbish. If you are using k-omega or SST it should be much improved. But if your flow is only just turbulent and becoming laminar I would probably run it laminar.



Turbulence models add dissipation and so it should be easier to converge.

Hi
I apologize because of asking this question after a long time of posting this thread
Could you please tell me about a paper or book or another reference that confirms your argument about the drawbacks of k-e based model in simulating laminar flow?
regards,
mohammad

[ghorrocks]

I do not know of any reference. You can reference this forum thread if you like

The comment came from looking at the equations those models use and thinking about the implications. A reference like "Turbulence Modelling for CFD" by Wilcox might be helpful.