CFX Treatment of Laminar and Turbulent Flows
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 constantarea duct, then through a series of fins and then through a constantarea 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. 
Quote:
Quote:
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. Quote:
Quote:

Thank you!
I appreciate your detailed comments. This really helps!

Based on my experience with Fluent the komega 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 yplus values.
Howver this does not necessarily mean that the komega SST model is more accurate than the kepsilon 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 komega model gives a huge mass imbalance for the secondary species after a few hundred iterations, which does not occur when we use the kepsilon models. Has anyone else observed this behavior with komega model? 
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).

Excellent point! The komega model works very well but our species mass balance was totally wrong for some reason. We are currently using the kepsilon 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 komega model and not the other turbulence models.

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 komega 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 komega 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 :) 
Quote:
Could you help me  what is the conclusion from this thread: should we use the turbulence transition model (which one exactly?) or komega 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! 
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. 
Quote:

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.

Glenn, could you,please, recommend the suitable literature where I can see that 'For a ke based model you just get rubbish as this model does not handle low k well'?
Thanks! 
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/Kepsi...rbulence_model The komega 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. 
turbulence intensity
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. 
Quote:

All times are GMT 4. The time now is 06:40. 