CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   CFX Treatment of Laminar and Turbulent Flows (

Jade M March 18, 2010 13:32

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 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 March 18, 2010 18:01


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 March 19, 2010 11:05

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

wxmoore January 8, 2013 09:41

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 January 8, 2013 18:17

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 January 8, 2013 18:45

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 January 26, 2013 11:11

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 :)

All times are GMT -4. The time now is 20:09.