Laminar or Turbulent Model

[Anonymous]

Hello,

I am slightly confused about whether to choose laminar or turbulent flow for my simulation. From reading the Autodesk CFD article regarding Turbulence and the various models, it seems that if I choose laminar and the flow diverges within the first few iterations, then I should change it to a model such as the default k-epsilon model. 

I ran my model using k-epsilon for 300 iterations and achieved what seems like convergence. I tried to run the model using laminar flow for 300 iterations and was also able to run to completion, but it does not look as clean. Should I continue using the laminar model if the simulation is not aborting? 

Also, how can I tell if the simulation is reaching divergence? Will the simulation simply exit? 

I have attached convergence plots for both the laminar and turbulent models for your reference. 

[Jon.Wilde]

Hi,

You are probably OK to just run with the ke model.

Can you share a little more about the model?

A diverging model will typically stop with an error.

A converged model will stop with a happier message 🙂

[Anonymous]

Based on the problem condition and length scales you can realize if the flow is laminar or turbulent. Generally speaking, we rarely have laminar flows in industrial scale flows. Laminar flow exists in very narrow tubes or when the fluid has very high viscousity. Transition Reynolds number for basic flows can be found in Fluid Dynamics text books. 

[Anonymous]

Thank you very much! The model is basically just fluid flow through a threaded channel with a sleeve around it. The model appears to be reaching velocities of around 6-7,000 mm/s, but I am unsure how to calculate a length to gauge the Reynolds number.

[Anonymous]

Thank you very much. I was assuming that it would be turbulent flows which is why I started with the default k-epsilon model. I just wanted to verify that it would diverge with laminar flow to help validate the model I chose, but it didn't work out that way. Since I appear to be reaching better convergence with the k-epsilon model I will probably just stick with that.

I wanted to verify with those who are much more experienced that what I am doing is acceptable, since I am still very new to CFD and am trying to learn as I go .

[Anonymous]

One of the main questions I am trying to determine when running this simulation is whether the flow is laminar or turbulent. Is there a way to determine this using the simulation? It seems that I have to assume either condition and that the solver will use one or the other.

[srhusain]

Unless you are sure that your flow is laminar throughout the model, you can use the standard SST turbulence model, which can handle low turbulence/near-laminar flow as well as high turbulence conditions.

However, when running turbulent, you should monitor the Y+ values to ensure that it does not exceed 20 on the walls as this could indicate that the flow near these areas are asking for better boundary layer mesh resolution on account of high turbulence and shear.

Briefly, for the SST turbulence model there is no limit to how low a Y+ (corresponding to the fineness of the boundary layer mesh size) is allowed, but values greater than 20 will cause some inaccuracy in resolving the boundary layer.

On the other hand the k-epsilon is a very good turbulence model, but here you want to ensure that the Y+ values at the walls do not fall below 12 as this could cause convergence difficulty in addition to loss of accuracy. This model, however, can tolerate larger values of Y+ (up to around ~200) without appreciable loss of boundary layer resolution accuracy.

[Anonymous · Accepted solution]

The k-epsilon turbulence model assumes the entire domain is in the turbulent flow regime. The SST turbulence model will become laminar if appropriate. 

This method is very time consuming but if you must know whether your model is turbulent or laminar and you have no way of computing a Reynolds number, you could do the following:

1) Run your simulation with the k-epsilon turbulence model. (If your results seem reasonable at this point, you could assume turbulence)

2) Run your simulation with the laminar model. (If you cannot get it to converge, your simulation is likely turbulent)

3) Run your simulation with the SST turbulence model.

If the results from 1) and 3) are in relatively good agreement, your simulation is turbulent. If the results from 2) and 3) are in relatively good agreement, your model is laminar. If neither are the case, your model is likely transitional and the results from 3) would be the most accurate. All of this assumes that your mesh is appropriate for each scenario. 

[Anonymous]

Thank you very much for the detailed response.

What would be the difference between the standard SST turbulence model and the Low Re k-epsilon model? For the latter, it states that it "generally produces the same solution for high speed flows as k-epsilon" and it will "produce similar results to the Laminar selection for laminar flows". If I were to choose this model, how would I be able to tell where the flow is laminar and where it is turbulent?

Would the Mesh Enhancement layers that it refers to be found in the mesh advanced parameters?

I apologize for my lack of knowledge, but what are the Y+ values and where can I monitor them?

[Anonymous]

I will definitely try that as I have already done 1) and 2). Just to clarify, the standard SST model is the SST k-omega model? Would 300 iterations per model be sufficient or should I run more (~500) just to be safe?

In cases where I am unsure like this, would this be the best method to determine laminar vs turbulent flow? If the flow is transitional, how could I locate the areas in which the flow is laminar and where it is turbulent?

For my mesh, I use autosize, and then choose both Surface Refinement and Gap Refinement, and set the Fluid Gap Elements to 3 (since I have a thin gap). Are there other parameters that I should generally be working with to generate an appropriate mesh? Is there a location describing what each parameter is and how it would affect the mesh?

[Anonymous]

Yes, use the SST k-omega turbulence model.

You should always run the model until convergence is achieved, regardless of the number of iterations. Whether that is 300 iterations, 500 iterations, 5,000+ iterations depends on the complexity of the simulation and the convergence criteria. 

I'm not sure if this is the "best" method. It is time consuming and may not be appropriate for all scenarios.

You could plot the turbulent intensity to estimate regions of turbulence. Enable this result by clicking "Result Quantities" in the Solve dialog box. While you're there, also enable Wall model y+. 

After your solution has converged, you will be able to plot the y+ values on the surface of your model. Modify the inflation layers by clicking on "Enhancement" in the mesh dialog box and adjusting the parameters. Click the blue "?" icon in that window to read information on each of the parameters. Re-run your model until you achieve appropriate y+ values for the turbulence model you are using. 

[Anonymous]

Thank you very much, I will try this and report back later!

[Anonymous]

I completed the comparison allowing each model 500 iterations. Both the k epsilon and SST models converged right around 360 iterations, while the laminar flow went the full 500 iterations. From the graphs, it appears that the k epsilon and SST models closely match, however they differ quite differently with regards to TED (Turbulent Energy Dissipation?). Attached are all three convergence plots.

How exactly is the Turbulence Intensity calculated and what would be a qualitative way to think about the range? Is it arbitrary to whatever the maximum is for the simulation or is some set value (i.e. 10 or 15) a threshold for laminar to turbulent flow?

From what I was reading online, the Y+ variable relates to how far off the wall the wall functions are valid for, and should generally be kept between 35-200. Is there an article by Autodesk to read more about this variable that would give me more insight about it and what I should be aiming for? In your previous post regarding the appropriate range for the Y+ value for each model, how did you come by that information?

[srhusain]

I would not be too concerned with TED values being different,because the two models are just different and they have very different behavior very close to the walls- what is critical is the behavior of the velocities, pressure, wall shear, and heat transfer at the wall (if running thermal).

My recommendations for the Y+ values and limits are somewhat approximate and these can vary depending on the scale of the model (size, characteristic velocities) vs. the scale of the turbulence such as the Kolmogorov microscales. Having said that, I recommend looking up "Turbulence Modeling", by D. C. Wilcox for details on the SST anf k-e models.

[Anonymous]

"what is critical is the behavior of the velocities, pressure, wall shear, and heat transfer at the wall (if running thermal)"

I am planning to add thermal results after understanding the current simulation better. Between the k-epsilon and SST model, given that their TED is different, which would you recommend for a thermal result and why? For these values, besides verifying mesh independence, what would you suggest I do to help ensure valid simulation results?

"Having said that, I recommend looking up "Turbulence Modeling", by D. C. Wilcox for details on the SST anf k-e models."

Thank you very much for the recommendation, I will look into that. Would that book also detail what the Turbulence Intensity value represents and how I can interpret it?

[srhusain]

For accurate thermal results, use the SST model, and your mesh needs to fine near the wall such that y+ is less than 1.0. This is regardless of your concern for the difference in TED values, for the same reason I had mentioned earlier, which is that near the wall, the wall functions take over the modeling of the shear stress and fluxes differently for different turbulence models.
The Wilcox book has all the information for turbulence intensity- you can also Google it.

[Anonymous]

Thank you very much for all of your help!

[srhusain]

Turbulence intensity is the ratio of the root mean square of the velocity fluctuations to the magnitude of the velocity of the mean flow. Its is as simple as that.
Obviously, for purely laminar flow this value is zero, but intensity is only one parameter among several that characterizes the turbulence of the flow. A more comprehensive picture is given by the turbulent energy spectrum which indicates how energy cascades from the largest eddies (eddies in size comparable to the geometry of the model) to the smallest down to the molecular scale of viscosity.
Moreover, as one transitions from purely laminar to low levels of turbulence, there is no clear threshold.
For most flows, you can use a turbulence intensity that ranges from 1 to 5% at the inlets, and moreover, this choice is largely of little consequence as long as the inlet is "sufficiently" far upstream of where you are trying to get accurate simulation results. Exactly how far upstream id "sufficient" varies widely from model to model and it is based on experience- there is no rule of thumb.

[Anonymous]

I believe I understand it now thank you very much for your explanation!

Is the Turbulent Energy Spectrum something that I can choose as a result quantity for my simulations?

For the inlet if I specify that the flow is Fully Developed would this satisfy the requirement, or should I make the inlet physically long enough for flow to fully develop?

[srhusain]

Sorry, you cannot choose the spectrum as a result quantity- unlike other result quantities, it is much more complicated.
Fully developed flow BC that is available in CFD is not exactly fully developed in the context of turbulent flow presently- so to ensure physically fully developed flow you will need to extend the distance from the inlet.