[JulioPieri]

Hello guys!

I've being experimenting with different turbulence models to see how they affect the flow mixing.

I noticed that the "laminar" viscous/turbulence model, which doesn't apply any modeling, gives a much more realistic result [picture attached]. I know that RANS models average the quantities, and that's why they have a "diffused" look. Also, as expected, refining the mesh captures even finer structures on the laminar model - increasing the "resolution" of the figures.

For instance, the cavity tutorial (OpenFOAM) ran with laminar shows results that are visually much more appealing. Actually, the coarse mesh+laminar gives a (visually) similar result as the fine mesh+k-eps.

I suspect that the results look better, but all quantities may be much more inaccurate. Also, I suspect that a mesh-refinement study would lead to endless changes in the quantities.

I'd like to discuss:
1) Is it possible to extract any good info from a laminar model with a mesh that is, of course, not refined enough for a typical DNS simulation? I mean, besides the pretty figures... Do the figures represent anything actually?
2) Is there any situation where using laminar model would be useful, without an extremely refined mesh?
3) What are the cautions to take when using the laminar model?
4) On industrial applications, how to judge if the results from a "coarse" mesh using laminar/DNS are better/worse than the usual RAS model?

I'm having a hard time distrusting the figures... the solver also runs smoother than using turbulence models. Any ideas would be good!

[FMDenaro]

Originally Posted by JulioPieri

Hello guys!

I've being experimenting with different turbulence models to see how they affect the flow mixing.

I noticed that the "laminar" viscous/turbulence model, which doesn't apply any modeling, gives a much more realistic result [picture attached]. I know that RANS models average the quantities, and that's why they have a "diffused" look. Also, as expected, refining the mesh captures even finer structures on the laminar model - increasing the "resolution" of the figures.

For instance, the cavity tutorial (OpenFOAM) ran with laminar shows results that are visually much more appealing. Actually, the coarse mesh+laminar gives a (visually) similar result as the fine mesh+k-eps.

I suspect that the results look better, but all quantities may be much more inaccurate. Also, I suspect that a mesh-refinement study would lead to endless changes in the quantities.

I'd like to discuss:
1) Is it possible to extract any good info from a laminar model with a mesh that is, of course, not refined enough for a typical DNS simulation? I mean, besides the pretty figures... Do the figures represent anything actually?
2) Is there any situation where using laminar model would be useful, without an extremely refined mesh?
3) What are the cautions to take when using the laminar model?
4) On industrial applications, how to judge if the results from a "coarse" mesh using laminar/DNS are better/worse than the usual RAS model?

I'm having a hard time distrusting the figures... the solver also runs smoother than using turbulence models. Any ideas would be good!

What you are asking is if an unresolved simulation where no closure model is explicitly supplied can work or not.
This topic is well documented in literature, denoted as "unresolved DNS" or better as "LES no model". The grid and the numerical discretization act as implicit filter (space and time), that is your "laminar" model say just to solve the NSE on a condition where wavenumber components of the solution cannot be represented.
Now this idea is quite old, dated to Deardoff, and the unresolved components were modelled by suitable additional (with dissipative character) terms.


Later, some authors had the idea that is not necessary to add explicilty further terms, just the action of the numerical scheme is sufficient when a dissipative character is present (Boris called MILES the FCT scheme).
At present, this method is denoted as ILES and is quite used.
However, this idea is in conflict with the traditional old school (Stanford in primis) where a physical SGS model is considered mandatory.


I suggest to search for the large literature.

[JulioPieri]

Originally Posted by FMDenaro

What you are asking is if an unresolved simulation where no closure model is explicitly supplied can work or not.
This topic is well documented in literature, denoted as "unresolved DNS" or better as "LES no model". The grid and the numerical discretization act as implicit filter (space and time), that is your "laminar" model say just to solve the NSE on a condition where wavenumber components of the solution cannot be represented.
Now this idea is quite old, dated to Deardoff, and the unresolved components were modelled by suitable additional (with dissipative character) terms.


Later, some authors had the idea that is not necessary to add explicilty further terms, just the action of the numerical scheme is sufficient when a dissipative character is present (Boris called MILES the FCT scheme).
At present, this method is denoted as ILES and is quite used.
However, this idea is in conflict with the traditional old school (Stanford in primis) where a physical SGS model is considered mandatory.


I suggest to search for the large literature.

Hi Prof. Denaro, thank you for your reply.

I indeed need more research on the topic. Could you please point me some books/papers related to that (and to other CFD foundation knowledge)?

As for the project I have in hand, do you think there is any off-the-shelf solution/criteria do decide whether my unresolved DNS is giving any useful (and sufficient) results? When in doubt, would you recommend prioritizing the closed RANS models even though the laminar results look appealing?

[FMDenaro]

Originally Posted by JulioPieri

Hi Prof. Denaro, thank you for your reply.

I indeed need more research on the topic. Could you please point me some books/papers related to that (and to other CFD foundation knowledge)?

As for the project I have in hand, do you think there is any off-the-shelf solution/criteria do decide whether my unresolved DNS is giving any useful (and sufficient) results? When in doubt, would you recommend prioritizing the closed RANS models even though the laminar results look appealing?

First, you have to run a 3d case for a sufficient number of time units in such a way to disregard the memory of the arbitrary initial conditions. Generally, that happens when the volume averaged kinetic energy starts to oscillate in time around a constant mean value.
Then you need to evaluate some statistics. Do you have some direction when the flow is homogeneous? In such a case you must compute the energy spectra to check if you have or not an energy pile-up close to the Nyquist frequency. That a good indicator that your no model simulation can Approximate the physics of the flow.

[JulioPieri]

Originally Posted by FMDenaro

First, you have to run a 3d case for a sufficient number of time units in such a way to disregard the memory of the arbitrary initial conditions. Generally, that happens when the volume averaged kinetic energy starts to oscillate in time around a constant mean value.
Then you need to evaluate some statistics. Do you have some direction when the flow is homogeneous? In such a case you must compute the energy spectra to check if you have or not an energy pile-up close to the Nyquist frequency. That a good indicator that your no model simulation can Approximate the physics of the flow.

If I had any energy pile-up, wouldn't my simulation just blow-up (seen by an increasing difficulty to converge some variables)? I mean, the fact that it is able to run for some time isn't a good indicative that the mesh/schemes are dissipating the turbulent KE generated?

[FMDenaro]

Originally Posted by JulioPieri

If I had any energy pile-up, wouldn't my simulation just blow-up (seen by an increasing difficulty to converge some variables)? I mean, the fact that it is able to run for some time isn't a good indicative that the mesh/schemes are dissipating the turbulent KE generated?

No, the pile-up can exists without leading to a numerical instability. You can have some situations where this energy pile-up is balanced by the diffusion terms in the local truncation error. The simulation can run for very very long time without blow-up. But what you see is the presence of small vortical structures that are not physical.

[JulioPieri]

Originally Posted by FMDenaro

No, the pile-up can exists without leading to a numerical instability. You can have some situations where this energy pile-up is balanced by the diffusion terms in the local truncation error. The simulation can run for very very long time without blow-up. But what you see is the presence of small vortical structures that are not physical.

Interesting... I don't see how I could practically do that calculation for my simulations. I have to come up with something else, or just use RANS.

What about using a Re/Peclet number criterion? For instance, having a local cell Re lower than, say, 200 would make it somewhat "locally laminar" (sorry for this fluid dynamics atrocity), therefore suitable for a unresolved DNS of such scale... Remotely makes any sense?

[FMDenaro]

Originally Posted by JulioPieri

Interesting... I don't see how I could practically do that calculation for my simulations. I have to come up with something else, or just use RANS.

What about using a Re/Peclet number criterion? For instance, having a local cell Re lower than, say, 200 would make it somewhat "locally laminar" (sorry for this fluid dynamics atrocity), therefore suitable for a unresolved DNS of such scale... Remotely makes any sense?

No, the local cel Re number says only if you are resolving or not the lowest turbulent structure.
Only the computation of some high order statistics can assess if your simulation is acceptable.
Could you give details of your flow problem?

[JulioPieri]

Originally Posted by FMDenaro

No, the local cel Re number says only if you are resolving or not the lowest turbulent structure.
Only the computation of some high order statistics can assess if your simulation is acceptable.
Could you give details of your flow problem?

Thank you for willing to help me. I'd be glad to share the details with you. Let's move to e-mail/private message? pieri175@gmail.com , in case you're ok with that. I can show you the domain and explain the problem.

[FMDenaro]

Originally Posted by JulioPieri

Thank you for willing to help me. I'd be glad to share the details with you. Let's move to e-mail/private message? pieri175@gmail.com , in case you're ok with that. I can show you the domain and explain the problem.

You can't make public the details here ?

Use the email: denaro@unina.it

[LuckyTran]

Would you confirm that whether you are comparing unsteady laminar with steady RANS or unsteady RANS? It looks like you are comparing with a steady RANS simulation and not an unsteady RANS.

[JulioPieri]

Originally Posted by FMDenaro

You can't make public the details here ?

Use the email: denaro@unina.it

I can share some info here yes, but not detailed figures. Let's save the email in case more clarifications are needed.

The problem is studying the temperature at the outlet of a flame-tube boiler. If the values are higher than a threshold, a specific type of slag (supposedly) forms and clogs the tubes. Therefore, I need to essentially study the mixing of the flow, analyze the max(T) at the outlet during some seconds of operation and compare the results of different load scenarios. With this hypothesis verified, I might then proceed to assessing possible solutions.

From the figure attached: the air comes in from the bottom and from the small nozzles on the wall. The outlet is vertical face pointing to the right of the scene.

A few assumptions that I'm making:
- Since it's a biomass boiler, I'm not modeling combustion. Solid fuel combustion would be too much for this project. Instead, I'm injecting hot air from the primary air duct (below the fuel grate), at the correct temperature so that the overall energy & mass balance is preserved. Also, secondary air is injected in some nozzles (modeled as square openings) throughout the water-wall.
- Firstly I was not using species diffusion, but I decided to recently include them (with same fractions as the flue gas), just to be more precise in the emission/absorption model (CO2 and H2O, mainly).
- The geometry is simple, though slightly big. I'm working with about 1milion elements, refining the mesh around high velocity regions (few cm from the secondary air inlets), and around a geometric detail inside the domain. This detail is where most of the elements are spent: it consists of 30 tubes appended to the water-wall, next to each other. To capture this detail I needed very fine elements around it.

I'm running a transient (Euler) simulation, with Courant number kept below 0,9 for stability.

Let me know if you need more details.

The main investigation now is whether the results from the Laminar model are somewhat better than the uRANS ones (Realizable kEpsilon, with default parameters). The results from the Laminar model are more consistent with what I'm observing in the field and with what I was expecting to see. Based on the recent uRANS results, I'm with very few cards to argument, risking to invalidate my main hypothesis for the problem.

[FMDenaro]

Originally Posted by JulioPieri

I can share some info here yes, but not detailed figures. Let's save the email in case more clarifications are needed.

The problem is studying the temperature at the outlet of a flame-tube boiler. If the values are higher than a threshold, a specific type of slag (supposedly) forms and clogs the tubes. Therefore, I need to essentially study the mixing of the flow, analyze the max(T) at the outlet during some seconds of operation and compare the results of different load scenarios. With this hypothesis verified, I might then proceed to assessing possible solutions.

From the figure attached: the air comes in from the bottom and from the small nozzles on the wall. The outlet is vertical face pointing to the right of the scene.

A few assumptions that I'm making:
- Since it's a biomass boiler, I'm not modeling combustion. Solid fuel combustion would be too much for this project. Instead, I'm injecting hot air from the primary air duct (below the fuel grate), at the correct temperature so that the overall energy & mass balance is preserved. Also, secondary air is injected in some nozzles (modeled as square openings) throughout the water-wall.
- Firstly I was not using species diffusion, but I decided to recently include them (with same fractions as the flue gas), just to be more precise in the emission/absorption model (CO2 and H2O, mainly).
- The geometry is simple, though slightly big. I'm working with about 1milion elements, refining the mesh around high velocity regions (few cm from the secondary air inlets), and around a geometric detail inside the domain. This detail is where most of the elements are spent: it consists of 30 tubes appended to the water-wall, next to each other. To capture this detail I needed very fine elements around it.

I'm running a transient (Euler) simulation, with Courant number kept below 0,9 for stability.

Let me know if you need more details.

The main investigation now is whether the results from the Laminar model are somewhat better than the uRANS ones (Realizable kEpsilon, with default parameters). The results from the Laminar model are more consistent with what I'm observing in the field and with what I was expecting to see. Based on the uRANS ones, I'd be on the very edge of my argumentation, risking to invalidate my main hypothesis for the problem.

To be honest, 1 million nodes seems to be a too low resolution to trust in the results.

However, you have to realize that the variables resolved in URANS cannot be compared to those you get from a no-model LES. They are apple vs onion...

First of all, are you able to get some probe into the domain and register the values for a long time? At least you could get the temporal spectra in some points far from the walls.
Second, what are the parameters you can use for comparisons?(experimentla data?)

[JulioPieri]

Originally Posted by FMDenaro

To be honest, 1 million nodes seems to be a too low resolution to trust in the results.

However, you have to realize that the variables resolved in URANS cannot be compared to those you get from a no-model LES. They are apple vs onion...

First of all, are you able to get some probe into the domain and register the values for a long time? At least you could get the temporal spectra in some points far from the walls.
Second, what are the parameters you can use for comparisons?(experimentla data?)

You mean that the uRANS tries to account for the influence (through modeling) of the lower scale turbulence, whereas the Laminar skips it?
I do have some probes, but they didn't run for long time yet, only about 100 registries.

I have 4 probes placed in the physical boiler that I have historical data for comparison. Also, there is the expected peak temperature at the outlet (above which would nucleate the slag) - it does occur in the laminar case, but doesn't in the uRANS, by a difference of as much as 200 degrees. It's, however, a loose end of the model: as I tweek the film-coefficient of the wall tubes, this value can easily change.

[FMDenaro]

Originally Posted by JulioPieri

You mean that the uRANS tries to account for the influence (through modeling) of the lower scale turbulence, whereas the Laminar skips it?
I do have some probes, but they didn't run for long time yet, only about 100 registries.

I have 4 probes placed in the physical boiler that I have historical data for comparison. Also, there is the expected peak temperature at the outlet (above which would nucleate the slag) - it does occur in the laminar case, but doesn't in the uRANS, by a difference of as much as 200 degrees. It's, however, a loose end of the model: as I tweek the film-coefficient of the wall tubes, this value can easily change.

URANS solution is based on the idea of a time-averaging or ensemble-averaging. Thus, the variables differs from the LES no-model where you have a spatially filtered variable.



A better comparison would be to integrate both along a certain period of time, that is trynig to get the statistically steady fields.


However, I suspect you have problems in your setting.
Try to do the spectra from the sampled temporal data.


No further measured parameters to compare?

[JulioPieri]

Originally Posted by FMDenaro

URANS solution is based on the idea of a time-averaging or ensemble-averaging. Thus, the variables differs from the LES no-model where you have a spatially filtered variable.



A better comparison would be to integrate both along a certain period of time, that is trynig to get the statistically steady fields.


However, I suspect you have problems in your setting.
Try to do the spectra from the sampled temporal data.


No further measured parameters to compare?

Do you think the spatially filter variables in a course mesh like mine would be "too filtered", thus leading to meaningless results?

At the outlet, the statistically steady fields show a reasonably distributed temperature. However, since peaks in temperature is what causes the problem in the boiler, I'd say the instantaneous field is what should be analyzed, don't you think?

What setting you suspect I might be doing wrong?

I'll process the data to get the spectral info and post it here later today or tomorrow.

I don't have any other parameter to compare. Actually, I do have air flow, and other typical boiler operational parameters, but they are dependent on instruments that might not be properly calibrated.

[FMDenaro]

Originally Posted by JulioPieri

Do you think the spatially filter variables in a course mesh like mine would be "too filtered", thus leading to meaningless results?

At the outlet, the statistically steady fields show a reasonably distributed temperature. However, since peaks in temperature is what causes the problem in the boiler, I'd say the instantaneous field is what should be analyzed, don't you think?

What setting you suspect I might be doing wrong?

I'll process the data to get the spectral info and post it here later today or tomorrow.

I don't have any other parameter to compare. Actually, I do have air flow, and other typical boiler operational parameters, but they are dependent on instruments that might not be properly calibrated.

A too large filters size (that is grid size) has effects in the range of resolved components but this is not the only effect.

I don't know the type of discretizzation and the accuracy order you adopted but that will cause a further filtering effect.

Then, depending on the scheme, the action of the local truncation error can be diffusive, dispersive, dissipative ...without an explicit turbulent model you should consider that is the local truncation error that acts.



Your geometry is quite simple but the flow is complex.



As general rules, the LES with an explicit model adopts a typical grid size h+ =O(20-30) along directions of homogenity but several nodes at y+ <1 along normal-to walls direction.

Thus a further question is if you use wall modelled BCs.


In any case, you don't have experimental measurements to validate your simulation, therefore you have to assess the validity of your solution using all the items you can do. That is also a grid refinement with millions of nodes.

[JulioPieri]

Originally Posted by FMDenaro

A too large filters size (that is grid size) has effects in the range of resolved components but this is not the only effect.

I don't know the type of discretizzation and the accuracy order you adopted but that will cause a further filtering effect.

Then, depending on the scheme, the action of the local truncation error can be diffusive, dispersive, dissipative ...without an explicit turbulent model you should consider that is the local truncation error that acts.



Your geometry is quite simple but the flow is complex.



As general rules, the LES with an explicit model adopts a typical grid size h+ =O(20-30) along directions of homogenity but several nodes at y+ <1 along normal-to walls direction.

Thus a further question is if you use wall modelled BCs.


In any case, you don't have experimental measurements to validate your simulation, therefore you have to assess the validity of your solution using all the items you can do. That is also a grid refinement with millions of nodes.

I see... So I might be too optimistic when seeing the results from unresolved DNS. I'm mostly using limitedLinear discretization scheme.

Do you think I can extract useful results from my grid as is? Even from a "simple" turb model like KE?

I'm using wall functions at the BCs for the turbulence quantities.

One option is that I might be able to simplify the geometry by removing the tubes inside the domain (either completely, or replacing it by a porous zone); that would give me a bunch of elements to redistribute throughout the domain. Maybe that will improve the accuracy.

About the lack of data, it is indeed a problem. I'm not expecting to get quantitatively accurate results. I intend to study "trends". I proceed tweeking the parameters to get an abstract "base case" and assess changes from that case. Then, I intend to observe trends of improvement, rather than the _actual_ (quantitative) gain. So, I can say "changing this operational parameter proved to have a good effect on the results, about 10-15% improvement", for instance.

[FMDenaro]

My suggestion is to start simplifying the geometry as much as possible.


But ... it would be good if you first use your code, in no-model condition, to simulate a standard case like the plane channel flow at Re_tau=590. You have a lot of data to compare in terms of velocity profiles, rms and spectra.
This way, you can have an idea of the quality of the code on a well controlled case and then apply it on your specific problem.

[LuckyTran]

How are you deciding that the laminar case is better than RANS with no data? Because the results of the openfoam tutorial is more colorful?

I am distrusting that your laminar case is actually producing better results than the RANS because at the coarse mesh sizes we are talking about, the same spatial structures should be present in the urans as you see in the unsteady laminar case. I feel like there is more human interpretation error than actual CFD error.