[Time4Tea]

Hi, something I have been wondering about is what would be the expected effect of using a mesh that is too coarse, particularly with regards to the 'drag' measured through a valve? Realizable k-epsilon is the turbulence model that I am particularly interested in.

My thinking is that an overly coarse mesh would probably add in some artificial 'numerical viscosity', because it will model the boundary layer as being thicker than it really is. Also, it will probably give a bad prediction of boundary layer attachment as the flow turns round corners. Therefore, the drag would tend to be too high, and so it would under-predict the flow rate through a valve for a given pressure drop.

Does that sound correct, or is there a flaw in my reasoning?

[FMDenaro]

Originally Posted by Time4Tea

Hi, something I have been wondering about is what would be the expected effect of using a mesh that is too coarse, particularly with regards to the 'drag' measured through a valve? Realizable k-epsilon is the turbulence model that I am particularly interested in.

My thinking is that an overly coarse mesh would probably add in some artificial 'numerical viscosity', because it will model the boundary layer as being thicker than it really is. Also, it will probably give a bad prediction of boundary layer attachment as the flow turns round corners. Therefore, the drag would tend to be too high, and so it would under-predict the flow rate through a valve for a given pressure drop.

Does that sound correct, or is there a flaw in my reasoning?

The numerical viscosity is an issue appearing from the discretization of the convective terms rather then from the grid (even if it depends on the grid size). Actually, you can have also discretizations that do not produce numerical viscosity. As you are working with RANS formulation, the additional viscosity is produced by the turbulence model. The effect of the grid resolution on the viscous drag can be easily seen by considering the tangential stress that requires the discretization of the normal derivative of the streamwise velocity. If the no-slip condition is prescribed the derivatives depends on the distance of the grid size from the wall. If you do not describe correctly the viscous sub-layer such derivative is poorly computed.

[Time4Tea]

Originally Posted by FMDenaro

The numerical viscosity is an issue appearing from the discretization of the convective terms rather then from the grid (even if it depends on the grid size). Actually, you can have also discretizations that do not produce numerical viscosity. As you are working with RANS formulation, the additional viscosity is produced by the turbulence model. The effect of the grid resolution on the viscous drag can be easily seen by considering the tangential stress that requires the discretization of the normal derivative of the streamwise velocity. If the no-slip condition is prescribed the derivatives depends on the distance of the grid size from the wall. If you do not describe correctly the viscous sub-layer such derivative is poorly computed.

Ok. So, let's say I use a grid that is very coarse and doesn't adequately resolve the boundary layer (no inflation layers, very large wall y+ ...), does that mean the computed velocity gradient at the wall would be too low? I.e. it would actually under-estimate the frictional drag?


Would it also depend on what type of wall function I use? Most typically, I use standard or non-equilibrium wall functions in FLUENT for the valves I analyze.

[FMDenaro]

Originally Posted by Time4Tea

Ok. So, let's say I use a grid that is very coarse and doesn't adequately resolve the boundary layer (no inflation layers, very large wall y+ ...), does that mean the computed velocity gradient at the wall would be too low? I.e. it would actually under-estimate the frictional drag?


Would it also depend on what type of wall function I use? Most typically, I use standard or non-equilibrium wall functions in FLUENT for the valves I analyze.

- yes, the stress should result lower than the actual


- If you apply any sort of wall modelled BCs (instead of the natural no-slip velocity BC) there is no further discussion about the stress at the wall: you are somehow already prescribing it and you do not describe the viscous sub-layer. Thus, you cannot pretend to predict what you have already prescribed as BC.

[Time4Tea]

Originally Posted by FMDenaro

- If you apply any sort of wall modelled BCs (instead of the natural no-slip velocity BC) there is no further discussion about the stress at the wall: you are somehow already prescribing it and you do not describe the viscous sub-layer. Thus, you cannot pretend to predict what you have already prescribed as BC.

I'm not sure I fully understand what you are saying here:


- Surely, even with a wall function, the non-slip condition at the wall still has to be respected?


- Also, doesn't the near-wall velocity profile that is modeled by the function still have to be determined by the solver, based on the wall y+ and 'free-stream' velocity? So, how is the wall shear stress being 'prescribed' in that situation, where a wall function is being used?

[FMDenaro]

Originally Posted by Time4Tea

I'm not sure I fully understand what you are saying here:


- Surely, even with a wall function, the non-slip condition at the wall still has to be respected?


- Also, doesn't the near-wall velocity profile that is modeled by the function still have to be determined by the solver, based on the wall y+ and 'free-stream' velocity? So, how is the wall shear stress being 'prescribed' in that situation, where a wall function is being used?

Generally speaking, the wall modelled BCs do not prescribe the no-slip velocity at the wall (y+=0)! Conversely, it is assumed you have a fully developed averaged velocity profile and considers the wall line like a fluid line at some y+ value. In other words, you cannot think to predict the drag when you are assuming that you already know a specific type of velocity profile.
Of course, the flow behind a valve is very far to be similar to the assumed wall laws.
I suggest to serach for similar posts in this forum

[Time4Tea]

Originally Posted by FMDenaro

Generally speaking, the wall modelled BCs do not prescribe the no-slip velocity at the wall (y+=0)! Conversely, it is assumed you have a fully developed averaged velocity profile and considers the wall line like a fluid line at some y+ value. In other words, you cannot think to predict the drag when you are assuming that you already know a specific type of velocity profile.
Of course, the flow behind a valve is very far to be similar to the assumed wall laws.
I suggest to serach for similar posts in this forum

Hmm. What you say is interesting and it differs from my understanding of how the k-epsilon wall functions work. I will have to do some more background reading into the subject.


My understanding is that the wall function is assuming a known normalized velocity profile in the boundary layer, but that the profile still has to be scaled during the solution to give an accurate representation of the boundary layer thickness. So, it seems to me that the predicted shear stress might still depend on the mesh resolution. However, perhaps I have some misconception.


Out of interest, what type of RANS turbulence model/wall function would you recommend for modeling an industrial flow through a globe-type control valve (which has a lot of swirling and separation)?

[FMDenaro]

Originally Posted by Time4Tea

Hmm. What you say is interesting and it differs from my understanding of how the k-epsilon wall functions work. I will have to do some more background reading into the subject.


My understanding is that the wall function is assuming a known normalized velocity profile in the boundary layer, but that the profile still has to be scaled during the solution to give an accurate representation of the boundary layer thickness. So, it seems to me that the predicted shear stress might still depend on the mesh resolution. However, perhaps I have some misconception.


Out of interest, what type of RANS turbulence model/wall function would you recommend for modeling an industrial flow through a globe-type control valve (which has a lot of swirling and separation)?

When you assume that only a "scaling" must be determined on a know velocity profile what do you think are you prescribing? The key to understand is that a fully developed boundary layer profile is supposed and of course this is not true in a lot of wall turbulence flows.

The flow around a valve is rich of separated flow region, a case in which DES/LES is suitable.

[Time4Tea]

Originally Posted by FMDenaro

When you assume that only a "scaling" must be determined on a know velocity profile what do you think are you prescribing? The key to understand is that a fully developed boundary layer profile is supposed and of course this is not true in a lot of wall turbulence flows.

The flow around a valve is rich of separated flow region, a case in which DES/LES is suitable.

As I understand it, the prescribed velocity profile has to 'match up' with the free-stream velocity away from the wall, which is calculated during the solution. Otherwise, the velocity profile would be discontinuous and unrealistic. That is what I meant by 'scaling': the normalized velocity profile is fixed (u+ = y+ in the viscous sublayer), but u+ is normalized by the free-stream velocity. Even in a fully-developed boundary layer, the wall shear stress will be higher, if the free-stream velocity is higher.



I see what you mean though, that a fully-developed boundary layer is assumed, which will not be accurate in some situations.


So, you would not recommend using RANS at all for modeling flow through a valve? I agree that DES/LES would be ideal; however, I don't think they are really practical in an industrial setting.

[FMDenaro]

Originally Posted by Time4Tea

As I understand it, the prescribed velocity profile has to 'match up' with the free-stream velocity away from the wall, which is calculated during the solution. Otherwise, the velocity profile would be discontinuous and unrealistic. That is what I meant by 'scaling': the normalized velocity profile is fixed (u+ = y+ in the viscous sublayer), but u+ is normalized by the free-stream velocity. Even in a fully-developed boundary layer, the wall shear stress will be higher, if the free-stream velocity is higher.



I see what you mean though, that a fully-developed boundary layer is assumed, which will not be accurate in some situations.


So, you would not recommend using RANS at all for modeling flow through a valve? I agree that DES/LES would be ideal; however, I don't think they are really practical in an industrial setting.

You can read about the wall functions and the limits in this approach in the book of Wilcox.



Considering at present DES/LES for a flow around a valve should be considered almost mandatory at present, even in industrial applications.

This study (https://www.researchgate.net/publica...utomobile_2003) was done 16 years ago on a notebook, almost as a joke, don't you think that now the computational power can do better ??

[Time4Tea]

Originally Posted by FMDenaro

You can read about the wall functions and the limits in this approach in the book of Wilcox.

Considering at present DES/LES for a flow around a valve should be considered almost mandatory at present, even in industrial applications.

This study (https://www.researchgate.net/publica...utomobile_2003) was done 16 years ago on a notebook, almost as a joke, don't you think that now the computational power can do better ??

Thank you for linking that paper, it is very interesting. I am curious though, how many cells did the mesh contain (approximately)? Also, how finely was the near-wall region modeled (what was the wall y+)? (I didn't see those mentioned in the text).

Comparing that example to the valves that I simulate on a daily/weekly basis, I have to say the valves I work with are quite a lot more complex than that geometrically. Typically, I use a half-symmetric model with 5-10 inflation layers (maximum wall y+ about 200). The cell count is typically in the range of 5-6 million cells.

I work for a large multinational and have access to a modern supercomputer. Using 40 cores, a steady, incompressible solution in FLUENT using RANS (k-epsilon) takes about an hour to an hour and a half.

The thing is, it's not just about the solving time. There is also time involved with set-up, pre- and post-processing. I would expect LES to take longer to solve, as it is transient, especially if the boundary layer needs to be more finely modeled. But then, on top of that, there will be more processing time required to deal with transient results, averaging, etc. Plus, the large increase in the amount of data that will be generated and need to be stored/handled, compared to a simple, steady result.

Of course, I accept that DES/LES would be more accurate than RANS in most situations. But, if it will increase the amount of time to setup and perform a solution by 3-4x, then that just isn't practical for me, given the time and resource constraints that I have to work under. I often need to do 5, 6 or more valve internal flow simulations in a week.

That is why I was asking, if I have to use RANS due to my constraints (even though it is not as accurate), what turbulence model and wall modeling method would you recommend for an internal (incompressible) flow through a control valve?