[RaulCA]

Originally Posted by zahraseif

Hi Raul,

Thank you for your feedback. To me, it seems that nCellsPerEddy should be a parameter to control the eddy density parameter mentioned in the paper (d), but it seems that in OpenFOAM implementation we only have this parameter to control the eddy density. It is not very straightforward to understand although. I hope we can get more into this BC through this forum.

Regards,

Zahra

Hello Zahra,
Although it is not documented, the BC looks for the variable d that specifies the eddy density, and if not found it defaults to 1. You can put it in the BC dict and you will see that the volume of eddies generated will vary.
As I explained in the previous post, delta and nCellsPerEddy are to create an upper and lower bound for L respectively. In the initialization L is calculated as:

L=max(nCellsPerEddy*localMeshSize, min(L, kappa*delta))

where kappa is the vonKarman constant
I'm interested in the validation you are talking about, did you make it for the channel395 or did you try for other cases with different scales? Did you apply the correction in the source code for C1 as someone in this thread pointed out?

[zahraseif]

Originally Posted by RaulCA

Hello Zahra,
Although it is not documented, the BC looks for the variable d that specifies the eddy density, and if not found it defaults to 1. You can put it in the BC dict and you will see that the volume of eddies generated will vary.
As I explained in the previous post, delta and nCellsPerEddy are to create an upper and lower bound for L respectively. In the initialization L is calculated as:

L=max(nCellsPerEddy*localMeshSize, min(L, kappa*delta))

where kappa is the vonKarman constant
I'm interested in the validation you are talking about, did you make it for the channel395 or did you try for other cases with different scales? Did you apply the correction in the source code for C1 as someone in this thread pointed out?

Hi Raul,

Thank you again for your further discussion. Yes, you are right about the fact that eddy density could be provided in the BC setup for DFSEM. Still, I am wondering what would happen if we provide the value for both d and eddy length scales? Since the value for d is evaluated from the eddy length scales. Also, I have observed the effect of the parameter nCellsPerEddy on the level of the fluctuations and downstream flow development and turbulence decay. That's why I presumed that this parameter also controls the inlet eddy characteristics.

About the C1, I did not change that. I tried DFSEM with OpenFOAM versions of 1712 and 1906. It seems that in the latest version they made the correction, since I was not able at all to validate my results with v1712. And yes, I did my validation with channel395 test case.

Regards,

Zahra

[RaulCA]

Originally Posted by zahraseif

Hi Raul,

Thank you again for your further discussion. Yes, you are right about the fact that eddy density could be provided in the BC setup for DFSEM. Still, I am wondering what would happen if we provide the value for both d and eddy length scales? Since the value for d is evaluated from the eddy length scales. Also, I have observed the effect of the parameter nCellsPerEddy on the level of the fluctuations and downstream flow development and turbulence decay. That's why I presumed that this parameter also controls the inlet eddy characteristics.

About the C1, I did not change that. I tried DFSEM with OpenFOAM versions of 1712 and 1906. It seems that in the latest version they made the correction, since I was not able at all to validate my results with v1712. And yes, I did my validation with channel395 test case.

Regards,

Zahra

Hello Zahra,
just to clarify some things. Indeed the eddy length scales and eddy density are related, but you must provide both of them. Eddy length scales "L" must be specified because the BC must know the sizes of the eddies it has to input, and eddy density is 1 by default unless different value is provided. Then, eddy density is calculated dividing the sum of the volumes of all the eddies by the volume of the BC "Eddy Box". The point is that the BC doesn't know how many eddies it has to input, so what it does is start adding eddies to the domain. With every eddy added, the eddy total volume will increase and the eddy density too. It only stops adding eddies when the eddy density is equal or larger than the specified eddy density "d" (that defaults to 1 if not provided).

About the C1 change, it is related to the scale of the domain. It works well for the channel395 case but for bigger domains people encountered high velocities due to bad scaling of the C1 parameter (and I didn't see any changes in v1912).

[zahraseif]

Originally Posted by RaulCA

Hello Zahra,
just to clarify some things. Indeed the eddy length scales and eddy density are related, but you must provide both of them. Eddy length scales "L" must be specified because the BC must know the sizes of the eddies it has to input, and eddy density is 1 by default unless different value is provided. Then, eddy density is calculated dividing the sum of the volumes of all the eddies by the volume of the BC "Eddy Box". The point is that the BC doesn't know how many eddies it has to input, so what it does is start adding eddies to the domain. With every eddy added, the eddy total volume will increase and the eddy density too. It only stops adding eddies when the eddy density is equal or larger than the specified eddy density "d" (that defaults to 1 if not provided).

About the C1 change, it is related to the scale of the domain. It works well for the channel395 case but for bigger domains people encountered high velocities due to bad scaling of the C1 parameter (and I didn't see any changes in v1912).

Hello Raul,

Thank you again for continuing this discussion and your explanation. As I clearly observed the effect of the parameter nCellsPerEddy by changing it from 1 to 3 and 5 on the level of the fluctuations and downstream flow development, I am a bit confused if this parameter effects d, since it can affect L, and therefore d will not remain constant with changing this parameter. In the paper, the effect of d was emphasized on downstream flow development, what I observed was the effect of nCellsPerEddy. Thank you for letting me know your opinion.

Regards,

Zahra

[XJ_Wang]

Hi Gang,

How did you prepare R and L before running the simulation? In another post, Michael said he got the R by running a k-e model and then extract the R value by postprocessing. Could you please give me some instructions? Thank you very much!

[HPE]

Hi,

- You can extract the Reynolds stress tensor (R) field in many ways. One way is to use turbulenceFields function object.

Hope it helps.

[XJ_Wang]

Thanks, Herpes!

It seems that I have to do a RANS simulation before my LES simulation to get the R(Reynolds stress tensor) and L(turbulent length) since I don't have the experimental data. Am I right?

I was wondering except postprocessing of RANS simulation, is there another way to get the R and L for this inlet method?

Thank you very much!
Cheers,
Xiangjie

[HPE]

- Yes.
- You can do estimations for R and L based on the literature.

[XJ_Wang]

Thank you Herpes!

Now without the experimental data, I think it's an easy way to get the R and L by RANS simulation instead of estimating them.

I just went through Poletto's paper for another time and found that in his paper, he said the R and L could be obtained by RANS.

Cheers!
Xiangjie

[Sandeep lamba]

Originally Posted by XJ_Wang

Thank you Herpes!

Now without the experimental data, I think it's an easy way to get the R and L by RANS simulation instead of estimating them.

I just went through Poletto's paper for another time and found that in his paper, he said the R and L could be obtained by RANS.

Cheers!
Xiangjie

Hi, I am just starting working with DFSEM turbulent inlet boundary conditions for LES. can anyone please guide me how to extract R and L from RANS data?
I am also confused if I need to extract it for whole domain or just at the inlet. Actually in one tutorial I noticed that we can give these values in tabular form.

Kind regards

[HPE]

You can use the turbulenceFields function object to extract the R and L data.

You need to provide entries for the boundary only, not the entire domain.

One of the pimpleFoam/LES tutorials exemplify this. Please search it (Cant recall its name, but it is not the chan395DFSEM tutorial.)

[mAlletto]

Usually one runs a rans simulation and extracts R and L at the plane of interest. The inlet should be avoided since a fully developed flow is desirable. For a channel flow the outlet is a good location to extract R and L. I think there is also a thread here which discusses it. A bit of googling Will help to find it

[chen112p]

Does anyone experience HUGE pressure fluctuation in the domain when using DFSEM with a incompressible solver (pimple)? In the attachment there's U field and p field i recorded from the center plane of one simple channel flow (left: inlet, top: symmetry, sides (not showing): symmetry, right: outlet, bottom: wall).

I found this issue when I was using timeVaryingMappedFixedValue boundary condition to inject a recorded time series of velocity field into the domain.

[Sandeep lamba]

Originally Posted by chen112p

Does anyone experience HUGE pressure fluctuation in the domain when using DFSEM with a incompressible solver (pimple)? In the attachment there's U field and p field i recorded from the center plane of one simple channel flow (left: inlet, top: symmetry, sides (not showing): symmetry, right: outlet, bottom: wall).

I found this issue when I was using timeVaryingMappedFixedValue boundary condition to inject a recorded time series of velocity field into the domain.

I experienced similar behaviour. What boundary conditions you are using at outlet for U and p?

[chen112p]

I used inletOutlet for U and fixedValue with value 0 for pressure, pretty standard.

[mAlletto]

Originally Posted by chen112p

Does anyone experience HUGE pressure fluctuation in the domain when using DFSEM with a incompressible solver (pimple)? In the attachment there's U field and p field i recorded from the center plane of one simple channel flow (left: inlet, top: symmetry, sides (not showing): symmetry, right: outlet, bottom: wall).

I found this issue when I was using timeVaryingMappedFixedValue boundary condition to inject a recorded time series of velocity field into the domain.

Usually you have huge pressure variation right at the inlet if your inlow velocity does not satisfy the continuity equation.