Dear all,
I am trying to find out the role that this following parameters play on the initialization of the turbulent flow and whether they affect one another. I am using a k-w SST(2 scales model):
1) Reference length in Reference values: Does it play a role in the calculation of the specific dissipation rate (w)?
2) Reference velocity in Reference values: Does it play a role in the calculation of the turbulent kinetic energy (k)?
3) How value to set for the hydraulic diameter, which I have to impose in the boundary condition under Turbulence (Calculation by turbulent intensity), for a problem of external hydrodynamic ?
Best Regards,
FA
Initializing turbulent flow
Forum rules
Please read the forum usage recommendations before posting.
Please read the forum usage recommendations before posting.
-
Martin FERRAND
- Posts: 47
- Joined: Wed Mar 14, 2012 10:06 am
Re: Initializing turbulent flow
Hello,
Concerning the initialisation you can read paragraph 6.3 of the user guide of version 5.0 for instance.
Concerning the inlet BC for turbulence, you can either chose established profile with an hydraulic diameter given by the user, or hydraulic diameter and a turbulence intensity.
See for instance the Doxygen doc:
https://www.code-saturne.org/cms/sites/ ... _diam.html
Best Regards
Martin
Concerning the initialisation you can read paragraph 6.3 of the user guide of version 5.0 for instance.
Concerning the inlet BC for turbulence, you can either chose established profile with an hydraulic diameter given by the user, or hydraulic diameter and a turbulence intensity.
See for instance the Doxygen doc:
https://www.code-saturne.org/cms/sites/ ... _diam.html
Best Regards
Martin
Re: Initializing turbulent flow
Hi Martin,
Thank you for your answer.
In the user guide I can see clearly how k and w are initialize. I still have few doubts though:
1)The expression for the initialization of k (k=1.5(0.02*UREF)^2) is the same of this more generic expression which I found in literature (k=1.5(U*I)^2) ? In this case I is the turbulent intensity. Comparing the two expression I may infer that 0.02 corresponds to the turbulent intensity I! Is that correct or I have been missing something..?
2) By doing the second calculation of k (https://www.code-saturne.org/cms/sites/ ... _diam.html ) for the inlet boundary conditions implies that another value of k is calculated ( referring to 1))
My doubt is to know how all work togheter?
In my case, because I am doing a code to code comparison with a previous study I would like to impose turbulent intensity( I ) and turbulent viscosity ratio (muT/mu) from which the code calculate (initialization) all the remaining turbulent quantities.
Thank you for your help,
FA
Thank you for your answer.
In the user guide I can see clearly how k and w are initialize. I still have few doubts though:
1)The expression for the initialization of k (k=1.5(0.02*UREF)^2) is the same of this more generic expression which I found in literature (k=1.5(U*I)^2) ? In this case I is the turbulent intensity. Comparing the two expression I may infer that 0.02 corresponds to the turbulent intensity I! Is that correct or I have been missing something..?
2) By doing the second calculation of k (https://www.code-saturne.org/cms/sites/ ... _diam.html ) for the inlet boundary conditions implies that another value of k is calculated ( referring to 1))
My doubt is to know how all work togheter?
In my case, because I am doing a code to code comparison with a previous study I would like to impose turbulent intensity( I ) and turbulent viscosity ratio (muT/mu) from which the code calculate (initialization) all the remaining turbulent quantities.
Thank you for your help,
FA
Re: Initializing turbulent flow
Hi everybody,
Maybe I was not clear enough in the past message. I will try to give you more information:
I do not know what values to give ( if the best strategy is calculation by formula..) to k and w in the BC (inlet) in order to indirectly prescribe turbulent viscosity ratio and turbulent intensity.
I looked in the theory guide whether any equations were available to relate k, omega, turbulent intensity and turbulent viscosity ratio but I have not found anything ( there is something similar though for the k-epsilon model ).
Regards,
FA
Maybe I was not clear enough in the past message. I will try to give you more information:
I do not know what values to give ( if the best strategy is calculation by formula..) to k and w in the BC (inlet) in order to indirectly prescribe turbulent viscosity ratio and turbulent intensity.
I looked in the theory guide whether any equations were available to relate k, omega, turbulent intensity and turbulent viscosity ratio but I have not found anything ( there is something similar though for the k-epsilon model ).
Regards,
FA
Re: Initializing turbulent flow
Hello.
Setting turbulence parameters at the inlet BC may be quite challenging depending on what is your problem (the same is for the pressure field for inlet BCs).
Turbulence parameters are characteristics of the flow, like velocity components and pressure. You cannot just calculate them. These formulae are only very-very rough approximations and are not applicable in many cases.
So if you have the complex velocity/pressure field at the inlet (like a flow past the gas turbine at the duct inlet), you cannot set turbulence as easy as with those simple correlations. Acceptable and easy practical approach may be setting constant values of k and omega based on your experience for particular type of cases. But we consider that the best you can use in most practical cases is zero-gradient for k and omega at the inlet BC (we use mostly Ansys CFX where this is just one of BC options, for Saturne you will need the user subroutine). I compared the results for the swirled flow in conical duct past the gas turbine obtained with CFX (zero gradients for turbulence at BC) and Saturne (constant k and omega based on CFX results at the inlet, very roughly). The match was not perfect but acceptable.
The best you can use is known fields for k and omega at the inlet. But this field is usually not available (in our practice there was just 1 or 2 such cases). Ths's why you can try to obtain this field yourself extending the calculation domain backwards, it it's possible. For example, if you have the inlet somewhere in the duct (channel) you can add the upstream part of the duct to the model and set absolutely plain BC at the inlet of this part. The flow will develop so at your current BC position you will have plausible turbulence field.
It's usually not discussed, but the same thing is actual for the pressure field. When you use the velocity/flow BC you cannot set pressure field and when you use the pressure BC you cannot set velocity. So, in first case, you obtain the inlet pressure field with the CFD code that may be absolutely not applicable to complex flows (for example, for swirling flows). It seems to be the fundamental limitation. Being CFD engineer, you can only accept the fact that, in complex fields, BCs should be placed at some distance from/to the area of interest to allow the flow to "accomodate to geometry", to develop at least correct structure at the inlet of the area of interest. The same is applicable for the general topic of setting any BCs, including outlet ones. This is a part of why CFD results may be user-dependent in many cases.
Setting turbulence parameters at the inlet BC may be quite challenging depending on what is your problem (the same is for the pressure field for inlet BCs).
Turbulence parameters are characteristics of the flow, like velocity components and pressure. You cannot just calculate them. These formulae are only very-very rough approximations and are not applicable in many cases.
So if you have the complex velocity/pressure field at the inlet (like a flow past the gas turbine at the duct inlet), you cannot set turbulence as easy as with those simple correlations. Acceptable and easy practical approach may be setting constant values of k and omega based on your experience for particular type of cases. But we consider that the best you can use in most practical cases is zero-gradient for k and omega at the inlet BC (we use mostly Ansys CFX where this is just one of BC options, for Saturne you will need the user subroutine). I compared the results for the swirled flow in conical duct past the gas turbine obtained with CFX (zero gradients for turbulence at BC) and Saturne (constant k and omega based on CFX results at the inlet, very roughly). The match was not perfect but acceptable.
The best you can use is known fields for k and omega at the inlet. But this field is usually not available (in our practice there was just 1 or 2 such cases). Ths's why you can try to obtain this field yourself extending the calculation domain backwards, it it's possible. For example, if you have the inlet somewhere in the duct (channel) you can add the upstream part of the duct to the model and set absolutely plain BC at the inlet of this part. The flow will develop so at your current BC position you will have plausible turbulence field.
It's usually not discussed, but the same thing is actual for the pressure field. When you use the velocity/flow BC you cannot set pressure field and when you use the pressure BC you cannot set velocity. So, in first case, you obtain the inlet pressure field with the CFD code that may be absolutely not applicable to complex flows (for example, for swirling flows). It seems to be the fundamental limitation. Being CFD engineer, you can only accept the fact that, in complex fields, BCs should be placed at some distance from/to the area of interest to allow the flow to "accomodate to geometry", to develop at least correct structure at the inlet of the area of interest. The same is applicable for the general topic of setting any BCs, including outlet ones. This is a part of why CFD results may be user-dependent in many cases.