[amir_14]

hi dear friend
i have 2 question (PLZ)

1.how can i define the wall spacing to the first grid point from an airfoil surface in ansys?

2.how can i partition my computational grid into to two zones to predict laminar to turbulent transitions ?

[cfd seeker]

1.how can i define the wall spacing to the first grid point from an airfoil surface in ansys?

Which software you are using for meshing? structured or unstructured grid?

2.how can i partition my computational grid into to two zones to predict laminar to turbulent transitions ?

Why you want to partition your grid for the said purpose? Fluent has incorporated two new turbulence models i.e k-kl-w(3 eqs) and transition kw(4 eqs) to capture laminar to turbulent transition. For these models there is no need to partition your grid. You should only worru about proper wall y+(<1) and proper stream-wise mesh resolution.

[cfd seeker]

1.how can i define the wall spacing to the first grid point from an airfoil surface in ansys?

Which software you are using for meshing? structured or unstructured grid?

2.how can i partition my computational grid into to two zones to predict laminar to turbulent transitions ?

Why you want to partition your grid for the said purpose? Fluent has incorporated two new turbulence models i.e k-kl-w(3 eqs) and transition kw(4 eqs) to capture laminar to turbulent transition. For these models there is no need to partition your grid. You should only worru about proper wall y+(<1) and proper stream-wise mesh resolution.

[amir_14]

Originally Posted by cfd seeker

Which software you are using for meshing? structured or unstructured grid?


Why you want to partition your grid for the said purpose? Fluent has incorporated two new turbulence models i.e k-kl-w(3 eqs) and transition kw(4 eqs) to capture laminar to turbulent transition. For these models there is no need to partition your grid. You should only worru about proper wall y+(<1) and proper stream-wise mesh resolution.

tnx cfd seeker

i am using ansis workbench for a structured grid
can you help me for a better software?


i want survey laminar separation bubble at low angle of attack on an airfoil with Spalart-Allmaras model,
in this condition a laminar to turbulent transitions occurs

[cfd seeker]

can you help me for a better software?

ICEM CFD

i want survey laminar separation bubble at low angle of attack on an airfoil with Spalart-Allmaras model,
in this condition a laminar to turbulent transitions occurs

Laminar separation is something else and transition is something else...What is the Re. No of your simulation?

[amir_14]

Originally Posted by cfd seeker

ICEM CFD


Laminar separation is something else and transition is something else...What is the Re. No of your simulation?

yes
Re is 100000
i want model Laminar separation on airfoil that Continues to turbulent


i try to do this:

"Simple RANS modeling lacks the ability to accurately predict laminar to turbulent transitions. It is typical that when using RANS modeling, the transition location is specified by the user. In FLUENT, this was done by partitioning the computational grid into to two zones. The location of the partition varies depending on the location of the laminar separation, which is analogous to the angle of attack to the airfoil. The partition is placed at the location that causes the greatest aerodynamic performance loss while still forming the separation bubble for each selected angle of attack."

[cfd seeker]

"Simple RANS modeling lacks the ability to accurately predict laminar to turbulent transitions. It is typical that when using RANS modeling, the transition location is specified by the user. In FLUENT, this was done by partitioning the computational grid into to two zones. The location of the partition varies depending on the location of the laminar separation, which is analogous to the angle of attack to the airfoil. The partition is placed at the location that causes the greatest aerodynamic performance loss while still forming the separation bubble for each selected angle of attack."

I agree with this but these quotes were valid when I was still a school boy
I have already told you that now fluent has incorporated two new RANS turbulence models which are capable of capturing laminar to turbulent transition. Read the Theory/ Modelling guide of Fluent 12 and onwards, you will find a nice materials on these turbulence models. Do concentrate on reading especially the grid requirements for these models which are obviously the difficult part in the process

[Ebrahim]

Hi Amir

1. if you want to find it in your solver(for example FLUENT), and if you use a turbulence model, you can easily find the distance of near wall cells to the walls by using the known values of u_star and y_plus.

2. do you want to partition it before solving the flow or during the flow solution? in other words, do you know the boundary of the 2 partitions?

[amir_14]

Originally Posted by Ebrahim

Hi Amir

1. if you want to find it in your solver(for example FLUENT), and if you use a turbulence model, you can easily find the distance of near wall cells to the walls by using the known values of u_star and y_plus.

2. do you want to partition it before solving the flow or during the flow solution? in other words, do you know the boundary of the 2 partitions?

hi dear Ebrahim
tanx for your answer

[Far]

I have done some projects on the Low pressure turbine transition prediction and passive control of separation (see the signature below) and got good resutls.

Now I am working on the validation of three equation model (K, Kl, w aka walter's model) and SST transition model (4 eq). I usually follow these guidelines:

1. Walter model gives the laminar to turbulent transition in very less no of iterations. order of 1 to 2 no of iterations was observed

2. Walter model works satisfactorily in steady state mode.

3. Use second order equations for all turbulence quantities including momentum equation.

4. Atleast 40 (may be up to 100) nodes in side boundary layer are needed along with stream-wise mesh refinement at the expected location of transition. Keep the expansion rate below 1.15.

5. For the prediction of vortex shedding inside the boundary layer and downstream use the fine time step (order of 1 to 10 micro-second)

6. Use the flat plate turbulent boundary layer formulae to estimate the first cell height (Y+) and total boundary layer thickness. This step needs some trail and error.

7. Keep in mind laminar boundary layer is thinner than the turbulent boundary for same Reynolds number (considering the point 6). Also boundary layer thickness is inversely proportional to Reynolds no.

8. You dont need the two zones.

[amir_14]

Originally Posted by Far

I have done some projects on the Low pressure turbine transition prediction and passive control of separation (see the signature below) and got good resutls.

Now I am working on the validation of three equation model (K, Kl, w aka walter's model) and SST transition model (4 eq). I usually follow these guidelines:

1. Walter model gives the laminar to turbulent transition in very less no of iterations. order of 1 to 2 no of iterations was observed

2. Walter model works satisfactorily in steady state mode.

3. Use second order equations for all turbulence quantities including momentum equation.

4. Atleast 40 (may be up to 100) nodes in side boundary layer are needed along with stream-wise mesh refinement at the expected location of transition. Keep the expansion rate below 1.15.

5. For the prediction of vortex shedding inside the boundary layer and downstream use the fine time step (order of 1 to 10 micro-second)

6. Use the flat plate turbulent boundary layer formulae to estimate the first cell height (Y+) and total boundary layer thickness. This step needs some trail and error.

7. Keep in mind laminar boundary layer is thinner than the turbulent boundary for same Reynolds number (considering the point 6). Also boundary layer thickness is inversely proportional to Reynolds no.

8. You dont need the two zones.

tanx dear far
I want model flow over on a s809 airfoil @ some angle off attack from 2 to 20
Should i predict laminar to turbulent transition location for low angle?

[Far]

but at higher angles still you have laminar flow at leading edge ! isnt it?

If at the higher angles transition models fail, so do the base line two equation models.

You may be required to run the case as unsteady at higher AOA

[amir_14]

Originally Posted by Far

but at higher angles still you have laminar flow at leading edge ! isnt it?

If at the higher angles transition models fail, so do the base line two equation models.

You may be required to run the case as unsteady at higher AOA

yes, it occurs at higher angles
can any turbulence models in fluent model this flow at all angle of attack?
with spalart-allmaras model i should specify transition location but i have't this data for 10^5 Re.
can you help me about this and "Walter model"?

[Far]

Here we have used SST gamma theta model
http://asmedl.org/getabs/servlet/Get...ifs=yes&ref=no

Now I am applying the walters model and will show you some results. As far settings are concerned I have already mentioned above and there is no constant which you need to set for this model.