[Far]

I was thinking of more smooth mesh. Here it is...

[Bollonga]

Originally Posted by Far

I was thinking of more smooth mesh. Here it it . ...

How are those curved edges made? Splines curves?

[Far]

Blocking > Edit edge (s) > Link edge

Source edge : The edge whose shape you need to copy to other edge.

Target edge : Whose shape is to be changed

Factor : 1 -3 . I've used factor of 3

[Bollonga]

Originally Posted by Far

I have used pressure based coupled solver. Other options used are : High order term relaxation. 2nd order flow scheme. Cournt number 20,000.

up and down boundaries are slip walls. Did not specify the turbulence level, used default settings.

It works for me too! You're the man!

I've applied this same setup with k-epsilon Realizable model to the 3D flat plate case with 70º angle of attack I've been dealing with. It's working too! I think the key is the courant number modification.
How does it afect to increase it from default 200 to 20,000?

What is the different between slip zero shear stress wall and symmetry BC?

I'm using default k and epsilon at the inlet but I'm gonna need to modifiy them. Would this make me change the mesh or reducing even more under-relax factors?

For how long should I maintain the reduced under-relax factors? It's making my simulations pretty slow...

[Far]

I've applied this same setup with k-epsilon Realizable model to the 3D flat plate case with 70º angle of attack I've been dealing with. It's working too! I think the key is the courant number modification.

It is cournt number for pressure-based coupled solver which couples continuity and momentum equation only. So the definition is not same as the cournt number we study in CFD course.

How does it afect to increase it from default 200 to 20,000?

Fluent guide says, you can increase it to 200,000 and it worked for me for transition modelling of low pressure turbine. In fact this model was used first time for the the low pressure turbine case (i can give you that paper which made use of Fluent's pressure based coupled solver) due to fact that there is strong coupling of continuty and momentum equation. And when Simple type algorithms are used (which couples pressure - velocity fields loosely) they introduce errors for this class of problems and make the convergence difficult.

What is the different between slip zero shear stress wall and symmetry BC?

Both are same except that you need plane surface aligned with any plane for symmetry condition while slip condition can be applied to any surface. In fact I use slip condition due to my past practice. Some friends here always use symmetry condition. But in my point of view results should be same.

I'm using default k and epsilon at the inlet but I'm gonna need to modifiy them. Would this make me change the mesh or reducing even more under-relax factors?

Why you want to change them? Do you want to match some test conditions for which you have specific values of turbulence parameters. Any how , you dont need to change any thing.

For how long should I maintain the reduced under-relax factors? It's making my simulations pretty slow..

For pressure based coupled solver, we don't have option for URF!

[Bollonga]

Originally Posted by Far

Why you want to change them? Do you want to match some test conditions for which you have specific values of turbulence parameters. Any how , you dont need to change any thing.

Yes, I need to match some test turbulence conditions.

Originally Posted by Far

For pressure based coupled solver, we don't have option for URF!

In the solution controls panel there's the option to modify explicit relaxation factors for momentum and pressure and under-relaxation factors for density, body forces, k, epsilon and turbulent viscosity. I've reduced to half all that values. Once the solution is converging, can I change them to default without risking the convergence?
Can I change to 2nd order schemes for k and epsilon to get a more accurate solution?

[Far]

In the solution controls panel there's the option to modify explicit relaxation factors for momentum and pressure and under-relaxation factors for density, body forces, k, epsilon and turbulent viscosity. I've reduced to half all that values. Once the solution is converging, can I change them to default without risking the convergence?

Ah those parameters. You can play with them. Generally speaking, I use default values.

Can I change to 2nd order schemes for k and epsilon to get a more accurate solution?

I don't think turbulence needs second order accuracy. If you are not modelling transition type of flows, results wont change much. In transition dominated flows, I have observed no separation at all when used first order turbulence discretization.

Just think, you have already averaged out the quantities and now you want to add the averaged change in mean flow due to turbulence. How accurate would be averaged quantities with 2nd order accuracy . Probably you will get same averaged values

[Bollonga]

Even if it's converging, CD and CL are far from their correct values. I guess I have to let the simulation run longer. The problem is it's too slow!
I'm simulating the transient case for the 70º inclined flat plate with adaptive timestepping from 1e-3 to 1e-6 but it's always take a timesetp between 1e-5 and 1e-6 s. I've put 50 iterations per timestep.
I need at least 1s of simulation and it taking 1 day to do 4e-4s...