[Amit_Pawarpawar]

i am trying to solve flow over cylinder(D=25 mm). Re=35000 so velocity 17.0 m\s.
but i don't understand how to input the targeted Re and custom reference pressure
the solution i got on lines of a test case file shows that refrence pressure was 0.33 and Re in terms of power 6
help me understand how to apply proper freestream properties

[Vino]

Hi Amit,

I am also having some problem with setting FREE STREAM PRESSURE and by default it takes as "pressure=density*vel*vel".

[hlk]

Thank you for your questions
The values that need to be set vary by the model (Euler or navier-stokes), and can be found in the tutorial files.
Euler: to get a desired reynolds number and velocity, calculate the associated freestream pressure, temperature, and mach number. Set these in the config file.

Navier-Stokes: specify the Reynolds number, Reynolds length (reference length used in the reynolds number), mach number, and freestream temperature.

For both, the other values will be calculated by the code. Setting the reference values to something other than 1.0 will nondimensionalize the problem.

[Amit_Pawarpawar]

i have a problem ongoing for a long time, i want to simulate incompressible turbulent flow over a cylinder
target Re is 35000
Cylinder dia is 30 mm
freestream velocity is 17.038 m/s
but i cant get the result matching the igarshi curve for pressure coefficient

[hlk]

For an example of incompressible RANS config file settings, please see the TestCases/incomp_rans folder.

Separation and the transition to turbulence are classically difficult to predict, and are sensitive to factors such as grid refinement, choice of turbulence model, and 3-d effects.

[Amit_Pawarpawar]

but with the same grid i got the result in fluent

[hlk]

Originally Posted by Amit_Pawarpawar

but with the same grid i got the result in fluent

What configuration settings are you using? Is the solution slightly different or not converging at all?

For the incompressible solver, the reynolds length is always set to 1.0, make sure you have calculated your reynolds number as per meter to take that into account.
Some other things to try are to double check your boundary conditions, which turbulence model you are using, and whether the solution is converged.

[Amit_Pawarpawar]

i m trying SST model. does it mean i have to manipulate my velocity to achieve the targeted Re number.
what cfg details you want
please share your email-id i will mail you cfg file

[hlk]

whoops, my apologies, it looks the most recent version does use the freestream values rather than the Reynolds number, go ahead and specify the freestream values that produce the Reynolds number you're looking for.
Have you set KIND_TURB_MODEL to SST, and other problem definition settings similar to TestCases/incomp_rans/naca0012?
If it is a problem with convergence, try lowering the CFL number.

[Vino]

Hi hlk,

I am doing the Artificial compressibility based incompressible flow simulation using SU2. I tried the default cylinder test case(incomp_navierstokes) using artificial compressibility method and I am getting negative pressure values. I would like to know whether it is a bug in the solver or something else. Your help will be very valuable for me to further progress in my work.

[fpalacios]

Originally Posted by Vino

Hi hlk,

I am doing the Artificial compressibility based incompressible flow simulation using SU2. I tried the default cylinder test case(incomp_navierstokes) using artificial compressibility method and I am getting negative pressure values. I would like to know whether it is a bug in the solver or something else. Your help will be very valuable for me to further progress in my work.

Hi,

Please note that the pressure at the infinity is 0, so we are measuring relative changes of the pressure with respect to the value at the infinity (for that reason, a negative number makes sense).

Do not forget that there is a nondimensionalization in the code

-- Input conditions:
Bulk modulus: 142000 Pa.
Artificial compressibility factor: 1 Pa.
Free-stream pressure: 0 Pa.
Free-stream density: 998.2 kg/m^3.
Free-stream velocity: (8e-06, 0) m/s. Magnitude: 8e-06 m/s.
Free-stream viscosity: 0.000798 N.s/m^2.
-- Reference values:
Reference pressure: 6.38848e-08 Pa.
Reference density: 998.2 kg/m^3.
Reference velocity: 8e-06 m/s.
Reference length: 1 m.
Reference viscosity: 0.0079856 N.s/m^2.


So... to compute the pressure in Pascal you should multiply the pressure value by the reference pressure and then add the value to the pressure at the infinity.

Thanks for using SU2,

Cheers,
Francisco

[Vino]

Thank you.

Is it possible to set the Reference pressure as well as Free stream pressure to 101325 pa ?

[Vino]

Hi,

I would like to simulate incompressible turbulent Backward facing step and I need to give variable velocity profile(ex: parabolic) at inlet of the domain. I could not find any such tutorial problems. Can someone tell me how to set it in config file?

Thanks in advance.!!!

[fpalacios]

Originally Posted by Vino

Hi,

I would like to simulate incompressible turbulent Backward facing step and I need to give variable velocity profile(ex: parabolic) at inlet of the domain. I could not find any such tutorial problems. Can someone tell me how to set it in config file?

Thanks in advance.!!!

For the time being you should manual change the subroutine
void CEulerSolver::BC_Inlet(CGeometry *geometry, CSolver **solver_container,
CNumerics *conv_numerics, CNumerics *visc_numerics, CConfig *config, unsigned short val_marker) {

in particular, in line 6844 (solver_direct_mean.cpp) you can specify the value of the velocity. As you probably know you can get the value of the y coordinate using
double YCoord = geometry->node[iPoint]->GetCoord(1);

I hope this help,

Best,
Francisco