
[Sponsors] 
August 1, 2014, 03:45 
incompressible solver

#1 
New Member
Amit
Join Date: Jul 2014
Posts: 11
Rep Power: 4 
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 

August 6, 2014, 17:51 

#2 
Senior Member
Vino
Join Date: Mar 2013
Location: India
Posts: 115
Rep Power: 5 
Hi Amit,
I am also having some problem with setting FREE STREAM PRESSURE and by default it takes as "pressure=density*vel*vel". 

August 9, 2014, 22:33 

#3 
Senior Member
Heather Kline
Join Date: Jun 2013
Posts: 241
Rep Power: 6 
Thank you for your questions
The values that need to be set vary by the model (Euler or navierstokes), 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. NavierStokes: 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. 

August 20, 2014, 02:05 

#4 
New Member
Amit
Join Date: Jul 2014
Posts: 11
Rep Power: 4 
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 

August 22, 2014, 01:15 

#5 
Senior Member
Heather Kline
Join Date: Jun 2013
Posts: 241
Rep Power: 6 
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 3d effects. 

August 22, 2014, 16:29 

#6 
New Member
Amit
Join Date: Jul 2014
Posts: 11
Rep Power: 4 
but with the same grid i got the result in fluent


August 24, 2014, 17:15 

#7 
Senior Member
Heather Kline
Join Date: Jun 2013
Posts: 241
Rep Power: 6 
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. 

August 25, 2014, 06:51 

#8 
New Member
Amit
Join Date: Jul 2014
Posts: 11
Rep Power: 4 
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 emailid i will mail you cfg file 

August 28, 2014, 01:24 

#9 
Senior Member
Heather Kline
Join Date: Jun 2013
Posts: 241
Rep Power: 6 
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. 

August 28, 2014, 07:23 
Artificial compressibilitySU2

#10 
Senior Member
Vino
Join Date: Mar 2013
Location: India
Posts: 115
Rep Power: 5 
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. 

August 28, 2014, 15:20 

#11  
Super Moderator
Francisco Palacios
Join Date: Jan 2013
Location: Long Beach, CA
Posts: 342
Rep Power: 6 
Quote:
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. Freestream pressure: 0 Pa. Freestream density: 998.2 kg/m^3. Freestream velocity: (8e06, 0) m/s. Magnitude: 8e06 m/s. Freestream viscosity: 0.000798 N.s/m^2.  Reference values: Reference pressure: 6.38848e08 Pa. Reference density: 998.2 kg/m^3. Reference velocity: 8e06 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 

August 29, 2014, 12:29 

#12 
Senior Member
Vino
Join Date: Mar 2013
Location: India
Posts: 115
Rep Power: 5 
Thank you.
Is it possible to set the Reference pressure as well as Free stream pressure to 101325 pa ? 

August 31, 2014, 14:12 
Variable velocity profile at inlet of the domain in SU2 config file

#13 
Senior Member
Vino
Join Date: Mar 2013
Location: India
Posts: 115
Rep Power: 5 
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.!!! 

September 9, 2014, 01:09 

#14  
Super Moderator
Francisco Palacios
Join Date: Jan 2013
Location: Long Beach, CA
Posts: 342
Rep Power: 6 
Quote:
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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Solver for Laminar incompressible transient flow  RTom  OpenFOAM  4  March 24, 2014 23:51 
LES solver with variable density for incompressible liquids  matthias  OpenFOAM Running, Solving & CFD  1  April 26, 2010 05:46 
An FASMultigrid solver for steady incompressible viscous flow  luca_g  OpenFOAM Running, Solving & CFD  3  September 21, 2009 02:30 
compressible two phase flow in CFX4.4  youngan  CFX  0  July 1, 2003 23:32 
Incompressible flow solver (staggered grid)  J. Ehrhard  Main CFD Forum  1  October 8, 1998 19:47 