CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Verification & Validation

laminar Flow over a sphere(laminar vs KOmegaSST simulation)

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 12, 2023, 01:50
Default laminar Flow over a sphere(laminar vs KOmegaSST simulation)
  #1
Senior Member
 
Farzad Faraji
Join Date: Nov 2019
Posts: 205
Rep Power: 7
farzadmech is on a distinguished road
Hello all
I am simulating flow over a sphere at Re = 881 where Drag coefficient must be almost Cd=0.5. I simulate it using both using laminar and Turbulent models(KOmegaSST). for laminar simulation, I get Cd ~0.5 but fort the Turbulent simulation, first of all it takes very long tome to converge and even after convergence, it gives Cd~0.65(Actually it has not fully converged yet, see attached figure). Now I have two questions;
1- what happens if I use turbulent model to simulate laminar flow?
2- when should I expect convergence based on the attached figure?

Thanks,
Farzad
Attached Images
File Type: jpg photo_2023-03-12_00-39-10.jpg (103.0 KB, 37 views)
farzadmech is offline   Reply With Quote

Old   March 15, 2023, 22:01
Default Sphere in Re-881 with laminar and kOemgaSST(SimpleFoam)
  #2
Senior Member
 
Farzad Faraji
Join Date: Nov 2019
Posts: 205
Rep Power: 7
farzadmech is on a distinguished road
I did test with laminar and kOmegaSST for sphere and airfoil and as I told earlier it predict higher drag Coefficient, but flow field visually seems correct. I repeat it with airfoil with angle of attack = 30 degree and not only drag coefficient is different, but also flow field is visually seems incorrect, why?

Also, I want to test below methods too, but they fail at the very beginning of the simulation;
1) SpalartAllmaras (fails at the beginning iterations),
2) kOmegaSSTLM (fails at the beginning iterations) ,
3) kOmegaSSTSAS (Selecting LES delta type vanDriest Killed)

Should I change my boundary conditions when I switch from kOmegaSST to other models?



Thanks,
Farzad
Attached Images
File Type: jpg Spheree.jpg (45.3 KB, 31 views)
File Type: jpg Airfoil.jpg (80.1 KB, 21 views)
farzadmech is offline   Reply With Quote

Old   March 20, 2023, 06:49
Default
  #3
Senior Member
 
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 363
Rep Power: 8
geth03 is on a distinguished road
Quote:
Originally Posted by farzadmech View Post
Hello all
I am simulating flow over a sphere at Re = 881 where Drag coefficient must be almost Cd=0.5. I simulate it using both using laminar and Turbulent models(KOmegaSST). for laminar simulation, I get Cd ~0.5 but fort the Turbulent simulation, first of all it takes very long tome to converge and even after convergence, it gives Cd~0.65(Actually it has not fully converged yet, see attached figure). Now I have two questions;
1- what happens if I use turbulent model to simulate laminar flow?
2- when should I expect convergence based on the attached figure?

Thanks,
Farzad
1. one should not use a turbulence model when the flow is laminar. turbulence models use special boundary conditions to mimic real turbulence behaviour at walls. that will lead to wrong pressure and turbulent viscosity and thus to wrong drag coefficients for laminar cases.
2. for convergence you should always monitor the value of interest, in your case the drag coefficient. if it does not change or only oscillates between two stable extremes, you can say that based on your case setup that value is your solution.
geth03 is offline   Reply With Quote

Old   March 20, 2023, 07:00
Default
  #4
Senior Member
 
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 363
Rep Power: 8
geth03 is on a distinguished road
Quote:
Originally Posted by farzadmech View Post
I did test with laminar and kOmegaSST for sphere and airfoil and as I told earlier it predict higher drag Coefficient, but flow field visually seems correct. I repeat it with airfoil with angle of attack = 30 degree and not only drag coefficient is different, but also flow field is visually seems incorrect, why?

Also, I want to test below methods too, but they fail at the very beginning of the simulation;
1) SpalartAllmaras (fails at the beginning iterations),
2) kOmegaSSTLM (fails at the beginning iterations) ,
3) kOmegaSSTSAS (Selecting LES delta type vanDriest Killed)

Should I change my boundary conditions when I switch from kOmegaSST to other models?



Thanks,
Farzad
you should always check if your boundary conditions are ok with the chosen turbulence model and also with your mesh sizing at the wall. for example, you should not expect good solution when your y+-value is 1 and you use k-Epsilon, which is valid only for y+=30 at least.
i think to predict good pressure distribution for forces around bodies you want to resolve the wall boundary layer, check your BC for your chosen turbuluence model if it supports boundary resolution.

if you have problems with convergence, first start your simulation with first order upwind schemes for advection terms: div(phi,u), div(phi,k) etc.
you can also use higher viscosity values.
after that try using lower viscosity with the previous converged solution. after that switch your div(phi,u) to second order upwind, and not change turbulence schemes.
once converged change your schemes for turbulence to second order scheme also.

try this step by step approach, do not rush to find a perfect solution right from your first try.
geth03 is offline   Reply With Quote

Reply

Tags
komegasst, laminar, openfaom, sphere

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Laminar flow and wall roughness junbbung FLUENT 2 November 26, 2022 21:22
SU2 NACA0012 Transitional flow simulation Convergence Issues morgJ SU2 0 July 21, 2022 07:42
Different peak velocity for laminar and turbulent models of Reynolds Number-500 flow vronti Main CFD Forum 2 July 12, 2022 10:36
unable to run dynamic mesh(6dof) and wave UDF shedo Fluent UDF and Scheme Programming 0 July 1, 2022 17:22
High velocity in Laminar flow Manojmech FLUENT 0 November 3, 2016 04:37


All times are GMT -4. The time now is 21:39.