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

(Help) CD error simulating laminar steady-state flow over a sphere [OpenFOAM]

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 13, 2017, 09:36
Default (Help) CD error simulating laminar steady-state flow over a sphere [OpenFOAM]
  #1
Member
 
Join Date: May 2017
Posts: 47
Rep Power: 5
LThomes is on a distinguished road
Hello,
Iím having some trouble simulating laminar steady-state flow over a sphere (OpenFOAM). The solution is converged but Iím having about 15% error on the drag coefficient (CD) for 10 < Re < 100, and about 20% for Re <= 1. Please, see some pictures of my simulation in this website http://imgur.com/a/AxIWE.
  1. Mesh
    Iíve tested finer meshes, and the mesh is converged. (The CD of this one differs only 1.5% from a 15.4% more refined mesh)
  2. Solution convergence and CD
  3. Post-processing
    From picture "Pressure over the sphere and U streamlines for Re = 80", it seems like the flow isnít steady (because of the different size of the recirculation zone), but shouldnít it be for Re = 80? The separation zone is increasing the pressure in the back of the sphere, is that right?
  4. Results
    I think that thereís something strange with the pressure field, because for very low Reynolds numbers (<= 1) the drag should be predominantly viscous (my guess would be viscous CD > 90%).
  5. Simulation parameters
    Iím using simpleFoam solver (SIMPLE algorithm), GAMG for pressure (p) field and smoothSolver for velocity field (U) (see pictures for fvSoultion and fvSchemes). Iíve already changed those field solvers (PGC, GAMG, Ö), refined the mesh, reduced the tolerance of p, checked the boundary conditions and checked the size of the fluid domain, but the results barely change.

Does anyone have any clue whatís wrong, please?
Thanks in advance.
LThomes is offline   Reply With Quote

Old   June 13, 2017, 10:16
Default
  #2
Senior Member
 
piu58's Avatar
 
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 588
Rep Power: 10
piu58 is on a distinguished road
Calculating pressures is one of the harder task in CFD, harder than calculation velocities. The reason: The pressure is calculated in an indirect way (by correction velocities.

The case you simulated is dome by others too. You may compare their results with the experimental findings of Schlichting: Deviations are more normal than absent.
__________________
Uwe Pilz
--
Die der Hauptbewegung Łberlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daŖ ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950)
piu58 is offline   Reply With Quote

Old   June 13, 2017, 12:45
Default
  #3
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 5,666
Rep Power: 60
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
You could check your solution compared to the analytical solution for the flow around a sphere at low Re number...
How do you compute the stress at the wall?
FMDenaro is offline   Reply With Quote

Old   June 14, 2017, 08:32
Default
  #4
Member
 
Join Date: May 2017
Posts: 47
Rep Power: 5
LThomes is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
You could check your solution compared to the analytical solution for the flow around a sphere at low Re number...
How do you compute the stress at the wall?
There's a code that you write in the controlDict file that calculates the viscous ("integral of the shear stress on the area") and pressure drag.
LThomes is offline   Reply With Quote

Old   June 21, 2017, 07:39
Default
  #5
Member
 
Join Date: May 2017
Posts: 47
Rep Power: 5
LThomes is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
You could check your solution compared to the analytical solution for the flow around a sphere at low Re number...
How do you compute the stress at the wall?
I compared the simulation's with the analytical's velocities beginning at the top of the sphere and ending at the boundary of the domain (for Re = 0.05). The error is around 20%, just like the CD error. And the error of the velocity u (x axis) of the first node is 21.4%. Perhaps, the shearStress (=viscosity*du/dz) is following this error.
u.jpgw.jpg
Observations:
  • The freestream velocity is 1 m/s and the velocity far away from the sphere is 1.03 m/s. Is that normal?
  • I guess the analytical solution is not 100% correct, because the velocity will only be equal as the freestream velocity when z -> infinity;
  • u = velocity in the x axis (freestream direction)
  • w = velocity in the z axis

Any idea of what could be wrong in the simulation?

Thanks
LThomes is offline   Reply With Quote

Old   June 30, 2017, 08:31
Default
  #6
Member
 
Join Date: May 2017
Posts: 47
Rep Power: 5
LThomes is on a distinguished road
I found the problem, I was using a first order interpolation scheme for the advection term (Gauss upwind). So I did some research in the OpenFOAM User Guide and chose the Gauss linearUpwind, which is a second order scheme. And that was the problem indeed! After I did that I'm having a 1,3%-error for 20 < Re < 200. Unfortunately, for very low Reynolds numbers (Re = 1 and 0.5) the results are still the same.
p+Stream-Re80.jpg
LThomes is offline   Reply With Quote

Reply

Tags
drag, laminar, openfoam, sphere, steady

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
Issues on the simulation of high-speed compressible flow within turbomachinery dowlee OpenFOAM Running, Solving & CFD 9 February 5, 2021 10:15
is it possible to predict how long it takes to reach steady state solution in unstead Alimohamadi_nasr CFX 4 November 11, 2013 06:11
Flow Across Tube Banks - Transient vs Steady State HeatTransferFan CFX 11 September 28, 2012 14:21
convergence problem in 3D steady state, laminar flow in a bath vajiheh FLUENT 0 July 10, 2009 12:18
About the difference between steady and unsteady problems Lisa Main CFD Forum 11 July 5, 2000 14:37


All times are GMT -4. The time now is 12:52.