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

Experimental data vs SimpleFoam sphere test case : Cd do not match

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

Like Tree2Likes
  • 2 Post By sail

Reply
 
LinkBack Thread Tools Display Modes
Old   November 2, 2012, 06:04
Default Experimental data vs SimpleFoam sphere test case : Cd do not match
  #1
New Member
 
edy
Join Date: Jul 2012
Location: Tokyo
Posts: 6
Rep Power: 0
alsdia is on a distinguished road
Objective: compare the experimental drag coefficient of a sphere with the value obtained with simpleFOAM.

I took the report Simulation of Flow Past a Sphere using the Fluent Code
that you can find here:
http://www.dtic.mil/cgi-bin/GetTRDoc?AD=ADA494935

at page 26 they present a table where they compared the Cd obtained from experimental data and from Fluent at different Reynolds.

I wanted to check if using SimpleFOAM I was able to obtain the same drag coefficient. I started with the last case, Re = 10^6, inlet speed 14.6m/s
I prepared the sphere 1m of diameter and put it inside a box.
The case file are copied from the motorbike tutorial, and I modified inside only the name for my new boundary conditions.

Compared to the results presented in page 26 [experimental Cd has a value ranging from 0.08(Constantinescu, G.S. and Squires) to 0.142(Jones, W.P. and Launder, B.E.), Fluent Cd estimation = 0.048] my SimpleFoam Cd is too small: Cd = 0.0125609. My StarCCM analysis gives Cd = 0.0719. Yet if we compare the maximum pressures of the two codes they are quite similar: simpleFoam sphere max pressure * 1.205 = 106.399 * 1.205 =128.2108Pa ~ 129.1Pa of StarCCM. So why the Cd are so different? Looking at the pictures enclosed do you think that the quality mesh is good enough to model properly the boundary layer? What could be the reason of such big discrepancy?

Thank you for your help

------------------------------------------------------------------------------------------------------------------------
the sphere case is saved @
https://www.dropbox.com/sh/gg1ypj0c1...vYI_k/OpenFOAM
the mesh was created in starCCM and exported to OpenFOAM via ccm26ToFoam, checkMesh OK
Attached Images
File Type: jpg sphere.mesh.zoom.jpg (43.8 KB, 72 views)
File Type: jpg simpleFoam.sphere.streamlines.jpg (56.7 KB, 63 views)
File Type: jpeg starccm.sphere.pressure.jpeg (88.5 KB, 50 views)
File Type: jpg sphere.mesh.jpg (53.7 KB, 67 views)
alsdia is offline   Reply With Quote

Old   November 2, 2012, 06:37
Default
  #2
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 7
sail is on a distinguished road
reading the pdf you posted it looks that for the R1E6 case in fluent the drag is approx 0.12-0.14.

the discrepancy is caused by the turbulence.

they used LES and you have k-epsilon on a bac mesh with no layers on the walls and big differences in volume near the wall.

if you do not have the resources to run LES and want to stick with RANSE at least try using k-omega sst, a fully resolved Boudary layer with a y+ < 1, at least 20 layers in the normal direction and take spacial care in making the volume of the cells change as smoothly as possible.

also, given the semplicity of the geometry, you might want to use a conformal mesh (a cell face is not divided in two by other neighbor cells)

ah, almost forgot, probably your domain should be bigger an all the dimensions
sharonyue and vbnhfylbh like this.
__________________
http://www.leadingedge.it/
Naval architecture and CFD consultancy
sail is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
OF 1.6 | Ubuntu 9.10 (64bit) | GLIBCXX_3.4.11 not found piprus OpenFOAM Installation 22 February 25, 2010 14:43
Problems in compiling paraview in Suse 10.3 platform chiven OpenFOAM Installation 3 December 1, 2009 08:21
gmsh2ToFoam sarajags_89 OpenFOAM 0 November 24, 2009 23:50
How to update polyPatchbs localPoints liu OpenFOAM Running, Solving & CFD 6 December 30, 2005 18:27
Simulated data vs. experimental data moiami FLUENT 0 December 19, 2002 02:03


All times are GMT -4. The time now is 10:10.