CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Verification & Validation (http://www.cfd-online.com/Forums/openfoam-verification-validation/)
-   -   Experimental data vs SimpleFoam sphere test case : Cd do not match (http://www.cfd-online.com/Forums/openfoam-verification-validation/108826-experimental-data-vs-simplefoam-sphere-test-case-cd-do-not-match.html)

 alsdia November 2, 2012 06:04

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

4 Attachment(s)
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:

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?

------------------------------------------------------------------------------------------------------------------------
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

 sail November 2, 2012 06:37

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

 All times are GMT -4. The time now is 14:50.