
[Sponsors] 
July 11, 2006, 13:57 
Excerpt from ~/OpenFOAM/OpenFO

#1 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 14 
Excerpt from ~/OpenFOAM/OpenFOAM1.3/src/postProcessing/incompressible/liftDrag/liftDrag.C :
scalar qRef = 0.5*magSqr(Uinf); scalar Fref = qRef*Aref; vector pressureCoeff = pressureForce/Fref; vector viscousCoeff = viscousForce/Fref; return (pressureCoeff + viscousCoeff)  flowDirection*(flowDirection & (pressureCoeff + viscousCoeff)); Can somone kindly point out what the return statement is doing in the last line. Specifically, what is being subtracted? Thanks. 

July 13, 2006, 08:16 
It is returning the lift part

#2 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
It is returning the lift part of the force coefficient.
i.e. (pressureCoeff + viscousCoeff) = total force coefficient vector flowDirection*(flowDirection & (pressureCoeff + viscousCoeff)) = the part of the force coefficient in the direction of the flow. 

July 13, 2006, 09:01 
Thanks a lot Eugene!

#3 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 14 
Thanks a lot Eugene!


July 28, 2006, 12:11 
For a 2D case, it appears that

#4 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 14 
For a 2D case, it appears that the liftDrag/OpenFOAM routines use the third number specified in the latter part of the vertices section[1] in the blockMeshDict file, as the depth (which is used in the calculation of projected area, hence the diomensionless force coefficients). Changing this number, say by an order of magnitude, changes the lift/drag coefficients etc. by the same order. Someone please correct me if I am wrong.
[1] For instance the number 0.1 in the following example: bla bla bla... convertToMeters 1; vertices ( (0 0 0) (1.16 0 0) (1.17 0 0) (1.515 0 0) (0 0.015 0) (1.16 0.015 0) (1.17 0.015 0) (1.515 0.015 0) (0 0.025 0) (1.16 0.025 0) (1.17 0.025 0) (1.515 0.025 0) (0 0.04 0) (1.16 0.04 0) (1.17 0.04 0) (1.515 0.04 0) (0 0 0.1) (1.16 0 0.1) (1.17 0 0.1) (1.515 0 0.1) (0 0.015 0.1) (1.16 0.015 0.1) (1.17 0.015 0.1) (1.515 0.015 0.1) (0 0.025 0.1) (1.16 0.025 0.1) (1.17 0.025 0.1) (1.515 0.025 0.1) (0 0.04 0.1) (1.16 0.04 0.1) (1.17 0.04 0.1) (1.515 0.04 0.1) ); 

October 3, 2007, 18:02 
Despite being a very old threa

#5 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 14 
Despite being a very old thread, I wish to add an important observation especially for all those trying out 2D cases and using the liftDrag utility and/or its derivatives that were posted in this forum.
As mentioned above, the distance in the third direction is used to estimate the force coefficients, in particular the force on the wall patch itself. As a result even if you specify a constant projected area (say unity) when finally calculating Cd/Cl etc., the pressure used to calculate the force will be multiplied by the area of the patch as Foam sees it. For instance, if you consider a square obstacle with dimensions D x D x L in a channel, then for a 2D case, you might create the blockMeshDict file as shown above (i.e. L = 0.1). In this case, the liftDrag calculation will assume that the area that needs to be multiplied by the pressure to get the force is D times L. Ideally then, for a 2D case, one wants L to be unity. This needs to be reflected in the blockMeshDict. Aside notes for the checkMesh utility maintainer: You may want to consider adding an extra check for the 2D case. If I use a unit length in the third direction and the typical grid size in the other two directions is very small compared to unity, then checkMesh reports that 1 Mesh check (very high aspect ratio) failed due to a high aspect ratio. For a 2D case, the grid sizes in the third direction should be neglected when checkMesh estimates the aspect ratio. [madhavan@jinshi ~]$ checkMesh . franke_et_al_re_40 /**\  =========    \ / F ield  OpenFOAM: The Open Source CFD Toolbox   \ / O peration  Version: 1.4.1   \ / A nd  Web: http://www.openfoam.org   \/ M anipulation   \**/ Exec : checkMesh . franke_et_al_re_40 Date : Oct 03 2007 Time : 14:22:32 Host : jinshi PID : 26061 Root : /home/madhavan Case : franke_et_al_re_40 Nprocs : 1 Create time Create polyMesh for time = constant Time = constant Mesh stats points: 3064640 edges: 7656160 faces: 6121120 internal faces: 3056480 cells: 1529600 boundary patches: 5 point zones: 0 face zones: 0 cell zones: 0 Number of cells of each type: hexahedra: 1529600 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Topological cell zipup check OK. Face vertices OK. Faceface connectivity OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface ChannelWalls 3200 6404 ok (not multiply connected) ObstacleWalls 320 640 ok (not multiply connected) vinlet 960 1922 ok (not multiply connected) poutlet 960 1922 ok (not multiply connected) frontAndBack 3059200 3064640 ok (not multiply connected) Checking geometry... Domain bounding box: (0.0125 0.015 0) (0.03750000000000001 0.015 1) Boundary openness (3.509809764395274e17 2.895593055626086e15 1.174630898377996e17) OK. ***High aspect ratio cells found, Max aspect ratio: 32000.0000000204, number of cells 1529600 <<Writing 1529600 cells with high aspect ratio to set highAspectRatioCells Minumum face area = 9.765624999993512e10. Maximum face area = 3.125000000001737e05. Face area magnitudes OK. Min volume = 9.765624999992789e10. Max volume = 9.765625000006704e10. Total volume = 0.001493749999965185. Cell volumes OK. Mesh nonorthogonality Max: 8.537736462515939e07 average: 0 Nonorthogonality check OK. Face pyramids OK. Max skewness = 8.881810217858113e12 OK. Min/max edge length = 3.124999999998268e05 1 OK. All angles in faces OK. Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 0.9999999999999996 All face flatness OK. Failed 1 mesh checks. End 

October 4, 2007, 02:39 
I really do not agree with thi

#6 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,806
Rep Power: 25 
I really do not agree with this: if it were so, it would be trivial to fix the width of all OpenFOAM meshes in 2D to unit width and be done with it.
The issue stems from the way I calculate cell volume and face area, by decomposition into triangles and pyramids. In extremely stretched cells, this will accumulate the roundoff errors, sometimes in a nasty way, which will mess up the accuracy in the rest of the code. Therefore, you are much better creating the mesh such that the cells in the third direction look decent (avoiding the discretisation error in surface and volume calculation) and then using a POCKET CALCULATOR to divide the forces by the width. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

October 4, 2007, 02:52 
Thanks for the recommendation

#7 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 14 
Thanks for the recommendation Dr. Jasak. I was unaware of these other issues. So to sum up, the idea is to create a 2D geometry with a decent width in the third direction (i.e. acceptable aspect ratio). I am presently comparing the pressure and viscous drag coefficient predictions with a paper. I will report the results soon.


October 4, 2007, 10:25 
For 3D surfaces, high aspect

#8 
Member
Doug Baldwin
Join Date: Mar 2009
Posts: 53
Rep Power: 10 
For 3D surfaces, high aspect ratio cells seem inevitable when yplus is 1 or 2, unless the wall is discritized into an unreasonably large number of very tiny pieces. My high aspect ratio cells at the wall have low skew. This appears to me to not be a problem because the OF results match wind tunnel data. I'm new to this community, so could be missing something obvious.


March 28, 2008, 11:55 
Hi to all,
i am calculating

#9 
New Member
Fabian Korn
Join Date: Mar 2009
Location: Heilbronn, Germany
Posts: 21
Rep Power: 10 
Hi to all,
i am calculating a 3D cylinder case and try to calculate the drag coefficient. The CD/Cl tool seems to work in a 2D case, but i get a negative result for my 3D case. I sue a dynSmagotinsky at Re around 200. If i divide Cd by my depth i am close to the result i want to have, but i get the same result for Re=200 and Re=500 what is absolutly not reasenable. Can anybody help me, i have no idea what to do. Fabian 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Question to liftDrag  hoochie  OpenFOAM PostProcessing  29  September 19, 2014 03:38 
TurbForce term in liftDrag utility  kumar2  OpenFOAM PostProcessing  11  August 11, 2010 03:52 
LiftDrag Utility for Compressible Flow Fields  shaun  OpenFOAM Running, Solving & CFD  9  September 16, 2008 05:36 
LiftDrag utility from v12 to v141  cfdphil  OpenFOAM Running, Solving & CFD  2  December 5, 2007 06:49 
LiftDrag utility not available  guggi  OpenFOAM Running, Solving & CFD  1  August 2, 2006 12:36 