# TurbForce term in liftDrag utility

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

 April 17, 2006, 20:31 Hello I have a question on #1 Senior Member   kumar Join Date: Mar 2009 Posts: 112 Rep Power: 8 Hello I have a question on the turbForce term in the liftDrag.C (../src/postprocessing/incompressible/liftDrag/liftDrag.C ). Laminar Flow -------------- In the laminar case the drag is the pressure drag + x_component of the wall shear stress . although i am not an expert in C++ , i could make out that -mu.value()*U.boundaryField()[patchLabel].snGrad()*mesh.magSf().boundaryField()[ patchLabel] is approximately meu*velocityGradient*area . Am i correct ? 2. turbulent drag -------------------- In turbulent flow the wall shear stress is (according to ferziger and peric) rho*(u_tau)^2. which equals rho*(C_meu)^0.25*k*sqrt(k)*vel_parallel_wall/(ln(n+E)) But the formulation given in liftDrag.C is totally different . first the laminar drag is found out ( even in turbulent case ) . then the turbulent drag is found ( this does not at all resemble the expression given by say ferziger , peric). then these 2 are added. could someone tell me why this procedure is adopted and where i am wrong ? i am stuck with my comparison. thanks a lot kumar

 April 18, 2006, 14:42 Hello all, Could someone co #2 Senior Member   kumar Join Date: Mar 2009 Posts: 112 Rep Power: 8 Hello all, Could someone comment on this post ? i am stuck with my results thanks in advance kumar

 April 25, 2006, 06:00 Hi kumar, I'm very sorry th #3 Member   Anja Stretz Join Date: Mar 2009 Posts: 92 Rep Power: 8 Hi kumar, I'm very sorry that I can't help you, but maybe you can answer some of my questions? - where do I get the mu field from? - how do I have to change the code for a compressible fluid? - where do I have to write the code? - how can I actually use it? - where do I find the results thanks Anja

 April 25, 2006, 08:04 Hi Kumar, the difference be #4 Senior Member   Markus Hartinger Join Date: Mar 2009 Posts: 102 Rep Power: 8 Hi Kumar, the difference between laminar and turbulent navier-stokes equations are the reynolds-stresses. So you can simply take the laminar forces and add the forces due to the reynolds-stresses. laminar: mu.value()*U.boundaryField()[patchLabel].snGrad()* mesh.magSf().boundaryField()[patchLabel] means: viscosity * velocity gradient normal to surface * area turbulent: - mesh.Sf().boundaryField()[patchLabel] & turbulence->R()().boundaryField()[patchLabel] means: surface vector(length equal to area) &(dot-product) reynolds stress tensor the calculation is general, given a stress tensor which is calculated from your choice of turbulence model regards markus

 April 25, 2006, 16:24 Hi Anja, Let me try to answ #5 Senior Member   kumar Join Date: Mar 2009 Posts: 112 Rep Power: 8 Hi Anja, Let me try to answer your questions . 1. mu field ------------- the liftDrag utility uses nu ( mu/density ). this is set in the transportProperties in your case directory. 2. Compressible fluid since liftDrag utitlity uses nu , you may have to modify the utility itself. 3. writing the code. The liftDrag.C ( & associated codes ) code resides in /OpenFoam-1.2/application/utilities/postProcessing/miscellaneous/liftDrag/ . This program while executing calls another program also called liftDrag.C ( & associated programs ) in ../src/postProcessing/incompressible/liftDrag/ the liftDrag.C in /miscellaneous/../ calls createNu.H . createNu.H then opens transportProperties file ( this resides in the case directory )gets nu ( mu/rho ) . You can give a different nu by either modifying the transportProperties file . however you can also modify the later part of createNu.H to say for example read a certain different value , but here again , we are still talking about nu ( NOT mu) to modify the code . copy the code to your /applications directory and follow the instructions in user manual . also refer other wonderful posts ( search with liftDrag in openFoam ) Once you compile your program you are ready to go! hope this helps regards kumar

 April 25, 2006, 17:24 Hi Markus Thanks a lot for #6 Senior Member   kumar Join Date: Mar 2009 Posts: 112 Rep Power: 8 Hi Markus Thanks a lot for your reply. i hope i can trouble you with one more question. In the case of ke models the reynolds shear stress are not calculated . this means that the wall shear stress given in liftDrag utility is an approximate formulation because in the turbulent case - while using ke model - the wall shear stress is (according to ferziger and peric) rho*(u_tau)^2. which equals rho*(C_meu)^0.25*k*sqrt(k)*vel_parallel_wall/(ln(n+E)) , but the utility does not calculate this and approximates with the laminar formulation. Am i correct ? regards kumar

 April 26, 2006, 07:07 Hi Kumar, if you look for t #7 Senior Member   Markus Hartinger Join Date: Mar 2009 Posts: 102 Rep Power: 8 Hi Kumar, if you look for the k-eps model in src/turbulenceModels/incompressible/kEpsilon the reynolds stresses are calculated according to the boussinesq approximation common to all k-eps models. ((2.0/3.0)*I)*k_ - nut_*2*symm(fvc::grad(U_)) the turbulence viscosity nut is calculated like nut_ = Cmu*sqr(k_)/(epsilon_ + epsilonSmall_) with standard wall function approach to get the wall values for nut (wallViscosityI.H) with yPlusLam = 11.63 if (yPlus > yPlusLam_) { nutw[facei] = nuw[facei] *(yPlus*kappa_/log(E_*yPlus) - 1); } else { nutw[facei] = 0.0; } regards markus and pierre

 April 26, 2006, 20:56 Hi Markus & Pierre Thanks a #8 Senior Member   kumar Join Date: Mar 2009 Posts: 112 Rep Power: 8 Hi Markus & Pierre Thanks a lot for the replies regards kumar

 April 27, 2006, 09:52 Hi all, also thanks from my s #9 Member   Anja Stretz Join Date: Mar 2009 Posts: 92 Rep Power: 8 Hi all, also thanks from my side. Anja

 August 25, 2006, 02:35 Hi, I want to implement the vi #10 newbee Guest   Posts: n/a Hi, I want to implement the viscous dissipation rate in my application. the term which im hopeing to get implemented is 1/2*1/Cp*(R()() & R ()()) on acount that R()() = tau/rho. However the implementation of the dot product of R()() is not accepted. Does anyone know how to do this? Thanks /erik

 August 3, 2010, 10:41 #11 Member     Alessandro Join Date: Nov 2009 Posts: 67 Rep Power: 7 Hi to everybody, does anybody know where this equation nuw[facei] *(yPlus*kappa_/log(E_*yPlus) - 1); is coming from?? Thanks in advance __________________

August 11, 2010, 03:52
#12
Member

Alessandro
Join Date: Nov 2009
Posts: 67
Rep Power: 7
Quote:
 Originally Posted by 83_Ale_83 Hi to everybody, does anybody know where this equation nuw[facei] *(yPlus*kappa_/log(E_*yPlus) - 1); is coming from?? Thanks in advance
Anyone?
Thanks again
__________________

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post ryan_m OpenFOAM Running, Solving & CFD 2 August 24, 2009 21:26 shaun OpenFOAM Running, Solving & CFD 9 September 16, 2008 05:36 msrinath80 OpenFOAM Running, Solving & CFD 8 March 28, 2008 11:55 cfdphil OpenFOAM Running, Solving & CFD 2 December 5, 2007 06:49 guggi OpenFOAM Running, Solving & CFD 1 August 2, 2006 12:36

All times are GMT -4. The time now is 23:58.