CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Post-Processing

TurbForce term in liftDrag utility

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 17, 2006, 20:31
Default Hello I have a question on
  #1
Senior Member
 
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 8
kumar2 is on a distinguished road
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
kumar2 is offline   Reply With Quote

Old   April 18, 2006, 14:42
Default Hello all, Could someone co
  #2
Senior Member
 
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 8
kumar2 is on a distinguished road
Hello all,

Could someone comment on this post ?

i am stuck with my results

thanks in advance

kumar
kumar2 is offline   Reply With Quote

Old   April 25, 2006, 06:00
Default Hi kumar, I'm very sorry th
  #3
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
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
anja is offline   Reply With Quote

Old   April 25, 2006, 08:04
Default Hi Kumar, the difference be
  #4
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 8
hartinger is on a distinguished road
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
hartinger is offline   Reply With Quote

Old   April 25, 2006, 16:24
Default Hi Anja, Let me try to answ
  #5
Senior Member
 
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 8
kumar2 is on a distinguished road
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
kumar2 is offline   Reply With Quote

Old   April 25, 2006, 17:24
Default Hi Markus Thanks a lot for
  #6
Senior Member
 
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 8
kumar2 is on a distinguished road
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
kumar2 is offline   Reply With Quote

Old   April 26, 2006, 07:07
Default Hi Kumar, if you look for t
  #7
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 8
hartinger is on a distinguished road
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
hartinger is offline   Reply With Quote

Old   April 26, 2006, 20:56
Default Hi Markus & Pierre Thanks a
  #8
Senior Member
 
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 8
kumar2 is on a distinguished road
Hi Markus & Pierre

Thanks a lot for the replies

regards

kumar
kumar2 is offline   Reply With Quote

Old   April 27, 2006, 09:52
Default Hi all, also thanks from my s
  #9
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
Hi all,
also thanks from my side.

Anja
anja is offline   Reply With Quote

Old   August 25, 2006, 02:35
Default 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
  Reply With Quote

Old   August 3, 2010, 10:41
Default
  #11
Member
 
83_Ale_83's Avatar
 
Alessandro
Join Date: Nov 2009
Posts: 67
Rep Power: 7
83_Ale_83 is on a distinguished road
Hi to everybody, does anybody know where this equation

nuw[facei] *(yPlus*kappa_/log(E_*yPlus) - 1);

is coming from??

Thanks in advance
__________________

83_Ale_83 is offline   Reply With Quote

Old   August 11, 2010, 03:52
Default
  #12
Member
 
83_Ale_83's Avatar
 
Alessandro
Join Date: Nov 2009
Posts: 67
Rep Power: 7
83_Ale_83 is on a distinguished road
Quote:
Originally Posted by 83_Ale_83 View Post
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
__________________

83_Ale_83 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
LiftDrag for 141 ryan_m OpenFOAM Running, Solving & CFD 2 August 24, 2009 21:26
LiftDrag Utility for Compressible Flow Fields shaun OpenFOAM Running, Solving & CFD 9 September 16, 2008 05:36
LiftDrag utility question msrinath80 OpenFOAM Running, Solving & CFD 8 March 28, 2008 11:55
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


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