Hello all, im trying to cal
 

Hello all,

im trying to calculate some cases from fluent, to evaluate the results of OpenFOAM. The cases consist of a wing (2D) in a flow and Im interested in the forces in X and Y-direction. So I changed the liftDrag-tool to print the vectors from the pressure-, visous- and turbulenceforce. With this vectors, I hoped to get more or less the same results than from fluent. In fact they are not, the forces are much to low.
I filled in the right value of nue, because liftDrag is working with it. So, does anybody have a clue where could be the problem?

And a second question, I raed in the forum, that calculating incompressible means to compute p* but not p. To get the real pressure I have to multiply p* with rho.
But if p* isnt p, is the function

pressureForce = sum
(
p.boundaryField()[patchLabel]
*mesh.Sf().boundaryField()[patchLabel]
);

in liftDrag correct? Because p in this case is p* as far as I can see.

thx in advance

There is a very detailed discu
 

There is a very detailed discussion on lift/drag on the "Running/Solving CFD" forum. Check it out. For the record, I have compared the lift and drag coefficients using both OpenFOAM and Fluent for the case of 2D laminar unsteady vortex shedding past a square cylinder. They compare quite well!

And I compared lift/drag for a
 

And I compared lift/drag for a 2D laminar flow around fixed and moving circular cylinders. Comparison with Fluent / Literature is quite good, and OpenFoam is faster, especially the new 1.4!

hi, I am new for OpenCFD. Ac
 

hi,
I am new for OpenCFD. Actually I have to do the simulation for flow past fixed circular cylinder of radius 10cm in 2D incompressible viscous laminar unsteady flow in water. Lift/drag has to compare with the fluent result.
Can any one suggest that,which solver I have to use(simple or piso) and also which scheme and what value for other factor should be used or whole steps.
My reynolds number is 3000.
thanx
Rk

Hi Ranjan, Welcome OpenFoa
 

Hi Ranjan,

Welcome OpenFoam, it is a very good piece of code and perfectly suitable for your problem. I am also dealing with laminar flows and performed certain tests using circular cylinders in a freestream at Re=150. For detailed info, take a look at:

http://www.aero.lr.tudelft.nl/~frank/index.php?id=research/cfd/OpenFOAM/validati on/OpenFOAM

For the problem of a static cylinder in a freestream, you'll have to use icoFoam with PISO and central discretisation. For a static cylinder I use the fully Crank Nicholson timescheme and for moving cylinders I use the backward scheme (with icoDyMFoam). From my experience, OpenFoam 1.4 is a lot faster than 1.3, so try this new version.

One more question. You are aware that the flow around circular cylinders becomes turbulent at about Re=180, right? When you want to solve for turbulence you need the solver turbFoam.....

Goodluck and keep me informed about your results!

Regards, Frank

Hi Frank, I will be giving
 

Hi Frank,

I will be giving a presentation in my university concerning the use of GNU/Linux clusters in solving CFD problems. I was wondering if I could use your CFD movies from your webpage as examples. I will reference your movies to your webpage. Would that be OK?

Hi pUI, It OK with me. Just
 

Hi pUI,

It OK with me. Just refer to my website and mention the Delft University of Technology. Btw, which movies are you referring to? And what is your university?

Frank

Will do Frank. Thanks! I'm fro
 

Will do Frank. Thanks! I'm from University of Alberta (www.ualberta.ca), Chemical and Materials Engineering Department.

Hello all, I asked the ques
 

Hello all,

I asked the questions in the beginning of this thread. Thanks for your replies! I worked through the "Running/Solving CFD"-discussion first, but it didnt answer my question, as I get it. Maybe it is answered and my english is to limitted http://www.cfd-online.com/OpenFOAM_D...part/happy.gif
So I opened this thread.
My main-problem is the function for the pressure sum. In this function the pressureforce is calculated with p*. So the pressureforce is not a force, it is a force/rho. I solved the problem with multiplying rho to my pressurefield, with this I get p and not p*. After doing this, the results are looking good.
To clear things, Im not interested in the coefficients which are calculated, Im interested in the forces. I calculate the coefficients by myself. So I added the instruction to liftDrag to print out the force-vectors and as I get it they work "wrong" as they compute in the usual style force/rho instead of a force.
I hope you are able to understand what I meant.

BTW: Did anyone of you try computing an airfoil in 2D? I do right now and Im getting always a velocity in z-direction. I posted this problem in another thread and I dont want to activate the same topic here, but if you did, I would be interested in your setup of files. Some other people gave me hints, about possible causes, but all possible causes were absolutly ok in my case.

Anyway thank you
RW

RW- I am also trying to get
 

RW-

I am also trying to get a 2D airfoil case running using a C-grid. I'm having a really tough time with the boundary conditions for some reason. I found this thread that suggests getting it running in potentialFoam first:
http://www.cfd-online.com/OpenFOAM_D...tml?1181162568
but I haven't had any luck with that either. I've posted in two other threads along the same lines:

http://www.cfd-online.com/OpenFOAM_D...tml?1179501415

and

http://www.cfd-online.com/OpenFOAM_D...tml?1181080719

If you get something running, I'd be very interested in knowing what your using for initial conditions, boundary conditions, and the other initial setup files for the case.

Thanks.

-Doug

RW: Apologies for the delayed
 

RW: Apologies for the delayed reply. Can you rephrase your question if possible in a single sentence. I'm unable to follow it at present.

Hello All- One more questio
 

Hello All-

One more question. OpenFOAM 1.4 doesn't come with a pre-compiled liftDrag executable. When I try to compile it, I get errors telling me:

make: *** No rule to make target '/blah/blah/blah.h' needed by 'liftDrag.dep'. Stop

I figured it wasn't finding the .h files and located a bunch of them. It seems that liftDrag.dep was written for 1.2 and that many of the files have been moved for 1.4. Locating the files alleviated the problem for most of the .h files. However, there are a bunch of .h files that I can't find anywhere in the OpenFOAM-1.4 installation. This includes liftDrag.h. I assume many of you are running liftDrag on 1.4 and just wondered how you got it to compile when so many of the .h files listed in liftDrag.dep don't even exist in the installation.

Thanks for you help.

-Doug

Yes, liftDrag compiles trivial
 

Yes, liftDrag compiles trivially in OpenFOAM 1.4. I have given detailed instructions[1] in the forum on how to install it in OF 1.3. If you follow the same procedure for OF 1.4 it will work. I use it on OF 1.4 without any problems.

[1] http://www.cfd-online.com/OpenFOAM_D...es/1/2299.html

I read somewhere in the forum that it is on the TODO list for a future OpenFOAM version. So I'm guessing that we should have have native liftDrag support sooner or later.

Good Luck!!!!

Yes, liftDrag compiles trivial
 

Yes, liftDrag compiles trivially in OpenFOAM 1.4. I have given detailed instructions[1] in the forum on how to install it in OF 1.3. If you follow the same procedure for OF 1.4 it will work. I use it on OF 1.4 without any problems.

[1] http://www.cfd-online.com/OpenFOAM_D...es/1/2299.html

I read somewhere in the forum that it is on the TODO list for a future OpenFOAM version. So I'm guessing that we should have have native liftDrag support sooner or later.

Good Luck!!!!

Thank you! I just compiled lif
 

Thank you! I just compiled liftDrag in 1.4. Thanks for the detailed explanation of your other post in the other thread.

-Doug

Hey there, pUI, no case to
 

Hey there,

pUI, no case to apologize, we all got our work to do.
My question in one sentence would be:
Did anyone of you tried to simulate an airfoil in 2D with simpleFoam or rhoSimpleFoam?

Im getting always a velocity in z-direction which makes it hard to qualify my values for liftdrag, allthough they look good. As I said, I wrote about it in another thread, so it isnt wise to discuss it here, but unless I tried a lot with no success Im interested in the setup files, for 2D-cases in case of an airfoil, which got no velocity in z-direction.

RW

Hello, all I just compiled
 

Hello, all

I just compiled liftDrag in 1.4. And I found it is available for interFoam, but it cannot be applied to icoFoam and oodles, I guess the problem is around here:
--------------------------------------------------
scalar Aref = sum
(
(Uav & mesh.Sf().boundaryField()[patchI])*
pos(Uav & mesh.Sf().boundaryField()[patchI])
);

// Reference length
boundBox patchBounds
(
mesh.boundaryMesh()[patchI].localPoints()
);

scalar Lref =
mag(Uav & (patchBounds.max() - patchBounds.min()))
/(mag(Uav) + VSMALL);
--------------------------------------------------
could anyone give some comments on these lines that why I cannot use liftDrag here and how to modify it.
Thanks

Have a good day!

Daniel

Hello Forum, I just install
 

Hello Forum,

I just installed the utility liftDrag as suggested in:

http://www.cfd-online.com/OpenFOAM_D...es/1/2299.html

I am running a very simple case in simpleFoam. I have a naca0012 at 0 angle of attack, and k-epsilon for modeling turbulence. I get the analysis to converge nicely, pressure looks good, velocity, k, epsolin, etc. look very good. When I run liftDrag . naca0012 -time 700 for example, I get this output:

[gtg627eOpenFOAM@ruzzene03 simpleFoam]$ liftDrag . naca0012 -time 700
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : liftDrag . naca0012 -time 700
Date : Oct 29 2007
Time : 03:42:42
Host : ruzzene03
PID : 9647
Root : /home/gtg627eOpenFOAM/OpenFOAM/gtg627eOpenFOAM-1.4.1/run/tutorials/simpleFoam
Case : naca0012
Nprocs : 1
Create time

Create mesh for time = 700

Time = 700
Reading U

Reading p

Inlet velocity: (50 0 0)
Wall patch 1 named airfoiln :
Reference area: 0.297421 Reference length: 1 Drag coefficient: 0.00116109 Lift coefficient: (0 8.21932e-05 -1.32776e-21) Moment coefficient: (-2.05483e-06 2.90273e-05 -1.95907e-05)

This result seems to not include viscous forces. The drag for a naca0012 at 0 deg and Re ~ 3 million should be approximately 0.0058, from "theory of wing sections."

Thank you in advance for any comments,

Alessandro

Sorry I meant to post the abov
 

Sorry I meant to post the above message in the following thread:

http://www.cfd-online.com/OpenFOAM_D...es/1/2299.html

I have performed a validation
 

I have performed a validation for laminar flows and I am confident that the utility accounts for both components. For turbulence please see the other threads on liftDrag. You may have to add some features.

Srinath Madhavan, I figured
 

Srinath Madhavan,

I figured out how to compute the drag for turbulent cases; however, I have doubts about the results obtained from liftDrag.C.

I followed the instructions in the following thread:

http://www.cfd-online.com/OpenFOAM_D...s/1/5067.html?


The reason why I am doubful is because I have a simple naca0012 at 0 angle of attack, and OpenFOAM predicts a total drag of 0.00314, which is well below the experimental value of 0.0058 from "theory of wing sections." Later this evening, I tried the same case at 4-deg angle of attack, and now I get a total drag of 0.008 and a lift coefficient of 0.05. For this case, the drag should be approximately 0.006 and the coefficient of lift shuld be about 0.5.

I ran checkMesh and got no errors.
Everything is incompressible, inlet V = 50 m/s
chord = 1 m
k-epsilon model:

inlet k = 0.375
inlet epsilon 0.03

Everything is reasonable, the analysis converges reasonably well, but the force coefficients are off. As Vincent suggested in

http://www.cfd-online.com/OpenFOAM_D...s/1/5067.html?

I will compare pressure coefficent, velocity distribution, etc. For the pressure coefficient, however, I will have to do a little coding.

It is possible that my analysis is ill-posed, but it converges well, and both velocity and pressure seem very reasonable.

Thank you,

Alessandro

Alessandro, I understand your
 

Alessandro, I understand your problem. However, the minute turbulence models enter the picture, I switch off the need for accurate experimental predictions in my head. A bad habit, but nevertheless quite true most of the time. Anyways, I would be interested in knowing whether you have tried the same case with Fluent or CFX and if so what dimensionless force coefficients (lift, drag etc.) do they predict?

Could someone verify that the
 

Could someone verify that the turbulent drag calculation using liftDrag is correct......we are finding differences....anyone?

Frank

Hi Frank & others, I am som
 

Hi Frank & others,

I am somewhat confused as to why most posts in this forum suggest that modifications are required to the liftDrag utility if one has to obtain lift/drag predictions when using turbulence models. If the function of a turbulence model is to simulate (or more accurately, emulate) turbulent behavior in the fluid and if this is reasonably well done by the turbulence model in question, then turbulent behavior should automatically show up in the result (i.e. in the primitive variables u,v,w,p). Then all that remains is using these results in the integration of shear and pressure forces over the walls in question, which should directly give the correct lift and drag coefficients. Turbulent viscosity should not enter the picture at this stage as it is merely a means to get to the correct (hopefully) u,v,w and p. So when lift/drag forces are calculated, one should only use the actual density/viscosity of the fluid in question and not the turbulent viscosity?

To put it in a nutshell, if the velocity and pressure fields are accurate in space (and in time for transient problems), then the liftDrag utility should give the correct forces without any modifications.

I would appreciate if someone can correct me if I am wrong.

Hi Srinath, In fact, this i
 

Hi Srinath,

In fact, this is exactly what I meant by my previous question. A turbulence model is used to give a better solution of u,v,w,p when the flow is turbulent. So, in fact the boundary layer becomes fuller (compared to laminar flow) which has its influence on the viscous drag, just like the laminar case. In my view, the turbulent viscosity term is not needed in the drag/lift calculation......

Anyone else??

Frank

btw, I did not wrote this utility, but made some modifications such that integration in icoFoam i.e. becomes easier....

Works like this: tauw = nu
 

Works like this:

tauw = nu * dU/dy_wall right?

Except we do not have dU/dy_wall, we have dU/dy_0 between the first node and the wall. Thus we calculate wall shear using a wall function. To keep things compact in the momentum equation we stick the wall function in the turbulent viscosity so that:

tauw = nuEff_wall * dU/dy_0

So the use of turbulent viscosity to calculate the wall shear is purely an artifact used by OpenFOAM to store the influence of the wall function - nuEff_wall.

Allright, so in the turbulent
 

Allright, so in the turbulent case the viscous force calculation contains some turbulent contribution.....via wall function.

Then, why is there still need for a turb force contribution,present in liftDrag, derived from turbulence->R().

Frank

Because (for example in kEpsil
 

Because (for example in kEpsilon) turbulence->R() is calculated from

2/3*I*k - nut_*2*symm(grad(U))

The wall boundary of nut_ contains the effect of the wall function. (See "#include "wallViscosity.H" line 88 kEpsilon.C)

Formally and for consistency w
 

Formally and for consistency we should have a correction for snGrad(U) on the wall to get the correct drag though.

Does anyone feel like changing them all?

Hrv

Drag coefficient amplitude
 

Hello everyone,

I need some assistance on understanding why in the drag coefficient time diagram, i am getting the correct frequency according to the Re number but the amplitude is totally different from past studies in papers. more specifically it should oscillate around 1.44 and mine oscillates around 3. Also in other cases with different mesh it drops to 0.3. although frequency is correct. Does anybody know about amplitude dependency on either numerical or physical factors that could help me understand why. I am using openfoam and i have also used another code (non commercial) that shows the same thing.

Regards
Konstantine