CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Velocity Uz in 2D

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 31, 2007, 03:22
Default Hello there, Im computing s
  #1
hoochie
Guest
 
Posts: n/a
Hello there,

Im computing some cases of an airfoil in 2D. My results are looking terrible, because OpenFoam seems to compute a velocity in z-direction which shouldnt be there. This can be seen in paraFoam.
So I changed my boundary conditions from empty to symmetry plane, in hope to fix this problem. It didnt. Do you have any clue why this mistake appears? Or did you have problems of the same kind in past and solved them?

Thx in advance
  Reply With Quote

Old   May 31, 2007, 03:35
Default Is your mesh flat? Are the bo
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22
hjasak will become famous soon enough
Is your mesh flat? Are the boundary conditions OK?

If you want an example where everything works fine in 2-D to start comparing against, have a look at the lid-driven cavity tutorial.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 31, 2007, 04:11
Default Hello Hrvoje, thx for your
  #3
hoochie
Guest
 
Posts: n/a
Hello Hrvoje,

thx for your answer. I converted a 2D- mesh from fluent to OpenFOAM. OpenFOAM put a front and back patch as empty in my mesh and it got a thickness of 1 cell. Like in the lid-driven cavity too.
My boundary conditions are very sipmle for this case, so I dont think they will be wrong.
On the left I got a velocity- inlet, on the right a pressure- outlet, top and down patches are symmetry planes and in the middle I got my airfoil as a wall with wallfunctions.
By the way, computing it first order with upwind isn't causing any problems. But I need it second order computed to get realistic results.
Whenever I compute it second order with linear I get a high value of velocity in z-direction.

For example, my inlet velocity is 29.21 m/s in x-direction, after 5000 Iterationsteps I have got a velocity in z about 54 m/s.

Any suggestions?
  Reply With Quote

Old   May 31, 2007, 16:39
Default Well, you are using fully impl
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22
hjasak will become famous soon enough
Well, you are using fully implicit central differencing on a case with very little damping. I would recommend starting with a stabilised second order differencing scheme like

GammaV 0.2

This will still give you second order and should get rid of the z-velocity.

What is your max Co number? With full central differencing you have to be very careful, i.e. keep it below 1.

Good hunting,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 1, 2007, 06:07
Default Hello Hrv, I computed now m
  #5
hoochie
Guest
 
Posts: n/a
Hello Hrv,

I computed now my case with different schemes for div(phi, u), i tried:

linearLimitedV 1.0
vanLeerV 1.0
SFCD
GammaV 0.2 and 1.0

The results are looking good, but I get always a velocity in z-direction which is growing during iterations. Of course they are not as high as with linear, but they are still present and increasing.
Beyond that, I computed theese cases also with "symmetry plane" instead of "empty" at front and back plane. With "symmetry plane" the convergence looks much better and the z-velocity is much lower than with "empty" (After 2000 iterationsteps, empty: about 1.5 m/s, symmetry plane: about 0.05 m/s).
But still there is a velocity in z-direction

Edit: I forgot to mention, that Im working with simpleFoam, so steadystate and incompressible

greetings
RW
  Reply With Quote

Old   June 1, 2007, 06:20
Default In that case, I know what your
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22
hjasak will become famous soon enough
In that case, I know what your problem is: your geometry is not perfectly flat.

Try running checkMesh and see what it says. I think we also have an application called flattenMesh, which may help sort this out.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 1, 2007, 06:27
Default Hello Hrv, this is my check
  #7
hoochie
Guest
 
Posts: n/a
Hello Hrv,

this is my checkMesh- Result:

Checking geometry...
Boundary openness in x-direction = 6.10623e-16
Boundary openness in y-direction = 2.72005e-15
Boundary openness in z-direction = 0
Boundary closed (OK).
Max cell openness = 1.11022e-16 Max aspect ratio = 10.812. All cells OK.

Minumum face area = 1.09727e-06. Maximum face area = 0.549449. Face area magnit udes OK.

Min volume = 6.82782e-07. Max volume = 0.159888. Total volume = 301.103. Cell volumes OK.

Mesh non-orthogonality Max: 42.4074 average: 5.76578
Non-orthogonality check OK.

Face pyramids OK.

Max skewness = 41.9705 percent. Face skewness OK.

Minumum edge length = 0.000827862. Maximum edge length = 0.882998.

All angles in faces are convex or less than 10 degrees concave.

Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 1
All faces are flat in that the ratio between projected and actual area is > 0.8

Geometry check done.

Looks fine to me, or did I miss something?

RW
  Reply With Quote

Old   June 1, 2007, 06:59
Default Hmm, looks fine. There may be
  #8
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22
hjasak will become famous soon enough
Hmm, looks fine. There may be an instability in the way you prescribed boundary conditions, but now I'm really clutching at straws. Are you using Gauss gradients or least squares?

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 1, 2007, 07:19
Default Im using Gauss- gradients, but
  #9
hoochie
Guest
 
Posts: n/a
Im using Gauss- gradients, but upwind for turbulence:

grad(p) Gauss linear;
grad(U) Gauss linear;
grad(epsilon) Gauss upwind phi;
grad(k) Gauss upwind phi;
snGradCorr(U) Gauss linear;
snGradCorr(p) Gauss linear;
grad(magSqr(U)) Gauss linear;
grad(magSqr(p)) Gauss linear;
snGradCorr(epsilon) Gauss upwind phi;
snGradCorr(k) Gauss upwind phi;

RW
  Reply With Quote

Old   June 1, 2007, 07:29
Default Not good: in ALL gradients you
  #10
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22
hjasak will become famous soon enough
Not good: in ALL gradients you should be using either linear or harmonic interpolation. This is not a convection term, where you need to stabilise the scheme with respect to the flux - that lot will be under divSchemes.

Try again and please let me know what happened.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 1, 2007, 07:54
Default Mmm I cant find a way to set u
  #11
hoochie
Guest
 
Posts: n/a
Mmm I cant find a way to set up "harmonic" in grad-schemes. OpenFOAM tells me it is not available.
Harmonic is neither in the list of Gauss nor in the list of gradschemes.

RW
  Reply With Quote

Old   June 1, 2007, 07:58
Default Edit: Running the case with al
  #12
hoochie
Guest
 
Posts: n/a
Edit: Running the case with all grad-schemes to linear is having no effect on the Uz. After 1000 Iterationsteps I have got 3 m/s in z-direction

RW
  Reply With Quote

Old   June 1, 2007, 08:26
Default Do you use an older version of
  #13
Member
 
Rolando Maier
Join Date: Mar 2009
Posts: 89
Rep Power: 9
rolando is on a distinguished road
Do you use an older version of OpenFoam?

Are you sure, that your empty boundaries are REALLY orthogonal to the z-direction?

Rolando
rolando is offline   Reply With Quote

Old   June 1, 2007, 08:37
Default Hello Roland, Im using OF 1
  #14
hoochie
Guest
 
Posts: n/a
Hello Roland,

Im using OF 1.4.

All I can say is, that checkMesh is telling me my mesh is flat and in the conversion from Fluent-mesh to OpenFOAM-mesh both empty-planes were created, so I assume they are orthogonal to the z- direction.
Is there any special tool apart from checkMesh which will give more information about that?

RW
  Reply With Quote

Old   June 1, 2007, 09:03
Default I donīt think there is an othe
  #15
Member
 
Rolando Maier
Join Date: Mar 2009
Posts: 89
Rep Power: 9
rolando is on a distinguished road
I donīt think there is an other tool to do this checking.

What does your mesh look like? Is it a planar mesh with only one cell in z-direction?
This would exclude cells of tetraeder and pyramid types.

Rolando
rolando is offline   Reply With Quote

Old   June 1, 2007, 09:26
Default Yes my mesh is a mesh with one
  #16
hoochie
Guest
 
Posts: n/a
Yes my mesh is a mesh with one cell in z-direction. It has been an unstructured 2D-mesh and was converted into the OpenFOAM-mesh.

RW
  Reply With Quote

Old   June 6, 2007, 19:21
Default This could be an issue with yo
  #17
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 13
msrinath80 is on a distinguished road
This could be an issue with your geometry import. The simplest way to test it is to put in a little extra effort and try to build your airfoil using blockMesh. If the Uz velocity problem goes away, that's your clue!

I trust blockMesh more than any other converter no matter how extensively they have been tested because it was written specifically with OpenFOAM in mind. Since yours is a fairly simple 2D airfoil you could get away with blockMesh.

Check this thread for some blockMesh Airfoil hints:
http://www.cfd-online.com/OpenFOAM_D...es/1/3508.html
msrinath80 is offline   Reply With Quote

Old   June 7, 2007, 12:02
Default Hello pUI thank you for you
  #18
hoochie
Guest
 
Posts: n/a
Hello pUI

thank you for your idea, its a good one, I will check this out!

RW
  Reply With Quote

Old   June 7, 2007, 13:25
Default Hello again, by the way ano
  #19
hoochie
Guest
 
Posts: n/a
Hello again,

by the way another question, if Im computing my case with front- and back-plane as empty, no Uz is calculated in the computation, but in the end it is still present, with high values. Does this Uz will have an effect on my other results for Ux, Uy and p, or is it possible to ignore those Uz- values and take the rest for 100 percent accuracy? Maybe a programmer can answer this.
I really dont get, how a velocity in z-direction can exist, if it is not calculated, maybe some error during interpolation?

Thx in advance

RW
  Reply With Quote

Old   June 7, 2007, 14:14
Default No interpolation: what is your
  #20
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,784
Rep Power: 22
hjasak will become famous soon enough
No interpolation: what is your z-velocity in the initial field for U? Throw aweay all results and try again.

Please let me know,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
Steady pipe flow mean velocity higher than inlet velocity anita OpenFOAM Running, Solving & CFD 7 September 25, 2012 05:35
Velocity profile as an velocity intlet condition kees FLUENT 3 April 16, 2008 18:35
velocity profile as an velocity inlet condition KEES Main CFD Forum 0 April 15, 2008 11:26
Head loss function of velocity^2 or velocity^1? jrg Main CFD Forum 1 November 19, 2007 14:09
how to plot RMS velocity (fluctuating velocity) nash Main CFD Forum 0 October 18, 2006 16:37


All times are GMT -4. The time now is 13:25.