CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

a little smaller Strouhal number

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 16, 2013, 07:07
Default a little smaller Strouhal number
  #1
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
hi everyone!
I am simulating flow around cylinder at Re=100. But no matter how I tried, the St number I am obtaining remains 1.4, for which an accurater one is 1.6.
does someone have any suggestion on how to get the accurate St number?

my case setup is like this:
D=1, U=1, nu=0.01, no turbulence model.

any help is appreciated!
kkpal is offline   Reply With Quote

Old   May 16, 2013, 07:18
Default
  #2
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
Hi, what size is your domain, i.e. how many D upstream and downstream of the cylinder?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   May 16, 2013, 07:33
Default
  #3
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
Hi, what size is your domain, i.e. how many D upstream and downstream of the cylinder?
Thank you for your quick reply.
upstream, top and bottom distance are all 20D, downstream 40D. I've tried refine my mesh, but the result is not satisfactory.
kkpal is offline   Reply With Quote

Old   May 16, 2013, 07:36
Default
  #4
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
Can you also tell us the density and the viscosity?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   May 16, 2013, 08:00
Default
  #5
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
Can you also tell us the density and the viscosity?
the density rho is set to be 1, and the kinematic viscosity is 0.01. With velocity=1 and Diameter=1, that makes Re =100.
the software I'm using is OpenFoam.
I get quite good result in terms of drag and lift coefficients, but for St, it's always smaller.
kkpal is offline   Reply With Quote

Old   May 16, 2013, 08:40
Default
  #6
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
How many time steps per cycle do you have? How much do the residuals go down each time step? How large is the domain perpendicular to the flow?

Maybe you want to have a look at this thread:
http://www.cfd-online.com/Forums/mai...r-re-40-a.html
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   May 16, 2013, 09:40
Default
  #7
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
How many time steps per cycle do you have? How much do the residuals go down each time step? How large is the domain perpendicular to the flow?

Maybe you want to have a look at this thread:
http://www.cfd-online.com/Forums/mai...r-re-40-a.html
My timestep is decided by the Courant number=0.5, in my case deltaT is around 0.01s. Suppose St=0.2, vortex shedding period is around 5s, so there are 500 timesteps for each shedding cycle.

" the domain perpendicular to the flow", do you mean the height of the Z axis? it is 0.1D, as D=1, it should be 0.1. My case is 2d so I think it does not matter.

As for the residuals, in OpenFoam different variables have different residuals, here is my setting for residuals in openfoam
Code:
solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0.01;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    pFinal
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    "(U|k|epsilon)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }

    "(U|k|epsilon)Final"
    {
        $U;
        tolerance       1e-05;
        relTol          0;
    }
}

I will have a look at that post first.
thanks for your help! phillipp
you are very kind!
kkpal is offline   Reply With Quote

Old   May 16, 2013, 09:43
Default
  #8
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
500 time steps is really huge... 50 should be by far enough as far as I know.

No, sorry I don't mean the hight of the cylinder but the "other" dimension of your 2d flow domain. But sorry I just saw that you already wrote "2*20D" in your previous post...

What about your grid? Can you post a picture of it? How many cells do you have?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   May 16, 2013, 09:49
Default
  #9
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
here is a picture of the domain and mesh.
mesh information:
70900 elements
47488 vertices

by the way, do you have a similar mesh file that yields good St number? if you have, could you please send to me so i can test in my own case?
Attached Images
File Type: jpg domain.jpg (98.3 KB, 21 views)
kkpal is offline   Reply With Quote

Old   May 16, 2013, 09:55
Default
  #10
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
No, unfortunately not, and I am currently running computationally expesive simulations, so I can't just give it a try...
Maybe tomorrow.

Btw: You mean St=0.16 and not 1.6 in your first post, right?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   May 16, 2013, 10:06
Default
  #11
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
yes, that's what i mean. my St number is 1.4, which I think is too low. actually according to the references i found, St should be around 1.65 when Re is 100.
If you have time, please help me with that mesh file, this problem has been haunting me for a week!
It's 23pm in japan now and I need to go home.
i will let you know if i have any progress.
thank you again for you kind help!
have a nice evening!
kkpal is offline   Reply With Quote

Old   May 16, 2013, 12:01
Default Mesh is available
  #12
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,329
Blog Entries: 6
Rep Power: 45
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Quote:
Originally Posted by kkpal View Post
here is a picture of the domain and mesh.
mesh information:
70900 elements
47488 vertices

by the way, do you have a similar mesh file that yields good St number? if you have, could you please send to me so i can test in my own case?
Mesh can be downloaded from links given in thread
http://www.cfd-online.com/Forums/mai...r-re-40-a.html

Possible issues are:

1. Mesh

2. Convergence (reduce convergence level to 1e-19). Laminar flow should be converged more tightly.

3. Method of determining the strouhal number including the manipulation of transient data

4. Time step size

Quote:
Originally Posted by kkpal View Post
yes, that's what i mean. my St number is 1.4, which I think is too low. actually according to the references i found, St should be around 1.65 when Re is 100.
Are you talking about Cd ?

Few results from Ansys documentation for similar case:


Last edited by Far; May 16, 2013 at 12:15. Reason: adding something more
Far is offline   Reply With Quote

Old   May 16, 2013, 13:23
Default
  #13
Senior Member
 
cfdnewbie
Join Date: Mar 2010
Posts: 557
Rep Power: 13
cfdnewbie is on a distinguished road
What type of BCs are you applying on the free surfaces? What quantity do you use to measur Str? How do you determine the frequency? By FFT or by eye? Have you validated your code for other cases?
cfdnewbie is offline   Reply With Quote

Old   May 17, 2013, 01:48
Default
  #14
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
For Far:
yes, I made a mistake in the previous post.
My St is 0.14 while the accurate one should be 0.16.
I'm trying lowering the convergence level to 1e-12 because lowering to 1e-18 really takes a lot of time. I will post the result when it is finished.
As for the two pictures you posted, I think in my case, both timestep per cycle(in my case 500 timesteps per cycle) and number of nodes(in my case 47488 vertices) are fine enough.

For cfdnewbie:

inlet
U: fixed value (1 0 0)
p: zeroGradient

outlet
U: zeroGradient
p: fixed value 0

cylinderwall
U: fixed value (0 0 0)
p: zeroGradient

sidewall
U: slip
p: slip

frontandback
U,p: empty (indicate 2D)

I used the data from Cl(lift force coefficients) to calculate the Str. Both Fourier transform and direct observe from the Cl plot diagram yield the same result.

since I am using OpenFoam, I suppose the code itself should be correct, the problem is I have to find the appropriate mesh and settings.
Actually what I am trying to solve is a validation case, after this I will perform some simulations with higher Re and more sophisticated geometry.
kkpal is offline   Reply With Quote

Old   May 17, 2013, 01:54
Default
  #15
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
You should have a look at the boundary layer at your cylinder and see how many grid points you use to resolve it.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   May 17, 2013, 01:58
Default
  #16
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
The result of convergence level 1e-12 has come out. St remains 1.44.
It seems the problem does not come from convergence level.

the numerical schemes I'm using is like this:
Code:
ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
    grad(U)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss limitedLinearV 0.5;
    div(phi,k)      Gauss limitedLinear 0.5;
    div(phi,epsilon) Gauss limitedLinear 0.5;
    div(phi,R)      Gauss limitedLinear 0.5;
    div(R)          Gauss linear;
    div(phi,nuTilda) Gauss limitedLinear 0.5;
    div((nuEff*dev(T(grad(U))))) Gauss cubic;
}

laplacianSchemes
{
    default         none;
    laplacian(nuEff,U) Gauss linear corrected;
    laplacian((1|A(U)),p) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DepsilonEff,epsilon) Gauss linear corrected;
    laplacian(DREff,R) Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
    interpolate(U)  linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}
Do you think I need to change one thing or two?
kkpal is offline   Reply With Quote

Old   May 17, 2013, 03:40
Default
  #17
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,329
Blog Entries: 6
Rep Power: 45
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
You can find mesh here : http://www.cfd-online.com/Forums/ansys-meshing/96191-meshing-gambit-analysis-flow-past-cylinders.html.

Try it and see whether you get better results or not?
  1. How many cycles you are considering for finding St no? .
  2. did you include initial transients?
  3. After how many cycles you collected data?
  4. What time step you are using and how did you calculate it?
  5. I would use maximum 50-60 time steps per cycle and at least 3-4 cycles when initial transient are vanished!!!
PS : openfoam related question can be best answered in openfoam forum
Far is offline   Reply With Quote

Old   May 17, 2013, 05:59
Default
  #18
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
Philipp: here is a zoom in look of the mesh near the cylinder. I've tried dividing the perimeter of the cylinder into 128 and 200, but with no luck.

Sijal: here is a picuture of the Cl plot.
For FFT, I cut the former part of this plot and used the steady one do calculate frequency. for example, in this case I used 160s~240s to do FFT. I also calculated frequency by manually observe the time difference between two peaks in the steady part.
I decide timestep by courant number<0.5, and usually timestep is 0.01 or smaller, depending on the smallest grid size and mesh fineness. One disadvangtage of this is that my timestep is not even. When doing FFT, I used EXCEL to first get a time-uniformly distributed data by linear interpolation, then perform FFT in matlab using this data with a constant timestep.

besides, the mesh you provided seems problematic when converting to openfoam mesh, anyway I am working to solve this.
Attached Images
File Type: jpg zoomin.jpg (53.2 KB, 12 views)
File Type: jpg Cl plot.jpg (60.1 KB, 17 views)
kkpal is offline   Reply With Quote

Old   May 17, 2013, 06:14
Default
  #19
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
Sorry, I mean the actual flow field (e.g. velocity), not the mesh.
You should have a look at the spatial sampling of the velocity, perpendicular to the wall. You need to ensure, that the boundary sheath grid spacing is fine enough to capture the relevant effects...
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   May 17, 2013, 20:30
Default
  #20
Senior Member
 
Join Date: Jan 2013
Posts: 121
Rep Power: 6
kkpal is on a distinguished road
dear all

my problem of getting smaller Str number is now solved.

It turns out that my mesh is Ok, the problem lies in the under-relaxation factor I employed in this unsteady cases. It is found out when using under relaxation in unsteady cases, the simulation won't be time-accurate, so in my case Drag and lift coefficients are OK but vortex shedding frequency becomes bad. I removed the relaxation factors in my settings and then the right results came out.

anyway, I really appreciate your help in this thread!
kkpal 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
compressible flow in turbocharger riesotto OpenFOAM 50 May 26, 2014 01:47
ERROR #001100279 has occurred in subroutine ErrAction. smnaryal CFX 7 January 3, 2013 19:09
error in parallel run immortality OpenFOAM Running, Solving & CFD 7 January 1, 2013 14:35
Problem with decomposePar tool vinz OpenFOAM Pre-Processing 18 January 26, 2011 03:17
strouhal number for ellipse ek Main CFD Forum 2 December 25, 2008 00:15


All times are GMT -4. The time now is 18:10.