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

simpleFoam with kOmegaSST

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 3, 2014, 08:05
Default simpleFoam with kOmegaSST
  #1
Member
 
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 10
ilpaso is on a distinguished road
I'm trying to run a case with simpleFoam and kOmegaSST.

The geometry is a cycinder (diameter 3mm) with a shrinkage (diameter 1.2mm). Length 117mm
the estimated Reynolds is about 1700. (U=4.42 m/s diameter 1.2mm)

First I've to define the k and omega. According with THIS page w=sqrt(k)/L. L (turbolence length scale) is defined L=0.038*d.
The result of all these formulas are k=4.78 and w=4.8e5!!!!!

I've read THIS and with these formulas k=0.073 and w=k/epsilon=27

I am very confused.
can anyone help me?

thank you
ilpaso is offline   Reply With Quote

Old   April 3, 2014, 08:46
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,668
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Hi,

surely someone can help you. What's your question besides a possibility of help?
alexeym is offline   Reply With Quote

Old   April 3, 2014, 09:06
Default
  #3
Member
 
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 10
ilpaso is on a distinguished road
Hi,
the question is:
what are the right formulas for k-w turbolence model in order to write the right values of k and w and not random values?

thank you.
ilpaso is offline   Reply With Quote

Old   April 3, 2014, 09:17
Default
  #4
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,668
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Are you trying to set initial values, boundary conditions, anything else?

For example if you look into turbulentMixingLengthFrequencyInletFvPatchScalarFi eld.H and turbulentIntensityKineticEnergyInletFvPatchScalarF ield.H you find the formulas OpenFOAM is using for calculating k and w from given intensity and length scale:

k = 1.5*(UI)^2

and

w = sqrt(k)/(L*Cmu^0.25)

Intensity depends on the case (from below 0.01 upto 0.2), L can be taken equal to 0.038D.
alexeym is offline   Reply With Quote

Old   April 3, 2014, 10:01
Default
  #5
Member
 
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 10
ilpaso is on a distinguished road
I'm trying to set up the entire case.
After the geometry the next step is to choose the right model (I hope).
But I didn't understand the formulas and I didn't find any reference in the userguide.

At the end of THIS wiki page there is a formula about w a bit different from your. w=Cmu^0.25 * sqrt(k) / L
Is this wrong?


with the formulas you wrote, if:
I = Re^(-1/8)*0.16=0,06 (supposed Ux=4.42, Uy=0, Uz=0, x is the axis of cylinder)
L = diam * 0.038= (1.2e-3)*0.038= 4.56e-5
k = 1.5*(Ux * I)^2 = 0,105
then w=13000

are they reasonable?
ilpaso is offline   Reply With Quote

Old   April 3, 2014, 10:19
Default
  #6
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,668
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
Formula in the wiki is Cmu^(-0.25)*sqrt(k)/L and is the same as I've cited from source code.

Here are links to FLUENT and ESI Group pages on defining turbulence parameters:

http://combust.hit.edu.cn:8080/fluen...ug/node175.htm

http://support.esi-cfd.com/esi-users/turb_parameters/

They are not much different from the wiki page.

Take a look at tutorials using kOmegaSST, check the typical values in the tutorial, compare with yours.
alexeym is offline   Reply With Quote

Old   April 4, 2014, 04:34
Default
  #7
Member
 
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 10
ilpaso is on a distinguished road
Thank you for the links.
My model goes to convergence in about 320 iterations. (with simpleFoam and k-w turbolence model (not komegaSST)
What do you think about this result? I'm running iterative simulations and any improvement is appreciated.
The mesh has about 160000 hexahedra elements.
Attached here you can find my case if you want take a look........
There is not the mesh because it is 28Mb but there is an image of the geometry
The main diameter is 3mm and at the shrinkage the diameter is 1.2mm
Attached Images
File Type: png case.png (14.5 KB, 15 views)
Attached Files
File Type: zip myCase.zip (12.1 KB, 2 views)
ilpaso is offline   Reply With Quote

Old   April 4, 2014, 04:50
Default
  #8
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,668
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
Send a message via Skype™ to alexeym
As I don't know your final aim, I can't say anything about results.

Case converged? Results seems to be reasonable? OK, go to the next problem.

You've shown geometry but not the mesh itself. Maybe you need to increase density near the walls, check y+.

You'd like to decrease number of iterations/calculation time? Play with discretisation schemes and linear system solvers.
alexeym is offline   Reply With Quote

Old   April 4, 2014, 05:48
Default
  #9
Member
 
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 10
ilpaso is on a distinguished road
thank you Alexey!
Your suggestions are always precious!

Only for info:
the mesh is structured with increased density near the wall.
Attached here there are 2 images.
I'm learning step by step
Attached Images
File Type: jpg front.jpg (64.3 KB, 19 views)
File Type: jpg lateral.jpg (52.7 KB, 22 views)
ilpaso is offline   Reply With Quote

Old   April 7, 2014, 05:06
Default
  #10
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 20
RodriguezFatz will become famous soon enough
Davide, are you sure you mean "structured"? This doesn't look like a structured mesh, I guess you mean a hexa-mesh, right?
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   April 7, 2014, 06:04
Default
  #11
Member
 
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 10
ilpaso is on a distinguished road
I Philipp,
thank you for your reply! Every day reading this forum I can reflect as I am ignorant about the cfd world.

Ok. My mesh is not structured. Can I say it is hybrid: structured at the boundary layer and not structured in the middle?

Thank you
ilpaso is offline   Reply With Quote

Old   April 7, 2014, 06:12
Default
  #12
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 20
RodriguezFatz will become famous soon enough
Structured or not just describes the way the data is stored in the memory. Having a box meshed by hexas with dx=dy=dz doesn't necessarily mean, that the mesh is structured. But it can be. I think most solvers use only unstructed meshes. Your mesh is probably just completely unstructured.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz 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
simpleFoam kOmegaSST LowRe pressure divergence Pat84 OpenFOAM Running, Solving & CFD 2 August 12, 2013 17:42
OpenFOAM 2.x simpleFoam and kOmegaSST convergence and wall treatment gillimaniac OpenFOAM Running, Solving & CFD 6 August 1, 2013 01:36
interFoam vs. simpleFoam channel flow comparison DanM OpenFOAM Running, Solving & CFD 11 January 5, 2013 07:21
Problem running simpleFoam with kOmegaSST turbulence model matzbanni OpenFOAM Running, Solving & CFD 5 November 3, 2012 07:45
Wrong calculation of nut in the kOmegaSST turbulence model FelixL OpenFOAM Bugs 27 March 27, 2012 09:02


All times are GMT -4. The time now is 14:06.