
[Sponsors] 
April 3, 2014, 09:05 
simpleFoam with kOmegaSST

#1 
Member
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 13 
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 

April 3, 2014, 09:46 

#2 
Senior Member

Hi,
surely someone can help you. What's your question besides a possibility of help? 

April 3, 2014, 10:06 

#3 
Member
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 13 
Hi,
the question is: what are the right formulas for kw turbolence model in order to write the right values of k and w and not random values? thank you. 

April 3, 2014, 10:17 

#4 
Senior Member

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. 

April 3, 2014, 11:01 

#5 
Member
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 13 
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= (1.2e3)*0.038= 4.56e5 k = 1.5*(Ux * I)^2 = 0,105 then w=13000 are they reasonable? 

April 3, 2014, 11:19 

#6 
Senior Member

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.esicfd.com/esiusers/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. 

April 4, 2014, 05:34 

#7 
Member
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 13 
Thank you for the links.
My model goes to convergence in about 320 iterations. (with simpleFoam and kw 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 

April 4, 2014, 05:50 

#8 
Senior Member

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. 

April 4, 2014, 06:48 

#9 
Member
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 13 
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 

April 7, 2014, 06:06 

#10 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Davide, are you sure you mean "structured"? This doesn't look like a structured mesh, I guess you mean a hexamesh, right?
__________________
The skeleton ran out of shampoo in the shower. 

April 7, 2014, 07:04 

#11 
Member
Davide Pasini
Join Date: Mar 2009
Posts: 34
Rep Power: 13 
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 

April 7, 2014, 07:12 

#12 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
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. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
interFoam vs. simpleFoam channel flow comparison  DanM  OpenFOAM Running, Solving & CFD  12  January 31, 2020 16:26 
simpleFoam kOmegaSST LowRe pressure divergence  Pat84  OpenFOAM Running, Solving & CFD  2  August 12, 2013 18:42 
OpenFOAM 2.x simpleFoam and kOmegaSST convergence and wall treatment  gillimaniac  OpenFOAM Running, Solving & CFD  6  August 1, 2013 02:36 
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 10:02 