
[Sponsors] 
March 10, 2013, 15:42 
fineness of a mesh

#1 
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 3 
Good evening,
I am a new CFD user, I have to simulate a burner with reactingFoam but I'm not sure of the fineness of my mesh. The chamber is a cylinder 50 cm long and has a diameter of 20 cm Since it is a axisymmetric problem, I try to simulate only a wedge of the cylinder of 5° and one cell thick. I suppose the mesh is finner at the inlet and near the wall , and is coarser at the outlet. but how many cells do I have to set? or either what is the necessary size of the smallest cell ?  First if I use the RANS calculation ? Is there a thumb rule like with LES simulation? h<30 n where h is the grid size and n is the kolmogorov length scale Thank you in advance for you answer Cam 

March 17, 2013, 04:16 

#2 
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 3 
Nobody can help me?


March 17, 2013, 06:50 

#3 
Senior Member
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 292
Rep Power: 11 
Hi Camille,
The best way of determining the number of cells required, is by performing a grid sensitivity study. Start by solving your problem on a coarse grid and systematically refine it. For each simulation, calculate a parameter that is of importance for you (something similar like the drag force on a cylinder). At a certain moment the parameter will stop changing with increasing number of cells and that's the number of cells you would want to use. Have fun! Cheers, L 

March 17, 2013, 07:38 

#4 
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 3 
Hi Lieven,
Thank you very much for your answer, I'll try this and let you know. So if I have to try simulation for différent meshes I have to know how long I have to simulate the case? In laminar I think it is common to simulate a certain time to ensure we are in steady state such as 10 times the real time needed. Is it right? c.f. user guide U22 In a first time I'm using RANS so does it has an impact ? the velocity : U = 5.77 m/s the chamber's length : L = 51e2 m so the time needed for the mix to run along the chamber : t = L/U = 0.088 seconds so if I simulate 1 s it is far enough, is it? And what if I use kEpsilon model? and then LES ? Thank you for your help Cam 

March 21, 2013, 10:22 

#5 
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 488
Rep Power: 17 
Just to add a little to what has been said. For RANS, in addition to grid size independence, your turbulence model will have some y+ value requirements. You will need to run a simulation, determine the y+ and then adjust the mesh appropriately (refining or even remeshing). Different turbulence models will need different y+ values.
__________________
Dan


March 24, 2013, 10:22 

#6 
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 3 
Hi Dan,
thank you for you response. So I 'd like to use the app here : http://www.cfdonline.com/Tools/yplus.php but I'm not sur of all my parameters... Input Freestream velocity: 5.77 [m/s] Density: 0.6709 (for CH4) [kg/m3] Dynamic viscosity: 1.5e5 [kg/ms] Boundary layer length: ?? don't know [m] Desired Y+ value: ?? don't know [] Output Reynolds number: [] Estimated wall distance: [m] So I don't know either the boundary layer length neither de desired Y+ value ? And what will I do with the results? :/ Sorry I m a bit lost... 

March 24, 2013, 10:28 

#7 
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 3 
I stil don't know how long do I have to simulate the case?
with combustion turned on TRUE and chemistry turned ON with laminarRASModel in turbulenceProperties it took more than 1 day and 20 hours to run on 8 CPU in parallel and then fail at 1.4 seconds... :/ 

March 24, 2013, 11:26 

#8 
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 488
Rep Power: 17 
With problems that are in really complex systems, its best to stage your solution procedure to push towards an overall solution. Do cold flow, i.e. no temperature, no reactions, no radiation...just momentum. Then slowly make your simulation more complicated by adding turbulence, temperature, chemistry, etc. and you will move towards your final goal.
For y+, use the yPlusRAS utility in OpenFOAM. It is a post processing tool, so run your cold flow to steadystate and then get your yPlus values. Remesh were necessary, map the values from your old solution to your new mesh with mapFields and then continue until you get an appropriate yPlus value for that turbulence model. Once this is good....then move onto more complicated physics by adding temperature. Make sure to check you y+ when you move to new physics as it may change from the added transport effects.
__________________
Dan


March 26, 2013, 16:24 

#9  
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 3 
Hi Dan,
thank you for the precisions. I ll try to run my case in "cold flow" and then postProcess it with the yPlusRas utility for which I'll surely have some questions... but for the moment then : I switch off turbulence, combustion and chemistry such that : chemistryProperties > chemistry off; combustionProperties > combustionModel PaSR<psiChemistryCombustionModel>; active false; tubulenceProperties > simulationType RASModel; > RASProperties laminar; You told also no temperature , so what does that mean in term of BC? here is my T bcs , what should I change to run cold flow? And how longdo I have to run the case to be in steady state ? My chamber is a cylinder of 0.51 m long with 0.22 m of diameter and the initial velocity is 5.77 m/s. the inlet is a circle with 0.035 m diameter. Quote:


March 26, 2013, 16:45 

#10 
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 488
Rep Power: 17 
As an optional method (preferred), you could use simpleFoam. A laminar or turbulent steadystate solver for isothermal, incompressible, nonreacting flows. The take that flow field and move back to your current solver.
__________________
Dan


March 26, 2013, 16:50 

#11 
Senior Member
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 292
Rep Power: 11 
If you set if you set the RASProperties to laminar, you will probably never reach steady state. Wel ok, it depends on the Reynolds number (with very low Re you might reach a steady state) but since you want to use a RASModel I'm assuming the flow will be turbulent.
So my advice, either run the laminarcase for 100 timesteps or so and enable then the turbulence model (you can simply do this with the 'turbulence on/off' flag instead of changing the RASModel in RASProperties). This way you simply get a better initial velocity field for the turbulence model. Or alternatively, you can simply try to start your simulation with the RASModel enabled. I you don't set the time step too big, this will work as well... Cheers, L 

March 27, 2013, 14:22 

#12  
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 3 
Hello,
Well here is my case, http://dfiles.eu/files/y5fimgxvz I ran it with icoFoam , no chemistry, no combustion an RASModel for turbulence.  first I ran it also without transportProperties file but to use the yPlusRAS utilty, OF asked me this file. Then I added it with cinematic viscosity 1e5 m²/s and transportModel Newtonian.. Now I check the yPlus files in each timeStep but it is value 0 everywhere.. so what am I suppose to understand? is it because I have this message at each time step : Quote:
In another case (ran with reactingFoam I tested YPlusRAs utility with compressible option but OF told me at each time step : Quote:
Thank you for your help Last edited by camille131; March 27, 2013 at 14:40. Reason: more to say .. 

March 27, 2013, 14:57 

#13 
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 488
Rep Power: 17 
There seems to be some miscommunication here
Your ultimate goal is to get a full simulation of a reacting flow in a chamber. In order to do that you will need a flow field, species transport, and possibly temperature field. In a previous post, I suggest you start with solving only momentum, and if the system is in a regime in which steadystate flow can be achieved, I would use simpleFoam. SimpleFoam is a steady state solver for isothermal flows. it can model both laminar and turbulent (using RANS) flows where the user defines what turbulence model to use e.g. laminar, kEpsilon, etc.
__________________
Dan


March 27, 2013, 15:15 

#14 
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 3 
Sorry I am lost . I thought I had to use yPlusRAS utility on the simple case with only transport.
Isn't it ok for the case I just posted? 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Star CCM Overset Mesh Error (Rotating Turbine)  thezack  CDadapco  3  December 11, 2013 03:09 
[ICEM] surface mesh merging problem  everest  ANSYS Meshing & Geometry  39  June 5, 2013 19:02 
Inner geometry gets lost exporting mesh from ICEM CFD to CFXPre  powpow  CFX  3  December 20, 2012 09:14 
[ICEM] Problem making structural mesh on a surface  froztbear  ANSYS Meshing & Geometry  1  November 10, 2011 08:52 
snappyHexMesh won't work  zeros everywhere!  sc298  OpenFOAM Native Meshers: snappyHexMesh and Others  2  March 27, 2011 21:11 