DNS of liquid sheets using interfoam and blockMesh
Hello forum,
I would like to know if it is possible to perform a Direct Numerical Simulation of a liquid sheet using interfoam for relatively low Re numbers. I would like to know the maximum number of cells that blockMesh can handle without any errors. I am using OF1.5. However i know the limitations of Interface compression scheme, but the main aim of my study is to study the accuracy of interface compression scheme for primary atomization problems. I am also performing some les simulations using lesInterfoam but i want to know the possibility of performing a DNS using interfoam. My main concern is about blockMesh, as i am not sure if it can handle cells of the range of 0.5 micrometer. any suggestions would be appreciated. bye with regards K.Suresh kumar 
OpenFOAM has no problems in handling the small cells. I am not exactly sure of interface compression scheme but the numerical schemes for convection in openfoam may be dissipative for performing DNS unless you refine the grid.

Hello harish,
Thankyou for your reply. As you mentioned that the convective schemes of OpenFOAM may not be sufficient unless i have fine meshes. I have some comments on this: Recently I read the paper "Direct Numerical simulation and analysis of instability enhancing parameters in Liquid sheets at moderate Reynolds numbers" Wolfgang sander and Bernhard Weignand, Physics of Fluids 20, 053301 (2008). In this paper it is mentioned that Based on the theory of universal equilibrium by kolmogrov which is, lamda_k = L_t/Re_t^(3/4), Re_t = rho_l u^' L_t/mu_l Estimating L_t~~ D/10 and u^'~~0.1U_0 for turbulent channel flows, the smallest scale lamda_k appearing within the range of Re=30007000 for liquid sheets is on the order of 13micromter. The grid spacing used in this paper varies between 4 and 11.4 micrometer. The spatial discretization used is second order accurate, seocnd order upwind approximation for convection terms and central differences elsewhere. Basically the fully conservative momentum convection and volume fraction transport, momentum diffusion are explicitly treated. So my question is if i have a mesh resolution of that specified above will my DNS calculation with interFOAM be ok. Secondly do I have any second order upwind scheme implemented in OF1.5. Provided If i have a mesh according to the above specified resolution, ans since i am using interfoam what would be your choice for the convection schemes. My Reynolds nummber is approximately 2000. sorry for the long mail. bye with regards K.Suresh kumar 
As your Reynolds number is pretty low, you would not incure really high computational cost (N_DNS ~ Re^2.25). You can use filteredLinear scheme for the convection term and central for rest. Filteredlinear uses upwind in regions required (using boundedness criterion or some other criterion, which I do not remember, check openfoam forum for discussion) and switches to central in rest of the region. Also as OpenFOAM has really not been employed for performing DNS and publishing papers, I would suggest you to work on different levels of grid refinement to confirm that your simulations are accurate.
Good luck. 
Hello Harish,
I have been working on making mesh for the DNS case. I have some small problems with the mesh, so i thought i would discuss it with you, i tried to generate the mesh with a cell size of 1e6 m in both x and y direcitons. First i was not able to generate the mesh on my laptop since i have a 32 bit Ubuntu with a 32 bit OF installation. So then i moved the mesh files to the cluster as it is a 64 bit machine with 64 bit OF and generated the mesh sucessfully. But then i wanted to visualize the mesh. In my university the cluster does not support graphical interface, so i cannot view the mesh. Then i tried to bring the mesh to my 32 bit version and tried to use ParaFOAM to view the mesh, then it gives me an error saying that cannot process some cells. I thought this could be a problem of the 32 bit version, so then i installed the 64 bit version of OF on my personal laptop on Ubuntu 9.04. Then i tried to load the mesh again using ParaFOAM and then it just crashes after long time, while trying to load the mesh. I doubt if it is a problem of RAM, it is a 2GB ram, but i am not sure if this is the problem. I tried to run the checkMesh utility on the mesh, and unfortunately even the checkMesh takes a long time to run, but i am posting the message down that i got from the checkMesh Exec : checkMesh Date : Oct 09 2009 Time : 15:08:31 Host : kcluster116 PID : 13958 Case : /home/clusterusers/kkannan/DNS_mesh nProcs : 1 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = constant Time = constant Mesh stats points: 16314102 internal points: 0 faces: 32607050 internal faces: 16292950 cells: 8150000 boundary patches: 6 point zones: 0 face zones: 0 cell zones: 0 Number of cells of each type: hexahedra: 8150000 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology inlet 50 102 ok (nonclosed singly connected) outlet 4050 8102 ok (nonclosed singly connected) channelWalls 2000 4004 ok (nonclosed singly connected) walls 4000 8004 ok (nonclosed singly connected) sides 4000 8004 ok (nonclosed singly connected) frontBack 16300000 16314102 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0.00205 0.002 0) (0.002 0.001 1e05) I am not sure if this problem is due to the insufficent ram memory, or is it a problem with ParaFOAM and also with the checkMESH script. Any comments on how to check my mesh will be helpful. bye with regards K.Suresh kumar 
ParaFOAM has been problematic for a longtime due to the dependence on the correct version of Qt. You can instead convert your data to VTK format by using foamToVTK and then visuvalize your data using paraview. 2 GB of RAM will not be sufficient to run the case. For visuvalization, it should not be a problem.

Hello,
I would like to know how did you simulate the DNS wit interFoam. I am new user in OF and I am interested in such simulation. Can you or anybody tell me how should I link interfoam with DNS solver. I know its basic question but this is because I am new. Another question: IS it possible to simulate on part of your case with DNS( i.e in PiPE section ) and another part with LES ( The tank which is connected to the pipe). I would be so grateful if you guys help me. Thanks Mehran Quote:

Hello farhagim,
In interFoam if you do not select any turbulence model, and if you make your mesh fine enough to resolve the smallest structures, based on the theory of the universl equilibrium by Kolmogrov which you can find in the book of batchelor. Then i guess you cam perform a DNS simulation. But you should be careful in selecting the spatial and time discretization schemes. I have not yet performed a DNS simulation, i only tried to generate a mesh. But if you want some literature on the DNS using LESVOF methods, i can give you. regrds K.Suresh kumar 
Thanks for your reply.. I would be appreciated if you give me some of the literatures..Do you have any idea that IS it possible to simulate one part of your case with DNS( i.e in PiPE section ) and another part with LES ( The tank which is connected to the pipe).
Mehran Quote:

All times are GMT 4. The time now is 03:41. 