# Different nu effects the amount of gravity?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 January 29, 2015, 10:01 Different nu effects the amount of gravity? #1 Member   Rickard Hidefjäll Join Date: Jun 2009 Location: Uppsala, Sweden Posts: 39 Rep Power: 15 Hi look at http://youtu.be/ueMCheEpMrk interMixingFoam with nu=1; in the square hanging in the air (marked as other. The colon on the left side have nu=1e-6 equal to water. The colon are falling faster than the square. It should be the other way around of the fact that the square just have air under and not water. And look at http://youtu.be/oKsIfmoJc6w interMixingFoam with nu=1e-6 in the square hanging in the air (marked as other. The colon on the left side have nu=1e-6 equal to water. The colon are now falling equal fast as the square, which it didn't in the other video http://youtu.be/ueMCheEpMrk . Is something wrong with the software? Or have I done some thing wrong? Here is the changes of the interMixingFoam : (I ran both it in parallel with 8 cores, but that should not effect the result. it took app. 45 minutes.) In transportProperties Code: // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // phases (air other water); air { transportModel Newtonian; nu nu [0 2 -1 0 0 0 0] 1.48e-05; rho rho [1 -3 0 0 0 0 0] 1; } other { transportModel Newtonian; nu nu [0 2 -1 0 0 0 0] 1; //change this to 1e-6 to get the ohter simulation. rho rho [1 -3 0 0 0 0 0] 1010; } water { transportModel Newtonian; nu nu [0 2 -1 0 0 0 0] 1e-6; rho rho [1 -3 0 0 0 0 0] 1000; } // Surface tension coefficients sigma12 sigma12 [1 0 -2 0 0 0 0] 0.05; sigma13 sigma13 [1 0 -2 0 0 0 0] 0.04; // Diffusivity between miscible phases D23 D23 [0 2 -1 0 0 0 0] 3e-09; // ************************************************************************* // in setFieldsDict Code: // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // defaultFieldValues ( volScalarFieldValue alpha.air 1 volScalarFieldValue alpha.other 0 volScalarFieldValue alpha.water 0 ); regions ( boxToCell { box (0 0 -1) (0.1461 0.292 1); fieldValues ( volScalarFieldValue alpha.air 0 volScalarFieldValue alpha.other 0 volScalarFieldValue alpha.water 1 ); } boxToCell { box (0.2 0.3 -1) (0.4 0.5 1); fieldValues ( volScalarFieldValue alpha.air 0 volScalarFieldValue alpha.other 1 volScalarFieldValue alpha.water 0 ); } ); // ************************************************************************* // controlDict Code: // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application interMixingFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 5; deltaT 0.0001; writeControl adjustableRunTime; writeInterval 0.01; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression compressed; timeFormat general; timePrecision 6; runTimeModifiable yes; adjustTimeStep yes; //adjustTimeStep no; maxCo 0.5; maxAlphaCo 0.5; maxDeltaT 1; // ************************************************************************* // blockMeshDict Code: // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 0.146; vertices ( (0 0 0) (2 0 0) (2.16438 0 0) (4 0 0) (0 0.32876 0) (2 0.32876 0) (2.16438 0.32876 0) (4 0.32876 0) (0 4 0) (2 4 0) (2.16438 4 0) (4 4 0) (0 0 0.1) (2 0 0.1) (2.16438 0 0.1) (4 0 0.1) (0 0.32876 0.1) (2 0.32876 0.1) (2.16438 0.32876 0.1) (4 0.32876 0.1) (0 4 0.1) (2 4 0.1) (2.16438 4 0.1) (4 4 0.1) ); blocks ( hex (0 1 5 4 12 13 17 16) (92 32 1) simpleGrading (1 1 1) hex (2 3 7 6 14 15 19 18) (76 32 1) simpleGrading (1 1 1) hex (4 5 9 8 16 17 21 20) (92 168 1) simpleGrading (1 1 1) hex (5 6 10 9 17 18 22 21) (16 168 1) simpleGrading (1 1 1) hex (6 7 11 10 18 19 23 22) (76 168 1) simpleGrading (1 1 1) ); edges ( ); boundary ( leftWall { type wall; faces ( (0 12 16 4) (4 16 20 8) ); } rightWall { type wall; faces ( (7 19 15 3) (11 23 19 7) ); } lowerWall { type wall; faces ( (0 1 13 12) (1 5 17 13) (5 6 18 17) (2 14 18 6) (2 3 15 14) ); } atmosphere { type patch; faces ( (8 20 21 9) (9 21 22 10) (10 22 23 11) ); } ); mergePatchPairs ( ); // ************************************************************************* // Last edited by wyldckat; January 29, 2015 at 16:49. Reason: Added [CODE][/CODE]

 January 29, 2015, 16:57 #2 Retired Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,968 Blog Entries: 45 Rep Power: 126 Greetings Rickard, This is so cool! It looks like a magic trick ! My best guesses without testing are: A fluid with nu=1 has a good gliding capability, since the fluid particles don't tear apart. The pressure is not homogeneous enough at the initial time. The solver might not be usable for such a high nu value. I'll have a look into it during this coming weekend. But first a few questions: Which OpenFOAM version are you using? Are you using the tutorial "multiphase/interMixingFoam/laminar/damBreak" as a basis? Best regards, Bruno SkunkWorks likes this. __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

 January 29, 2015, 17:47 #3 Member   Rickard Hidefjäll Join Date: Jun 2009 Location: Uppsala, Sweden Posts: 39 Rep Power: 15 Hi! And thanks! I use OpenFOAM 2.3.1 Kubuntu 14.04 i7 3.2Ghz (the first edition) 24Gb RAM (It took 45 minutes used all 8 core) Regards / Rickard Hidefjäll --------------- Sorry! Yes I do use the interMixingFoam tutorial case from start. Last edited by wyldckat; January 31, 2015 at 08:38. Reason: merged posts, since they were posted a minute apart

 January 31, 2015, 09:12 #4 Retired Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,968 Blog Entries: 45 Rep Power: 126 Hi Rickard, Well this is certainly an interesting test case that can showcase the importance of the dynamic viscosity (mu) between fluids. Here's an example of what I'm referring to: Code: air { transportModel Newtonian; nu nu [0 2 -1 0 0 0 0] 1.48e-05; rho rho [1 -3 0 0 0 0 0] 1; } other { transportModel Newtonian; nu nu [0 2 -1 0 0 0 0] 1.48e-1; rho rho [1 -3 0 0 0 0 0] 1000; } water { transportModel Newtonian; nu nu [0 2 -1 0 0 0 0] 1e-6; rho rho [1 -3 0 0 0 0 0] 1000; } Now, in case you're not aware, this is briefly explained here: http://openfoamwiki.net/index.php/FA...ble_solvers.3F is the dynamic viscosity (mu). is the fluid's density (rho). is the kinematic viscosity (nu). And why is the dynamic viscosity important? If you look at the values in the example above: air: other: water: Now, if you subtract the largest from the smallest: 1.48e2 - 1.48e-05 = 147.9999852 Notice anything strange yet? Well, it's simple: the solver was not designed to compensate for such large numerical discrepancies, because "147.9999852" is almost identical to "148", which means that the number of computational errors that occur due to this very small difference are far greater than the remaining values being calculated. If you increase even more to , the block barely moves. As time progresses, it then happens something very similar to this: http://www.cfd-online.com/Forums/ope...ckerboard.html Note: the reason for choosing for the "other" fluid was because I was confusing how dynamic and kinematic viscosity relate to each other. Conclusion: this is not a bug. It simply means that the solver was not designed to handle such large differences in the fluids' properties. Best regards, Bruno linyanx likes this. __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM Last edited by wyldckat; January 31, 2015 at 09:21. Reason: fixed mathematical expressions

 February 1, 2015, 18:09 Thanks a lot! #5 Member   Rickard Hidefjäll Join Date: Jun 2009 Location: Uppsala, Sweden Posts: 39 Rep Power: 15 Hi and Thanks for a fast and lightning response! Do you have a suitable solver in mind? My goal is to simulate a new kind of toilette. Best regards / Rickard Hidefjäll

 February 3, 2015, 15:58 #6 Retired Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,968 Blog Entries: 45 Rep Power: 126 Hi Rickard, I've never used it myself, but perhaps multiphaseEulerFoam can get the job done? For more details: http://www.cfd-online.com/Forums/ope...eulerfoam.html Best regards, Bruno __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

 February 3, 2015, 15:59 #7 Member   Rickard Hidefjäll Join Date: Jun 2009 Location: Uppsala, Sweden Posts: 39 Rep Power: 15 Lots ofta tank !!!

 Tags bug?, intermixingfoam

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post aroma STAR-CCM+ 1 April 10, 2013 11:18 archdevil Main CFD Forum 9 May 16, 2012 14:31 rajani FLUENT 0 February 16, 2005 03:45 Drona CFX 7 November 22, 2001 11:28 Anthony Wachs FLUENT 2 July 25, 2001 08:07

All times are GMT -4. The time now is 14:18.

 Contact Us - CFD Online - Privacy Statement - Top