# "Glitches" in k and omega

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

 January 20, 2013, 16:54 "Glitches" in k and omega #1 Member   Join Date: Jan 2011 Posts: 45 Rep Power: 7 Hi, I am simulating the flow in a channel using a modified simpleFoam and the k-omega-SST model. Every now and then, the solver can't solve for k or omega and their values just explode. Sometimes the simulation recovers from that state within a few hundred timesteps, sometimes it doesn't. Here is a sample output for a normal timestep and a problematic one: Code: ```Time = 4180 DILUPBiCG: Solving for Ux, Initial residual = 0.002454946797335455, Final residual = 2.118201461652769e-08, No Iterations 6 DILUPBiCG: Solving for Uy, Initial residual = 0.001256415853039685, Final residual = 1.037692770489594e-08, No Iterations 6 DILUPBiCG: Solving for Uz, Initial residual = 0.003283733002456741, Final residual = 2.981279918575045e-09, No Iterations 7 GAMG: Solving for p, Initial residual = 0.02201556239585755, Final residual = 1.282423077370965e-07, No Iterations 16 GAMG: Solving for p, Initial residual = 0.008240116175764454, Final residual = 8.139580885669834e-08, No Iterations 12 time step continuity errors : sum local = 1.531473863748542e-06, global = -7.156743507425181e-15, cumulative = -1.45393053629309e-12 DILUPBiCG: Solving for omega, Initial residual = 8.626697921486998e-06, Final residual = 8.156673087094997e-11, No Iterations 5 bounding omega, min: -877.5914029924204 max: 9963507.932995282 average: 104575.2141635721 DILUPBiCG: Solving for k, Initial residual = 0.003874747711704138, Final residual = 5.92104344143439e-09, No Iterations 7 bounding k, min: -0.0001332252168376633 max: 0.05713142005592581 average: 0.003205000635194682 S_PRO= 4.802711559863782e-06W/K S_PRO,D= 2.028083115231596e-06W/K S_PRO,D'= 2.774628444632186e-06W/K S_PRO,C= 0W/K S_PRO,C'= 0W/K ExecutionTime = 1411.6 s ClockTime = 1434 s Time = 4181 DILUPBiCG: Solving for Ux, Initial residual = 0.002460388678483852, Final residual = 9.17931475513598e-10, No Iterations 7 DILUPBiCG: Solving for Uy, Initial residual = 0.001256478971499746, Final residual = 1.16998685088727e-08, No Iterations 6 DILUPBiCG: Solving for Uz, Initial residual = 0.003284937635407826, Final residual = 2.670988173110144e-08, No Iterations 5 GAMG: Solving for p, Initial residual = 0.02191503352549878, Final residual = 1.226826542535508e-07, No Iterations 16 GAMG: Solving for p, Initial residual = 0.008195653865403671, Final residual = 7.521263032788438e-08, No Iterations 12 time step continuity errors : sum local = 1.415562053229773e-06, global = 1.775764236376485e-15, cumulative = -1.452154772056713e-12 DILUPBiCG: Solving for omega, Initial residual = 8.719510075834142e-06, Final residual = 4808428634545.903, No Iterations 1001 bounding omega, min: -2.164755144508585e+21 max: 3.598949521217116e+21 average: 1.308210762796994e+17 DILUPBiCG: Solving for k, Initial residual = 0.3147840750606549, Final residual = 1.995451694496316e-16, No Iterations 1 bounding k, min: -4.418770186074049e-05 max: 0.05208677946321078 average: 0.001778830031969948 S_PRO= 1262457298.893128W/K S_PRO,D= 2.02929169556324e-06W/K S_PRO,D'= 1262457298.893126W/K S_PRO,C= 0W/K S_PRO,C'= 0W/K ExecutionTime = 1448.59 s ClockTime = 1471 s``` I changed some values in my fvSolution during this simulation, but not when this behavior occured. My fvSchemes for k and omega: Code: ```ddtSchemes { default steadyState; } gradSchemes { default cellLimited Gauss linear 1; } divSchemes { default Gauss linear; div(phi,U) Gauss limitedLinearV 1; div(phi,T) Gauss upwind; } laplacianSchemes { default Gauss linear limited 0.333; } interpolationSchemes { default linear; } snGradSchemes { default limited 0.333; } fluxRequired { default no; p; }``` relTol for k and omega is 1e-5, relaxationFactors are 0.7 (I had them as low as 0.3, but glitches occured as well) Has anyone some advice for me regarding what could be wrong and what I could do about this? Regards Christoph

 January 21, 2013, 15:08 #2 Member   Eric Robertson Join Date: Jul 2012 Posts: 95 Rep Power: 6 Try dropping your relaxation factor for omega and/or k to something less than 0.1, i.e. 0.05 or so. I have recently run a kOmegaSST sim on a submarine and would have similar issues with the bounding omega exploding. Dropping the relaxation to 0.05 fixed it for me.

 January 21, 2013, 19:00 #3 Senior Member     Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 581 Rep Power: 20 Also, you have your default divScheme set to Gauss linear...which is unbounded. You might want to explicitly set the divScheme for your turbulence parameters to something bounded.

 January 22, 2013, 06:31 #4 Member   Join Date: Jan 2011 Posts: 45 Rep Power: 7 Thanks to both of you, I will have to try a number of different things now. A relaxation factor of 0.1 or even 0.05 sounds really low, but I'll give it a shot if all else fails. I tried a limited scheme: Code: `div(phi,omega) Gauss limitedLinear 0 1e9;` which gave me a floating point exception when I restarted the simulation with this scheme enabled, but enabling it afterwards worked (odd!?) I am currently using a smooth solver, which also seems to run without glithces in k and omega but it's slower than before.

 January 22, 2013, 17:08 #5 Senior Member     Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 581 Rep Power: 20 I personally have an affinity to the upwind family. For 2.1.x, you could try Code: `div(phi,omega) Gauss linearUpwind grad(omega);` with Code: `grad(omega) cellLimited leastSquares 1.0;` and then you can choose from the limiters Code: ```cellMDLimited cellLimited faceMDLimited faceLimited``` where these are arranged in order or least diffuse to most diffuse (citation cellMDLimited vs. cellLimited). I like them because they are a little dissipative and help when finding a solution. Also, believe I read in some ANSYS documentation that limiters can lead to stalling of the solution (maybe only in FLUENT?), so be aware of that.

 January 23, 2013, 06:16 #6 Member   Join Date: Jan 2011 Posts: 45 Rep Power: 7 I have OF 2.0.1 here, but I can use your suggestion anyway (at least OF didn't complain). These are my fvSchemes now: Code: ```gradSchemes { default cellLimited Gauss linear 1; grad(omega) cellLimited leastSquares 1.0; } divSchemes { default Gauss linear; div(phi,U) Gauss limitedLinearV 1; div(phi,omega) Gauss linearUpwind grad(omega); }``` Let's see if it blows up again!

 January 24, 2013, 14:51 #7 Member   Join Date: Jan 2011 Posts: 45 Rep Power: 7 Well, I'm not seeing any problems regarding the glitches I described, but as they only show up occasionally I can't be sure that the schemes you suggested actually did the trick. One problem though: I have cyclic boundaries and it seems that the suggested schemes have amplified oscillations I already had in my solution.

 January 28, 2013, 11:33 #8 Senior Member     Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 581 Rep Power: 20 you're still using Gauss linear as a default scheme for some of your variables. This linear scheme may be the source of your errors. I would change your default scheme to none, run your solver and then set each one of the schemes manually in your fvSchemes dictionary.

January 29, 2013, 04:57
#9
Member

Join Date: Jan 2011
Posts: 45
Rep Power: 7
Quote:
 Originally Posted by chegdan you're still using Gauss linear as a default scheme for some of your variables. This linear scheme may be the source of your errors.
Are you now referring to the glitches I described in the first post or to the oscillations I mentioned in my latest post? However, I now have all schemes set manually, but I have no experience regarding what might be suitable or not.

 Thread Tools 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post aljazari OpenFOAM Running, Solving & CFD 0 November 15, 2012 12:18 cm_jubayer OpenFOAM 1 August 26, 2011 13:18 dancfd OpenFOAM Pre-Processing 0 June 9, 2011 23:25 john_w OpenFOAM Running, Solving & CFD 2 September 22, 2009 05:15 cbarry OpenFOAM 3 August 18, 2009 10:09

All times are GMT -4. The time now is 00:21.