Hello again.
Now I am running
Hello again.
Now I am running a simple 3dmesh with a sphere in a freestream. I am using simpleFoam. During the first few timesteps everything looks good but after a while the magnitudes of "timestep continuity errors", "bounding epsilon" and "bounding k" increases. Anyone knows why? What are typical values of k and epsilon? Is kepsilon the same turbulence model as komega? Thank you! /Marcus 
Heya,
kepsilon and komega
Heya,
kepsilon and komega (as the name suggests) are two different models. As for your problems, it seems that the discretisation needs tuning: you should not be getting the bouding messages on k and epsilon because if this continues, the solution will blow up. For a better continuity error, try tightening the (relative) pressure tolerance  that's the second number behind p in system/fvSolution (you know where, right?) Enjoy, Hrv 
Thank you.
Yes, i know wher
Thank you.
Yes, i know where. /ham 
Okey, I tried to tightening th
Okey, I tried to tightening the relative pressure tolerance and yes I got better continuity.
But I guess this is like everything else, a compromise. So when I get better continuity by tightening the pressure tolerance I must be get some negative sideeffects? /marcus 
Hi, Im having a similar proble
Hi, Im having a similar problem where I get all between 50 to 1000 itterations on pressure. when choosing a relative tolerance closer to 0.9 (which is hish) I get most often only one itteration and still low values of continuity. This is what the print out looks like. Is it anything to worry about and should I modify it for a more correct answer?
Time = 0.5 BICCG: Solving for Ux, Initial residual = 0.135647, Final residual = 0.000552089, No Iterations 1 BICCG: Solving for Uy, Initial residual = 0.101647, Final residual = 0.000369054, No Iterations 1 BICCG: Solving for Uz, Initial residual = 0.0413855, Final residual = 0.000171168, No Iterations 1 ICCG: Solving for p, Initial residual = 0.0443585, Final residual = 0.0381298, No Iterations 964 time step continuity errors : sum local = 0.00204006, global = 1.59512e05, cumulative = 0.00112614 Creating alphaEff. BICCG: Solving for T, Initial residual = 0.237459, Final residual = 0.0189455, No Iterations 88 BICCG: Solving for epsilon, Initial residual = 0.0176145, Final residual = 8.30749e11, No Iterations 1 BICCG: Solving for k, Initial residual = 0.147769, Final residual = 0.00053236, No Iterations 1 ExecutionTime = 22.51 s Time = 0.6 BICCG: Solving for Ux, Initial residual = 0.238292, Final residual = 0.000707662, No Iterations 1 BICCG: Solving for Uy, Initial residual = 0.191797, Final residual = 0.000584621, No Iterations 1 BICCG: Solving for Uz, Initial residual = 0.130177, Final residual = 0.000364168, No Iterations 1 ICCG: Solving for p, Initial residual = 0.0319587, Final residual = 0.0173633, No Iterations 1 time step continuity errors : sum local = 0.00206456, global = 0.000150139, cumulative = 0.000976002 Creating alphaEff. BICCG: Solving for T, Initial residual = 0.181806, Final residual = 0.0121908, No Iterations 89 BICCG: Solving for epsilon, Initial residual = 0.040725, Final residual = 8.54144e11, No Iterations 1 BICCG: Solving for k, Initial residual = 0.127848, Final residual = 0.000452815, No Iterations 1 ExecutionTime = 24.83 s Thanks /Erik 
But I guess this is like every
Quote:
As for you Erik, try using the AMG solver, this will make it faster. Hrv Hrv 
Hi,
I'm also facing the sa
Hi,
I'm also facing the same kind of problem. I'm working on turbfoam , in my case both epsilon and k are getting bounded and on increasing relative tolerance of either of them they still are bounding and no of iterations is reduced to "1". What can i do to stop it from bounding.........my work has almost come to halt because of this ...please somone reply soon 
A common cause of negative k a
A common cause of negative k and/or epsilon is an unbounded convection scheme. Switching div(phi,k) and div(phi,epsilon) to "Gauss upwind;" in fvSchemes generally prevents unbounded solutions.
If you are getting negative k and epsilon values despite using upwind for convection, then you probably have some very nasty cells and will have to start looking at reducing your explicit nonorthogonal correction contribution. I must point out though that small negative kepsilon values that cause the bounding routines to trigger are not in themselves problematic. I.e. you can run just fine with bounding removing small negative values of k and epsilon as long as there are no other problems. 
Hi,
I am having the same prob
Hi,
I am having the same problem with a negative k that appears to be causing my case to crash. I have tried changing the div(phi,k) to upwind but still get the same problemit crashes after about two iterations. I am using lesInterFoam. Is there maybe something wrong with my boundary specification? I have two pressureInletOutletVelocity boundaries and two fixed value velocity inlets. Any help would be greatly appreciated! 
I forgot to also mention that
I forgot to also mention that I am using the locDynOneEqEddy LES model although I have also tried a few others and gotten the same problem.

Hello Foamers,
I have a bouding problem in my geometry too, but the bouding value is: Code:
bounding epsilon, min: 1.58155e17 max: 0.0864828 average: 0.0667376 Normally I thought high values are for bounding... Well my pressure calculation is very bad and after 700 timesteps I get 1000 Iterations in the pressure equation. ... I know that problem by using wrong boundary conditions but therefor its not possible to set other BC. 
Hi Tobi,
Reply can be late, even though bounding epsilon or k, it can be because of the improper initial values and the schemes which you are using for your div scheme. while using Gauss Linear I was facing this problem, you can fix this problem changing your scheme to upwind for epsilon. Thanks, Aadhavan 
All times are GMT 4. The time now is 11:58. 