Negative alpha1 using interDyMFoam
Hi,
I am currently trying to do a simulation with a high speed water jet acting on rotating Pelton buckets. Unfortunately, the simulation crashes before giving me any results. The alpha1 minimum volume fractions are negative, and I wonder if this is what is making the simulation crash? I am not sure about the setup of fvSolution and fvSchemes, so my guess is that these cause the negative alphas. The log output of some early timesteps: Code:
Interface Courant Number mean: 1.624315938e-07 max: 0.1091097517 Code:
/*--------------------------------*- C++ -*----------------------------------*\ Code:
/*--------------------------------*- C++ -*----------------------------------*\ |
I don't think so. The values are so small that they shouldn't be causing any problems.
|
Hi,
Thank you for your response! In that case there must be another reason for the simulation to crash. I get the error message: Code:
[1] #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" Code:
Interface Courant Number mean: 2.578325543e-06 max: 0.1973915059 fvSolution: Code:
/*--------------------------------*- C++ -*----------------------------------*\ Code:
/*--------------------------------*- C++ -*----------------------------------*\ |
If you're still having problems, try the following:
Test maxAlphaCo=0.1. Keep the momentum predictor enabled. Try relTol=0 on p_rgh, and finally try running GAMG with pure GaussSeidel instead of using DIC. |
Thank you very much for your quick reply! I will try that and let you know if it works or not.
|
Crashed again unfortunately, at the same time as before. Does the error message make any sense?
Code:
[1] #0 Foam::error::printStack(Foam::Ostream&) at ??:? 1. I am simulating with turbulenceProperties set to laminar, while a turbulence model should in reality be applied. 2. I have a symmetryplane along the jet and have heard that this BC sometimes causes instabilities with multiphase-simulations. Does this sound reasonable? I will try to run some more simulations during the weekend. For k and epsilon i will use: k=2.45504; //k=(2/3)(Uref*Ti)², Ti=0,05 turb intensity (Versteeg, 2007) epsilon=255.38893; //epsilon=0,0845^(3/4)*(k^(3/2))/(0,07L) L=Diameter of jet=0,04 |
Hello,
You are using interDyMFoam with AMI i guess. On your last iteration befor crash, you get : Quote:
Solution: either improve your mesh, or lower your time stepping a bit may help. regards, olivier |
Quote:
As you can see in the screenshot below, the AMI-patches are not perfectly circular (AMI1 and AMI2 showing). I guess that might be what is causing it to crash? I guess I should go back to snappyHexMesh then, and refine the AMI-interface further. https://dl.dropbox.com/u/2820596/donut-mesh13-AMI.png |
hello,
Finer interface doesn't help here (and this may even be worst !). What's matter is your mesh should not overlap or create hole: try a different "matchTolerance" in your boundary file, and check your geometry (interface should be circular). And if you want good result with AMI, try to use an more uniform mesh at interface, i.e not a fine on one side, and coarse on the other. regards, olivier |
Quote:
So you mean that if I increase the matchTolerance, e.g. from 0.0001 to 0.001, my simulation might be more stable? The problem is that the interface is not perfectly circular. I tried to adjust the settings in snappyHexMeshDict, but I couldn't figure out how to resolve it. The mesh in the interface gets affected by the geometries around, resulting in "bumps" several places around the interface. Please see the attached images for explanation. Any tips and tricks to improve my mesh and simulation are greatly appreciated! Regards, Jone Whole domain, rotating region with buckets and stationary part with water jet: https://dl.dropbox.com/u/2820596/donut-mesh13.png "Bump" created in the AMI-interface because of buckets: https://dl.dropbox.com/u/2820596/donut-mesh13-bump.png |
Hi,
have you tried using div(phi,alpha) Gauss vanLeer01 this scheme should bound alpha between 0 and 1 Regards, Christian |
Quote:
I am currently working on making a better mesh, hope to achieve this today so I can try running the simulation again. It turns out that a circular AMI-interface is difficult to obtain together with the refinements I want, but I think I will manage somehow. |
I finally got the simulation running, but I discovered some weird behavior of the flow so far.
1. The jet gets cut when meeting the AMI-interface, spreading along the AMI-patches on both sides (picture 1). 2. A hole is created in the isovolume at the jet inlet (picture 2). Still, when I check the value of alpha1 graphically in paraView (see picture 3), it seems that alpha1 has the max value in those cells. Has anyone seen this type of behavior before? Regards, Jone Picture 1: https://dl.dropbox.com/u/2820596/mesh14-jetcut-AMI.png Picture 2: https://dl.dropbox.com/u/2820596/mesh14-inlethole.png Picture 3: https://dl.dropbox.com/u/2820596/mes...-wireframe.png |
I wonder if anyone has an idea of what is causing these effects?
There seems to be a strong diffusion of the jet. The behavior along the symmetryPlane is very strange, as I would expect the water to have the maximum speed (38.38ms-1) along this. Problematic effects:
Here is a picture with another mesh. It shows an isovolume with 0.1<alpha1<1: https://dl.dropbox.com/u/2820596/mes...tdiffusion.png The same jet with the symmetryPlane facing up: https://dl.dropbox.com/u/2820596/mes...onsymmetry.png |
Anyone?
I tried to check the effect of the symmetryPlane by replacing it with zeroGradient for U, p_rgh and alpha1. As you can see from the pictures it looks a lot better (though far from perfect) with the zeroGradient BC. Is there a bug in the symmetryPlane-condition? symmetryPlane BC applied to patch: https://dl.dropbox.com/u/2820596/mes...metryplane.png zeroGradient BC applied to patch: https://dl.dropbox.com/u/2820596/mes...roGradient.png |
All times are GMT -4. The time now is 01:00. |