Learning Forum

[piggh18]

I am currently running 2D transient multiphase VOF simulation with a rigid body dynamic mesh (smoothing and remeshing). For most of the simulation, the residuals converge fine but slowly increase in number of iterations required to advance. I was wondering why this may be and was also wondering why this curve shape is appearing in residuals specifically continuity.

Any advice for aiding the continuity convergence will be greatly appreciated!!

[Rob]

You may have only 1000 iterations worth of residuals stored in the file, so stop & start can cause the behaviour towards the 296500-299500 range (give or take). Then there's the rate of mesh motion and flow changes relative to timestep. I'm wary of the above as the residuals don't look to be dropping far enough. How are the monitors looking? 

[piggh18]

Rob,

I also have used VOF stabilization settings as well as velocity limiting treatment under the methods section in attempt to improve the stability but that hasn't worked well either. Along with this, I performed the VOF check and followed most of the suggested actions. I am using open channel wave conditions as well. Would too short of a numerical beach at the end of the tank be cause for failure?

thanks!

[piggh18]

Thanks for the reply!

You are correct that the continuity residual was not dropping far enough (1e-3). In the beginning of the simulation, everything would converge within ~10 iterations. After each timestep, the continuity residual would slowly increase its initial 'guess' until the residual would no longer converge below 1e-3. I've tried implicit update and solution stabilization thinking that this may be a dynamic mesh issue. My problem there is I'm not totally sure what values to use for the inputs of these settings.

Thank you again!

[Rob]

Time step and MDM may be a problem. How fast are things moving relative to the cell size and time step? 

[piggh18]

Cell size surrounding the rigid body is 0.0023 m triangles. The non dynamic domain is structued with a sizing of 0.001 m. I am trying to recreate results form a previous study and matched my models as closely as I could to theirs. They reported a peak angular velocity of ~400 deg/s where the body 0.31 m long from its axis of rotation. Given that I wouldn't expect a linear velocity higher than 2.5 m/s.

[Rob]

Why is the refined mesh around the object coarser than the bulk? 

[piggh18]

My apologies, refined mesh is 0.0023 triangular, rest of domain is structured 0.005.

[Rob]

Timestep size? How fast is the fluid moving? 

[piggh18]

timestep is 0.001s. My inlet boundary is open channel wave with averaged phase velocity of 0 m/s in attempt to model wave tank conditions.

[piggh18]

I'm not sure what the fluid velocity is but I don't expect it to be more than ~5 m/s

[Rob]

Drop the time step: that should help convergence. If the flow crosses a cell in a time step the step is too big. If remeshing means cells "cross" in a time step, the step is too big.  Try 0.0001s and see how that behaves. 

[piggh18]

Soudns good thank you. Do you have any recommendations for solution stabilization under solver options or implict update?

[Rob]

I can only refer to what's in the manual, or AIS content. My general tip is if you don't know why you're about to change something, leave it alone! Turning solution stabilisation on being a good idea, messing with the coefficients being a little less so.