Learning Forum

[moritz.mantel]

Hello everyone,

i´m doing a transient, open channel flow simulation and it´s working fine in the beginning, but i keep on getting errors from time to time in my simulation, where the velocity magnitude at one point is about 100000 m/s, while it should be maximal about 10 m/s. These errors are only in one time step and i don´t quite understand whats happening there. I´m using the explicit volume of fluid formulation, and when the error occurs the simulation stops, because the global courant number is higher than 250 for the time step. I also tried adaptive time stepping with maximal step change factor of 100 and a very small minimal time step size, but the simulation is still stopping when the error occurs. (What is really sad because i actually want to let the computer do it´s thing over night)

So the first question, does anyone have an idea ehy these errors in the velocity occur ? Until the error the simulation looks always very reasonable with no errors in any value. (??)

The second question, is it possible to "jump" back to some time steps before the error and initialize the calculation with that time step, so that i can change my setup and hopefully the error will not occur with the changed setup. 

the third question, should i actually use the implicit volume of fluid formulation to avoid errors like this ? 

I can provide any kind of information to my simulation, screenshots, animations and so on if you are interested, or if needed to answer my questions.

Thank you very much,

Moritz 

[moritz.mantel]

By the way, the errors alway occur in the primary phase wich is air and not in the secondary phase, water, which i am interested in.

[Amine Ben Hadj Ali]

Might due to poor mesh, large time size and wrong model settings / BC's. Provide some more information as screenshots and report the mesh quality.

 

[moritz.mantel]

Here are some pictures of my Meshing

[moritz.mantel]

Here are some pictures of the solver setup

[moritz.mantel]

Here are some pictures of the error that occurs and the isosurface and velocity vectors right before the error occurs

[moritz.mantel]

Velocity Volume Rendering of the Error

 

[Rob]

That looks like a convergence issue: something happens at around 7s which causes the problem. 

[moritz.mantel]

That sure is right, but i have no idea why that problem occurs. 

So does anyone have an idea why these extremely high velocitys in the air are arising ? 

And is it possible to set the solution back to some time-steps before the error so that i can change the settings and let Fluent calculate further with the changed settings ? 

Thank you very much.

 

[Karthik Remella]

Hello,

This is definitely a convergence issue as Rob points out rightly.

As Amine asked you earlier, what is your mesh quality? Maximum skewness and Minimum orthogonal quality? Could you please share the numbers here? It is not very clear from your screenshot.

Secondly, in your adaptive time-step settings, why is your max step change factor 100? Could you please revert this number to the default factor of 1.2. Also, you need not go as conservative as 1e-10. I'd strongly suggest that you calculate your minimum time-step size based on CFL = 1 and go one order of magnitude (on the conservative side). That should be sufficient.

Also, to answer your last question - unless you have saved the data file before t = 7 s, you will not be able to go back. If you have not done it already, it might be a good idea to periodically write your data file.

Thanks.

Karthik

[moritz.mantel]

Hi Kremella,

thanks for your answer. I just changed the time step change factors, hoping that Fluent could change the time step size enopugh to avoid the error of the global courant number higher than 250. I ran the simulation before with the default time step change factor and the same error occured, also with fixed time steps with different time step sizes.

The problem with the CFL is, that the global velocity magnitude in the simulation is actually around 10-20 m/s, but in one time step, when the error occurs it changes to a completely unrealistic high value of about 100000m/s and Fluent is not able to set the time step small enough to avoid the error of reaching a courant number higher than 250. I guess if i could find the problem which leads to these high velocitys in the air, the simulation would work fine, because until the error occurs everything is looking quite nice and realistic.

[moritz.mantel]

Here are screenshots to element quality, skewness, aspect ratio and orthogonal quality.

All the cells with poor element quality are located in the inflation layers of the bridge, is there any method to avoid this ? 

[moritz.mantel]

[Rob]

You have cells with over 0.95 skew, if the free surface hits these it's going to have stability issues. 

Remember inflation meshing is to help with flow that's along a surface. They're not necessarily much use when you have strong separation and or multiple phases. 

[moritz.mantel]

Yes, the inflation layers are located at the surface i am interested in, to reduce the y+ value along these surfaces. I am looking for the drag coefficient of the body around which i created the inflation layers. The free surface actually should not hit the inflation meshing (except in the beginning of the simulation), because the water is flowing completely over the body.

Thank you for your help

[moritz.mantel]

Do you think i should refine the Mesh around my body of influence to avoid poor mesh quality in the inflation meshing region ?

I´m not sure if this helps because it seems to me like the error does not occur in the inflation region.

[Amine Ben Hadj Ali]

Try to improve mesh quality and increase grid density in the free surface region. Your adaptive time step method is wrong. Use conservative change factors: 0.5 and 1.08. Always store recovery files to get started before point of divergence. Use implicit VOF formulation to be more relaxed regarding CFL. Use max Global CFL as 5.

[moritz.mantel]

Thank you very much Amine

[moritz.mantel]

When i try to use the implicit formulation the simulation crashes very fast, the velocity magnitude ist going from 10 m/s to 30000000m/s in about three time steps and then a floating point exception is reported.

The Method settings for the Implicit formulation are the default settings.

Do you have an idea why this happens ? 

Thanks, Moritz