[andon6141]

Hello,

i have a few problems to simulate my stirred tank in transient mode.

First i create in Ansys DM a stirred tank --> image (tank_cad)

The resultig mesh --> image (mesh)

I use the MRF to simulate the stir in steady mode. That works fine-->image (steady)

But when i try to simulate in transient mode with moving mesh ... ansys shows the error " Update-Dynamic-Mesh faild. Negative cell volume detected"

I am a beginner in Fluent and would be happy if someone can help me ....

[CeesH]

Hi Anton,
Did you choose the dynamic mesh option for moving mesh? That is not necesarry for a sliding mesh simulation - you can choose mesh motion instead of frame motion in the cell zone menu, and things should work.

Some more general things, the mesh itself looks pretty messy. Is the convergence of your results (power number/average velocity in domain) ok? And did you do a mesh dependency study? I'd expect you could use sweep meshing for pretty large parts of the domain - pretty much all but the rotorzone - that might improve mesh quality and keep the mesh count low...

[andon6141]

Hey thanks for your fast answer,

i select the moving mesh for the rotation zone in the cell zone conditions

so also for the blade mesh

and the rotorwall is defined as moving wall in the bondary conditions

the convergence in steady mode is ok ....

i know that the mesh is not really nice..... sorry for the question but what you mean with mesh dependency study?

the dynamic mesh is not activated .... should i use the dynamic mesh ?

[CeesH]

You shouldn't use dynamic mesh - I thought maybe you were because of the error.

If the rotorwall is defined as moving, does it have a speed? Since the mesh is already moving, the rotor should not be moving with respect to the surrounding cell zone (or set as a moving wall with rotating speed 0 to the surrounding mesh)

A mesh dependency study is to see if the results you find depend on the mesh; you run the same simulation with several mesh densities to see if the flow field differences between them, and if integral properties converge to some value, like the power number (you can typically look the expected value for the power number up in literature to compare with experiments).

In the case of stirred tanks, quite often the power number is underestimated; the denser the mesh, the better the agreement with the experimental value - it's up to you to decide which level of agreement is good enough.

[ghost82]

In addition to CeesH's advices I add that if you want to use moving mesh you must define interfaces between rotor and stator zones.
With that setup the mesh rotates with time, not as the mrf approach in which the mesh is static and you don't need interfaces.

[CeesH]

Good point!

[andon6141]

Hey

a big thank you to CeesH ans ghost82 ... the solution was to define interfaces between the rot ans stat ....

Thank you guys ... and my last question ... do somebody have a good tutorial for problems with moving meshes and the meshing itself ?

[CeesH]

Do you have access to the ANSYS costumer portal (or can you get access?)

There are a lot of tutorials there, including some on (2D) sliding meshes, and also various tutorials about meshing strategies. If you can get access, I'd recommend you to get it. If I remember correctly, the introduction to ANSYS meshing contains instructions on how to split up a stirred tank with a complicated impeller into zones, and use different meshing strategies in different zones. The geometry is quite alike yours, a well defined tank which can be meshed by sweeping, and a complex impeller geometry requiring tetrahedrons.