CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Immersed solid with cavitation (https://www.cfd-online.com/Forums/cfx/153847-immersed-solid-cavitation.html)

shivasluzz June 4, 2015 23:42

Immersed solid with cavitation
 
I am doing a simulation of gear pump with low inlet pressure condition.
I use 2 fluids (liquid and vapor) and set saturation pressure to account for the 'cavitation effects'.
The solver says 'immersed solid with muliphase combination' is not supported. But the solver runs and converges. Can I use the result or not?
In help documentation, it is given that 'mulitphase flow does not properly INTERACT with immersed solid'.
Here "INTERACT' means what?
I want to check only the reduction in mass flow if cavitation occurs? So can i use the result?

shivasluzz June 5, 2015 08:05

the results are converged to the sufficient accurancy (rms : 1e-6)...
i could see the pressure of vapour also..
but there is only one warning during starting that 'Warning: You have used Immersed solids with Mulitphase option. This combination is not supported'
Is that solution is totally wrong?

ghorrocks June 6, 2015 00:47

If the fluid cavitates then yes, you results are likely to be completely wrong. Immersed solids cannot account for varying density. But if you do not cavitate or the cavitation volume is small then you might be OK.

shivasluzz June 9, 2015 10:42

Thanks ghorrocks for your reply! Then I think deforming mesh is the only option.. But is it possible to simulate Gear mesh motion?

ghorrocks June 9, 2015 18:34

For a gear pump that will be tricky. the only way it is going to work is with dynamic remeshing.

shivasluzz June 9, 2015 23:10

Dynamic remeshing? Is is not same as Mesh displacement?

Please share some link or some similar example...

ghorrocks June 9, 2015 23:26

Moving mesh is where the mesh topology remains the same but it is distorted to move. It is only suitable for small ranges of motion. Dynamic remeshing is where moving mesh is used up until the mesh quality drops below a defined criteria, then a remesh is triggered and a new mesh generated and the simulation continues on the new mesh. This obviously involves interaction with the meshing software.

I think there are example dynamic remeshing simulations on the ANSYS customer webpage. ANSYS support will also have some I suspect.

vivjk94 December 30, 2021 08:12

Hi, hope you have found the solution of your problem.
 
Quote:

Originally Posted by shivasluzz (Post 548969)
I am doing a simulation of gear pump with low inlet pressure condition.
I use 2 fluids (liquid and vapor) and set saturation pressure to account for the 'cavitation effects'.
The solver says 'immersed solid with muliphase combination' is not supported. But the solver runs and converges. Can I use the result or not?
In help documentation, it is given that 'mulitphase flow does not properly INTERACT with immersed solid'.
Here "INTERACT' means what?

I want to check only the reduction in mass flow if cavitation occurs? So can i use the result?


Hi, I would like to know how did you model the cavitation in gear pump? I hear you can do it in fluent. If you have solved your problem please share your procedure and computation time. I am also in same problem.

Gert-Jan December 30, 2021 08:28

You can do gear pumps in CFX using the Twinmesh technology (https://www.twinmesh.com/)
Alternatively do this in Fluent (or Star-CCM+) using Deforming mesh or Overset-Meshing.
All approaches are difficult and require a lot of perseverance.

Using Immersed solids is a bad idea. The solids only affect the velocity of the continuous phase, and completely ignore Volume fractions, temperatures, and other scalars. They go though the solids as if there are not there.
Therefore, its applicalbility is quite limited. Only use it for a very rough approximation.


All times are GMT -4. The time now is 08:15.