Learning Forum

[GHAZWAN.ALWAN]

Hello,

I have been trying to simulate moving air balloon in water domain in fluent.
2D domain. 1.2 m high and 0.6 m wide which represents water. A circle near the bottom of 12 cm in diameter is filled with air to represent the balloon. Both are created in spaceclaim. I tried both options: make both domain as one surface, but two different domains, then tried having them as two surfaces with shared topology.

In meshing, three sides are walls, while the top is open to air (reference pressure set to 0).
In fluent materials: made liquid water for the water domain, then created a solid material for the circle and gave it a density of 1.22 kg/m3, to represent air.
The other settings are: transient, gravity -9.81 in y-direction, dynamic mesh (smoothgin and remeshing), six DOF (in it, created a body of 0.01 kg and moves in y direction only), created two Dynamic Mesh Zones (rigid body which is the circle, deformable body which is the water domain).

When I “Preview Mesh Motion” what I see is that the circle falls through the water domain! I tried several things, but I do not see what I am missing. It looks like the shared edges of the circle are not actually connected between the two domains.
Now, even after I run the simulation, it drops and goes through the bottom. The correct solution is that it should go up due to buoyancy forces.
Could you please help?

Once again, I think I am missing something to tell fluent that when the circle is moving, the domain water domain must interact accordingly and push the circle upwards and deform the mesh (and later re-mesh)

Thank you

 

[Mark O]

You cannot reliably preview mesh motion with 6dof. The 6dof motion depends on the flow solution. I suspect the fluid force is always zero and it is just applying gravity, which may be sufficient in this case.

 

You cannot do remeshing on quad elements. You will need to have tri elements.

 

Your picture looks like you have a non-conformal (i.e. disconnected mesh). If you generate a conformal mesh you should see a wall/wall-shadow pair and the wall thermal condition properties will  say coupled. 

 

 

If you generate a non-conformal mesh you will see two walls and you will need to create a mesh interface in Fluent to join the two disconnected meshes together. You cannot assume a mesh is connected if it initially looks connected in a picture. It could be that there are duplicate mesh nodes at the same location. When the circle starts moving the nodes move apart.

 

Please refer to the help for Spaceclaim and the meshing tool you are using on how to create a conformal mesh