[therockyy]

Hi fellas,

I think the variable 'nbl' is used to define the number or sequence of the mesh blocks in Flow-3D. But I cannot find the definition of it in the help file. I used more than 5 mesh blocks in my simulation, but the nbl only has a rage from 1 to 5 in the output. I didn't give it a limit in my code. Does it have an upper limit defined in Flow-3D orginal code?

Thanks a lot!

Yang

[MuxaB]

The limit for the number of mesh blocks is 500, and it is only set in the post-processor; the solver does not have that limit.

Are you customizing the solver?

[therockyy]

Yes, currently I'm using a customised code to tracking the surface entraiment during fill of casting mould. There are still some variables that I cannot understand in the customisation.

Can Flow-3D calculate the six different velocities of the face centres in one element (mesh cell)? or it only has one value, i.e. one velocity in the body centre of the element?

Thank you!

Yang

[MuxaB]

Originally Posted by therockyy

Yes, currently I'm using a customised code to tracking the surface entraiment during fill of casting mould. There are still some variables that I cannot understand in the customisation.

Can Flow-3D calculate the six different velocities of the face centres in one element (mesh cell)? or it only has one value, i.e. one velocity in the body centre of the element?

Thank you!

Yang

Velocity components are computed at call faces. For a cell ijk, (i,j,k), u(ijk) is the x-component at the high-x face, u(imjk) (i-1,j,k) is at low-x face and so on. The manual's chapter 9 has more details.

[therockyy]

Thanks, Michael.

I just checked the manual. It mentions that the u(ijk), v(ijk) and w(ijk) is the velocities at right, back and top faces respectively, that means the velocity at the left face of cell (ijk) is represented by the velocity at right face of cell (imjk). But how about the velocity at the left face of the far left cell? Is that the reason why Flow-3D using real cells and boundary cells around them?

By the way, when I asked a question about the calculated free surface in Flow-3D by VOF method, Jeff Burnham relpied that "the way FLOW-3D calculates the fluid free surface in sharp-interface problems uses special algorithms (TruVOF and FAVOR) so that the location of the free surface is accurately calculated independent of the mesh size". Does that mean the calculated free surface in Flow-3D is insensitive to mesh size? Since the definition of entrainment through NF values in the customization which I'm using is sensitive to the mesh size, I'm thinking if I can use another method to tracking the entrainment location.

Thanks a lot!

Yang

[MuxaB]

Originally Posted by therockyy

Thanks, Michael.

I just checked the manual. It mentions that the u(ijk), v(ijk) and w(ijk) is the velocities at right, back and top faces respectively, that means the velocity at the left face of cell (ijk) is represented by the velocity at right face of cell (imjk). But how about the velocity at the left face of the far left cell? Is that the reason why Flow-3D using real cells and boundary cells around them?

A: Yes, this is one of the reasons. The boundary cells are also used to set other BC variables like pressure and temperature.

By the way, when I asked a question about the calculated free surface in Flow-3D by VOF method, Jeff Burnham relpied that "the way FLOW-3D calculates the fluid free surface in sharp-interface problems uses special algorithms (TruVOF and FAVOR) so that the location of the free surface is accurately calculated independent of the mesh size". Does that mean the calculated free surface in Flow-3D is insensitive to mesh size? Since the definition of entrainment through NF values in the customization which I'm using is sensitive to the mesh size, I'm thinking if I can use another method to tracking the entrainment location.

A: What Jeff meant is that the interface is always kept sharp, that is, contained within one cell, as opposed to spread over several cells. Also the FAVOR method for processing geometry is independent of mesh to a degree in that one can change the mesh without changing geometry and vice versa, in contrast to body-fitted grids.

The solution in general, of course, depends on the resolution. For example, flow features that generally affect the free surface dynamics can be resolved only to the smallest mesh size, etc.

There is a class of relatively simple problems where mesh dependency of the free surface solution in FLOW-3D is minimal, but they are not representative of real world flows.

Thanks a lot!

Yang

ghjfghjsfgfsssssssssssssssssssssssssssssssssssssss sssssssssss
gfssssss