Learning Forum

[corne]

Dear,

I am an experienced user of Ansys Mechanical, but am currently trying out Ansys Fluent and I have some problems with that.

Let me first try to explain what I am modelling.

I want to do an analysis of wind load on an open top storage tank. So basically I have a cylindrical wall with a flat bottom for example 30 m diameter and 12 mm thick wall. If I want to perform a mechanical calculation for this structure I would use a surface model with shell elements.

I started to use this type of modelling in SpaceClaim for my model. Making the surface model of the shell is very simple, but then I needed to make the fluid domain. It doesn't seem possible to create the fluid domain using a surface model for the solid part. From this experience my first questions:

1. Can only solid models be used in Ansys Fluent?

2. If surface models can be used, how to create the fluid domain?

For now I modelled the cylindrical shell using a solid. First I tried to use a solid with the real thickness of the shell, but then I got problems when meshing. Apperently the mesh of the solid and the mesh of the fluid domain were too far off.

Then I modelled the cylindrical shell using a solid, but with a wall thickness of 100 mm. This gave no problems for the meshing. However it doesn't really represent my situation anymore. I don't think it will give large errors in the CFD analysis. However I am afraid I can't easily copy the pressure on the cylindrical wall to the mechanical model (which is the idea of the analysis) as the wall thickness is not correct in the CFD model but will be correct in the mechanical model. This leads me to the following questions:

3. if solids need to be used is it possible to use very thin solids such that it doesn't create issues with the mesh?

4. Can the pressure on the surfaces of the solid be transferred to mechanical, even if the thicknesses/locations are not completely correct? And if so, how to do this?

Thanks in advance for your valued replies.

[Rob]

In Fluent we use "solid" zones too, we just call them fluids. If you create one zone that is the volume of the tank and a second one for the outer domain you can label the surfaces you need to be walls. Have a look in the Help system tutorials to get some more ideas. In Fluent we can use thin walls (not dissimilar to a shell) provided there are fluid (volume) cells on one or both sides.  

Overall the geometry & mesh parts are very similar, it's just a case of applying the CFD terms and having a decent mesh. 

[peteroznewman]

Here is a relevant discussion that used faces to represent walls.

In your case, you would have a solid block to represent the wind tunnel of air, say 200 m long x 200 m wide x 100 m tall.  Then you create a solid cylinder with a 30 m diameter on the center of that 200 x 100 m floor to the height of the open tank.  Now you subtract that cylinder from the block, but keep the tool.  Now you have two solid bodies that don't interfere and you can turn on shared topology.  In Meshing, use Named Selections to name the cylindrical face Wall-tank, name the top circular face Interior, and name the bottom faces Floor.  Name one end of the wind tunnel Inlet and the other end Outlet. The other three sides of the wind tunnel can be named Symmetry.  Make sure both solid bodies are set to Fluid in the Properties.

After you mesh, in Fluent, you will end up with an open topped zero thickness tank that you can compute the pressure on the cylindrical face and transfer that to a Structural shell model.