[nav_5]

Hello there!!!!

I'm performing a benchmark between CFX and Fluent. I'd like to reproduce a tank filling process in a 2d axisimmetric geometry. The flux is supersonic, it is a kind of free expantion in the vacuum with a fixed pressurization rate of the vessel. I've setted the pressure profile and mass flux at the inlet of the 2d Fluent domain via UDF. The results are consistent with the experimental data. Unfortunatly I can't set the same boundary conditions in cfx. The cfx geometry is obviously a 2d geometry extruded along the third dimension. I have used pressure and velocity boundary conditions for a supersonic flow but the expected velocities are very low respect to exeperimantal data and Fluent computatio......any suggestion?

Thank you
Ivan

[flotus1]

As far as I know, CFX is not capable of simulating axisymmetric domains.
You need to model at least a slice of the geometry and apply symmetry or periodic boundary conditions at the cut faces.
A 2-dimensional domain extruded to the third dimension does not correspond to an axisymmetric flow.

From the FAQ section of the wiki:

Is there any way of doing a 2D simulation in CFX?

Yes. From a 2D mesh of the geometry, extrude it one element in the normal direction. For a 2D planar simulation this would be one element in the normal vector direction, for a 2D axisymmetric simulation this would be sweeping a small angle with one element. For the planar mesh the extrusion should be approximately equal to the smallest element edge length in the model, for the axisymmetric mesh the sweep should be a small angle, maximum 5° but smaller if you want high accuracy.
In CFX-Pre you should set the top and bottom faces of the extrusion as symmetry planes. If you want to include swirl in the model use periodic boundaries. The remaining boundaries should be set as walls, inlets, openings and outlets to define the flow.
The CFX documentation discusses 2D simulations and it is recommended you read it before proceeding.

[ghorrocks]

To model a 2D axisymmetric model you sweep rotate an angle rather than a translational extrude to generate the third dimension. Again this is a pretend 2D model and is poor in comparison to Fluent's true 2D model.

[evcelica]

Poor in what way? I can see axisymmetric being poor, as you will get a bad quality mesh, but what about a 2D when you actually extrude 1 element thick? Is fluent any better as far as results for these types of geometries?

[ghorrocks]

The CFX approach to 2D is poor as it is using a 3D solver, so it is solving the third dimension but that will always just evaluate to zero. This is a waste of CPU time, memory and results file size. A true 2D solver only solves in the two dimensions the model actually contains. This will make a 2D solver many times faster than a 3D solver on a single element thick model - I do not know the speedup factor for sure, but would guess it is 10-20 times faster.

And 2D axisymmetric adds the extra complication that the elements along the axis only sweep out a small wedge angle (5° is often the biggest angle used, smaller angles are used when accuracy is required) - but this is a terrible quality element. A true 2D axisymetric solver has no quality issue at the axis.

[evcelica]

OK this is what I figured, its just slower, and axisymmetric swept mesh is garbage.
I can't believe 10-20 times faster, that's incredible. I'm going to start to try and learn Fluent if it that much quicker in 2D.

[ghorrocks]

If you are doing lots of 2D runs then I would recommend you try another solver with a true 2d solver.

This is a frequently requested feature for CFX for many years and they have never done it. Sure it is a lot of work for the developers but it is a gaping hole in CFX's capability. They deserve to loose customers because of it.

[Vaaj]

Hey Nav5,

You said you input pressure profile and mass flux through UDFs did you use two udfs for this case?
Hey Alex,

I am also trying to simulate filling of air into chamber containing some air. Did you get answers for your simulation. I have a varying inlet mass and pressure. How do I initialize?
I have pressure profile data, mass flux, mass flow, temp, density variation with respect to different time steps and have UDFs of these. But nothing is realistic when i Simulate in Fluent. Do you have any solution strategy?