Hello everybody!

Is there anyone who succeeded in simulating a 2D axisymmetric flow with CFX4.2 without using the ">>simple grid" option in the command language) ? As usual, the manual is very scarce on information! Please drop me a line!

Regards

Andreas

Yes!

What is your problem?

Regards Jan

Hello Jan and thanks for answering my cry for help,

I've tried to set up a simple axisymmetric flow in 2D (fully developed pipe flow) with the main flow in the x-direction. The first question is how to handle the x-axis: I guess it is not possible to create a grid where the 1st cell coincides with the axis (i.e. r=0) itself as this would demand a cell type with only 5 sides instead of 6. So I have made the grid to begin at a very small radius (with a very small face there). Is this the way you did it?

Ok, then there is the thing with the outer surface (at the maximum radius). This is not supposed to be flat, but rounded. I suppose it can be forced to have this shape with the aid of splines when creating the edges of the face. But is the shape really of great importance when the flow is 2D? Is the flat surface a good enough approximation (or is it even exact?)?

To conclude, I tried to run the case but the only thing I get is error message: "ERROR: A 2-DIMENSIONAL GRID MUST HAVE Z ONLY DEPENDENT ON K THE CFX-4 SOLVER HAS BEEN STOPPED BY SUBROUTINE CREATE"

If the z-direction (which in my grid is the theta-direction) is supposed to be the normal of the symmetry plane(s) it must be allowed to vary with I and J, or else a grid of cylinder shape is not possible?!

Med venlig hilsen

Andreas

Hi Andreas,

There are several solutions to your problem. First, I assume that you are using build, the problem in mesh-build is a bit different. I also assume that you do not want to calculate a 360ï‚° model but a slice. If you want to do a full model then you should create it in a Cartesian framework with an O-grid patched to a H-grid, see figure 1 of the solver manual.5 (Page 11 in CFX4.2 manual)

You have to select in which way you want your model, there are at least two options,

You should read the online help in build about "Introduction to Analysis" – go to the analysis and press F1.

3D Cylindrical model

From your reply, I guess you are trying to create a 3D cylindrical model and having problems around the axis. Your must divide the surface seen in the r-theta direction into three surfaces, (see the above mentioned online help for a figure), with the corner of the lower surface on the axis. In this way, you do not need to begin the grid at a small radius. Extrude the three faces in the x-direction. If you have created the outer radius as a curve – Create curve – f.ex. 2D ArcAngels, then you also get a curved outer surface. Create the grid. Remember to set symmetry planes at the two surfaces in the circumferential direction.

On the analysis form, leave the Real geometry button as it is and change the Geom. File coord. System to (x,r,theta).

This should be all for this model

2D axisymmetric model.

This is the easiest model to make-work, use it whenever you can. In this model, you actually define your grid in x-r-Theta coordinates, which unfortunately means it can not always be used

Create a surface in the x-r plane, extrude it in the Z direction (in radians) to create a solid. Set a symmetry plane on the lower surface(r=0) and in the two faces in the circumferential direction. Remember if you want a 2D model then the mesh seed in the z direction should be 1, if you do not do this, then depending on the Global Edge length value there will be grid cells in the Z direction which of course is wrong for a 2D model. This is probably the reason for problem in the last point you mentioned in your reply. You can have grid cells in the Z direction but then you should define it as a 3D cylindrical problem in the command file.

Go to the analysis form and press on Type of Geometry and select Slab = Wedge in the solver. Remember in the command file to include the option – axis included.

Hope this helps,

Regards Jan

Hello and thanks for the effort,

but I do not have Build. Anyway, I have managed to create a grid consisting of a sector (it's the 2D axisymmetric flow I want) with inner radius at r=0 (which I did not think was possible) thanks to your "extrusion in the theta direction"-tip. Alright! I only use one cell in the theta direction as to achieve a "2D grid". The main flow direction is in the x-direction and corresponds to my I-direction of the block. The radial direction is the J-direction of the block. Which leaves the K direction to be my theta (circumferential) direction. Still, I get the error message:

ERROR: A 2-DIMENSIONAL GRID MUST HAVE Z ONLY DEPENDENT ON K THE CFX-4 SOLVER HAS BEEN STOPPED BY SUBROUTINE CREATE

when I try to solve. I use this in my command file:

>>OPTIONS

TWO DIMENSIONS

BODY FITTED GRID

CYLINDRICAL COORDINATES

AXIS INCLUDED

I've made sure that I did not forget to define the HIGH K, LOW K, LOW J planes as symmetry planes.

What do you think?

/Andreas

Hi again Andreas,

Now it is getting difficult, my memory about mesh-build (if that is what you use) is a bit rusty. My best clue now is to ask CFX user support!!!!

I can only remember two other points you should check. The J direction should increase away from the radius, but the error message you have is probably not related to that, else it would be something about low J on axis etc.

The error message you get could be related to if you have a variation of the grid in the Z direction (volume change), you must ensure that you have the same beginning and end angle for all your blocks (in your case with the 2D).

Try to create 1 face (and only one) in the x-r plane and extrude it, say, PI/2 in the z direction. Check the orientation, J increasing from the axis. Set symmetry planes on the 3 faces, create the inlet and outlet. Create the mesh seed, 1 cell in z direction. Write the grid. Do not use meshimport! Run your command file, be sure you only have an inlet U velocity. If this does not work, I do not know what to do.

Regards Jan

Hello Jan and thanks for your help,

I've now been enlightened that one should create a slab for the 2D axisymmetric flow and not a wedge which I have been doing. Sorry about the fuss.

Andreas

I am not a CFX user, but is very interested in your discussion. I don't quite understand why you need to take special care for the axis since as far as Finite-volume is concerned, that face has zero area and thus does not contribute to the discretised equations at all.

2d axisym modification has now been included in CFX-4.3 with a new keyword in >>OPTIONS

Good luck