Error on the interface of a rotating domain, r=0
 

I created a rotating domain around a fan and I am trying to launch a simulation with a stage mixing plane, but I get this kind of error on the interface.

ERROR #001100279 has occurred in subroutine ErrAction.
Message:
****** FATAL ERROR ****** The orthographic view transformation fa-
iled on domain interface "Interfaccia rotante". Failure may be d-
ue to r=0 included in transformed cylindrical coordinates of an i-
nterface with rotational relative motion. Another reason could b-
e that the interface contains faces that are parallel and others
that are perpendicular to the rotation axis.

I am understanding that maybe the problem is on the orthogonal surfaces, so I separated them and I tried to define 2 different groups of interfaces, but I get this one.

ERROR #001100279 has occurred in subroutine ErrAction.
Message:
Floating point exception: Zero divide

So I am thinking that maybe ANSYS solves the equations in cylindrical coordinates with the origin on the rotation axis , so when r->0, the solver is not capable to define the angle of the position, so trying to define different groups of interfaces does not change the result, but I am not sure that this is what is happening exactly.
I do not know if this is possible, but maybe there is a way to set the solver to use another frame of reference for the equations.

Anyway my question: is there a way to overcome this error?

Usually there should be no problems when setting up a calculation with rotating domains and interfaces.
But you can write 1000 words about it, a picture of your setup says more. So, please add one so we can help........

I understand, you are right.

Here you are some pics of my setup, let me know if you need other information.

Stationary domain.
Attachment 63870

Rotating domain.
Attachment 63871

Interface.
Attachment 63872

Second frame of reference.
Attachment 63873

The images Gert-Jan was referring to was images of your geometry. So please post some images of your geometry. You setup is best described by generating a CCL file and attaching that to a post.

How can I generate the CCL file? I am sorry if this is a stupid question, but I am a beginner and I never did it.



Here you are the pics of the geometry.

This is a section, the rotating domain is in red.
EDIT

And these are two views of the rotating domain (I used the orange face in CFX-Pre for the "coord 1" frame).
EDIT

When you run your case in the solver manager, you get a nice text window telling you what CFX is doing exactly. If you copy the contents of that text window to a text editor (e.g. Notepad) save and upload that file, then in fact you have a .ccl-file.


Regarding the interfaces,
- I don't understand it. You mention 1 interface, But don't you have 2? One at the inlet and one at the outlet of your rotor?
- It looks like you have a full 3D geometry. Then why do you use Stage interface? I would use General Connection & Frozen Rotor for both interfaces. That is all you need for a steady state calculation (as a start).
- I have never needed the Mesh Connection/Direct. So don't think you need it as well.
- The error tells me there is something wrong with the orientation of the interface around axis of rotation. Are you convinced you have setup your rotation coordinate correclty? Is the rotation around the z-coordinate of Coord 1. (=Coord1.3)?

OK, thanks, I did not know that the CCL file was the output in solver manager saved in a text file.

The shape of the geometry is complicated, so I used every surface of the rotating domain, I created a group and I used it as an interface.

That option was an attempt as a starting point, the main problem is that the solver does not start also if I use frozen rotor or transient. My goal is the full transient one.

OK, I am not sure what to say about this, because I always checked it, but maybe I did not understand the right purpose of this feature.

The rotating domain is a solid of revolution created in a CAD environment with a sketch. After in ANSYS (geometry) I only created the enclosure/inclosure around it (the stationary domain) and I did the boolean operation with the fan.

I did it! I created a new coordinate system (coord 1) with its origin in the center of that face and I used one of its axis for the rotation.

You should not put all surfaces in a single interface.
Create a unique interface for each every surface with a unique normal. I guess you'll have at least 2 or 3.

"Pitch change" = "none" solved my problem.
Thank you very much.