CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Is this correct? (Rotating domain) (http://www.cfd-online.com/Forums/cfx/77072-correct-rotating-domain.html)

paulo June 11, 2010 14:04

Is this correct? (Rotating domain)
 
1 Attachment(s)
Dear all,

I simulated a rotating cube with three domains (two static and one rotating). This is the result of the streamlines.

For me they seem very strange (I thought they would deflect only near the cube). :confused:

I apreciate any comments.

Best Regards,

Paulo Rocha

Attesz June 11, 2010 16:08

Hi,

your fluid has a very low velocity. What is your rotating speed? Don't forget, that you rotate not only the cube, but the whole flow field in the rotating domain.

paulo June 13, 2010 12:00

Thanks for the comment. In fact, I see that the whole domain is rotating. This is what was not desired. I would like to move the mesh (only), like this:

http://www.youtube.com/watch?v=1xZ3W3ST1Lo

The fluid doesn't rotate when it enters in the rotating zone. :confused:

Is this possible in CFX?

Thanks in advance.

Paulo Rocha

Attesz June 13, 2010 12:08

Yes, you should use moving mesh, which can be accurate then the rotating frames. But maybe smarter users will help you, i'm not experienced in it.

Anyway, your rotating domain is very large. You should define the rotating region only near that cube, but in your case, the moving mesh can be more suitable.

paulo June 14, 2010 10:42

Thank you very much Attila,

I will wait for better insights.

Best Regards,

Paulo Rocha

ghorrocks June 14, 2010 19:47

Quote:

Yes, you should use moving mesh
NO! Do not use moving mesh! This is a simple rotating frame of reference simulation so use multiple frames of reference, not moving mesh.

Your "problem" is that you are looking at velocity in the local frame of reference. Make the variable "velocity in stationary frame" and the streamlines will be as you expect.

Attesz June 15, 2010 04:03

Quote:

This is a simple rotating frame of reference simulation
I think this approach is better when the fluid zone really rotates. But here, the cube has low effect on the flow. In case of propellers, impellers etc it is suitable, but for example, for large wind turbines with only 2 blades it can be inaccurate, because the fluid between the blades doesn't have the same rotational speed than near the blades. Why isn't the moving mesh approach suitable here?

ghorrocks June 15, 2010 07:59

Quote:

I think this approach is better when the fluid zone really rotates.
Why? It only adds a huge computational load and convergence problems.

Quote:

the cube has low effect on the flow.
Then use the alternate rotation model in the rotating frame of reference.

Quote:

because the fluid between the blades doesn't have the same rotational speed than near the blades.
It is just a reference frame - it just means this fluid will have a velocity equal but opposite to the domain rotation. And the calculations remain accurate especially if the alternate rotation model is selected.

No, there is no cases where moving mesh is a better approach than a simple rotating frame of reference if the body just rotates.

Attesz June 15, 2010 08:02

Ok, thanks Glenn.

Attesz

paulo June 15, 2010 10:59

Dear Attila and Glenn,

I am really happy with your help. :)

I will try every tip tomorrow and post the results.

Best Regards,

Paulo Rocha

PS: It is only a test case. My intention is to put a wind turbine in the place of the cube.

paulo June 17, 2010 14:19

1 Attachment(s)
Here is the result. I think it is working fine now.

Thank you all.

Best Regards,

Paulo Rocha


All times are GMT -4. The time now is 02:37.