CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   why shroud velocity can't be set (http://www.cfd-online.com/Forums/cfx/85553-why-shroud-velocity-cant-set.html)

myleader March 1, 2011 07:57

why shroud velocity can't be set
 
1 Attachment(s)
I'm simulating a compressor, there is a rotating impeller in it, so I set a rotating domain around the compressor including shroud, back and diffuser.

Then I set the wall boundary for impeller with no wall velocity, and the wall boundary of the housing with counter rotating velocity, but some error occured. There is some hint, but I can't agree with it.

Code:

+--------------------------------------------------------------------+
 | ERROR #002100080 has occurred in subroutine CHECK_NORMV.          |
 | Message:                                                          |
 | The specified velocity vector on the boundary patch                |
 |                                                                    |
 |  back                                                              |
 |                                                                    |
 | has a significant normal component at one or more faces. One of    |
 | these face locations is                                            |
 |                                                                    |
 |  (x,y,z) = (-1.28389E-02,-9.78577E-03,-9.31152E-03).              |
 |                                                                    |
 | The angle between the specified velocity and the element surface is|
 |  32.872 degrees at this face. This is considered an error because |
 | it implies that the mesh is moving.  The following are possible    |
 | reasons for the error message:                                    |
 | 1. There is a setup error; for example, an incorrect axis of      |
 |    rotation.                                                      |
 | 2. There may be a meshing problem; for example, the nodes on a    |
 |    rotating surface might not lie on the surface of revolution.    |
 | 3. The boundary is curved and the mesh is very coarse. In this    |
 |    case, you may modify the tolerance by increasing the            |
 |    expert parameter 'tangential vector tolerance wall'            |
 |    from its default of 20 degrees.                                |
 +--------------------------------------------------------------------+

But every one can see, that boundary is orthogonal to x axis, I can't understand why the error message is like this.

Max Efficiency March 2, 2011 06:57

Two methods are possible:

A. Go in CFX-Pre and change the expert parameter as described.

B. Go in ICEM or MEshing and create a finer grid at the responsible surface/body with a higher resolution of surface angles (e.g. 15 instead of 25 degrees resolution).

Of course, you can combine both methods.

cfdgremlin March 2, 2011 09:54

Somewhere on your boundary 'back', which I think is the one defined with counter-rotation, there is a face/faces that have a significant normal component to the direction of rotation. This boundary needs to define a surface of revolution around the axis of rotation, otherwise it is unphysical.

The problem could be, as mentioned above, that the mesh quality is poor (e.g. some spurious faces ar included in the boundary), but it needs to be checked. If it is just mesh quality, then the tolerance can be lowered to get past the solver hard stop.

myleader March 2, 2011 20:38

Thank you for your help. Please let me explain something more.

The trouble happens not only at back boundary, it happens at shroud and diffuser boundary, too. They are all axis symmetry to x axis which I set to be the rotation axis.

I used CFX for some time. In the past, I use it to simulate impellers in open field such as wind turbine and ship impeller, so all the interface between rotation domain and static domain were fluid-fluid and frozen stator. This is the first time I meet the outer housing stagnation condition, and I set them to be counter rotating wall, but I fail. I'm really confused about this trouble.

Max Efficiency March 8, 2011 03:38

Please check if the x-axis in your 3d-model is really exactly at the some position compared with the rotation axis.

In other words:
It is possible that the axis of rotation and the x-axis are parallel, but not identical. Everything seems to be okay, but in reality the axis of rotation is wrong and the 3d-model has to be shifted. You have to move the model in a way, that x-axis and axis of rotation of model are identical.

...maybe that helps you. But unfortunately I don't think so.

joey2007 March 9, 2011 17:03

If you are not using the latest version of CFX, it may also help to try the latest version of CFX.

flilk October 18, 2011 04:12

hello,now i have the same problem with you (my simulation is about centrifugal pump with hub and shroud casing ).i have increased the tangential vector torlerance ,and it works,but i'm not sure wether i'm correct ,and now i don't know details about tangential vector torlerance ,like how to chose it's value ,and i don't know my simulation is correct or not?


All times are GMT -4. The time now is 14:38.