# CFX: ERROR #002100080: Significant Normal Component or MESH is moving

 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 27, 2012, 13:51 CFX: ERROR #002100080: Significant Normal Component or MESH is moving #1 New Member   Join Date: Aug 2012 Posts: 16 Rep Power: 4 Dear Sirs, I have a problem with ANSYS CFX. I am trying to do an multiphase analysis with water and air in a rotating default domain. In the attachment you can find the detailed problem description and the Step file with the geometry. OilPan.pdf http://dl.dropbox.com/u/66722906/Oil%20Pan.pdf OilPan.zip (STP File) http://dl.dropbox.com/u/66722906/CFD_Oil_Pan.zip I would appreciate your support in terms of my problem. Please find the error code below: ================================================== ==================== OUTER LOOP ITERATION = 1 CPU SECONDS = 2.293E+00 +--------------------------------------------------------------------+ | ERROR #002100080 has occurred in subroutine CHECK_NORMV. | | Message: | | The specified velocity vector on the boundary patch | | | | Rohr | | | | has a significant normal component at one or more faces. One of | | these face locations is | | | | (x,y,z) = ( 2.31316E-01,-1.46685E-02, 2.43947E-03). | | | | The angle between the specified velocity and the element surface is| | 81.624 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. | +--------------------------------------------------------------------+

 August 27, 2012, 18:47 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,825 Rep Power: 85 Does the scoop pipe rotate with the domain? Or is it meant to be stationary? I take it there are 4 scoop pipes in the full domain.

August 28, 2012, 02:44
#3
New Member

Join Date: Aug 2012
Posts: 16
Rep Power: 4
Hi ghorrocks, thank you for your effort.

No, the scoop pipe stands still. The whole domain rotates besides of the scoop pipe. Thats why I have chosen the boundary "counter rotating wall" in CFX. In the ansys help i found that the selected geometry rotates with -omega*r. So the absolut velocity will be zero.

The next step of the analysis will be to model the inlet geometry of the pipe because until know this is neglected. I just want to see what is the seperation angle of the water caused from the scoop pipe.

The number of scoop pipes depends on the required discharge of oil. In this case there are 4 scoop pipes. Thats why i have chosen a fourth of the whole.

Please find the sketch in the attachment. I hope this makes the system more clear.

Thank you in advance and best regards from Austria.
Attached Files
 Oil_Pan_Sketch.pdf (31.3 KB, 56 views)

 August 28, 2012, 07:21 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,825 Rep Power: 85 I see - in that case you have taken the wrong approach. If the scoop pipe is still then it needs to go into a stationary frame of reference, with the rotating bit in a rotating frame of reference, and are connected by a GGI. Have a look at the rotor/stator example for how to do this. Is there 1 scoop pipe or more than 1?

 August 28, 2012, 10:00 #5 New Member   Join Date: Aug 2012 Posts: 16 Rep Power: 4 hi ghorrocks, ok i will check this turorial. I used a fourth of the whole for my calculation model (90degrees) because i assume 4 scoop pipes on the whole system. To safe calcualtion time and mesh elements I used a fourth piece. So in my calculation model there is one, but in reality on 360° there are 4. Thanks, i will keep you updated.

 August 28, 2012, 19:31 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,825 Rep Power: 85 OK, so you have 4 scoop pipes and I think it was 10 paddles. So on the stationary frame of reference you can use 1/4 of the model, in the outer rotating frame of reference you can use 1/10 symmetry. This will make your simulation smaller and easier to manage.

 August 29, 2012, 01:34 #7 New Member   Join Date: Aug 2012 Posts: 16 Rep Power: 4 Good morging everybody, ghorrocks, yesterday i did the tutorial of the Rotor Stator (axial Turbine with TURBO GRID import). In principle now I understand what I have to do. But my question is how to set up the model. In the tutorial i have seen that there are two seperate domains used and connected via "Domain Interface". My Problem is, that the scoop pipe is inside of the Oil pan. Where do I have to define the cut (where do I have to create the interface) to be able to create two seperate 3D models and then two domains? The scoop pipe is just a cylindical cutout out of the oil pan volume.... Thank you in advance for you help

 August 29, 2012, 07:14 #8 New Member   Join Date: Aug 2012 Posts: 16 Rep Power: 4 Hello once again, I think now i got it. I did the wrong tutorial. there is a seconed one with a mixer. today evening I will do this one. As far as I found out in the help the problem is that i have not done 2 different domains. I will keep you updated. Thank you for your support.

 Tags free surface flow, multiphase

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20 mactech001 ANSYS Meshing & Geometry 0 November 5, 2009 03:19 songxguan CFX 7 June 28, 2009 21:05 eleazar solve everything CFX 5 March 6, 2007 02:41 Jesper CFX 5 February 2, 2007 04:43

All times are GMT -4. The time now is 05:50.