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

LinkBack  Thread Tools  Display Modes 
August 27, 2012, 13:51 
CFX: ERROR #002100080: Significant Normal Component or MESH is moving

#1 
New Member
Join Date: Aug 2012
Posts: 20
Rep Power: 6 
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) = ( 2.31316E01,1.46685E02, 2.43947E03).     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: 12,638
Rep Power: 98 
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: 20
Rep Power: 6 
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. 

August 28, 2012, 07:21 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98 
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: 20
Rep Power: 6 
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: 12,638
Rep Power: 98 
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: 20
Rep Power: 6 
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: 20
Rep Power: 6 
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  


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