[dreamchaser]

Hi,

I am trying to solve a problem related to Journal Bearings. I have attached a picture of my problem with the boundary conditions. My rotating wall is not working and I am getting the standard error below (at the end of the post). I know my rotation axis is correct (in z-direction).

Boundary Conditions are:
Inlet: 0 Pa static pressure
Outlet: 0 Pa static pressure
Wall: no slip wall
Circular Wall: Rotation with 1 rad/s
I am running steady state in-compressible.

Regarding the recommendation of changing 'tangential vector tolerance wall' from its default of 20 degrees, I went into CFX>>Insert>> Expert Parameter and saw the default 'Tangential vector tolerance' was set to 10. I raised this to 30 and still it did not work.

I believe the problem is in my mesh. The gap space is very small (10^-7m) and the wall is rotating at 1 rad/s. The viscosity is .5 Pas.
I have also attached a picture of my mesh I am using which contains 3000 elements. I have tried to bias the elements so to refine near the walls.

Any advice would be appreciated.

Thanks!


| The specified velocity vector on the boundary patch |
| |
| circularwall |
| |
| has a significant normal component at one or more faces. One of |
| these face locations is |
| |
| (x,y,z) = ( 5.83485E-02, 9.86245E-03,-6.73600E-06). |
| |
| The angle between the specified velocity and the element surface is|
| 89.907 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.

[ghorrocks]

With a massive change in length scale like this you are asking for trouble with numerical instability. You will need a very good quality mesh to keep this under control. I would make your mesh more evenly graded across the flow and make you inlet and outlets radial to the circle. This will help.

But your current problem is simply that you have define a tangential velocity which does not appear tangent to some mesh faces. This can be because:
* You have incorrectly selected some faces to apply the tangential velocity to
* Your mesh is wonky somewhere. I think this highly likely in your very thin region.

[dreamchaser]

Originally Posted by ghorrocks

With a massive change in length scale like this you are asking for trouble with numerical instability. You will need a very good quality mesh to keep this under control. I would make your mesh more evenly graded across the flow and make you inlet and outlets radial to the circle. This will help.

But your current problem is simply that you have define a tangential velocity which does not appear tangent to some mesh faces. This can be because:
* You have incorrectly selected some faces to apply the tangential velocity to
* Your mesh is wonky somewhere. I think this highly likely in your very thin region.

Hi Glenn,

Thanks for your response. I refined my mesh and am still getting the error.
(Picture of mesh is attached)

To clarify, I just set the circular wall to have a rotational velocity of 1 rad/s. I do not select any faces to apply this condition to. Just the circular edge.

I have a feeling it has to do with tolerancing. I am using ANSYS Workbench to make my geometry and mesh. I wanted to know if there was a tolerancing feature available? For example, since my domain is so small, there should be a tolerancing feature to set when I am generating a surface for the geometry. I think my surface is not fitting well enough onto the top of the circle so there is some nodes not touching it at the surface. I am not sure if your sketch and surface are supposed to be aligned with each other. If you see mines (attached pic) the circular region has a bit of waviness to it. Not sure why this is happening.

Another way I tried, was when importing the fluent.msh into CFX, I checked 'Duplicate Node Checking' and changed the default tolerance of 1e-04 to 1e-7. Still it did not work.

Another possible cause I am thinking is importing the mesh as a Fluent.msh. I know in the past, that sometimes when I would import from Gambit into another software, the mesh would not be generated properly and there would be uncovered faces. I am currently using ANSYS workbench to make my geometry and mesh. After making my geometry and mesh, I close ANSYS Workbench and open CFX and import the mesh. I do this because I always face an error in trying to launch CFX directly from ANSYS workbench. Since I always do a 2-D geometry it always gives me the error "Body is an unsuppressed body that does not enclose a volume. Only 3D meshes can be imported.."

Any insight would be greatly appreciated.

Thanks for your time

[jp_]

Quickly like this, you might want to ensure your center of rotation "Global Z" located at the center of rotation of your bearing, not the centroid of your mesh. You should be able to plot the velocity vector of the wall.

[dreamchaser]

Originally Posted by jp_

Quickly like this, you might want to ensure your center of rotation "Global Z" located at the center of rotation of your bearing, not the centroid of your mesh. You should be able to plot the velocity vector of the wall.

jp ,

Thanks so much!! That was the problem! I redid my geometry and put the origin at the center of rotation and it works now!