Finding vector parallel tolerance
 

Dear CFX users

After running a problem with a course mesh I tried to make another run, exactly as the previous but with a finer mesh. The way I make a finer mesh is to change the value in mesh control to a smaller value and rerun the problem. But after doing this I got an error message saying that the vector parallel tolerance value needed to be changed from 5 degrees to a slightly higher value in the expert parameter section. So....I have two questions:

1. Is my method right when making a finer mesh by choosing a smaller value in mesh control?

2. Where, in the expert parameter section can I find the vector parallel tolerance so I can change it to a higher value?

Re: Finding vector parallel tolerance
 

1. Changing the mesh resolution in this way is fine.

2. Edit your definition file with the definition file editor. Add the expert parameters section, then add the vector parallel tolerance parameter.

You should also check your mesh. Load your grid into CFX-Post, and highlight your symmetry plane. Change the color to the X, Y or Z grid coordinate (whichever your symmetry plane is normal to), change the plot range to a local range, and see if there is any variation in the color that looks funny. If this is the case then the grid is bad and the solver may not behave very robustly.

Neale.

Re: Finding vector parallel tolerance
 

Thank you so much for that excellent answer I got!!! Sincerely,

Dimitris

How to?
 

Hello,
Can someone expliain how and where to change this vecctoe parallel tolerance?

Thnak you

Vector parallel tolerance
 

How can I change the value of Vector parallel tolerance in CFX?

Thank you in advance

Like Neale already explained in 2002:
- go the CFX-Pre
- add Expert parameters
- look for vector parallel tolerance
- set the value to 5

If you need more than 5, remesh your geometry and pay attention to the mesh on your symmetry plane. Are you using ICEM?

Hello Gert-Jan,
I am trying to simulate fluid flow in gyroid structure and I got the same problem. I have created mesh using ICEM. May you please suggest how can I solve such a problem.

I tried changing the expert parameters as vector parallel tolerance = 5 and degeneracy check tolerance = 1 but still, get errors.

Please help!
Let me know if you need any further details.

Thanks in advance.

-Biltu Mahato

This is an old query. I really have no idea how to solve it. Could it be that you are trying to solve the flow in a wedge with periodic or Symmetry BC? And that your mesh is being detoriated in the angle at r=0?

To help you further we need:
- the output file, showing your error.
- the geometry
- the grid.

It is a cuboid (fluid) with gyroid (solid) removed. I can send you the file. Please let me know your email.

I would post some figures and the output file here on the forum. Then all members can take benefit from what you learn.

Geometry is a cuboid - gyroid as in the image below.
Attachment 85621

The mesh I used is as;
Attachment 85622

The setup is symmetric BC is four sides with inlet and outlet. The error observed for this setup of model is as;
Attachment 85623

I use ANSYS 18.2

If you define the body with multiple faces a symmetry plane you will get that error. You have to make each face its own symmetry plane.

In other words, each symmetry plane has to be a plane. Obviously.

I don't know what you are trying to solve exactly, but I hardly see any symmetry. Shouldn't you use periodic boundaries?

Ghorrocks,
I tried symmetric BC on individual faces instead of multiple faces altogether. But unfortunately, the solver gives a similar error as;

+--------------------------------------------------------------------+
| ERROR #002100013 has occurred in subroutine Chk_Splane. |
| Message: |
| The symmetry boundary condition requires that the boundary patch |
| mesh faces form a plane or axis. However, face set 3 in the |
| symmetry boundary patch |
| |
| Boundary 11 |
| |
| is not in a strict plane, which means that at least one of its |
| faces is not parallel to the others. To make the solver run |
| you can do one of the following: |
| |
| (1) Make sure that this symmetry boundary patch is in a plane or |
| axis by checking and regenerating the mesh. |
| (2) If the symmetry boundary patch is an axis rather than a |
| plane, change the tolerance of the degeneracy check by |
| increasing the value of the Solver Expert Parameter |
| 'degeneracy check tolerance' (the default value is 1.e-4). |
| (3) Increase the value of the Solver Expert Parameter |
| 'vector parallel tolerance' (the default value is 1 deg.). |
| Note that the accuracy of the symmetry condition may decrease |
| as the tolerance is increased. This is because the tolerance |
| is the number of degrees that a mesh face normal is allowed |
| to deviate from the average normal for the entire face set. |
+--------------------------------------------------------------------+

What do you recommend now?

Gert-Jan,
Its fluid flow through the domain. The symmetry here means no normal component of the velocity vector. It's not periodic.

The error message is very simple - it just says your boundary defined as a symmetry is not on a single plane. So load it up in a post processor and look at what you have defined as those boundary faces. You need to fix up whatever is out of the plane.

Probably you have a few elements on a symmetry plane that are not flat. Make sure all elements are on the same plane and have the same normal.
Either change the geometry or move nodes individually. In ICEM you have the possibility to align nodes such that they are in line. Know how to do this?

All of us somehow reached the conclusion that some elements are not flat in one/many faces. I agree.

I think the elements at the sharp corners (both curved and non-curved corners) are not in the plane. I am trying to attach some images but the website is forbidding me to do so.
So, guide me, how can I check the normal of elements? If it's not normal, how to make it normal?

I mentioned, you can do this in ICEM.
Alternatively, use free slip walls instead of symmetry, although this is a quite brutal workaround ;-)

Thank you Gert-Jan.
May you please share some youtube/other tutorials/links which could be helpful? I am kinda new in the IDEM world. ))