CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Finding vector parallel tolerance

Register Blogs Community New Posts Updated Threads Search

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 2, 2002, 07:09
Default Finding vector parallel tolerance
  #1
Dimitris
Guest
 
Posts: n/a
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?
  Reply With Quote

Old   September 3, 2002, 14:59
Default Re: Finding vector parallel tolerance
  #2
Neale
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   September 3, 2002, 15:44
Default Re: Finding vector parallel tolerance
  #3
Dimitris
Guest
 
Posts: n/a
Thank you so much for that excellent answer I got!!! Sincerely,

Dimitris
  Reply With Quote

Old   June 13, 2017, 12:14
Default How to?
  #4
New Member
 
Join Date: May 2015
Posts: 1
Rep Power: 0
redrahul is on a distinguished road
Hello,
Can someone expliain how and where to change this vecctoe parallel tolerance?

Thnak you
redrahul is offline   Reply With Quote

Old   February 1, 2018, 06:46
Default Vector parallel tolerance
  #5
New Member
 
Walaikorn
Join Date: Jan 2018
Posts: 1
Rep Power: 0
Walaikorn is on a distinguished road
How can I change the value of Vector parallel tolerance in CFX?

Thank you in advance
Walaikorn is offline   Reply With Quote

Old   February 1, 2018, 16:55
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
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?
Gert-Jan is offline   Reply With Quote

Old   July 27, 2021, 10:33
Default
  #7
New Member
 
biltu M
Join Date: Feb 2021
Posts: 17
Rep Power: 5
biltu is on a distinguished road
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
biltu is offline   Reply With Quote

Old   July 27, 2021, 16:00
Default
  #8
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
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.
Gert-Jan is offline   Reply With Quote

Old   July 28, 2021, 08:38
Default
  #9
New Member
 
biltu M
Join Date: Feb 2021
Posts: 17
Rep Power: 5
biltu is on a distinguished road
It is a cuboid (fluid) with gyroid (solid) removed. I can send you the file. Please let me know your email.
biltu is offline   Reply With Quote

Old   July 28, 2021, 12:31
Default
  #10
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
I would post some figures and the output file here on the forum. Then all members can take benefit from what you learn.
Gert-Jan is offline   Reply With Quote

Old   July 28, 2021, 13:06
Default
  #11
New Member
 
biltu M
Join Date: Feb 2021
Posts: 17
Rep Power: 5
biltu is on a distinguished road
Geometry is a cuboid - gyroid as in the image below.
Geom.PNG

The mesh I used is as;
Mesh.PNG

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

I use ANSYS 18.2
biltu is offline   Reply With Quote

Old   July 28, 2021, 19:29
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 29, 2021, 05:59
Default
  #13
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
I don't know what you are trying to solve exactly, but I hardly see any symmetry. Shouldn't you use periodic boundaries?
Gert-Jan is offline   Reply With Quote

Old   July 29, 2021, 06:23
Default
  #14
New Member
 
biltu M
Join Date: Feb 2021
Posts: 17
Rep Power: 5
biltu is on a distinguished road
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?
biltu is offline   Reply With Quote

Old   July 29, 2021, 06:25
Default
  #15
New Member
 
biltu M
Join Date: Feb 2021
Posts: 17
Rep Power: 5
biltu is on a distinguished road
Gert-Jan,
Its fluid flow through the domain. The symmetry here means no normal component of the velocity vector. It's not periodic.

Quote:
Originally Posted by Gert-Jan View Post
I don't know what you are trying to solve exactly, but I hardly see any symmetry. Shouldn't you use periodic boundaries?
biltu is offline   Reply With Quote

Old   July 29, 2021, 06:27
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 29, 2021, 06:43
Default
  #17
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
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?
Gert-Jan is offline   Reply With Quote

Old   July 29, 2021, 06:50
Default
  #18
New Member
 
biltu M
Join Date: Feb 2021
Posts: 17
Rep Power: 5
biltu is on a distinguished road
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?
biltu is offline   Reply With Quote

Old   July 29, 2021, 06:56
Default
  #19
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,928
Rep Power: 28
Gert-Jan will become famous soon enough
I mentioned, you can do this in ICEM.
Alternatively, use free slip walls instead of symmetry, although this is a quite brutal workaround ;-)
Gert-Jan is offline   Reply With Quote

Old   July 29, 2021, 06:59
Default
  #20
New Member
 
biltu M
Join Date: Feb 2021
Posts: 17
Rep Power: 5
biltu is on a distinguished road
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. ))

Quote:
Originally Posted by Gert-Jan View Post
I mentioned, you can do this in ICEM.
Alternatively, use free slip walls instead of symmetry, although this is a quite brutal workaround ;-)
biltu is offline   Reply With Quote

Reply


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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Setting the Topo Tolerance (with a script) ChristianF ANSYS Meshing & Geometry 2 August 18, 2011 10:56
turbDyMFoam and Convergence lordvon OpenFOAM 5 September 25, 2010 22:18
[GAMBIT] gambit global geometric tolerance alireza2475 ANSYS Meshing & Geometry 1 July 19, 2010 02:23
stitchMesh for uncongruent patches (stitch tolerance) beugold OpenFOAM 0 June 18, 2009 08:38
Tolerance in GAMBIT Help!!!!!! Lottar FLUENT 0 October 6, 2008 15:03


All times are GMT -4. The time now is 16:17.