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

Error message from moving mesh modelling

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 18, 2004, 14:19
Default Error message from moving mesh modelling
  #1
John
Guest
 
Posts: n/a
Hi, All

The following message came from CFX-solver when I tried to run Tutorial 20--a moving mesh problem. I rebuild the model but still get the same message. Can anyone help me figure out the reason for that?

Thanks

+-----------------------------------------------------+

| An error has occurred in cfx5solve: | | | | The CFX-5 solver could not be started, or exited with return code | | 255: . No results file has been created. | +--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+ | The following transient and backup files written by the CFX-5 | | solver have been saved in the directory | | c:\ValveFSI1_005: | | | | 0.trn | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | Unable to retrieve mon from working directory: Cannot move to | | c:\ValveFSI1_005\mon: Permission denied | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | Warning! | | | | An error has occurred during creation of a directory for | | additional output files. To avoid losing results, the working | | directory c:\ValveFSI1_005.dir will be kept at the | | end of the run. Please tidy this directory up yourself when you | | have extracted what you need from it. | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | The following user files have been saved in the directory | | c:\ValveFSI1_005: | | | | mon | +--------------------------------------------------------------------+

This run of the CFX-5 Solver has finished.
  Reply With Quote

Old   November 18, 2004, 14:21
Default Re: Error message from moving mesh modelling
  #2
John
Guest
 
Posts: n/a
Does moving mesh modelling need additional licence?

  Reply With Quote

Old   November 18, 2004, 16:21
Default Re: Error message from moving mesh modelling
  #3
Glenn Horrocks
Guest
 
Posts: n/a
Hi John,

You need the MFR (multiple frames of reference) key to use moving mesh.

Glenn Horrocks
  Reply With Quote

Old   November 18, 2004, 18:43
Default Re: Error message from moving mesh modelling
  #4
John
Guest
 
Posts: n/a
Hi, Glenn

Thanks a lot for your quick reply.

I am trying to figure out if CFX can model a type of flocculator, in which paddles vertically move up and down to mix the water (similar as in: http://www.myersequipment.com/walking.html). Could you please give some advice on this? Is it easy to model this kind of problem using CFX moving mesh?

Thanks!

John

  Reply With Quote

Old   November 19, 2004, 07:14
Default Re: Error message from moving mesh modelling
  #5
Rui
Guest
 
Posts: n/a
Hi,

It's a bug related to moving mesh. It was introduced with the patch and only occur in Windows. In Pre, open the command editor, and enter:

FLOW:

EXPERT PARAMETERS:

min mode el = 750

END

END

then click Process

You may also do this editing the CCL file.

If you have access to the CFX Community web site, take a look at: http://www-waterloo.ansys.com/cfxcom...p?TOPIC_ID=629
  Reply With Quote

Old   November 19, 2004, 16:18
Default Re: Error message from moving mesh modelling
  #6
John
Guest
 
Posts: n/a
Thanks, Rui.

The solver can run now. However it terminate again at timestep 52. The error information is as follows. Any idea about that?

Also, does it means whenever I want to use moving mesh I need to add those commands to CCL? How do you value the CFX's moving mesh capability?

Have a good weekend!

John

ERROR #002100010 has occurred in subroutine cVolSec. | | Message: | | One of the sector volumes of an element is equal to or less than | | zero. It means that there exists an illegal mesh, execution will | | be stopped immediately. | | The element sequential number is: 1984 | | The element label is: 1984 | | The sector volume is: -0.1929E-16 | | The location (x,y,z): -0.22324E-02 0.17637E-02 0.50000E-04
  Reply With Quote

Old   November 22, 2004, 16:22
Default Re: Error message from moving mesh modelling
  #7
Rui
Guest
 
Posts: n/a
Hi,

The error message just means what it says: "one of the sector volumes of an element is equal or less than zero". From the manual, CFX-Post, CCL and CEL in CFX-Post, page 208: "a sector volume is the portion of volume of an element touching a node that can be associated with that node". During the mesh deformation, the movement of the nodes lead to elements distortion. It may happen that a sector volume becomes equal or less than zero.

I did tutorial 20 and didn't have this problem. Check that the mesh motion is set to unspecified on the ValveVertWalls and to stationary on the CheckValve Default. I would say this is the reason for the error.

Yes, everytime you create a .def file using moving mesh, you have to add that expert parameter. But it just takes a few second to do it. The problem is when you want to edit the Run in Progress in CFX-Solver (it dinīt work for transient simulations in CFX-5.6), the parameter is deleted from the .def file and the Solver stops. Thus, you cannot do it when using moving mesh. CFX-5.7.1 will be released very soon, I hope they get this bug fixed.

I've started playing with the moving mesh capability just about a week ago, so I still don't have a well established opinion about it. However, it's obvious you can do things now you couldn't do before.

Regards,

Rui
  Reply With Quote

Old   November 23, 2004, 16:39
Default Re: Error message from moving mesh modelling
  #8
John
Guest
 
Posts: n/a
Hi, Rui. I appreciate your comments.I can use the moving mesh feature now. Thanks.

  Reply With Quote

Old   November 29, 2004, 16:06
Default Re: Error message from moving mesh modelling
  #9
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Getting the moving mesh to follow the required motion shouldn't be too hard. However, don't underestimate the time and effort involved to get an accurate answer.

Glenn Horrocks
  Reply With Quote

Reply

Thread Tools
Display Modes

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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 04:11
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 03:52
VOF with a moving mesh Jeremie FLUENT 1 November 26, 2008 08:55
Moving Mesh Run problem - Scientific Linux G. SE CD-adapco 2 May 7, 2008 07:15


All times are GMT -4. The time now is 13:29.