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.

Does moving mesh modelling need additional licence?

Hi John,

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

Glenn Horrocks

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

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

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

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 din´t 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

Hi, Rui. I appreciate your comments.I can use the moving mesh feature now. Thanks.

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