CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   The ANSYS CFX solver exited with return code 1 (http://www.cfd-online.com/Forums/cfx/90063-ansys-cfx-solver-exited-return-code-1-a.html)

kola77 June 29, 2011 16:22

The ANSYS CFX solver exited with return code 1
 
Hello everybody,
I am trying to conduct a simulation of a simple shell-tube heat exchanger, but as soon as I start the run the solver crashes with an error with the following explanation:

Quote:

If the isolated regions do not have the pressure level set either by the boundary conditions or using a reference pressure equation, you may encounter severe robustness problems.

This situation may have arisen because a domain interface was not properly defined during problem setup. Please carefully check the setup.

The solver will stop now and write a results file. The isolated regions can be visualised in CFX Post by making plots of the variable "Isolated Volumes".

If you are sure that the pressure level is set in each isolated fluid region then you can force the solver to turn off this check by setting the expert parameter "check isolated regions = f".

+--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | The ANSYS CFX solver exited with return code 1. | +--------------------------------------------------------------------+

End of solution stage.

I know this usually has something to do with problems of the geometry/mesh, but I couldn't find any noticeable glitches in mine. There were also no unconnected regions, the the interfaces seem to be correct. Nevertheless, what I have tried is the following:
  • I have carefully and several times reviewed my setup
  • I have redesigned my model from scratch
  • I have refined the mesh
  • I have tried to simulate a single pipe inside of a shell
All of the above ended with the same error, yet when I start an old file of another heat exchanger I have simulated a while ago it works fine. I have carefully examined my setup of that one and I can't fine any differences in the setup. If anybody has ANY idea what might be causing this I would be the happiest man on earth, since I am slowly getting desperate.

Is it possible that my installation of ANSYS is damaged in some way?

Thank you in advance for any potential help!

ghorrocks June 29, 2011 18:07

The error message tells you exactly what the problem is. If you have two or more fluid regions which are not connected then you need to set a pressure value in each of them. So the easiest way is to make sure each fluid region has a pressure inlet or outlet.

kola77 July 1, 2011 11:51

That's the problem. There are no regions which wouldn't have a boundary condition set. All of them are set to inlet/outlet, wall or interface. The reference pressure is set in each of them. I have tried several configurations, but still the solver keeps crashing.

Would you please be kind enough and take a couple of minutes to check my setup? I'm sure it's some newbie mistake that can be easily recognized. If so, it's here: http://www.megaupload.com/?d=N33WZTOW

Sanyo July 2, 2011 02:58

Check duplicate faces
 
Hi,

As Glenn said, its definitely problem of isolated fluid regions. Its because of unconnected regions. Sometimes duplicate/multiple faces remain unattended. Hence one or more fluid regions remain unconnected/ isolated. Please check the faces joining the regions. If faces are not connected, you could see the nonconformal mesh or multiple faces at same location.

You may also carry out one solution with the expert parameter "check isolated regions = f". This would enable you to understand the problem region.

Hope this helps.

Regards,

-Sanyo

ghorrocks July 2, 2011 06:58

Quote:

All of them are set to inlet/outlet, wall or interface.
That is not what I said. A velocity inlet and a mass flow outlet has not defined the pressure. One of the inlet and outlets in each region needs to be a pressure boundary to set the pressure.

kola77 July 2, 2011 09:11

All of the outlets had a pressure defined.

Anyway, I have managed to get it running, after changing the geometry a bit so i only had one outlet/inlet that splits into 13 later and not several regions defined as either one of them. After doing this it worked without a problem. Thank you for your help guys, much appreciated! Cheers!

mohw2002 January 1, 2013 16:48

HI FOR EVERY ONE
PLEASE I WORK ON MY GEOMETRY PIPE WITH ONE PERFORATION AND I MESH IT BY HEXA NOT TETRA BECAUSE I WANT TO CALCULATE WALL SHEAR STRESS BECAUSE HEXA GIVE US SMOOTH LINE WHEN WE ARE DRAWING THE BEHAVIOR OF WALL SHEAR AND PRESSURE DROP. WHEN I SENT THE MESH TO CFX IT CANNOT DID THE RESOLVING BECAUSE THE ERROR IS COMING AS BELOW HOW CAN I TREAT THIS PROBLEM. THE SIDE PLANE I PUT IT AFTER ONCE THE ERROR APPEAR. tHE SIDE PLANE IT IS VERTICAL AXIS FOR THE SIDE OF THE PIPE BECAUSE I DRAW HALF PIPE.


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 6 in the |
| symmetry boundary patch |
| |
| SIDE PLANE |
| |
| 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.

Sanyo January 2, 2013 08:44

Dear mohw2002,

It is a problem with symmetry boundary condition. Instead using symmetry, try using wall type BC with free slip.

Regards,

-Sanyo

mohw2002 January 2, 2013 17:11

Quote:

Originally Posted by Sanyo (Post 399735)
Dear mohw2002,

It is a problem with symmetry boundary condition. Instead using symmetry, try using wall type BC with free slip.

Regards,

-Sanyo

thanks for reply
I solved this problem because I made a mistake at ICEM CFD, I chose axis after did the mesh I was trying to solve it but without any success. I returned to ICEM CFD and delete the mesh and rearrange the parts.
Thanks
I have a diffucelet when I mesh by hexa do you have simple procedure or good tutorials?

Regards

susilo March 7, 2014 02:30

Error cfx solver
 
If the isolated regions do not have the pressure level set either by the boundary conditions or using a reference pressure equation, you may encounter severe robustness problems.

This situation may have arisen because a domain interface was not properly defined during problem setup. Please carefully check the setup.

The solver will stop now and write a results file. The isolated regions can be visualised in CFX Post by making plots of the variable "Isolated Volumes".

If you are sure that the pressure level is set in each isolated fluid region then you can force the solver to turn off this check by setting the expert parameter "check isolated regions = f".

+--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | The ANSYS CFX solver exited with return code 1. | +--------------------------------------------------------------------+

End of solution stage.

shelkeprithvi September 10, 2014 01:11

exited with return code 1
 
3 Attachment(s)
I am also having same problem with my geometry. In pre-CFX when I am giving symmetry as boundary condition at the mid section of the pipe those red arrows are surrounding only three sides of the green rectangle shown in the pictures attached. Can anyone tell me why I am getting this type of error.

ghorrocks September 10, 2014 06:08

You mean you are getting the isolated regions/pressure level is not set error? Isn't it obvious? Then you need to set a pressure level.

Sanyo September 10, 2014 09:20

Be Specific. . . Please!
 
Prithvi,

Be specific please. It is not clear whether you have an issue of arrows showing in 3 directions only or your solver exited with returned code 1.

If you are asking of arrows, it might be just a representation & actually solver has considered symmetry correctly. Have your solve crashed? If yes try to check physics setup. Give more details. :confused:

Regards,

Sanyo


All times are GMT -4. The time now is 11:25.