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

Stopped in routine ENFORCE_BOUNDS

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 22, 2010, 10:36
Default Stopped in routine ENFORCE_BOUNDS
  #1
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 7
camoesas is on a distinguished road
Hello Everybody,

Briefly before Christmas I have a CFD Problem...
Maybe anybode can help me:

I am doing a transient simulation with cavitation. First I have made a transient simulation with cavitation turned off as initial guess. Now I have turned on cavitation and the solver explodes after a few Iterations. I get pressure values of about 300 bar, which causes my solver to abort.
See the Outfile Below:

Quote:
Slave: 3
Slave: 3 Fatal bounds error detected
Slave: 3 ---------------------------
Slave: 3 Variable: Fluid 1.Density
Slave: 3 Locale : Innen
Parallel run: Received message from slave
-----------------------------------------
Slave partition : 3
Slave routine : ErrAction
Master location : RCVBUF,MSGTAG=1022
Message label : 001100279
Message follows below - :

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine ENFORCE_BOUNDS |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+
End of solution stage.
+--------------------------------------------------------------------+
| The following transient and backup files written by the ANSYS CFX |
| solver have been saved in the directory |
| D:\kavitation_01_004: |
| |
| 1353_full.trn |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| D:\kavitation_01_004: |
| |
| mon |
+--------------------------------------------------------------------+

This run of the ANSYS CFX Solver has finished.
Some Iterations before I got this Strange Notice:

Quote:
Parallel run: Received message from slave
-----------------------------------------
Slave partition : 3
Slave routine : EX_TABLE
Master location : End of Continuity Loop
Message label : 009100008
Message follows below - :
+--------------------------------------------------------------------+
| ****** Notice ****** |
| While evaluating Fluid 1.Temperature, |
| Absolute Pressure |
| went outside of its upper limit. Its maximum value was |
| 3.5814E+07. The bounds error was handled by extrapolation. |
| If this situation persists, consider increasing the table range. |
+--------------------------------------------------------------------+

Some Details for my Case:

- reference pressure: 0 atm
- timestep: 5.5e-5 s
- inlet: total pressure
- outlet1: opening
- outlet2: pressure outlet


Any Hints appreciated! Thanks in advance

Simon

More Details required?
camoesas is offline   Reply With Quote

Old   December 22, 2010, 17:21
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,442
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Your simulation is not converging well. Need to improve the numerical stability - smaller timesteps, better mesh quality and check the physics.
ghorrocks is offline   Reply With Quote

Old   December 23, 2010, 06:11
Default
  #3
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 7
camoesas is on a distinguished road
HI Glenn,

I have double checked the mesh quality, it is quite well:
Minimum Angle > 27
Determinant > 0.5

I decrease the timestep to nanoseconds (which is a valuable size for cavitation problems) and see after christmas if it helped.

Here some details for my cavitation model:
- Rayleigh Plesset
- Mean Diameter: 2e-6m
- Saturation Pressure: 0.02 bar

Merry Christmas!
camoesas is offline   Reply With Quote

Old   December 23, 2010, 06:21
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,442
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Mesh quality requirements are different for different physics models. The rules of thumb for single phase flow are often not appropriate for multi phase flow. I would spend some time to get the mesh as good as you can in the area of cavitation as it will pay dividends with improved convergence, better accuracy and reduced run time.

I would use adaptive time stepping to let it find its own time step size.
ghorrocks is offline   Reply With Quote

Old   January 12, 2011, 02:57
Default
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 7
camoesas is on a distinguished road
Hello Everybody and a Happy new Year!

Ive got my case running, it was a false Expert Parameter Setting, I had:
solve volfrc = f

Setting this parameter to true, keeps the solver running. But Convergence is still bad.

Anyway now I am facing a real annoying problem:
My outfile clearly states to write Pressure to Transient file:

Code:
     TRANSIENT RESULTS: Transient Results 1
       File Compression Level = Default
       Include Mesh = No
       Option = Selected Variables
       Output Variables List = Fluid 1.Density,Fluid 1.MassTransfer,Fluid \
         1.Velocity u,Fluid 1.Velocity v,Fluid 1.Velocity w,Fluid 2.Volume \
         Fraction,MassTransfer,Pressure,Total Pressure
But in Post I cant read pressure data, all other variables are available!

Has anybody a solution for this stupid problem?!

Thanks
camoesas is offline   Reply With Quote

Old   January 12, 2011, 05:10
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,442
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Your expert parameter turns the solving of the volume fraction equation off. You are not going to get far when you are not solving the equations.

I have no idea why pressure is not in the output file.
ghorrocks is offline   Reply With Quote

Old   January 13, 2011, 06:43
Default
  #7
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 7
camoesas is on a distinguished road
There is pressure in the out files indeed.
But I have to choose Solver Pressure instead of Pressure. This comes with the cavitation model. Its explained in the User Help
camoesas is offline   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
Stopped in routine ENFORCE_BOUNDS Ram CFX 1 April 1, 2008 07:36
user subroutine error CFDUSER CFX 2 December 9, 2006 06:31
user defined function cfduser CFX 0 April 29, 2006 10:58
CFX 10 User Sub Routine Claudia CFX 6 February 15, 2006 08:32
FORTRAN Routine - variable passing Malcolm CFX 1 August 11, 2005 18:51


All times are GMT -4. The time now is 21:52.