CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Stopped in routine ENFORCE_BOUNDS (http://www.cfd-online.com/Forums/cfx/83294-stopped-routine-enforce_bounds.html)

camoesas December 22, 2010 11:36

Stopped in routine ENFORCE_BOUNDS
 
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?

ghorrocks December 22, 2010 18:21

Your simulation is not converging well. Need to improve the numerical stability - smaller timesteps, better mesh quality and check the physics.

camoesas December 23, 2010 07:11

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!

ghorrocks December 23, 2010 07:21

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.

camoesas January 12, 2011 03:57

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

ghorrocks January 12, 2011 06:10

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.

camoesas January 13, 2011 07:43

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


All times are GMT -4. The time now is 21:38.