[ForgotMyUsername]

Hi All,

I'm doing a baby's first CFX coursework and I'm trying to run a simple aerofoil in an Air Ideal Gas simulation at 10,000 feet in supersonic flow. I've plugged in the correct pressure and temperature values, and initialised the domain before setting the inlet and outlets. Problem is, whenever I try to run the solver, it kicks out this error at outer loop 41;

Slave: 4
Slave: 4 Fatal bounds error detected
Slave: 4 ---------------------------
Slave: 4 Variable: Absolute Pressure
Slave: 4 Locale : Default Domain

Parallel run: Received message from slave
-----------------------------------------
Slave partition : 4
Slave routine : ErrAction
Master location : Message Handler
Message label : 001100279
Message follows below - :

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine ENFORCE_BOUNDS |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine MESG_RETRIEVE. |
| Message: |
| Stopping the run due to error(s) reported above |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| 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.


I've tried everything I can think of to solve it, but so far nothing's worked. Do any of you fine folks know what I might be doing wrong?

If you need, here's the full solver run file

[ghorrocks]

This message the absolute pressure has infringed a bounds error - almost certainly because it predicted a negative absolute pressure. In 99% of cases this is caused by poor numerical stability leading to wild swings in variable values, and probably divergence (but this error killed the run before it diverged).

You need to:
* improve mesh quality
* better initial conditions
* smaller time steps
* use the double precision solver
* Check the solver setup (you have a major problem here, read below)

In addition, this is a supersonic simulation so will be difficult to converge anyway. Make sure you read the CFX documentation on supersonic simulations and boundary conditions.

Also, looking at our output file:
* You have 6302 nodes in your mesh. This is very coarse and it is unlikely any thing useful would come from a mesh that coarse. In addition, meshes that coarse can cause convergence difficulties.
* Your mesh quality does not look good - minimum angle of 2.7 degrees and expansion factor of 93 is very poor. Supersonic simulations need very high mesh quality, especially near the shock(s).
* You have not set a pressure anywhere! As discussed in the output file the solver has just assumed the pressure at a point to be zero. This means it is not far from absolute zero to begin with. This appears to be a major error which must be corrected. You have to define the pressure somewhere.

[ForgotMyUsername]

Thanks GHorrocks, that worked fine!