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:

Some Iterations before I got this Strange Notice:


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?

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

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!

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.

Hello Everybody and a Happy new Year!

I´ve 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:

But in Post I cant read pressure data, all other variables are available!

Has anybody a solution for this stupid problem?!

Thanks

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.

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

I also encountered this problem. And what is the cause of this problem? I am so confused. I hope I can get your help. Thank you very much!

Could you post the message in the output file?

The <unknown> variable is out of bounds. the suggestion will depend on which variable is listed,

the error is as follows:
thank you!

Slave: 9
Slave: 9 Fatal bounds error detected
Slave: 9 ---------------------------
Slave: 9 Variable: Absolute Pressure
Slave: 9 Locale : S1

Parallel run: Received message from slave
-----------------------------------------
Slave partition : 9
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.

+--------------------------------------------------------------------+
| The following user files have been saved in the directory |
| D:/LUODAN/may/seal_pending/dp0_CFX12_Solution/CFX12_021: |
| |
| pids, mon |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| For CFX runs launched from Workbench, the final locations of |
| directories and files generated may differ from those shown. |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| Warning! |
| |
| After waiting for 60 seconds, 1 solver manager process(es) appear |
| not to have noticed that this run has ended. You may get errors |
| removing some files if they are still open in the solver manager. |
+--------------------------------------------------------------------+

You have a bounds error on the Absolute Pressure. The highest pressure CFX can handle is very high, 1E10Pa I suspect, but the absolute pressure cannot be zero or negative in compressible simulations. So something is causing the absolute pressure to exceed these limits.

Most of the time this is caused by numerical instability and the simulation is diverging. In this case this FAQ is relevant: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

In a small number of highly specialised cases the negative absolute pressure is real. These cases cannot be modelled by CFX. But they really only occur in extreme MEMS modelling cases so most people don't come across this (fortunately).

May multi-core parallel computing cause this Problem? Because the same case i simulated before did not arise such problems.Thank you!

It is unusual for multiprocessor to cause this type of error, but not impossible. It still suggests numerical instability, so the FAQ is applicable for that.

In order to really help you, we need to know what problem your are solving and what settings you used. Please share in text format.

I simulated the carbon dioxide two-phase flow in the seal. The settings are listed in the following text. Thank you！

You are using a complex and custom material model. They often cause strange errors and are often very hard to converge.

I see you have set a very small timescale factor, which suggests you have already tried lowering the time step to get convergence.

This simulation is too complex to debug on the forum. All I can recommend is the general procedure for getting complex material models to converge:
1) Do a run using simple, built-in material models, maybe single phase ideal gas. Make sure this runs well and stably before proceeding.
2) Then add the complex components one at a time. In your case maybe do a single phase model using your RGP model.
3) Then do a model using multiphase, but simple fluid properties (maybe ideal gas)
4) If all your complex models work OK by themselves then try combining them. Be prepared for all sorts of new and unexpected error messages :)

Looks like you are trying to solve a degassing process, with nucleation, while assuming equilibrium conditions. At least I don't see any user defined source terms.

Neverthelss this is a very difficult problem. I fully agree with Glenn. Start as simple as possible and step by step increase complexity by adding physics.

Yes, I have tried to simulate my case with single-phase RGP and it had a good convergence. I continued to simulate two-phase co2 flow and took the above results as initial conditions. But it is so hard to converge yet at a very small time step. Is this reasonable?

If the simulation is unstable then a very small time step will be required. If the simulation is not correctly set up then it will diverge no matter what time step you use.

You are doing a very complex simulation and you should expect it to be difficult to work working. It is also too complex to debug over the forum as it would take an expert many hours to do I suspect, and nobody has that sort of time to give to the forum. You are going to have to work this one out yourself I suspect.

Very helpful answers
 

This is all you ever hear on this forum, unfortunately.