CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   high speed flow, phase change problem (http://www.cfd-online.com/Forums/cfx/126496-high-speed-flow-phase-change-problem.html)

PYJG November 19, 2013 07:57

high speed flow, phase change problem
 
I am solving a problem in which the inlet is a high speed cryofluid in vapor state and there is a possibility of phase change. Please help
OUTER LOOP ITERATION = 8000 ( 720) CPU SECONDS = 9.357E+05 (1.895E+05)
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+
| U-Mom-Bulk | 0.96 | 2.9E-04 | 4.7E-02 | 1.1E-02 OK|
| V-Mom-Bulk | 0.83 | 1.6E-04 | 1.8E-02 | 4.5E-02 OK|
| W-Mom-Bulk | 0.85 | 4.7E-06 | 7.8E-04 | 4.2E-02 OK|
| P-Vol | 1.00 | 2.2E-05 | 2.4E-03 | 6.2 5.3E-02 OK|
+----------------------+------+---------+---------+------------------+
| Mass-Vapor | 1.00 | 9.4E-11 | 1.2E-08 | 5.9 6.4E-07 OK|
+----------------------+------+---------+---------+------------------+
| H-Energy-Vapor | 0.98 | 1.4E-03 | 1.2E-01 | 1.0E-03 OK|
| H-Energy-Liquid | 1.01 | 6.5E-05 | 7.5E-03 | 1.4E-07 OK|
| T-Energy | 0.90 | 1.3E-05 | 1.2E-03 | 7.1 1.0E-03 OK|
+----------------------+------+---------+---------+------------------+
| K-TurbKE-Bulk | 1.01 | 1.3E-04 | 1.7E-02 | 6.8 9.9E-04 OK|
| O-TurbFreq-Bulk | 0.75 | 2.5E-04 | 9.2E-02 | 7.4 2.1E-04 OK|
+----------------------+------+---------+---------+------------------+

+--------------------------------------------------------------------+
| Writing backup file 8000_full.bak |
| Name : Backup Results 1 |
| Type : Standard |
| Option : Iteration Interval |
+--------------------------------------------------------------------+
Slave: 3
Slave: 3 Fatal bounds error detected
Slave: 3 ---------------------------
Slave: 3 Variable: Vapor.Density
Slave: 3 Locale : Domain Interface 1 Side 2 1

Parallel run: Received message from slave
-----------------------------------------
Slave partition : 3
Slave routine : ErrAction
Master location : RCVBUF,MSGTAG=1082
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.

ghorrocks November 19, 2013 17:54

Assuming your physics is correctly set up then this problem is similar to the linear solver failure error. This FAQ tells you the key things to look at: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

PYJG November 20, 2013 14:40

Yes, I refined the mesh, tried running the model with double precision, viscous dissipation, reducing time steps, the model does not work. The model when setup to run thermal energy equation works just fine.

ghorrocks November 20, 2013 16:13

You are modelling high speed compressible flow with phase change. You have to expect convergence difficulties with a tough model like that. If you are not familiar with how to get convergence with tricky simulations then I suggest you simplify it and practise on more straight forward simulations - like try to model compressible ideal gas flow with some shock waves. You will learn a lot about obtaining convergence when you get those sort of simulations to converge.

PYJG November 21, 2013 10:58

Thanks Glenn. I appreciate your help. I am running a cases as per your suggestion.

PYJG November 21, 2013 12:42

Update-
(a)ideal gas compressible cases has not issues converging, I changed the material properties from ideal gas to real gas and then it started giving the same density error. Mach number calculated is high(~3.5) in the second iteration.

(b)I am using Argon, there is Souve Redlich Kwong, peng robinson, and redlich kwong model how to ensure which of them would be the correct one for real gas properties. I have been using ArRK model.

(c)Will increasing residual target from 1e-6 to 1e-4 help? Thanks for your suggestions, they have been very valuable

ghorrocks November 21, 2013 16:48

So it sounds like you have a problem with introducing real gas properties. This is very common, it is difficult to get these to converge at the best of times.

Loosening the convergence tolerance is OK for development, but once it is working you need to do a convergence sensitivity check to ensure you are tight enough for accuracy.

PYJG November 21, 2013 17:18

Yes, I used 10-4, 10-5 and 10-6 same issue persists. Any suggestions on getting convergence when using real gas properties?

ghorrocks November 22, 2013 04:43

Let me quote post #2:

Quote:

Assuming your physics is correctly set up then this problem is similar to the linear solver failure error. This FAQ tells you the key things to look at: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F
Your post after it says you tried some of the things discussed, but not all. Improving mesh quality, a better initial condition and several others are important to do as well.

PYJG November 26, 2013 15:58

Thank you for your kind help Glenn. It is very very valuable. Yes a better mesh did the job. Also, with real gas I cannot get completely converged properties, but I can monitor some important variables and see if they have reached equillibrium and the model shows that.

The problem so far has adiabatic boundary condition. Next step is to look at heat flux boundary condition. As soon as I apply a heat flux on the model that uses total energy and real gas properties the model fails with errors. So I decided to follow the earlier route of getting a converged solution with ideal gas properties+total energy model and using that as a starting solution for the real gas model. In doing that, if I monitor the temperature on the wall where I apply heat flux, the temperature does not rise very much even after I keep increasing the heat flux applied. Any suggestions? ( Mesh along wall has good inflation)

ghorrocks November 26, 2013 16:51

As your material properties get more complex then convergence gets harder. So that makes a high quality mesh, double precision, good initial conditions and those factors even more important.

I bet if you simplified your geometry down so you could apply a high quality hex mesh on it that you would have no problems with convergence at all. So the challenge is to generate a mesh of adequate quality on the real geometry.

PYJG November 26, 2013 17:11

My geometry is 2D( one element in thickness direction) axisymmetric 2 degree wedge. The mesh is refined to over 3.5million nodes for approximate rectangluar dimensions of 25mmx0.65mm. Inflation on walls. Y+ for adiabatic case was less than 5.Any suggestions on getting the heat transfer case to work?
The temperature on the wall where I am applying heat flux is not increasing

ghorrocks November 27, 2013 04:32

If you have tight restrictions on mesh quality it is going to be tough to do a 2D axisymmetric simulation. It means mesh the elements along the axis are wedges with a 2 angle and that is a terrible mesh quality.

I would try a larger wedge angle if possible. But even better, if you want to do serious 2D simulations I would change to another solver which supports proper 2D simulations (eg Fluent).

PYJG November 30, 2013 08:59

Thank you for your help it is very valuable. The same problem exists even if the geometry is rotated 360 degrees and mesh refined, inflation along wall . I used the high speed compressible wall heat transfer model and following notice/error appears. I don't see the term in expert parameter. Please help.
****** Notice ****** |
| The non-dimensional near wall temperature (T+) has been clipped |
| for calculation of Wall Heat Transfer Coefficient. |
| |
| Boundary Condition : front wall |
| T+ clip value = 1.0000E-10 |
| |
| If this situation persists and you are using the High Speed Model, |
| consider enabling Mach number based blending between low speed and |
| high speed wall functions. You can do so by specifying a Mach |
| number threshold as follows: |
| |
| EXPERT PARAMETERS: |
| highspeed wf mach threshold = 0.1 # default=0.0 (off) |
| END |

Slave: 3
Slave: 3 Fatal bounds error detected
Slave: 3 ---------------------------
Slave: 3 Variable: Density
Slave: 3 Locale : Default Domain

Parallel run: Received message from slave
-----------------------------------------
Slave partition : 3
Slave routine : ErrAction
Master location : BRCBUF,MSGTAG=1062
Message label : 001100279
Message follows below - :

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

PYJG November 30, 2013 11:32

Expert Parameter does not have this option to select, however, using command prompt type the following and click process.
FLOW: Flow Analysis 1
EXPERT PARAMETERS:
highspeed wf mach threshold = 0.1
END
END

I still get the same density error.

ghorrocks December 1, 2013 04:29

The root cause of this problem is much more likely to be a physical or numerical instability which is leading to temperatures less than absolute zero. This is quite common as you develop simulations using the real gas meterial property models.

This all points to the same thing I have been posting about all along - you need better mesh quality, a better initial condition, smaller timesteps, etc.


All times are GMT -4. The time now is 03:05.