
[Sponsors] 
September 18, 2015, 18:35 
Real gas NIST model problem

#1 
New Member
Join Date: Jun 2014
Posts: 13
Rep Power: 10 
Hello,
I am trying to run a simulation with real gas model from NIST using r134a as working fluid. When I try to initialisate or run the simulation I get the next message: Primitive Error at Node 0: REFPROP_error (203) from function: tprho (density) [TPRHO error 203] vapor iteration has not converged for T= 257.82 K, p =0.55582 MPA, rho (last guess) =0.39299 mol/L, x (mol frac) = 1.0000 I do not know how to make the Refprop function to converge. Anybody could give some advice about how to deal with it? Best regards. 

September 18, 2015, 19:20 

#2 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,015
Rep Power: 60 
Are you running a single phase or multiphase simulation? This can happen when you end up in a different phase (i.e. you should be in the supercritical phase or pure gas phase but somehow end up in the liquid phase).
If this is happening during initialization then check to make sure your initial conditions are consistent with the expected phase. If necessary, manually patch the pressure and temperature in affected zones/regions. 

September 20, 2015, 08:16 

#3 
New Member
Join Date: Jun 2014
Posts: 13
Rep Power: 10 
Hello,
I am running a single phase simulation. I am sure that the boundary conditions that I am setting are in single phase zone. The problem that I am trying to run is a singlephase ejector and the boundary conditions are two pressure inlets and one pressure outlet, the rest are wall and symmetry. The values of pressure and temperature in the error message do not seem to be in the single phase region but I do not know why it is trying to calculate this values since my boundary conditions are in singlephase. Thank you for any further help. 

September 20, 2015, 10:07 

#4 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,015
Rep Power: 60 
Check your initial conditions.


September 20, 2015, 11:05 

#5 
New Member
Join Date: Jun 2014
Posts: 13
Rep Power: 10 
Do you mean boundary conditions? or initial conditions? I have not set any initial conditions because I am running a steady simulation. And the boundary conditions I am pretty sure that are all of them in gas phase.
In the next link you can download my mesh and my script file if you want to have a look. https://www.dropbox.com/s/vivx4rkpjc...luent.zip?dl=0 Regards. 

October 26, 2016, 01:33 

#6 
New Member
Senthilkumar
Join Date: Oct 2012
Posts: 29
Rep Power: 11 
If anybody have solution to this problem, it will be helpful.
I am simulating a supersonic flow of supercritical CO2 through convergent divergent nozzle. Inlet condition Inlet : Pressure Inlet ;P0 = 95.7 bar T0 = 315K Real gas model : NIST 

February 27, 2017, 05:18 

#7 
New Member
Lucia
Join Date: Feb 2017
Posts: 1
Rep Power: 0 
Hello,
How did you solve this issue? I have a similar problem with a supersonic flow with R134a. Best regards, 

June 5, 2017, 02:50 

#8 
New Member
Senthilkumar
Join Date: Oct 2012
Posts: 29
Rep Power: 11 

September 27, 2017, 12:19 

#9 
New Member
Jeff Yam
Join Date: Sep 2017
Posts: 11
Rep Power: 7 
may i understand how cfx is works better than fluent in this case?


May 4, 2018, 15:23 

#10 
New Member
abas
Join Date: May 2014
Posts: 6
Rep Power: 10 
Hello,
I simulate CO2 as a real gas but I received the following error: vapor iteration has not converged Could anyone help me? 

May 4, 2018, 17:39 
sdddddds

#11  
New Member
abas
Join Date: May 2014
Posts: 6
Rep Power: 10 
Quote:
If you have found a way to overcome this problem, please let me know 

June 11, 2018, 22:54 

#12 
New Member
Join Date: May 2018
Posts: 3
Rep Power: 6 
I am simulating aflow of supercritical CO2 through dry gas seal.but there are some errors .can you help me


June 14, 2018, 13:13 

#13 
New Member
Senthilkumar
Join Date: Oct 2012
Posts: 29
Rep Power: 11 
I could not overcome this problem due to two reasons:
1. Pressure and temperature decreases due to the expansion of the fluid in the nozzle and conditions moves close to the critical point (saturation dome). Near critical point, the NIST does not converge and gives TPFlash Error!. 2. During initial iterations, the pressure and temperature may fall into the liquid or vapor state. An abrupt change in properties causes the solution to not to converge. A possible solution may be create a lookup table with continuous properties change as in "Pham, H. S., Alpy, N., Ferrasse, J. H., Boutin, O., Tothill, M., Quenaut, J., … Saez, M. (2016). An approach for establishing the performance maps of the scCO2compressor: Development and qualification by means of CFD simulations. International Journal of Heat and Fluid Flow, 61, 379–394. https://doi.org/10.1016/j.ijheatfluidflow.2016.05.017" P.S: Check your final solution for any cells in the domain does not have fluid at a state where you modified properties value (Read Pham et al.) 

June 14, 2018, 13:14 

#14 
New Member
Senthilkumar
Join Date: Oct 2012
Posts: 29
Rep Power: 11 

June 14, 2018, 13:20 

#15 
New Member
Senthilkumar
Join Date: Oct 2012
Posts: 29
Rep Power: 11 
CFX permit to use lookup table, so we can get a solution with coarse PT interval RGP table. Then slowly refine the RGP table.
Fluent does not allow to use external RGP table. Fluent allows only the RGP table generated by its inbuilt generator, even you cannot see the that RGP table generated by Fluent. We do not modify this RGP table in fluent for continues property change across saturation line. 

June 14, 2018, 21:05 

#16  
New Member
Join Date: May 2018
Posts: 3
Rep Power: 6 
Quote:
inlet 9MPa outlet 0.1mpa the fluid is co2 error is"invaild cp (5.214435J/Kgk) for real gas co2 vapor iteration has not converged for 0.1e09K p=0.101325 

June 19, 2018, 23:06 

#17 
New Member
Join Date: May 2018
Posts: 3
Rep Power: 6 
I am simulating the dry gas seal end face gas film, the gas is carbon dioxide, the inlet pressure is 9mpa, and the outlet pressure is atmospheric pressure.but some errors display .whatever i change the boundary conditions .
Error: REFPROP_error (203) from function: tprho (density) [TPRHO error 203] vapor iteration has not converged for T = 0.10000E09 K, P = 0.10132 MPa, rho (last guess) = 0.64165 mol/L, x (mol frac) = 1.00000 Error: REFPROP_error (203) from function: tprho (density) [TPRHO error 203] vapor iteration has not converged for T = 0.10000E09 K, P = 0.10132 MPa, rho (last guess) = 0.64165 mol/L, x (mol frac) = 1.00000 Error Object: #f 

June 21, 2018, 15:05 

#18 
New Member
Senthilkumar
Join Date: Oct 2012
Posts: 29
Rep Power: 11 
Reason for your problem:
Since your inlet pressure is 9MPa (close to critical pressure), there may be some region in your domain where Pressure may fall below the critical pressure due to overshoot/undershoot during initial iterations. Near critical point, SW EOS has the problem of convergence. Try this strategy 1. Use pressure coupling scheme 2. Set the lower limit of Pressure and Temperature to 75bar and 305K (it will throw warning stating that cells have limit pressure/temperature. Ignore it) 2. Turn of turbulence equations and energy equation 3. After getting some decent convergence trend, turn on turbulence equations 4. After getting very good convergence turn on energy equations (now no. of cells with lower P/T will decrease) P.S: This strategy is clearly explained by B. Monje "Design of supercritical carbon dioxide centrifugal compressors", 2014, Ph.D., Thesis 

November 26, 2020, 05:41 
fluent error

#19 
New Member
adithya ganapathiraju
Join Date: Jun 2020
Posts: 3
Rep Power: 4 
Hello,
I am running a transcritical methane flow where my fluid will reach supercritical condition. Now when the simulation is running i am getting warning regarding invalid cp. Can anyone help me to find the issue that i am facing. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Continuing User Defined Real Gas Model issues  aeroman  FLUENT  6  April 8, 2016 03:34 
Parallel User Defined Real Gas Model  aeroman  FLUENT  4  July 1, 2015 06:09 
How to model Liquid to Gas mass transfer (Stefan Problem) in Fluent?  hasib61  Fluent Multiphase  0  December 24, 2014 17:24 
how to hook this udf  shanu  FLUENT  1  August 26, 2011 10:48 
Redlich Kwong real gas model for species mixture Helium and Argon  anandabbai  FLUENT  0  May 29, 2009 02:04 