[jexposito]

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.

[LuckyTran]

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.

[jexposito]

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 single-phase 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 single-phase.

Thank you for any further help.

[LuckyTran]

Check your initial conditions.

[jexposito]

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.

[aero.senthilkumar]

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

[luropas]

Hello,

How did you solve this issue?

I have a similar problem with a supersonic flow with R134a.

Best regards,

[aero.senthilkumar]

Use CFX, it is a good option.

Originally Posted by luropas

Hello,

How did you solve this issue?

I have a similar problem with a supersonic flow with R134a.

Best regards,

[NozzleNoobie]

may i understand how cfx is works better than fluent in this case?

[aghagoli]

Hello,
I simulate CO2 as a real gas but I received the following error:
vapor iteration has not converged

Could anyone help me?

[aghagoli]

Originally Posted by aero.senthilkumar

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

could you solve the problem?
If you have found a way to overcome this problem, please let me know

[Xinlei Zhu]

Originally Posted by aero.senthilkumar

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

I am simulating aflow of supercritical CO2 through dry gas seal.but there are some errors .can you help me

[aero.senthilkumar]

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 look-up 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 sc-CO2compressor: 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.)

Originally Posted by aghagoli

could you solve the problem?
If you have found a way to overcome this problem, please let me know

[aero.senthilkumar]

Please explain your error.
If your getting same error as "aghagoli", follow my earlier thread.

Originally Posted by Xinlei Zhu

I am simulating aflow of supercritical CO2 through dry gas seal.but there are some errors .can you help me

[aero.senthilkumar]

CFX permit to use look-up 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.

Originally Posted by NozzleNoobie

may i understand how cfx is works better than fluent in this case?

[Xinlei Zhu]

Originally Posted by aero.senthilkumar

Please explain your error.
If your getting same error as "aghagoli", follow my earlier thread.

my model is dry gas seal
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 0.1e-09K p=0.101325

[Xinlei Zhu]

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 = 0.10000E-09 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 = 0.10000E-09 K, P = 0.10132 MPa, rho (last guess) = 0.64165 mol/L, x (mol frac) = 1.00000

Error Object: #f

[aero.senthilkumar]

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

[adithyaG]

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.