# RGP table for supercritical, gas and liquid phase

• 401 Views
• Last Post 20 February 2019
• Topic Is Solved
abbas posted this 14 February 2019

Hello everybody,

I am working on the pipe that high pressure and temperature CO2 (P=9Mpa and T=310K) enters into the pipe and with pressure (P=5Mpa) exits.

My question is: I create a Homogenous binary mixture. In my domain, at the inlet, I have supercritical CO2 (neither liquid nor vapor). So, for the inlet, I have to specify mass fraction at the inlet. What would be the mass fraction?

I checked my model.  I tried with pressure and temperature below supercritical, P=6Mpa and T=290K and quality of CO2=0.5. The simulation converged. So I think the problem should be related to the supercritical parameters.

Any suggestion about setting supercritical parameters in the inlet and two-phase at the outlet?

Best regards

Abbas

Order By: Standard | Newest | Votes
abenhadj posted this 14 February 2019

Have you tried with one? The interpolation should take care whether pressure above or below pcrit.

Best regards,

Amine

abbas posted this 14 February 2019

Hello Amine,

What do mean with one? Do you mean that one of the inlet valve (either pressure or temperature )above the critical and another below the critical point?

Thanks

abenhadj posted this 15 February 2019

I meant mass fraction equal to one at inlet.

Best regards,

Amine

abbas posted this 15 February 2019

Yes, I put 1 for a mass fraction as you can see in the picture but I got the error.

abenhadj posted this 16 February 2019

Which error?

Best regards,

Amine

abbas posted this 17 February 2019

Hello Amine,

The error was outflow.

However, I just tested a simple pipe that inlet pressure is 8Mpa and inlet temperature is 305K and the outlet pressure is 7Mpa and wall temperature is 290K. I want to see that CFX is able to solve this problem or not. Now, my RGP table boundary for pressure is 0.5Mpa to 50Mpa and temperature is 250K to 550K but it says that  "Table bounds warnings at: END OF TIME STEP". How is it possible?

Best regards

Abbas

abenhadj posted this 17 February 2019

This might be possible whenever within the AMG iterative solver the dependent variable to calculate he properties are out of bounds. This might disapper at the flow evolves but might indicate wrong settings, time scale size or even small table.

Best regards,

Amine

abenhadj posted this 17 February 2019

And Outflow, as error is manifold, might have several roots.

Best regards,

Amine

abbas posted this 18 February 2019

The problem cannot be the size of the table because the lower and upper table size for pressure and temperature are 0.5Mpa to 50Mpa and temperature is 250K to 550K and the simulation domain is a simple pipe that has one inlet and one outlet that inlet pressure is 8Mpa and inlet temperature is 305K.

abenhadj posted this 18 February 2019

So what do you think the issue is related to? As I said a super-critical Fluid is treated as being vapor.

Best regards,

Amine

abbas posted this 18 February 2019

The only warning that I am receiving is "Table bounds warnings" but I am pretty sure that all domain properties are inside the table.

Best regards,

Abbas

abenhadj posted this 18 February 2019

I am sorry but cannot debug further here if you are not providing any other info. Even if you think your pressure and temperature field are within the range of the table by iterating and interpolating from IP to Nodes and doing bi-linear and tri-linear operations somethings the variable are out of bounds. The whole issue might be related to something else which I cannot figure it out without any other further statements: material, boundaries, models... You can attach the definition file here perhaps some other forum members (NON-ANSYS-STUFF) can have a look into it.

Best regards,

Amine

abbas posted this 18 February 2019

Thanks for your help.

I am wondering how is it possible (# case 1) for the initial condition below the critical point, simulation for simple pipe is working but for (# case 2) initial condition upper critical point I got the overflow error (when I choose homogenous binary mixture for both cases). Also, when I choose initial condition upper critical point and choose just one material (vapor CO2) the simulation is working.

Best regards

Abbas

abenhadj posted this 18 February 2019

Please add information about the boundaries used as well as the material. I will then check on my side.

Best regards,

Amine

abbas posted this 18 February 2019

Thanks for your help. These are my domain and initial condition.

The material is as CO2 liquid and CO2 vapor which I generated them with ANSYS AFD.

abenhadj posted this 19 February 2019

Hi it is working for my simple pipe case with 0.5 MPa @ Inlet / 350 K, Operating Pressure 7 MPa.

@310K total temperature: one can notice that the run is not stable as the static temperature might be below the dome and the calculation is not so "easy" anymore. That is the region where the liquid become supercritical. But again it runs (simple test).

Best regards,

Amine

abbas posted this 19 February 2019

Thanks Amine,

Could you give me some screen shot from your simulation such as default domain and inlet and outlet setting and also number of mesh and length and width of the tube.

Best regards Abbas

abenhadj posted this 19 February 2019

Best regards,

Amine

abbas posted this 19 February 2019

Hello Amine,

Thanks for your help. I looked into your model, we both do the same procedure but I got the Floating point exception: Overflow. I think the problem should be meshing. But, I generate mesh in ICEM that quality of mesh is between 0.75 to 1 and Orthogonal Quality higher than 0.78. Here I attached the mesh of the pipe.

best regards

Abbas

abenhadj posted this 19 February 2019

Do you get overflow even if you set higher Total Temperature @Inlet?

Best regards,

Amine

abbas posted this 19 February 2019

Thanks for your quick reply. Yes. I set 7.5MPa for reference pressure. I set 340K and 0.5MPa for inlet and 0 for outlet. However, I get overflow error.

Best regards Abbas

abbas posted this 19 February 2019

That might not be logical. Can I use your mesh that you generate to see that I am going to the right way?

Best regards Abbas

abenhadj posted this 19 February 2019

Can you just use a coarser mesh to check if it is really mesh dependent?  Set solver settings to default.

Best regards,

Amine

abbas posted this 19 February 2019

I use coarser mesh however the result was the same (Floating point exception: Overflow.)

Is there any possibility that I use your mesh to see what is the problem?

Best regards,

Abbas

abenhadj posted this 19 February 2019

Lets check first: You can copy your CCL of all settings (Export>CCL select everything) here so that it can be checked.

Best regards,

Amine

abbas posted this 19 February 2019

Thanks for your help.

# State file created:  2019/02/19 156:28

# Build 19.3 2018-11-16T2336.098000

LIBRARY:

MATERIAL: CO2

Binary Material1 = CO2L

Binary Material2 = CO2V

Material Group = User

Option = Homogeneous Binary Mixture

SATURATION PROPERTIES:

Component Name = CO2V

Option = Table

Table Format = TASCflow RGP

Table Name = Dcfx/CO2-high.rgp

END

END

MATERIAL: CO2L

Material Group = User

Option = Pure Substance

Thermodynamic State = Liquid

PROPERTIES:

Component Name = CO2L

Option = Table

Table Format = TASCflow RGP

Table Name = Dcfx/CO2-high.rgp

END

END

MATERIAL: CO2V

Material Group = User

Option = Pure Substance

Thermodynamic State = Gas

PROPERTIES:

Component Name = CO2V

Option = Table

Table Format = TASCflow RGP

Table Name = Dcfx/CO2-high.rgp

END

END

END

FLOW: Flow Analysis 1

SOLUTION UNITS:

Angle Units = [rad]

Length Units = [m]

Mass Units = [kg]

Solid Angle Units = [sr]

Temperature Units = [K]

Time Units = [s]

END

ANALYSIS TYPE:

Option = Steady State

EXTERNAL SOLVER COUPLING:

Option = None

END

END

DOMAIN: Default Domain

Coord Frame = Coord 0

Domain Type = Fluid

Location = SOLID

BOUNDARY: Default Domain Default

Boundary Type = WALL

Location = WALL

BOUNDARY CONDITIONS:

HEAT TRANSFER:

Option = Adiabatic

END

MASS AND MOMENTUM:

Option = No Slip Wall

END

WALL ROUGHNESS:

Option = Smooth Wall

END

END

END

BOUNDARY: OUT

Boundary Type = OUTLET

Location = OUT

BOUNDARY CONDITIONS:

FLOW REGIME:

Option = Subsonic

END

MASS AND MOMENTUM:

Option = Static Pressure

Relative Pressure = 0 [Pa]

END

END

END

BOUNDARY: inlet

Boundary Type = INLET

Location = IN

BOUNDARY CONDITIONS:

COMPONENT: CO2V

Mass Fraction = 1

Option = Mass Fraction

END

FLOW DIRECTION:

Option = Normal to Boundary Condition

END

FLOW REGIME:

Option = Subsonic

END

HEAT TRANSFER:

Option = Total Temperature

Total Temperature = 350 [K]

END

MASS AND MOMENTUM:

Option = Total Pressure

Relative Pressure = 0.5 [MPa]

END

TURBULENCE:

Option = Medium Intensity and Eddy Viscosity Ratio

END

END

END

DOMAIN MODELS:

BUOYANCY MODEL:

Option = Non Buoyant

END

DOMAIN MOTION:

Option = Stationary

END

MESH DEFORMATION:

Option = None

END

REFERENCE PRESSURE:

Reference Pressure = 7.5 [MPa]

END

END

FLUID DEFINITION: Fluid 1

Material = CO2

Option = Material Library

MORPHOLOGY:

Option = Continuous Fluid

END

END

FLUID MODELS:

COMBUSTION MODEL:

Option = None

END

COMPONENT: CO2L

Option = Equilibrium Constraint

END

COMPONENT: CO2V

Option = Equilibrium Fraction

END

HEAT TRANSFER MODEL:

Include Viscous Work Term = True

Option = Total Energy

END

THERMAL RADIATION MODEL:

Option = None

END

TURBULENCE MODEL:

Option = k epsilon

END

TURBULENT WALL FUNCTIONS:

High Speed Model = Off

Option = Scalable

END

END

END

OUTPUT CONTROL:

RESULTS:

File Compression Level = Default

Option = Standard

END

END

SOLVER CONTROL:

Turbulence Numerics = First Order

ADVECTION SCHEME:

Option = High Resolution

END

CONVERGENCE CONTROL:

Length Scale Option = Conservative

Maximum Number of Iterations = 100

Minimum Number of Iterations = 1

Timescale Control = Auto Timescale

Timescale Factor = 1.0

END

CONVERGENCE CRITERIA:

Residual Target = 1.E-4

Residual Type = RMS

END

DYNAMIC MODEL CONTROL:

Global Dynamic Model Control = On

END

END

END

COMMAND FILE:

Version = 19.3

END

Best regards,

Abbas

abenhadj posted this 19 February 2019

I do not see any issues: I do not think it is mesh-related. Perhaps it has to do with the RGP tables. Another thing: Please enable beata feature and set for liquid component "subcooled". You are registered without a university mail address so that I won't able to dig deeper here.

Best regards,

Amine

• Liked by
abbas posted this 19 February 2019

Thanks for your help.

Now I change my email to university email address. Could you let me know how I can set liquid component "subcooled"?

Best regards,

Abbas

abbas posted this 20 February 2019

Thanks, Amine.

The problem was just subcooled. I hope others who have this problem could find this page.

Best regards

Abbas

abenhadj posted this 20 February 2019

Nice to see that the mesh was not the issue :-)

Please mark my answer as the solution of this case. Thanks.

Best regards,

Amine

abbas posted this 20 February 2019

Thanks again and yes this is good to see that mesh is not the problem. I marked as the problem is solved.

Best regards

Abbas