CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   Sc-CO2 (

tienmanhnguyen May 14, 2013 11:00

I'm simulating the flow of Sc-CO2 through a capillary nozzle with these parameters:
pressure inlet: 1.5*10^7 pa
temperture inlet: 350 K
outlet is atmospheric condition
I'm using EOS for real gas. however I can't set the pressure for inlet boundary conditions, instead, I use velocity. so, my question is how to set the supercritical properties for the flow?

Daniel C May 20, 2013 11:27

Okay you asked me via private message, but we should discuss it in the board, so it could be usefull for the community.

Your question was :

>>excuse me. I've seen in the forum that you had a trouble with supercritical CO2 properties. Have you solved it? I really want to know how. coz I'm working on the flow of Sc-CO2. sorry if this message bothers you. thanks.<<

I replied:

I used a RGP-Table for CO2 because the deviation was about 20% compared to ideal gas properties. In my case, only the temperature is above the critical temperature of CO2; the pressure was far below the critical pressure. So not really supercritical state. In your case I would strongly recommend to build your own table for CO2. That can be done with Tascflow or by coding, using the REFPROP dll's from NIST.

Then you runned into the following problem:

>>I selected co2 from the REFPROP database then I chose the liquid phase. however, my model didn't work. may you help me figure this out. I'm simulating the flow of sc-co2 through a nozzle, the pressure inlet is 150 bar and temperture is355k. outlet has the atmospheric conditions ( 1 at, 298 K) <<

Now I have some questions:

1. What does "my model didn't work" mean?

2. How did you copy the properties from RERPROP?

3. The RGP-Tables have their own File Format; did you read the documentation of CFX-Pre?

What I found in the documentation is:

In release 14.0, only the dry superheated vapor model is supported, corresponding to MODEL=3 in the .rgp file. Other settings of this parameter are ignored by the CFX-Solver, so all the saturation data that would normally be read when using the non-equilibrium (MODEL=1) or equilibrium (MODEL=2) models will be ignored. This means that the $$SAT_TABLE section does not have to exist under a $$$Database access key, that the SUPERCOOLING parameter can be zero and that only the $$SUPER_TABLE section is necessary.

I don't understand for what the SAT_TABLE section in the RGP-Table is designed, when it is just ignored. Maybe somebody can clarify this point. It should be possible to simulate CO2 in liquid Phase, shouldn't it?

tienmanhnguyen May 21, 2013 06:25

thanks Daniel. here are my answers:
2. I just simply typed those code:
> define/user-defined/real-gas-models/nist-real-gas-model
use NIST real gas? [no] yes*
select*real-gas*data*file*[""]* "co2.fld"
> define/user-defined/real-gas-models/set-phase
Select vapor phase (else liquid)?[no]
1. It runed into a error:
Internal error at line 1419 in file '..\..\src\rp_mstage.c'.
Divergence detected in AMG solver
3. I haven't read the CFX-pre yet. however I think I need to use "RGP-Tables generator" to create file format ".rgp", right?

Daniel C May 22, 2013 03:54

I have not worked with FLUENT yet, but it should be a general CFD problem. I think it is caused either by your boundary conditions or the mesh quality or the initial guess.

To begin with the boundary condition, you should start the Simulation with the most robust conditions. In CFX the most robust combination is velocity/mass flow at an inlet and static pressure at an outlet. In your case you have defined static pressure at an inlet and static pressure at an outlet this is very unreliable. You should sight the FLUENT documentation for recommended configurations of boundary conditions.

Now we come to the mesh quality. Check the Rate of Volume Change, it should be below 10 and the Aspect Ratio should not exceed 5000. You should also observe the skewness of your mesh. Make sure that the minimum angle is above 18 degree. Go to the mesh section in this forum to get a more precise advice.

And least the initial guess. You should always start with more simple physics to get the simualtion going and then use this solution as the initial guess for the more complex simulation. For instance try laminar flow instead of turbulent flow or use more simple turbulence models. Reduce the advection scheme to 1st order can also support the start-up.

Regarding the real gas properties, FLUENT seems to come with an interface for the NIST-database. You should use the buil-in capabilities of FLUENT instead of building your own rgp-tables. Your divergence problem is most likely caused by the problems mentioned above.

Hope that helped:)

With kind regards


Daniel C May 22, 2013 04:08


Originally Posted by tienmanhnguyen (Post 428849)
thanks Daniel. here are my answers:
2. I just simply typed those code:
> define/user-defined/real-gas-models/nist-real-gas-model
use NIST real gas? [no] yes*
select*real-gas*data*file*[""]* "co2.fld"

And by the way you certainly checked yes, right? ;)

All times are GMT -4. The time now is 12:25.