CFX error RGP file for CO2

Damagea · July 8, 2016, 09:57

I have to perform a calculation on a heat exchanger in which one of the fluid is CO2. I created a CFX RGP file covering the liquid, the gas and the supecritcal region of the phase state diagram. But I met one problem about CFX-solver.

FAKHREDDINE · July 26, 2016, 03:14

Hello

Are you solving the problem on one machine Windows or on Cluster platform Linux ?

Did you create the RGP file by yourself or you import it from NIST ?

AND you need to specify the competent name (CO2 for ur case ) of the fluid exactly as it is written inside the RGP file when you upload the file in CFX

Tell me if it works
windows.JPG

Damagea · August 2, 2016, 08:59

https://www.reddit.com/r/CFD/comment...al_properties/
There is a RGP and i changed it according to my need.But there was a problem when i upload the file in CFX.And i specify the competent name of the fluid exactly as it is written insisde the RGP

lablan · September 8, 2016, 22:19

Hello,

I am trying to create a RGP table for sCO2 as well to use in CFX. For this I am creating metastable state tables in which gas properties go into the liquid region. I have created the table but when I try to solve I receive an error stating "Encountered problem reading superheat data". I have gone off of the .rgp file attached to this thread but the only thing that I do not understand is how the saturation temperature and property dependent on the pressure was created at the end of each superheat table. Can anyone explain the way they got there values within the table? Most of my properties are beyond the critical point and thus they do not return a saturation temperature with the known pressure.

Any help would be greatly appreciated.

Thanks,

Lauren

lyfflynice · July 22, 2018, 04:03

Quote:

Originally Posted by Damagea

I have to perform a calculation on a heat exchanger in which one of the fluid is CO2. I created a CFX RGP file covering the liquid, the gas and the supecritcal region of the phase state diagram. But I met one problem about CFX-solver.

Dear Damagea,
How to define the Liquid property in the RGP file. Can you give me an example.

erginbayrak · September 14, 2022, 04:31

Hi, I have been trying to import the RGP file for supercritical CO2 to Ansys CFX. But I met one problem with CFX-solver as follows:
Thank you for your recommendations. Regards.

+--------------------------------------------------------------------+
| Buoyancy Reference Information |
+--------------------------------------------------------------------+

Domain Group: Default Domain

Buoyancy has been activated. The absolute pressure will include
hydrostatic pressure contribution, using the following reference
coordinates: (-5.44926E-17, 6.31409E-20, 3.00000E-04).

Fatal bounds error detected
---------------------------
Variable: Thermal Conductivity
Locale : Default Domain

+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

Details of error:-
----------------
Error detected by routine MAKDAT
CDANAM = LVAR CDTYPE = INTR ISIZE = 140
CRESLT = OLD

Current Directory : /FLOW/ALGORITHM/ZN1/SYSTEM/VARIABLES

+--------------------------------------------------------------------+
| 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 · September 14, 2022, 06:39

The error message says exactly what is going on.

The first section is a comment about how it is setting up the buoyancy calculation. You should read this and check that it is doing the correct thing. This is not an error or warning, just a message.

The second bit says there is a bounds error on thermal conductivity. This usually means the pressure or temperature has gone outside of the range of your material properties table. This table may have been defined by your RGP file or it could have come form elsewhere. Either way, the simulation went outside the range you defined. This might mean a bit of the simulation exceeds the range you defined (so you need to extend the range to cover the entire actual range) or your simulation has some numerical problems leading to non-physical values. Maybe it will converge and come good after a while, or maybe it will diverge.

evcelica · September 14, 2022, 15:57

What temperature and pressure are you at?
Are you using the liquid or vapor property tables from your .rgp file?
My guess is you may be using the wrong phase, hence variables are out of range in that table.

erginbayrak · September 15, 2022, 06:29

Quote:

Originally Posted by ghorrocks

The error message says exactly what is going on.

The first section is a comment about how it is setting up the buoyancy calculation. You should read this and check that it is doing the correct thing. This is not an error or warning, just a message.

The second bit says there is a bounds error on thermal conductivity. This usually means the pressure or temperature has gone outside of the range of your material properties table. This table may have been defined by your RGP file or it could have come form elsewhere. Either way, the simulation went outside the range you defined. This might mean a bit of the simulation exceeds the range you defined (so you need to extend the range to cover the entire actual range) or your simulation has some numerical problems leading to non-physical values. Maybe it will converge and come good after a while, or maybe it will diverge.

Thank you for your reply. Although I have extended the range, the CFX solver gives the same warnings.

erginbayrak · September 15, 2022, 06:34

Quote:

Originally Posted by evcelica

What temperature and pressure are you at?
Are you using the liquid or vapor property tables from your .rgp file?
My guess is you may be using the wrong phase, hence variables are out of range in that table.

My inlet temperature is 290K and the pressure outlet is 80 bar (the pressure change is so low through the pipe). Also, I am using liquid and vapor property tables.

$$$$HEADER
$$$CO2
1
$$PARAM
26
DESCRIPTION
CO2 (LIQUID)
NAME
CO2
INDEX
CO2
DATABASE
NIST PROPERTY DATABASE
MODEL
3
UNITS
1
PMIN_SUPERHEAT
7494582.6347656
PMAX_SUPERHEAT
8494319.9687500
TMIN_SUPERHEAT
250.0000066
TMAX_SUPERHEAT
750.0000199
TMIN_SATURATION
0.0000000
TMAX_SATURATION
304.1282000
P_CRITICAL
7377300.0000000
P_TRIPLE
517964.3433553
T_CRITICAL
304.1282000
T_TRIPLE
216.5920000
GAS_CONSTANT
188.9240578
TABLE_1
800 800
TABLE_2
800 800
TABLE_3
800 800
TABLE_4
800 800
TABLE_5
800 800
TABLE_6
800 800
TABLE_7
800 800
TABLE_8
800 800
TABLE_9
800 800
$$$CO2VAP
1
$$PARAM
26
DESCRIPTION
CO2 (VAPOR)
NAME
CO2VAP
INDEX
CO2VAP
DATABASE
NIST PROPERTY DATABASE
MODEL
3
UNITS
1
PMIN_SUPERHEAT
7494582.6347656
PMAX_SUPERHEAT
8494319.9687500
TMIN_SUPERHEAT
250.0000066
TMAX_SUPERHEAT
750.0000199
TMIN_SATURATION
250.0000066
TMAX_SATURATION
750.0000199
P_CRITICAL
7377300.0000000
P_TRIPLE
517964.3433553
T_CRITICAL
304.1282000
T_TRIPLE
216.5920000
GAS_CONSTANT
188.9240578
TABLE_1
800 800
TABLE_2
800 800
TABLE_3
800 800
TABLE_4
800 800
TABLE_5
800 800
TABLE_6
800 800
TABLE_7
800 800
TABLE_8
800 800
TABLE_9
800 800
$$$$DATA
$$$CO2
1
$$PARAM
26
DESCRIPTION
CO2 (LIQUID)
NAME
CO2
INDEX
CO2
DATABASE
NIST PROPERTY DATABASE
MODEL
3
UNITS
1
PMIN_SUPERHEAT
7494582.6347656
PMAX_SUPERHEAT
8494319.9687500
TMIN_SUPERHEAT
250.0000066
TMAX_SUPERHEAT
750.0000199
TMIN_SATURATION
250.0000066
TMAX_SATURATION
750.0000199
P_CRITICAL
7377300.0000000
P_TRIPLE
517964.3433553
T_CRITICAL
304.1282000
T_TRIPLE
216.5920000
GAS_CONSTANT
188.9240578
TABLE_1
800 800
TABLE_2
800 800
TABLE_3
800 800
TABLE_4
800 800
TABLE_5
800 800
TABLE_6
800 800
TABLE_7
800 800
TABLE_8
800 800
TABLE_9
800 800
$$SUPER_TABLE
values are continuing.

ghorrocks · September 15, 2022, 07:05

Quote:

Although I have extended the range, the CFX solver gives the same warnings.

OK, but there is much more you should try:
* save a results file just before the error and have a look at it. Is it physically realistic?
* Look at the convergence. Is it converging?

If it appears to be converging and realistic then you might need to increase the range. If it is not converging then you need to fix the convergence problem. If it is not realistic then you need to look at your simulation to see if it is correctly set up.

evcelica · September 15, 2022, 14:46

The fluid is using either one table or the other based on the the name you set them to (CO2 or CO2VAP) which are the names of the liquid and vapor tables. They are two different phases, and if you specified the table name to be "CO2" then you are using the liquid table, not the vapor table. In CFX, in the material properties, you have to use component name "CO2VAP" to use the vapor table. At 80 bar, you are supercritical, therefore you should be using only the vapor table, not the liquid table.

As I said in my last post: "My guess is you may be using the wrong phase, hence variables are out of range in that table." Which I'm now more confident in.
You are using the liquid table, not the vapor table as you should. So of course, data is out of range of the liquid table at 80 bar since CO2 is "vapor" above 73 bar.

September 14, 2022, 04:31	CFX error RGP file for supercritical CO2	#6
erginbayrak New Member ANTALYA Join Date: Sep 2017 Posts: 20 Rep Power: 8	Hi, I have been trying to import the RGP file for supercritical CO2 to Ansys CFX. But I met one problem with CFX-solver as follows: Thank you for your recommendations. Regards. +--------------------------------------------------------------------+ \| Buoyancy Reference Information \| +--------------------------------------------------------------------+ Domain Group: Default Domain Buoyancy has been activated. The absolute pressure will include hydrostatic pressure contribution, using the following reference coordinates: (-5.44926E-17, 6.31409E-20, 3.00000E-04). Fatal bounds error detected --------------------------- Variable: Thermal Conductivity Locale : Default Domain +--------------------------------------------------------------------+ \| Writing crash recovery file \| +--------------------------------------------------------------------+ Details of error:- ---------------- Error detected by routine MAKDAT CDANAM = LVAR CDTYPE = INTR ISIZE = 140 CRESLT = OLD Current Directory : /FLOW/ALGORITHM/ZN1/SYSTEM/VARIABLES +--------------------------------------------------------------------+ \| 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.

September 14, 2022, 06:39		#7
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,729 Rep Power: 143	The error message says exactly what is going on. The first section is a comment about how it is setting up the buoyancy calculation. You should read this and check that it is doing the correct thing. This is not an error or warning, just a message. The second bit says there is a bounds error on thermal conductivity. This usually means the pressure or temperature has gone outside of the range of your material properties table. This table may have been defined by your RGP file or it could have come form elsewhere. Either way, the simulation went outside the range you defined. This might mean a bit of the simulation exceeds the range you defined (so you need to extend the range to cover the entire actual range) or your simulation has some numerical problems leading to non-physical values. Maybe it will converge and come good after a while, or maybe it will diverge. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[swak4Foam] funkyDoCalc with OF2.3 massflow	NiFl	OpenFOAM Community Contributions	14	November 25, 2020 03:30
[OpenFOAM.org] Patches to compile OpenFOAM 2.2 on Mac OS X	gschaider	OpenFOAM Installation	136	October 10, 2017 17:25
SparceImage v1.7.x Issue on MAC OS X	rcarmi	OpenFOAM Installation	4	August 14, 2014 06:42
OpenFOAM on MinGW crosscompiler hosted on Linux	allenzhao	OpenFOAM Installation	127	January 30, 2009 19:08
ParaView Compilation	jakaranda	OpenFOAM Installation	3	October 27, 2008 11:46

July 26, 2016, 03:14		#2
FAKHREDDINE Member Yuva Join Date: Oct 2015 Location: Korea Rep of Posts: 33 Rep Power: 10	Hello Are you solving the problem on one machine Windows or on Cluster platform Linux ? Did you create the RGP file by yourself or you import it from NIST ? AND you need to specify the competent name (CO2 for ur case ) of the fluid exactly as it is written inside the RGP file when you upload the file in CFX Tell me if it works windows.JPG

August 2, 2016, 08:59		#3
Damagea New Member Select State Join Date: May 2016 Posts: 3 Rep Power: 10	https://www.reddit.com/r/CFD/comment...al_properties/ There is a RGP and i changed it according to my need.But there was a problem when i upload the file in CFX.And i specify the competent name of the fluid exactly as it is written insisde the RGP

September 8, 2016, 22:19		#4
lablan New Member Lauren Blanchette Join Date: Mar 2016 Posts: 9 Rep Power: 10	Hello, I am trying to create a RGP table for sCO2 as well to use in CFX. For this I am creating metastable state tables in which gas properties go into the liquid region. I have created the table but when I try to solve I receive an error stating "Encountered problem reading superheat data". I have gone off of the .rgp file attached to this thread but the only thing that I do not understand is how the saturation temperature and property dependent on the pressure was created at the end of each superheat table. Can anyone explain the way they got there values within the table? Most of my properties are beyond the critical point and thus they do not return a saturation temperature with the known pressure. Any help would be greatly appreciated. Thanks, Lauren

September 14, 2022, 15:57		#8
evcelica Senior Member Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 1,171 Rep Power: 23	What temperature and pressure are you at? Are you using the liquid or vapor property tables from your .rgp file? My guess is you may be using the wrong phase, hence variables are out of range in that table.

September 15, 2022, 14:46		#12
evcelica Senior Member Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 1,171 Rep Power: 23	The fluid is using either one table or the other based on the the name you set them to (CO2 or CO2VAP) which are the names of the liquid and vapor tables. They are two different phases, and if you specified the table name to be "CO2" then you are using the liquid table, not the vapor table. In CFX, in the material properties, you have to use component name "CO2VAP" to use the vapor table. At 80 bar, you are supercritical, therefore you should be using only the vapor table, not the liquid table. As I said in my last post: "My guess is you may be using the wrong phase, hence variables are out of range in that table." Which I'm now more confident in. You are using the liquid table, not the vapor table as you should. So of course, data is out of range of the liquid table at 80 bar since CO2 is "vapor" above 73 bar.