CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

CFX error RGP file for CO2

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 8, 2016, 09:57
Default CFX error RGP file for CO2
  #1
New Member
 
Select State
Join Date: May 2016
Posts: 3
Rep Power: 9
Damagea is on a distinguished road
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.
Attached Images
File Type: png 2.png (18.9 KB, 125 views)
Damagea is offline   Reply With Quote

Old   July 26, 2016, 03:14
Default
  #2
Member
 
Yuva
Join Date: Oct 2015
Location: Korea Rep of
Posts: 33
Rep Power: 10
FAKHREDDINE is on a distinguished road
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
FAKHREDDINE is offline   Reply With Quote

Old   August 2, 2016, 08:59
Default
  #3
New Member
 
Select State
Join Date: May 2016
Posts: 3
Rep Power: 9
Damagea is on a distinguished road
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
Damagea is offline   Reply With Quote

Old   September 8, 2016, 22:19
Default
  #4
New Member
 
Lauren Blanchette
Join Date: Mar 2016
Posts: 9
Rep Power: 10
lablan is on a distinguished road
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
lablan is offline   Reply With Quote

Old   July 22, 2018, 04:03
Default
  #5
New Member
 
Yafei Li
Join Date: Jul 2018
Location: CHIAN
Posts: 16
Rep Power: 7
lyfflynice is on a distinguished road
Quote:
Originally Posted by Damagea View Post
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.
lyfflynice is offline   Reply With Quote

Old   September 14, 2022, 04:31
Default CFX error RGP file for supercritical CO2
  #6
New Member
 
ANTALYA
Join Date: Sep 2017
Posts: 20
Rep Power: 8
erginbayrak is on a distinguished road
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.
erginbayrak is offline   Reply With Quote

Old   September 14, 2022, 06:39
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,692
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   September 14, 2022, 15:57
Default
  #8
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,167
Rep Power: 23
evcelica is on a distinguished road
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.
evcelica is offline   Reply With Quote

Old   September 15, 2022, 06:29
Default
  #9
New Member
 
ANTALYA
Join Date: Sep 2017
Posts: 20
Rep Power: 8
erginbayrak is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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 is offline   Reply With Quote

Old   September 15, 2022, 06:34
Default
  #10
New Member
 
ANTALYA
Join Date: Sep 2017
Posts: 20
Rep Power: 8
erginbayrak is on a distinguished road
Quote:
Originally Posted by evcelica View Post
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.
erginbayrak is offline   Reply With Quote

Old   September 15, 2022, 07:05
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,692
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   September 15, 2022, 14:46
Default
  #12
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,167
Rep Power: 23
evcelica is on a distinguished road
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.
evcelica is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 13:23.