|
[Sponsors] |
Creating SCO2 properties by using NIST to RGP. |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 14, 2020, 04:11 |
Creating SCO2 properties by using NIST to RGP.
|
#1 |
Member
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5 |
Hello!
I have to create an RGP file to input SCO2 properties to the CFX solver. I have found a program that converts a fluid database into the RGP file, but I have some problems handling this program. --------------------------------------------------------------------- # NIST-RGP.F iNPUT: # # IFLD=1 -> PH2 # IFLD=2 -> LOX # IFLD=3 -> PROPANE (C3H8) # IFLD=4 -> CO2 # IFLD=5 -> METHANE (CH4) # IFLD=6 -> ETHANE (C2H6) # IFLD=7 -> NITROGEN # IFLD=8 -> BUTANE (C4H10) # IFLD=9 -> R245FA # # NT NP NSAT IFLD # ______ _____ _____ _____ 810 810 810 4 # # # TMIN TMAX PMIN PMAX # [DEG R] [DEG R] [PSIA] [PSIA] # _______ _______ _________ ___________ 250. 400. 1015. 1232. --------------------------------------------------------------------- This is the setting properties of dat.txt file in the program. I want to calculate the fluid data between 7MPa and 8.5MPa, 0℃ and 100℃. I cannot understand how this file works. Based on the dimension in this file, I think the pressure input should be calculated as PSIA, and temperature as Kalvin. So I have entered those parameters because I want to get SCO2 properties. But as I activate this program, It turns out an error. --------------------------------------------------------------------- TPRHO failed so extrapolating saturation data IERR1 = 0 IERR2 = 202 J = 144 P/PC = 0.98445562506293216 Of course it didn't work in CFX solver. How can I convert the fluid database into RGP file? How can I use the dat.txt file perfectly? Anybody please help me. Thank you. |
|
June 15, 2020, 16:12 |
|
#2 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,166
Rep Power: 23 |
Temperature is Rankine, not Kelvin. It states that explicitly: "[deg R]"
|
|
June 15, 2020, 20:33 |
|
#3 | |
Member
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5 |
Quote:
Then how can I input the pressure and temperature data? As I input the data like below: # TMIN TMAX PMIN PMAX # [DEG R] [DEG R] [PSIA] [PSIA] # _______ _______ _________ ___________ 545. 650. 1069. 1232. It does not work. |
||
June 16, 2020, 08:44 |
|
#4 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,166
Rep Power: 23 |
Works perfectly fine for me using your inputs (I changed 810 to 100 to make it quicker, but that shouldn't matter).
1.) Do You have all the .fld files from refprop placed in the fluids folder? 2.) Do you have tabs in between you temperature and pressure data? |
|
June 16, 2020, 20:24 |
|
#5 | |
Member
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5 |
Quote:
2)Of course, I have. But it still have error TPRHO failed so extrapolating saturation data IERR1 = 0 IERR2 = 202 J = 2 P/PC = 0.99926348198524140 |
||
June 18, 2020, 12:50 |
|
#6 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,166
Rep Power: 23 |
I Didn't realize you were right below the critical pressure of 1070 psia.
Reduce you # of points from 810 down to something lower (400 worked for me) Or raise your minimum pressure up to at least the critical pressure. |
|
June 20, 2020, 02:00 |
|
#7 | |
Member
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5 |
Quote:
# NT NP NSAT IFLD # ______ _____ _____ _____ 400 400 400 4 # # # TMIN TMAX PMIN PMAX # [DEG R] [DEG R] [PSIA] [PSIA] # _______ _______ _________ ___________ 545. 650. 1080. 1232. But it still doesn't work. SATP failed so extrapolating vapor sat data J = 399 P/PC = 1.0000234477499255 [SATP error 141] pressure input to saturation routine is greater than critical pressure; P = 7.3775 MPa, Pcrit = 7.3773 MPa. It still comes out with error... |
||
June 22, 2020, 15:56 |
|
#8 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,166
Rep Power: 23 |
This worked for me:
# NT NP NSAT IFLD # ______ _____ _____ _____ 400 400 400 4 # # # TMIN TMAX PMIN PMAX # [DEG R] [DEG R] [PSIA] [PSIA] # _______ _______ _________ ___________ 545. 650. 1069. 1232. |
|
June 23, 2020, 21:15 |
|
#9 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,166
Rep Power: 23 |
Also, if you are only interested in supercritical properties, you can ignore that error, as there is no saturation curve in the supercritical region.
|
|
July 3, 2020, 03:26 |
|
#10 | |
Member
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5 |
Quote:
I had made rgp files based on your values: NT~NSAT = 400 , and I also made rgp file NT~NSAT = 1000, It comes out with an error of failing of extrapolating sat data. ---------------------------------------------------------- SATP failed so extrapolating vapor sat data J = 1791 P/PC = 1.0000010211152017 [SATP error 141] pressure input to saturation routine is greater than critical pressure; P = 7.3773 MPa, Pcrit = 7.3773 MPa. --------------------------------------------------------- Based on your reply, I ignored the error and input the rgp file into CFX solver. But it didn't work. It comes out with error. +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | Could not find component in TASCflow RGP file. | | | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | Encountered problem reading the RGP file header. | | | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | Stopped in routine SU_PROPS_RGP | | | | | | | | | | | +--------------------------------------------------------------------+ +--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | The ANSYS CFX solver exited with return code 1. No results file | | has been created. | +--------------------------------------------------------------------+ I had input the temperature of 349K, pressure of 7.991MPa, which are all inside of the interpolation range. But it didn't work. Do you know how I can solve this problem? I am very upset with this error that annoying me about 3 weeks. |
||
July 6, 2020, 11:29 |
|
#11 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,166
Rep Power: 23 |
Are you doing everything correctly in CFX-Pre? Sound's like it can't find the right component according to the error message.
What are you naming your component in Pre? I believe it should be "CO2Vap" You could try using one of the built in real gas equations of state for CO2 vapor if you can't get the rgp file to work. |
|
July 6, 2020, 22:51 |
|
#12 | |
Member
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5 |
Quote:
I found the problem: component name. In CFX and RGP file, there are component names, so I must fit those two component names. By fitting the name, I have solved the problem and I can input the RGP file successfully. Thank you very much! |
||
February 17, 2021, 14:39 |
|
#13 | |
New Member
Younis Najim
Join Date: Apr 2013
Location: Michigan State University
Posts: 12
Rep Power: 12 |
Quote:
Could you please explain how did you fix the component name? we are encountering similar issue. Thank you |
||
February 17, 2021, 15:45 |
|
#14 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,166
Rep Power: 23 |
It should say in your RGP file. Likely "CO2" for the liquid phase, and "CO2Vap" for the gas/supercritical phase. Gas/supercritical is when either the temperature OR pressure is above the critical point.
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Commercial meshers] Fluent3DMeshToFoam | simvun | OpenFOAM Meshing & Mesh Conversion | 50 | January 19, 2020 16:33 |
[blockMesh] Problems in creating a wedge type mesh | Joscha | OpenFOAM Meshing & Mesh Conversion | 28 | August 3, 2019 08:59 |
Problem in running ICEM grid in Openfoam | Tarak | OpenFOAM | 6 | September 9, 2011 18:51 |
Problems with Meshing: Collapsed Cells | Emmanuel Resch | Siemens | 1 | July 30, 2007 04:02 |
Creating new material properties in database | rajeev | FLUENT | 1 | July 13, 2001 04:06 |