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

My radial inflow turbine

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 7, 2016, 05:29
Unhappy My radial inflow turbine
  #1
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Hello all,

I would first thank you for your Q and A throughout the forum.
I've done successful simulation of my radial turbine using other software packages. I also followed the CFX tutorials regarding Axial turbine and centrifugal compressor. However, I'm designing a radial inflow turbine that is not available in the tutorial. As a starting point, I designed a simple rotor blade using RTD and exported it to Turbogrid and then to CFX. The results of CFX is totally different form the RTD. For example the efficiency is 67.7% in RTD while it is 100% in CFX ! I know there is an error somewhere but I can't find it.

I'm attaching a link for the dropbox where you can find the saved project (case.wbpj)

https://www.dropbox.com/s/1t7zrv15rd...files.zip?dl=0

https://www.dropbox.com/s/06yjmn9ly5...case.wbpj?dl=0


Your suggestions are highly appreciated

All the best
Abo Anas is offline   Reply With Quote

Old   December 7, 2016, 05:52
Default
  #2
Senior Member
 
Maxim
Join Date: Aug 2015
Location: Germany
Posts: 410
Rep Power: 9
-Maxim- is on a distinguished road
Hello Fuhaid and welcome to the forums.

I won't download zip-files from random people (and I am not allowed to on my work computer). So please share a few screenshots of your setup and your CCL-file and/or your OUT-file (copy and paste in the CODE environment here).

Furthermore I would like to point you to the FAQ:
https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F
-Maxim- is offline   Reply With Quote

Old   December 7, 2016, 06:21
Default
  #3
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Hi Maxim,

many thanks for your reply and I understand that you can not open such links.

I tried to copy and paste the screenshots but I could not so I uploaded them as jpg picture.
I noticed that the results in the CFD post are written as ''Compressor Performance Results) !


CFX Set Up

# State file created: 2016/12/07 11:10:00
# CFX-15.0.7 build 2014.04.26-07.00-131803

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: R1
Coord Frame = Coord 0
Domain Type = Fluid
Location = Inlet,Outlet,Passage Main
BOUNDARY: R1 Blade
Boundary Type = WALL
Frame Type = Rotating
Location = BLADE
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: R1 Hub
Boundary Type = WALL
Frame Type = Rotating
Location = INBlock HUB,OUTBlock HUB,Passage HUB
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: R1 Inlet
Boundary Type = INLET
Frame Type = Stationary
Location = INBlock INFLOW
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Option = Stationary Frame Total Temperature
Stationary Frame Total Temperature = 500 [K]
END
MASS AND MOMENTUM:
Option = Stationary Frame Total Pressure
Relative Pressure = 240 [kPa]
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: R1 Outlet
Boundary Type = OUTLET
Frame Type = Stationary
Location = OUTBlock OUTFLOW
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = 0.03846 [kg s^-1]
Option = Mass Flow Rate
END
END
END
BOUNDARY: R1 Shroud
Boundary Type = WALL
Frame Type = Rotating
Location = INBlock SHROUD,OUTBlock SHROUD,Passage SHROUD
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
WALL VELOCITY:
Option = Counter Rotating Wall
END
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: R1 to R1 Internal Side 1
Boundary Type = INTERFACE
Location = SHROUD TIP GGI SIDE 1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: R1 to R1 Internal Side 2
Boundary Type = INTERFACE
Location = SHROUD TIP GGI SIDE 2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: R1 to R1 Periodic 1 Side 1
Boundary Type = INTERFACE
Location = INBlock PER1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: R1 to R1 Periodic 1 Side 2
Boundary Type = INTERFACE
Location = INBlock PER2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: R1 to R1 Periodic 2 Side 1
Boundary Type = INTERFACE
Location = OUTBlock PER1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: R1 to R1 Periodic 2 Side 2
Boundary Type = INTERFACE
Location = OUTBlock PER2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: R1 to R1 Periodic 3 Side 1
Boundary Type = INTERFACE
Location = Passage PER1
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: R1 to R1 Periodic 3 Side 2
Boundary Type = INTERFACE
Location = Passage PER2
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Alternate Rotation Model = true
Angular Velocity = 60000 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 0 [Pa]
END
END
FLUID DEFINITION: Air Ideal Gas
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = Total Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = SST
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Automatic
END
END
END
DOMAIN INTERFACE: R1 to R1 Internal
Boundary List1 = R1 to R1 Internal Side 1
Boundary List2 = R1 to R1 Internal Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = None
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = None
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: R1 to R1 Periodic 1
Boundary List1 = R1 to R1 Periodic 1 Side 1
Boundary List2 = R1 to R1 Periodic 1 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Rotational Periodicity
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH CONNECTION:
Option = Automatic
END
END
DOMAIN INTERFACE: R1 to R1 Periodic 2
Boundary List1 = R1 to R1 Periodic 2 Side 1
Boundary List2 = R1 to R1 Periodic 2 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Rotational Periodicity
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH CONNECTION:
Option = Automatic
END
END
DOMAIN INTERFACE: R1 to R1 Periodic 3
Boundary List1 = R1 to R1 Periodic 3 Side 1
Boundary List2 = R1 to R1 Periodic 3 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Rotational Periodicity
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH CONNECTION:
Option = Automatic
END
END
OUTPUT CONTROL:
MONITOR OBJECTS:
EFFICIENCY OUTPUT:
Efficiency Calculation Method = Total to Static
Efficiency Type = Expansion
Inflow Boundary = R1 Inlet
Option = Output To Solver Monitor
Outflow Boundary = R1 Outlet
END
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR RESIDUALS:
Option = Full
END
MONITOR TOTALS:
Option = Full
END
END
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 200
Minimum Number of Iterations = 1
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END
CONVERGENCE CRITERIA:
Residual Target = 1e-06
Residual Type = MAX
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = On
END
END
END
COMMAND FILE:
Version = 15.0
END
Attached Images
File Type: jpg RTD Setup.jpg (94.3 KB, 58 views)
File Type: jpg RTD results.jpg (157.1 KB, 47 views)
File Type: jpg CFD post.jpg (101.9 KB, 40 views)
Abo Anas is offline   Reply With Quote

Old   December 7, 2016, 06:45
Default
  #4
Member
 
Join Date: Nov 2013
Posts: 57
Rep Power: 8
alirezame is on a distinguished road
Hello,

"Maximum Number of Iterations = 200"
most probably your simulation has not been converged yet!
alirezame is offline   Reply With Quote

Old   December 7, 2016, 06:55
Default
  #5
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Hello alirezame,

I set the maximum number of iterations to 3000 but I got same results with a very slight difference in the efficiency.
Abo Anas is offline   Reply With Quote

Old   December 7, 2016, 10:02
Default
  #6
Senior Member
 
Join Date: Jun 2009
Posts: 174
Rep Power: 13
turbo is on a distinguished road
Check your inlet swirl BC in CFX. It shows zero swirl, while your design wants 70 deg swirl.
turbo is offline   Reply With Quote

Old   December 7, 2016, 12:20
Default
  #7
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Hi Turbo,

Many thanks for your reply.
Is it possible to paly with the swirl angle in CFX? would you please show me how to change the angle from 0 to 70?
Abo Anas is offline   Reply With Quote

Old   December 7, 2016, 12:32
Default
  #8
Senior Member
 
Join Date: Feb 2011
Posts: 493
Rep Power: 14
Antanas is on a distinguished road
Quote:
Originally Posted by Abo Anas View Post
Hi Turbo,

Many thanks for your reply.
Is it possible to paly with the swirl angle in CFX? would you please show me how to change the angle from 0 to 70?
You can specify velocity by cart. or cyl. components
Antanas is offline   Reply With Quote

Old   December 7, 2016, 13:12
Default
  #9
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Hi Antanas,

Thank you for your reply.

are the X Y Z components are simply U W V, respectively?
Abo Anas is offline   Reply With Quote

Old   December 7, 2016, 13:37
Default
  #10
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 5
bparrelli is on a distinguished road
Please provide some screenshots from CFX-Pre so I can see your model. Also please answer the following:
  1. Are you modeling the nozzle and rotor together?
  2. Is the case single passage, or full 360 wheel?
  3. What boundary conditions are you employing at the inlet and outlet? For this type of problem, it's most stable to specify inlet total pressure and temperature, and outlet average static pressure.
  4. What is the inlet temperature and pressure to your model?
  5. What is the pressure ratio of the turbine (p0in/p0out)?
  6. What fluid and equation of state are you using?
  7. What is the rotor diameter and wheel rpm?
This problem is right in my wheelhouse...I solve these types of cases every day, so I can definitely help you if you give me more info.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   December 7, 2016, 13:58
Default
  #11
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Quote:
Originally Posted by bparrelli View Post
Please provide some screenshots from CFX-Pre so I can see your model. Also please answer the following:
  1. Are you modeling the nozzle and rotor together?
  2. Is the case single passage, or full 360 wheel?
  3. What boundary conditions are you employing at the inlet and outlet? For this type of problem, it's most stable to specify inlet total pressure and temperature, and outlet average static pressure.
  4. What is the inlet temperature and pressure to your model?
  5. What is the pressure ratio of the turbine (p0in/p0out)?
  6. What fluid and equation of state are you using?
  7. What is the rotor diameter and wheel rpm?
This problem is right in my wheelhouse...I solve these types of cases every day, so I can definitely help you if you give me more info.

Hi bparrelli,

Many thanks for your reply.

1. Only rotor
2. Single passage
3. I'm applying: inlet total pressure, inlet total temperature, and mass flow rate.
4. inlet total temp is 500K and inlet total pressure is 240 KPa
5. PR = 2.2
6. Ideal gas air
7. impeller wheel and speed are 86.041 mm and 60000 rpm

I uploaded the CCl file of the CFX pre in Maxim. I also attached the screenshot
Attached Images
File Type: jpg 1.jpg (76.8 KB, 27 views)
Abo Anas is offline   Reply With Quote

Old   December 7, 2016, 14:54
Default
  #12
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 5
bparrelli is on a distinguished road
Quote:
Originally Posted by Abo Anas View Post
Hi bparrelli,

Many thanks for your reply.

1. Only rotor
2. Single passage
3. I'm applying: inlet total pressure, inlet total temperature, and mass flow rate.
4. inlet total temp is 500K and inlet total pressure is 240 KPa
5. PR = 2.2
6. Ideal gas air
7. impeller wheel and speed are 86.041 mm and 60000 rpm

I uploaded the CCl file of the CFX pre in Maxim. I also attached the screenshot
Okay, got it. Is the 2.2 pressure ratio across the rotor only, or the entire turbine? If it's only the rotor, then the rotor is going to be choked. In any case, I recommend you enable some of the advanced options in the Solver control. Attached is a screenshot of the advanced setting I typically use for a radial inflow turbine case.

Also, your inlet conditions are fine, but if you're going to model the rotor without a nozzle, then you need to specify the nozzle swirl. Right now, you have the absolute velocity coming in normal to the rotor inlet boundary. This is fine if you're solving the problem in the relative frame, but I don't think you are. I have had convergence trouble modelling high inlet swirl in this type of problem before, and you may just have to model the nozzle with the rotor together to make it work. At a minimum, the models for my designs have a nozzle and a rotor modeled together. In reality, the flow coming into the rotor will be very non-uniform due to nozzle/rotor interaction, and employing inlet swirl is not sufficient to capture this effect. The only way to get the full physics, is to model the nozzle and rotor together with a mixing plane (stage) interface. If this is not an option at this time fore you, I would recommend calculating the flow parameters in the relative frame, and solving your rotor as a stationary nozzle.

Lastly, you want to use the pressures as your boundary conditions, not mass flow. This will give you more stable convergence. Your turbine U/C0 is only about 0.4, so your efficiency should not be very high (maybe 50-70%).

Try all this and let me know if that helps.
Attached Images
File Type: jpg Untitled.jpg (57.2 KB, 67 views)
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   December 7, 2016, 19:33
Default
  #13
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Dear Brian,

Many thanks for your detailed reply. That's highly appreciated.
I will try modelling both stator and rotor. But before that, could you please advise how to set the swirl angle in case of vsnelss rotor as the one I did? I think I can do it by setting the Cartesian coordinate instead of choosing normal to boundary. If this is the case, are x y z components mean simply u w v ?

Also, I sent you a private message. Would you kindly check it?

All the best
Abo Anas is offline   Reply With Quote

Old   December 7, 2016, 22:40
Default
  #14
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 5
bparrelli is on a distinguished road
Yes, but I'd recommend using cylindrical coordinates, as they're more appropriate for turbomachinery. I don't answer private messages, sorry. But if you're interested in my course, you can access it at the link in my signature below. There is also a webinar about the course tomorrow morning at 8am PST. You can sign up for it on the SolidProfessor website.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   December 8, 2016, 05:45
Default
  #15
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Thank you Brian. I'm keen to register in the courses.
I Know I asked many questions but hopefully this will be my last question:

I have the following velocity components at the rotor inlet, how can I convert them to cylindrical coordinates ( Axial component, Radial component and Theta component)?

U (Blade Speed)= 270.3 m/s,
W (Relative Velocity)= 96.1 m/s,
V2 (Absolute Velocity)= 280.4 m/s
Vr (Radial Velocity) = 95.9 m/s
Vw (Whirl Velocity) = 263.5 m/s

Many thanks
Abo Anas is offline   Reply With Quote

Old   December 8, 2016, 09:37
Default
  #16
Senior Member
 
Join Date: Jun 2009
Posts: 174
Rep Power: 13
turbo is on a distinguished road
You can go ahead without nozzle solving the rotor only.
Note CFX inlet swirl BC notations are different from turbomachinery velocity notations. The "u" is a unit vector of x-direction, "v" for y and "w" for z-direction, respectively. If your machine rotation axis is z-direction,
w = 0.0 (implying no axial flow at the rotor inlet)
u = -1.0 (implying downward inflow)
v = + tan 70 deg
turbo is offline   Reply With Quote

Old   December 8, 2016, 10:31
Default
  #17
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 5
bparrelli is on a distinguished road
If z is the rotation axis, then you can define it as follows:

axial coordinate = z
r = sqrt(x^2+y^2)
x = r*cos(theta)
y = r*sin(theta)

This is very basic stuff that you should find in many math textbooks.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli is offline   Reply With Quote

Old   December 11, 2016, 15:14
Default
  #18
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Dear Turbo and Brian,

Thank you for the continuous support.
I spent the weekend working on a new rotor blade but each time I got wrong results such as 100% total to static efficiency, lower mass flow rate values etc. I also don't know why it shows '' Compressor'' instead of turbine in the tabulated results.

I attached a link for my simulation and I also attached photos for those who don't to open anonymous links.

I would be very happy if you take a look at it and advise me

https://www.dropbox.com/s/qe8wsiv4cdlowp1/Try.zip?dl=0
Attached Images
File Type: jpg CFXpre_1.jpg (31.8 KB, 30 views)
File Type: jpg CFXpre_2.jpg (58.1 KB, 27 views)
File Type: jpg CFXpre_3.jpg (88.9 KB, 30 views)
File Type: jpg CFXpre_4.jpg (30.8 KB, 24 views)
File Type: jpg CFXpre_5.jpg (43.9 KB, 27 views)
Abo Anas is offline   Reply With Quote

Old   December 11, 2016, 15:15
Default
  #19
New Member
 
Ahmad Hari
Join Date: Dec 2016
Posts: 21
Rep Power: 5
Abo Anas is on a distinguished road
Continue of the attached photos

Just to let you, I'm using Cartesian coordinates based on comment by Turbo. I have a swirl angle (absolute flow angle) = 78.33 deg

Many thanks in advance
Attached Images
File Type: jpg CFXpre_6.jpg (44.5 KB, 30 views)
File Type: jpg CFXpre_7.jpg (87.3 KB, 25 views)
File Type: jpg CFXpre_8.jpg (81.0 KB, 23 views)
File Type: jpg Tabulated Results.jpg (61.4 KB, 32 views)
MDSHUJAN likes this.
Abo Anas is offline   Reply With Quote

Old   December 11, 2016, 18:57
Default
  #20
Member
 
Brian Parrelli
Join Date: Nov 2016
Location: Southern California
Posts: 41
Rep Power: 5
bparrelli is on a distinguished road
A few thoughts:

1. Did you make sure your direction of rotation is correct using the right hand rule?
2. You should calculate the rotor efficiency on your own. Don't rely on the tabulated results. You aren't modeling the nozzle so your total isentropic enthalpy drop across the turbine isn't captured. In any case, the correct way to calculate turbine efficiency is:
(Rotor torque x RPM) / (mdot*deltaHs)

I'll leave it to you to work out the units.
__________________
Brian Parrelli
Specialties: Turbomachinery, CFD
Professional Profile: Click Here

Do you want to become better at CFX? Sign up for my virtual course through SolidProfessor: "Introduction to ANSYS CFX" >>>
Click Here
bparrelli 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
Interface model for a radial inflow turbine kelinjose CFX 2 February 28, 2013 13:00
Spatially and time varying inflow - turbine simulation Alex_S FLUENT 4 July 19, 2012 02:45
CFX application to radial inflow gas turbine Chetan Mistry CFX 5 June 2, 2007 13:13
radial inflow turbine rotor periodicity problem Nanda FLUENT 1 July 17, 2006 14:52
radial inflow turbine rotor periodicity problem Nanda FLUENT 0 July 11, 2006 20:35


All times are GMT -4. The time now is 10:38.