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

CFD analaysis of Pelton turbine

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 30, 2013, 03:16
Post CFD analaysis of Pelton turbine
  #1
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
Does any body have link for references to execute cfd analysis of Pelton turbine using ANSYS CFX? Any link for tangential flow turbines like turgo turbines might be beneficial.
amodpanthee is offline   Reply With Quote

Old   April 30, 2013, 09:26
Default
  #2
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
Have a look at the CFX tutorials, they provide ample information.

OJ
oj.bulmer is offline   Reply With Quote

Old   May 1, 2013, 07:59
Default
  #3
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
Is there any specific tutorial for tangential flow turbines?
amodpanthee is offline   Reply With Quote

Old   May 1, 2013, 08:41
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I think there is no specific tut on pelton turbine. For pelton turbine you have to model full wheel and place the jets at appropriate location. Placing GGI between jets and wheel may not be recommended but you can try.

Meshing definitely would be the most time consuming part.

Make the CFD model (meshing, boundary conditions) and come back to further details. If you need help in meshing, you are also welcome.
Far is offline   Reply With Quote

Old   May 1, 2013, 08:57
Default domain
  #5
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
[IMG]file:///C:/Users/RENP-PID-437-1/Desktop/domain.JPG[/IMG]
amodpanthee is offline   Reply With Quote

Old   May 1, 2013, 09:00
Default domain
  #6
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
I have set the domain as shown in the pic....Is it OK to simulate with it?
Attached Images
File Type: jpg domain.jpg (65.3 KB, 94 views)
amodpanthee is offline   Reply With Quote

Old   May 1, 2013, 18:34
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,951
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This will probably work, as long as you only want to model 5 blades.

It can probably be optimised somewhat by doing a few things:
1) Put a wall instead of your outlet, excpet for at the bottom. This will converge much easier and should not affect things too much.
2) You probably do not need to model the nozzle in too much detail. I would just make it an inlet with the necessary velocity - unless the small velocity distribution across the jet is important.
ghorrocks is offline   Reply With Quote

Old   May 2, 2013, 07:39
Default trial simulation
  #8
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
I am running a trial on the model. The boundary conditions are set as shown in the attachment. It gave an unexpected result. Why is the direction of jet changed when it passes from stationary domain to the rotating domain. I think I have some problem with rotating domain.

I have 22 buckets rotating at 600 rpm and 2 nozzles of which I took 5 buckets and lower nozzle. The nozzles are not in symmetric locations. How to choose pitch value in such cases?
Attached Images
File Type: jpg boundary_trial.JPG (70.2 KB, 58 views)
File Type: jpg velocity_streamline.jpg (75.2 KB, 83 views)
amodpanthee is offline   Reply With Quote

Old   May 2, 2013, 15:16
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
At-least you need eleven blades and one nozzle. If nozzles are not symmetric then you need to use full wheel with two nozzles.
Far is offline   Reply With Quote

Old   May 2, 2013, 18:44
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,951
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The jet is not straight because you are plotting velocity in the local frame of reference. To get a straight jet plot in CFD-Post using "Velocity in Stationary Frame of Reference".
ghorrocks is offline   Reply With Quote

Old   May 2, 2013, 23:45
Default velocity in stationary frame
  #11
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
The direction does not change when we see it in stationary frame too
Attached Images
File Type: jpg velocity_stationary_frame.JPG (88.0 KB, 47 views)

Last edited by amodpanthee; May 3, 2013 at 00:36.
amodpanthee is offline   Reply With Quote

Old   May 3, 2013, 01:58
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by ghorrocks View Post
The jet is not straight because you are plotting velocity in the local frame of reference. To get a straight jet plot in CFD-Post using "Velocity in Stationary Frame of Reference".
did you give the rpm to runner?
Far is offline   Reply With Quote

Old   May 3, 2013, 02:55
Default
  #13
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
Yes of course..... Runner is rotating in anticlockwise direction. I have assigned value 600 rpm.
amodpanthee is offline   Reply With Quote

Old   May 5, 2013, 05:14
Default Flow Direction
  #14
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
I have problem with the direction of jet at interference between rotating and stationary domain, attached picutre. I think I have problem with defining the flow direction at Inlet.

I was trying to simulate a complete runner and got an error on setting the cartesian co-ordinates 0,0,0, attached picture. So, I tried simulating taking normal to boundary which runs, attached picture.....I ran it although it does not give desired result. So, I think the flow direction is the reason for deflecting the jet.

Is there any rule of thumb like right hand thumb rule or left hand thumb rule to define the flow direction? The two jets in my model are placed inclined at an angle 45 degree in second quadrant and third quadrant in XY plane. Changing the flow direction will probably help run the simulation correctly.

Any suggestions would be highly appreciated.
Attached Images
File Type: jpg CFX Analysis.jpg (69.9 KB, 68 views)
File Type: jpg CFX Analysis2.jpg (57.9 KB, 63 views)
File Type: jpg Inlet_stationary_error.jpg (54.4 KB, 61 views)
File Type: jpg Inlet_stationary_run.JPG (73.4 KB, 50 views)
amodpanthee is offline   Reply With Quote

Old   May 5, 2013, 06:03
Default Pelton
  #15
New Member
 
BhaskarD
Join Date: May 2012
Location: Nepal
Posts: 22
Rep Power: 5
Magma is on a distinguished road
Send a message via Skype™ to Magma
Quote:
Originally Posted by amodpanthee View Post
I have problem with the direction of jet at interference between rotating and stationary domain, attached picutre. I think I have problem with defining the flow direction at Inlet.

I was trying to simulate a complete runner and got an error on setting the cartesian co-ordinates 0,0,0, attached picture. So, I tried simulating taking normal to boundary which runs, attached picture.....I ran it although it does not give desired result. So, I think the flow direction is the reason for deflecting the jet.

Is there any rule of thumb like right hand thumb rule or left hand thumb rule to define the flow direction? The two jets in my model are placed inclined at an angle 45 degree in second quadrant and third quadrant in XY plane. Changing the flow direction will probably help run the simulation correctly.

Any suggestions would be highly appreciated.




Sir, What I believe is : if you are working with Cartesian coordinates, you must specify each components of velocity!! cheers!!!
Magma is offline   Reply With Quote

Old   May 5, 2013, 07:36
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,951
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Just use normal to the boundary for the inlet. No need to specify a direction.

Your jet is being deflected before it even gets to the pelton blades. This means something is fundamentally wrong with your setup to do this. What are streamlines of the air phase look like? If you have over-constrained the air phase it will deflect the water jet like this. I mean the air needs somewhere to go to get out of the way of the water jet.
ghorrocks is offline   Reply With Quote

Old   May 5, 2013, 09:44
Default
  #17
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Why are you using symmetry condition? if it strange to use symmetry condition for this type of flow where you don't know exactly where flow is going...


My suggestion :
we did similar study on tip injection effect on stall margin enhancement of transonic axial compressor rotor ( to be specific, NASA rotor 37)

http://arc.aiaa.org/doi/abs/10.2514/6.2012-329

http://www.researchgate.net/publicat...ow_Compressors

The point which I want to discuss is that " we have divided tip clearance into two parts : one was with rotating domain of rotor and second was with stationary domain of tip injection. So instead of putting interface at the intersection of jet and casing of compressor we gave it some space into the rotating domain.

I can locate that paper and send you if needed.
Far is offline   Reply With Quote

Old   May 5, 2013, 23:36
Default paper
  #18
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
Far

Can I get the full length paper? amodpanthi@ku.edu.np
amodpanthee is offline   Reply With Quote

Old   May 10, 2013, 13:18
Default
  #19
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Sorry for delay. did you get paper?


Last edited by Far; May 10, 2013 at 14:42.
Far is offline   Reply With Quote

Old   May 11, 2013, 02:46
Default
  #20
New Member
 
Amod Panthee
Join Date: Apr 2013
Location: Nepal
Posts: 18
Rep Power: 4
amodpanthee is on a distinguished road
Yes, I received the attachment. I am going through it.

Thank you
amodpanthee is offline   Reply With Quote

Reply

Tags
cfd, pelton turbine, tangential flow turbines

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
3 bladed Vertical Axis Wind Turbine transient CFD ArslanOZCAN FLUENT 1 February 5, 2011 09:34
Helical Turbine CFD gkadoo Main CFD Forum 0 April 22, 2010 03:28
ASME CFD Symposium Chris Kleijn Main CFD Forum 0 August 22, 2001 06:41
CFD Design...The CFD Future John C. Chien Main CFD Forum 19 October 6, 1999 11:57
public CFD Code development Heinz Wilkening Main CFD Forum 38 March 5, 1999 12:44


All times are GMT -4. The time now is 11:32.