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

Boundary condition setting regarding turbine simulation using CFX

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

Like Tree2Likes
  • 1 Post By tauqirnawaz
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   March 5, 2012, 11:15
Default Boundary condition setting regarding turbine simulation using CFX
  #1
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
To all CFD-ers,

Hi there, my name is LOH, a student from Malaysia. Currently I am researching on project regarding tidal turbine. I am using ANSYS CFX and Fluent for the simulation. There are some questions encountered in the simulation which I hope to seek some opinion and advices from all the experts here.

Firstly, tidal turbine is quite similar to that of wind turbine. Since wind energy already been research for more than 35 years, and with the availability of NREL phase 4 full scale wind turbine experiment, there are quite some numbers of numerical simulations work done on the performance prediction of particular turbine. The wind turbine in NREL is a 2 bladed machine, and the two blades are same in all aspects. Therefore, most of the authors of published works are doing their simulation with only a single blade domain analyzed (periodicity of 180deg). By referring to CFX workshop and documentation, compressor turbines are analyzed in similar fashion. Torque of one blade with respect to the rotating axis is get from simulation and multiplies by respective number of blades and speed of rotation for power calculation. So, I guess those authors are doing the same thing (please correct me if I am wrong).

In tidal turbine, the simulation is done in similar ways by all others researcher. A benchmark experiment from University of Southampton is done on 2005 and is used for numerical codes verification. Most of the verification published work analyses single blade domain too. The turbine is a three blades machine.

Since I am researching on some design of blade for power improvement, I carry out the same simulation as what all others do. I model the respecting blade, and run a single blade domain simulation by referring to some of the papers. Somehow, problems exist. Firstly, the results I get is far away from what it suppose to be. The expecting torque supposed to be in 20+ Nm range and I get it for more than 100 Nm. I thought it was some meshing issue, and try to solve the issue by improve the mesh quality by decrease the Y+ to meet the turbulence model requirement. The mesh I used is fully hexahedral blocked by ICEMCFD, the pre-mesh quality should be ok (determinant 2x2x2 is above 0.5). Somehow, the result doesn’t improve much, still in the range of 100 Nm. The torque value is monitored throughout the simulation and only be taken when the value doesn’t fluctuating much.

I am running out of idea and suspect that the error come from boundary condition setting. I would like invite all forum-er and expert to comment in the boundary condition setting. Here is the picture of my domain and boundary conditions setting:



Inlet : 1.73 m/s Normal speed
Outlet : Pressure outlet 0 gauge pressure
Farfield: No slip wall
Bottom wall : No slip wall
Blade : No slip wall
Periodic faces : rotational periodic interface

Latest Update 5 March 2012
Been try to run simulation using 180deg periodicity and 120deg periodicity, changing the boundary condition of farfield to free slip wall:
120deg : No slip wall – 112.14Nm
120deg : Free slip wall – 68.589Nm
180deg: No slip wall – 112.14Nm
180deg: Free slip wall – 50.065Nm

120 deg shall reflected 3 bladed machine and 180deg shall represent 2 bladed machine after multiply their respective number of blade….

Any input is welcome and appreciated…
Lacerlacer is offline   Reply With Quote

Old   March 5, 2012, 11:59
Default
  #2
Member
 
Raja_Bhai
Join Date: Feb 2012
Location: UK
Posts: 40
Rep Power: 5
tauqirnawaz is on a distinguished road
One problem immediately visible from the picture you have provided is the far field boundary, it seems that you have set it to pressure opening. You need to change it to wall boundary. Secondly it seems you have got only one domain?
tauqirnawaz is offline   Reply With Quote

Old   March 5, 2012, 20:16
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You do not need the far field to be a wall. It can be done using pressure boundaries but may have convergence issues.

Have you read the FAQ on accuracy?:
http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   March 5, 2012, 20:40
Default
  #4
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by tauqirnawaz View Post
One problem immediately visible from the picture you have provided is the far field boundary, it seems that you have set it to pressure opening. You need to change it to wall boundary. Secondly it seems you have got only one domain?
I already change it to wall boundary, the simulation was done using pressure outlet before and results is not acceptable also. The results that i show is using wall boundary,been try for free slip and no slip wall as well.
Lacerlacer is offline   Reply With Quote

Old   March 7, 2012, 10:16
Default
  #5
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by tauqirnawaz View Post
One problem immediately visible from the picture you have provided is the far field boundary, it seems that you have set it to pressure opening. You need to change it to wall boundary. Secondly it seems you have got only one domain?
Regarding the domain, u are trying to say that if i set one domain rotating, another one stationary? i got try on that, somehow, with single blade domain, it prompt alot of errors, mainly from the interface of rotating domain and stationary domain. May u share on how u set on that? the domain interface
Lacerlacer is offline   Reply With Quote

Old   March 7, 2012, 10:19
Default
  #6
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You do not need the far field to be a wall. It can be done using pressure boundaries but may have convergence issues.

Have you read the FAQ on accuracy?:
http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
I tried both pressure boundaries and wall boundary, results is quite similar. Convergence is achievable with tolerance of less than 1 percent fluctuation of torque value. the torque is get by torque_x()@blade , rotating axis is on X
Lacerlacer is offline   Reply With Quote

Old   March 7, 2012, 14:59
Default
  #7
Member
 
Raja_Bhai
Join Date: Feb 2012
Location: UK
Posts: 40
Rep Power: 5
tauqirnawaz is on a distinguished road
Quote:
Originally Posted by Lacerlacer View Post
Regarding the domain, u are trying to say that if i set one domain rotating, another one stationary? i got try on that, somehow, with single blade domain, it prompt alot of errors, mainly from the interface of rotating domain and stationary domain. May u share on how u set on that? the domain interface
It is a bit tricky to set up domain interfaces, it depends on your mesh and analysis type. If you can please take a screen print of the interface settings and a close view of the mesh at the interface then I would probably be able to comment.

http://hikwww2.fzk.de/hik/orga/hlr/A...interfaces.pdf
Lacerlacer likes this.
tauqirnawaz is offline   Reply With Quote

Old   March 7, 2012, 18:04
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,941
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This model can be done using either pressure or wall far field boundaries. Your problem is likely to be elsewhere.
Lacerlacer likes this.
ghorrocks is offline   Reply With Quote

Old   March 11, 2012, 01:20
Default
  #9
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by tauqirnawaz View Post
It is a bit tricky to set up domain interfaces, it depends on your mesh and analysis type. If you can please take a screen print of the interface settings and a close view of the mesh at the interface then I would probably be able to comment.

http://hikwww2.fzk.de/hik/orga/hlr/A...interfaces.pdf
I been simulate the two domain successfully, will post the results in short. Really thanks for the comments.
Lacerlacer is offline   Reply With Quote

Old   March 11, 2012, 11:21
Default
  #10
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by tauqirnawaz View Post
It is a bit tricky to set up domain interfaces, it depends on your mesh and analysis type. If you can please take a screen print of the interface settings and a close view of the mesh at the interface then I would probably be able to comment.

http://hikwww2.fzk.de/hik/orga/hlr/A...interfaces.pdf
http://www.cfd-online.com/Forums/mem...e-global-x.png
http://www.cfd-online.com/Forums/mem...-rotate-p2.png
http://www.cfd-online.com/Forums/mem...terface-p1.png
http://www.cfd-online.com/Forums/mem...al-cgi-180.png

Above is the pictures of interfaces for 180deg periodic domain(two blades). The setting of interface also shown.

Below is the pictures of interfaces for 120deg periodic domain(three blades):

http://www.cfd-online.com/Forums/mem...120deg-bcs.png
http://www.cfd-online.com/Forums/mem...-interface.png
http://www.cfd-online.com/Forums/mem...-interface.png
http://www.cfd-online.com/Forums/mem...eriodic-p2.png
http://www.cfd-online.com/Forums/mem...eriodic-p1.png

Simulation is Done for 120deg periodic interface with a rotating domain (inner one) and stationary domain (outer). The torque result got is even far from single domain interface. The mesh used is different, i was using full tetrahedral for the simulation. Torque value i got is 148.45Nm which is far from what it should be in that particular rotating speed (TSR of 7, responding on 40cm radius of blade). The referring literature for those torque value is " Power and Thrust measurement of marine current turbines under various hydrodynamic flow conditions in cavitation tunnel and a towing tank", by As Bahaj, A Molland J chaplin and W.Batten.

Any input is welcome...
Lacerlacer is offline   Reply With Quote

Old   March 12, 2012, 09:21
Default
  #11
Member
 
Raja_Bhai
Join Date: Feb 2012
Location: UK
Posts: 40
Rep Power: 5
tauqirnawaz is on a distinguished road
Quote:
Originally Posted by Lacerlacer View Post

Simulation is Done for 120deg periodic interface with a rotating domain (inner one) and stationary domain (outer). The torque result got is even far from single domain interface. The mesh used is different, i was using full tetrahedral for the simulation. Torque value i got is 148.45Nm which is far from what it should be in that particular rotating speed (TSR of 7, responding on 40cm radius of blade). The referring literature for those torque value is " Power and Thrust measurement of marine current turbines under various hydrodynamic flow conditions in cavitation tunnel and a towing tank", by As Bahaj, A Molland J chaplin and W.Batten.

Any input is welcome...
Hi Loh

1. The resolution of the pictures that you have sent is too low, so I am not able to identify them clearly.
2. I think you have combined all the interface surfaces in one interface, which is incorrect. You would have to define a separate interface for each surface of two domains that are touching each other, like top,bottom and side surfaces of the rotating domain.
3. It is also unclear from the pictures, that which "Frame Change" and "Mesh Connection options" have you chosen.
4. Please go through "http://iceberg.shef.ac.uk/docs/cfx-pdf/tutorials/Tut15MultiphaseMixer.pdf", to see how to define interfaces between rotating and stationery domains.
tauqirnawaz is offline   Reply With Quote

Old   March 12, 2012, 10:32
Thumbs up
  #12
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by tauqirnawaz View Post
Hi Loh

1. The resolution of the pictures that you have sent is too low, so I am not able to identify them clearly.
2. I think you have combined all the interface surfaces in one interface, which is incorrect. You would have to define a separate interface for each surface of two domains that are touching each other, like top,bottom and side surfaces of the rotating domain.
3. It is also unclear from the pictures, that which "Frame Change" and "Mesh Connection options" have you chosen.
4. Please go through "http://iceberg.shef.ac.uk/docs/cfx-pdf/tutorials/Tut15MultiphaseMixer.pdf", to see how to define interfaces between rotating and stationery domains.
Thanks alot for the suggestion! i will try that tutorial and set accordingly, really appreciate ur help~
Lacerlacer is offline   Reply With Quote

Reply

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
UDF setting wall boundary condition with a DEFINE_PROFILE NLao FLUENT 1 April 17, 2011 05:23
Setting outlet Pressure boundary condition using CAFFA code Mukund Pondkule Main CFD Forum 0 March 16, 2011 04:23
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
Warning 097- AB CD-adapco 6 November 15, 2004 05:41


All times are GMT -4. The time now is 05:32.