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

Simulation of NREL UAE Phase VI turbine

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

Like Tree7Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 22, 2012, 07:46
Default Stuck again
  #41
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 4
Lacerlacer is on a distinguished road
Quote:
Originally Posted by aqstax View Post
Actually I didn't use a boundary layer mesh at all. The reason was two-fold. One, I had problems with diversion on the turbulence parameters with the boundary layer on. Instead of trying to fix this, I realized the BL took up many mesh volumes. Instead, I kept the mesh as fine as possible close to the blade, and ran the k-ω SST model without transitional flows. This ensured my y+ was suitable for the simulation. For k-ω SST model with transitional flows, the y+ required is 1, requiring a very fine boundary layer.
Thus, I was able to refine the rest of my domain adequately as well, since the boundary layer did not take up that many cells anymore. My mesh was purely tet-unstructured. The results I'm achieving are very comparable to experimental results, and I don't really need a good resolution of the boundary layer, so this worked for me.
Hi aqstax,

How are u lately? hope u are doing fine there. I get stuck again in my simulation. I now stuck in results extracting. Mind share me how u actually get torque value from periodic domain u having there? My case was domain rotate about y axis, and i get the torque value of one blade by torque_y()@blade, is that alright? the torque value seem very very small , approaching zero no matter what RPM i used.

Regards,
Lacer
Lacerlacer is offline   Reply With Quote

Old   April 24, 2012, 19:14
Default
  #42
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Quote:
Originally Posted by Lacerlacer View Post
Hi aqstax,

How are u lately? hope u are doing fine there. I get stuck again in my simulation. I now stuck in results extracting. Mind share me how u actually get torque value from periodic domain u having there? My case was domain rotate about y axis, and i get the torque value of one blade by torque_y()@blade, is that alright? the torque value seem very very small , approaching zero no matter what RPM i used.

Regards,
Lacer
The toque is indeed the torque about the y-axis. Just to go to report>forces then select torque about y-axis for only the blade. Another thing is to make sure your blade is oriented the right way. Are you doing multiple reference frames or single? Are all your reference frames set to rotational with the correct axis (even the stationary ones)? Check each and every boundary condition carefully, it is very easy to be careless. RPM for NREL rotor is 72. It is fixed, and the only variable is the wind speed. If you are using Reynolds similarity (smaller model), if your model is 5 times smaller, your wind seed must become 5 times larger and RPM 25 times larger.

Also, you can set fluent to display and plot the coefficient of moment about the y-axis during your simulation, so you can end it early if you don't think it's going well. You can calculate the torque from that coefficient based on your reference vales.
aqstax is offline   Reply With Quote

Old   April 24, 2012, 21:45
Default
  #43
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 4
Lacerlacer is on a distinguished road
Quote:
Originally Posted by aqstax View Post
The toque is indeed the torque about the y-axis. Just to go to report>forces then select torque about y-axis for only the blade. Another thing is to make sure your blade is oriented the right way. Are you doing multiple reference frames or single? Are all your reference frames set to rotational with the correct axis (even the stationary ones)? Check each and every boundary condition carefully, it is very easy to be careless. RPM for NREL rotor is 72. It is fixed, and the only variable is the wind speed. If you are using Reynolds similarity (smaller model), if your model is 5 times smaller, your wind seed must become 5 times larger and RPM 25 times larger.

Also, you can set fluent to display and plot the coefficient of moment about the y-axis during your simulation, so you can end it early if you don't think it's going well. You can calculate the torque from that coefficient based on your reference vales.
Hi ,

THanks for the reply, the following picture is my setup:
http://www.cfd-online.com/Forums/mem...c-settings.png

My case is a tidal turbine,a 40cm radius tidal blade. Somehow i am using CFX to simulate it. There are two domains in the case, one smaller one with blade , another stationary bigger domain. From your reply, u saying that the stationary domain need to set rotate refer to Y axis right? i will try out that , set to rotate about y axis, and RPM of zero. About the multi frame reference, i think this one should all refer to y axis, am i right?

Regards,
LOH AC
Lacerlacer is offline   Reply With Quote

Old   April 25, 2012, 06:56
Default
  #44
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Quote:
Originally Posted by Lacerlacer View Post
Hi ,

THanks for the reply, the following picture is my setup:
http://www.cfd-online.com/Forums/mem...c-settings.png

My case is a tidal turbine,a 40cm radius tidal blade. Somehow i am using CFX to simulate it. There are two domains in the case, one smaller one with blade , another stationary bigger domain. From your reply, u saying that the stationary domain need to set rotate refer to Y axis right? i will try out that , set to rotate about y axis, and RPM of zero. About the multi frame reference, i think this one should all refer to y axis, am i right?

Regards,
LOH AC
dont set it to rotate. set the periodic boundary in the stationary domain to rotational and set its axis to the y-axis. for the stationary domain, set it's rotational axis, but leave it as stationary.
Lacerlacer likes this.
aqstax is offline   Reply With Quote

Old   July 13, 2012, 06:54
Default
  #45
New Member
 
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 4
monaya flower is on a distinguished road
hi aqstax
how did you create prismatic boundary layer in Gambit . i tried to do it but i can't
monaya flower is offline   Reply With Quote

Old   July 16, 2012, 00:56
Default
  #46
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Quote:
Originally Posted by monaya flower View Post
hi aqstax
how did you create prismatic boundary layer in Gambit . i tried to do it but i can't
It is indeed difficult to do so. Are you unable to generate the BL, or you can't mesh after that? The ends of the airfoil cross-sections (the leading and trailing) need to be closed in the BL. Means you can't have lines extending from there. In order to divide the geometry into smaller parts, I have lines extending out from the 0.3c point on the pressure and suction surfaces of the airfoil, rather than the leading and trailing edges.

It takes a lot of trial and error to get it right, and it is very hard to explain exactly what to do. Ensure you have a triangular mesh on your faces before adding the boundary layer, and make sure all the parameters (height, growth rate) are acceptable.

Also, be sure to assess whether you need the BL at all. Usually people use BLs when they need to observe the boundary layer flows in detail, or if they need a very small y+. For me, I used k-w SST without transitional flows, and that didnt require such a small y+, so I did away with the boundary layer (caused too much trouble) since I was more interested in the aerodynamics and wake flow.
aqstax is offline   Reply With Quote

Old   July 16, 2012, 12:33
Default
  #47
New Member
 
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 4
monaya flower is on a distinguished road
hey aqastax

thanks alot for your reply . are you egyptian
monaya flower is offline   Reply With Quote

Old   July 18, 2012, 23:54
Default
  #48
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Haha, no I'm from Singapore
aqstax is offline   Reply With Quote

Old   July 25, 2012, 16:00
Default
  #49
New Member
 
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 4
monaya flower is on a distinguished road
hey aqstax

i am trying to simulate NREL wind turbine but the torque is very high , it's about 4000 N.m at velocity 10 m/s .. my mesh is about 2.5 million cell , i use k-w sst model , Ti is .5 ,and viscosity ratio 10, MRF
can you help me ?
monaya flower is offline   Reply With Quote

Old   July 29, 2012, 01:21
Default
  #50
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Quote:
Originally Posted by monaya flower View Post
hey aqstax

i am trying to simulate NREL wind turbine but the torque is very high , it's about 4000 N.m at velocity 10 m/s .. my mesh is about 2.5 million cell , i use k-w sst model , Ti is .5 ,and viscosity ratio 10, MRF
can you help me ?
It was a long process for me to get it right, and I'm afraid it has been for everyone who has attempted this simulation. You need to ensure the upstream and downstream boundaries are far enough to have little effect on the flow. I used +10D and -10D from the rotor centre. Your mesh must fit the y+ profile of the turbulence model, especially around the rotor (xy-plot>turbulence properties> y+). And 2.5 million is unlikely to work, I personally used 8.7 million cells. Are you using periodic? Unfortunately I can't tell you much more with the details you have given me. Have you done a thorough lit review? It will give you a lot of clue and insight as to how to run your simulation and how to fix it.
aqstax is offline   Reply With Quote

Old   July 29, 2012, 06:05
Default
  #51
New Member
 
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 4
monaya flower is on a distinguished road
hey aqstax
first ,thank
you for your reply. my upstream and downdtream boundaries are +3Dand -6D from the rotor centre .is this enough or should i increase it? yes my mesh is periodic . are you use 8.7 million cells for the whole domain or just for half domain ,i use 2.5 million for the half domain . what boundary condition did you use for the half cylinder and did you use hub or not ? and what turbulence intensity and viscosity ratio in the velocity boundary condition ?
and in your opinion what should i take care about it to get good results ?
monaya flower is offline   Reply With Quote

Old   July 29, 2012, 13:05
Default
  #52
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Quote:
Originally Posted by monaya flower View Post
hey aqstax
first ,thank
you for your reply. my upstream and downdtream boundaries are +3Dand -6D from the rotor centre .is this enough or should i increase it? yes my mesh is periodic . are you use 8.7 million cells for the whole domain or just for half domain ,i use 2.5 million for the half domain . what boundary condition did you use for the half cylinder and did you use hub or not ? and what turbulence intensity and viscosity ratio in the velocity boundary condition ?
and in your opinion what should i take care about it to get good results ?
I used 8.7 mil in periodic. My full domain was half the NASA-Ames wind tunnel, and rectangular in shape (read earlier posts in this thread). I did not use a hub, as the hub complicated the geometry too much and did not contribute much to the aerodynamics anyway. I used 0.5% TI and 10 for viscosity ratio. you can try symmetry for the outer domain, and outflow for the outlet domain. the thing that really matters is your mesh distribution. You have to keep trying till you get the right growth. There needs to be a good concentration around the rotor, and can ease up away from it.
aqstax is offline   Reply With Quote

Old   August 7, 2012, 18:40
Default
  #53
New Member
 
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 4
monaya flower is on a distinguished road
hey aqstax

thank you for your help.
now i used 8 million cells . with boundary layer , the first row is .00002 with 1.2 growth factor and 12 layers . i devided the domain to two domains ,small domain around the blade(i set it moving frame ) and the bigger domain (stationary) .and 5D for the upstream and 10D forthe down stream . i used MRF with relative velocity formulation (is that right ) . should i use kw sst with transition or without transition .
monaya flower is offline   Reply With Quote

Old   August 7, 2012, 18:56
Default
  #54
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Quote:
Originally Posted by monaya flower View Post
hey aqstax

thank you for your help.
now i used 8 million cells . with boundary layer , the first row is .00002 with 1.2 growth factor and 12 layers . i devided the domain to two domains ,small domain around the blade(i set it moving frame ) and the bigger domain (stationary) .and 5D for the upstream and 10D forthe down stream . i used MRF with relative velocity formulation (is that right ) . should i use kw sst with transition or without transition .
From what you're telling me, I guess with transition would be more advisable. Run the simulation once (will take you a few days for a decent convergence) using parallel processes (at least 4, but 6-8 would be better). Then check the y+ at the rotor (xy plot). if it is in the neither here nor there, then either refine your BL or dont use it. for k-w SST with transition, recommended is y+=1 otherwise y+<4-5 is acceptable. Also, first 10 layers must be within the region where local Re <200. Without transition, 30<y+<300, although values closer to 30 are more desirable.
aqstax is offline   Reply With Quote

Old   August 7, 2012, 19:16
Default
  #55
New Member
 
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 4
monaya flower is on a distinguished road
should i start the solution with k-epsilon and when it achieve some convergence use kw sst with transtion or start with kw sst with transition
.and what velocity formulation should i use relative or absolute (i use mrf)
monaya flower is offline   Reply With Quote

Old   August 12, 2012, 12:25
Default
  #56
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Quote:
Originally Posted by monaya flower View Post
should i start the solution with k-epsilon and when it achieve some convergence use kw sst with transtion or start with kw sst with transition
.and what velocity formulation should i use relative or absolute (i use mrf)
From my experience, while there are those who say relative velocity formulation is better, I found no particular difference. I would say absolute is easier to understand. In my opinion, changing the turbulence model is always a bad idea. The formulation is different, and when you change, you will find a big jump in the residuals for the turbulence parameters. In any case, there is no particular difference in speed of solution, since both are two-equation models. You could try a first-order scheme to speed up the solution and switch to second order when nearing convergence.
aqstax is offline   Reply With Quote

Old   December 28, 2012, 02:14
Default
  #57
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 4
Lacerlacer is on a distinguished road
Quote:
Originally Posted by aqstax View Post
dont set it to rotate. set the periodic boundary in the stationary domain to rotational and set its axis to the y-axis. for the stationary domain, set it's rotational axis, but leave it as stationary.
Hi,

I finally get my simulation correct. The solution found to be i was using a wrong geometry >.< After modify it to a proper one, i get my results very close to experimental one.
Lacerlacer is offline   Reply With Quote

Old   January 4, 2013, 15:18
Default
  #58
New Member
 
imad
Join Date: Dec 2012
Location: algiers
Posts: 1
Rep Power: 0
imothep is on a distinguished road
Quote:
Originally Posted by Lacerlacer View Post
Hi,

I finally get my simulation correct. The solution found to be i was using a wrong geometry >.< After modify it to a proper one, i get my results very close to experimental one.
hi
very close for the root bending moment also?
imothep is offline   Reply With Quote

Old   January 31, 2013, 21:13
Default
  #59
Member
 
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 44
Rep Power: 4
aqstax is on a distinguished road
Hi everyone, I'm terribly sorry for the late reply, as I've been busy getting married!

Lacer, that is fantastic to hear! It really is a frustrating process, but once you get it right, it gets faster the next time around!

Imhotep, generally, if your distribution of thrust force across the blade is similar, you will have similar root bending moments as well.

If anyone has any more queries, please do not hesitate to post here! I'll try to check in as often as possible. Also, feel free to drop me a personal message, but I'd prefer a post in the forum as more people can refer to it and learn from it.
aqstax is offline   Reply With Quote

Old   October 16, 2013, 13:19
Default
  #60
Member
 
Paulo
Join Date: Jun 2011
Posts: 31
Rep Power: 5
strobel is on a distinguished road
I'm trying do this simulation, but i'm getting around 60% of experimental values to power coefficient at 7 m/s. I refined mesh in upstream and downstrean and got any improvement. I'm doing full domain with around 32M elements. My y+ is fine (max=5) for SST. I have no idea what iwm doing wrong. I have suspicious that i'm using wrong geometry. Can anyone send me the geometry?
paulostrobel@gmail.com
Attached Images
File Type: jpg mesh_1.jpg (65.8 KB, 25 views)
File Type: jpg mesh_2.jpg (90.1 KB, 27 views)
strobel is offline   Reply With Quote

Reply

Tags
mrf, multiple reference frame, nrel, wind turbine

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
Torque of wind turbine simulation caohan FLUENT 8 August 11, 2014 23:01
Wind turbine simulation Saturn Main CFD Forum 1 June 12, 2006 03:57
CFX-TASCflow, wind turbine simulation Sac CFX 0 June 7, 2004 03:33
simulation of three dimensional flow in turbine md nizee Main CFD Forum 2 December 6, 2000 02:08
Turbine flow simulation data Mohan Varma Main CFD Forum 3 October 18, 1999 09:27


All times are GMT -4. The time now is 10:07.