|
[Sponsors] |
April 22, 2012, 08:46 |
Stuck again
|
#41 | |
New Member
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 14 |
Quote:
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 |
||
April 24, 2012, 20:14 |
|
#42 | |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
Quote:
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. |
||
April 24, 2012, 22:45 |
|
#43 | |
New Member
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 14 |
Quote:
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 |
||
April 25, 2012, 07:56 |
|
#44 | |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
Quote:
|
||
July 13, 2012, 07:54 |
|
#45 |
New Member
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 14 |
hi aqstax
how did you create prismatic boundary layer in Gambit . i tried to do it but i can't |
|
July 16, 2012, 01:56 |
|
#46 | |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
Quote:
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. |
||
July 16, 2012, 13:33 |
|
#47 |
New Member
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 14 |
hey aqastax
thanks alot for your reply . are you egyptian |
|
July 19, 2012, 00:54 |
|
#48 |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
Haha, no I'm from Singapore
|
|
July 25, 2012, 17:00 |
|
#49 |
New Member
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 14 |
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 ? |
|
July 29, 2012, 02:21 |
|
#50 |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
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.
|
|
July 29, 2012, 07:05 |
|
#51 |
New Member
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 14 |
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 ? |
|
July 29, 2012, 14:05 |
|
#52 | |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
Quote:
|
||
August 7, 2012, 19:40 |
|
#53 |
New Member
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 14 |
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 . |
|
August 7, 2012, 19:56 |
|
#54 | |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
Quote:
|
||
August 7, 2012, 20:16 |
|
#55 |
New Member
monaya flower
Join Date: Jun 2012
Posts: 14
Rep Power: 14 |
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) |
|
August 12, 2012, 13:25 |
|
#56 |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
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.
|
|
December 28, 2012, 03:14 |
|
#57 | |
New Member
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 14 |
Quote:
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. |
||
January 4, 2013, 16:18 |
|
#58 |
New Member
imad
Join Date: Dec 2012
Location: algiers
Posts: 1
Rep Power: 0 |
||
January 31, 2013, 22:13 |
|
#59 |
Member
Abdulqadir Aziz
Join Date: Jan 2012
Posts: 45
Rep Power: 0 |
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. |
|
October 16, 2013, 14:19 |
|
#60 |
Member
Paulo
Join Date: Jun 2011
Posts: 34
Rep Power: 15 |
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 |
|
Tags |
mrf, multiple reference frame, nrel, wind turbine |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Torque of wind turbine simulation | caohan | FLUENT | 8 | August 12, 2014 00:01 |
Wind turbine simulation | Saturn | Main CFD Forum | 1 | June 12, 2006 04:57 |
CFX-TASCflow, wind turbine simulation | Sac | CFX | 0 | June 7, 2004 04:33 |
simulation of three dimensional flow in turbine | md nizee | Main CFD Forum | 2 | December 6, 2000 03:08 |
Turbine flow simulation data | Mohan Varma | Main CFD Forum | 3 | October 18, 1999 10:27 |