Stuck again
 

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.

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.

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.

hey aqastax

thanks alot for your reply . are you egyptian

Haha, no I'm from Singapore

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.

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.

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.

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.

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?

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.

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