[aqstax]

Originally Posted by Lacerlacer

Yea, that's true. I had learnt to mesh the turbine and domain for more than half year. By the way, what kind of mesh u are using? I am using hybrid mesh. Boundary layer on the blade, and quite a coarse mesh for other place ( which contribute to the error ,half compare to experiment).

regards,
Lacer

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.

[Lacerlacer]

Originally Posted by aqstax

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.

Thanks for the reply. So the tet-unstructured work good for you. I shall try on the tet-unstructured as well as hex-structured mesh then. Have a nice day.

Regards,
Lacer

[Lacerlacer]

Originally Posted by aqstax

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

[aqstax]

Originally Posted by Lacerlacer

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.

[Lacerlacer]

Originally Posted by aqstax

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

[aqstax]

Originally Posted by Lacerlacer

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]

Originally Posted by aqstax

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.

[imothep]

Originally Posted by Lacerlacer

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?

[aqstax]

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.

[strobel]

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