[JonasII]

Hello everyone!
I'm working on vertical axis wind turbine modeling (VAWT) in Ansys CFX.
On my model turbine consists from 3 blades, everyone of them assigned as separate surface.
I need to get power/force/etc., both on the entire blade and on its sections.

For this I used the Iso Clip tool. Please see power by sections. (turbine located at 45 degree angle to the air flow)
Left and right blade sides divided to 8 sections, as a result, we have 16 sections on entire blade. Power data for each section is located above corresponding section on attached screenshot.
Total power from the left blade side: 111.0 [W]
Total power from the right blade side: -16.9 [W]
Total power: 94.1 [W]

Let's check calculations:
Iso clip entire blade (Blade length along Z axis from -2.37m to 2.37m)
So we get power on entire blade, calculated from Iso clip: ~94.1 [W]
If we use the same blade from mesh region.
We get power on entire blade, calculated from mesh region: ~-50.6 [W]

And what we have? If I use in my calculations geometry from Iso Clip tool, I have one result, if I use directly geometry from mesh region I have different result.

Please advice me.
Splitting blade by Iso Clip tool leads to loose accuracy?
What else (instead Iso Clip) I should use to get data from different blade sections? (without reconfiguring, splitting each blade to separate surfaces and then resolving model)

Thanks in advance.

[JonasII]

What about the problem, I mentioned before.
I have found limitations in CFD-Post help (CFD-Post interpolates results...):
limitations....JPG
Then I have splitted in my model every blade to 16 equivalent sections, also boundary layer of every blade section (in total, in model I have 48 identical sections in full wind turbine) has the same mesh. Thanks to this I can do precisely comparative analysis between different blades and their sections too.
Mesh of rotating domain:
mesh 01.jpg

Fine mesh in boundary layer:
mesh fine.jpg

Velocity in computation model on 90 degree wind direction:
velocity 90 deg.jpg

Splitted power on splitted blade (As modeling result):
Splitted blade power.jpg
If you have any questions, or you need additional info from modeling results, please write me, you're welcome!

[Opaque]

Not certain what you meant by loss of accuracy when using IsoClip tool.

The accuracy of your solution is determined by the original mesh selected for the simulation. Any calculation that is done consistent with the original discretization of the solver used should maintain/not increase the truncation error.

If you have already created a mesh with named regions for the section of interest, you should be able to use the same expressions you are using in CFD-Post in CFX-Pre and let the solver computes them for you.

Are you using an expression set that cannot be ported back to the CFX-Pre setup?

[ghorrocks]

In addition to Opaque's comment, some of your images look pretty blocky which suggests you are using a coarse mesh - at least away from the blades. You should do a mesh sensitivity study before looking at the numerical results in detail.

FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

[JonasII]

Originally Posted by opaque

not certain what you meant by loss of accuracy when using isoclip tool.

Thanks for your interest to this topic.

So, we have calculated model, in my case wind turbine. Every turbine blade is named.

If in CFD-Post calculations I use named geometry - I get one result, but if in CFD-Post calculations I use the same geometry, but after isoclip tool, i get another result (in this case Isoclip tool don't cutoff anything, cutting limits are greater than geometry dimensions).

So, as a result, if I need to know the data on the specific part of blade, i can't trust isoclip tool, instead I need to split geometry before meshing. And this splitted geometry use in future for data extraction in CFD-Post calculations.

Originally Posted by opaque

Are you using an expression set that cannot be ported back to the cfx-pre setup?

The most expressions I use, are from CFX-Pre stage.

[JonasII]

Originally Posted by ghorrocks

In addition to Opaque's comment, some of your images look pretty blocky which suggests you are using a coarse mesh - at least away from the blades. You should do a mesh sensitivity study before looking at the numerical results in detail.

FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Thanks for your interest!
Yes, on posted image mesh quality seems coarse, but actually there are 25 mesh layers on boundary layer, which height is 25mm. The first cell ∆y1 height is 0.075mm. Bias factor is 50. Y+ value = 9.375. Blade chord length is about 160mm.

According mesh study, which done through EVR distribution analysis, for my geometry and model settings, is enough first mesh cell ∆y1 = 0.2mm.
(I have attached some pictures).

Computation model mesh statistics (for info):
Rotating domain 10,7 M mesh elements
Stationary domain 2,5 M mesh elements

Thanks again for interest, and if I'm wrong, please advice me.

EVR 01.jpg
EVR 002.jpg

[ghorrocks]

Good to see you have checked your mesh close to the foil. But my comment was referring to the mesh away from the foil. You should check the mesh away from the foil as well.

[JonasII]

Originally Posted by ghorrocks

Good to see you have checked your mesh close to the foil. But my comment was referring to the mesh away from the foil. You should check the mesh away from the foil as well.

Hmm, it turns out I misunderstood you... Thanks for the clarification.
I have checked mesh away from blade too (on virtual border between interior space and outer side of the boundary layer near blade wall).
Thank you for helpful advises!