|
[Sponsors] |
How to split air blade in CFX Post without loosing accuracy |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 8, 2020, 06:32 |
How to split air blade in CFX Post without loosing accuracy
|
#1 |
New Member
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5 |
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. |
|
May 12, 2021, 14:54 |
The problem solved
|
#2 |
New Member
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5 |
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! |
|
May 12, 2021, 17:10 |
|
#3 |
Senior Member
Join Date: Jun 2009
Posts: 1,865
Rep Power: 33 |
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?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
May 12, 2021, 19:38 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 |
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
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
May 13, 2021, 13:45 |
|
#5 | |
New Member
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5 |
Quote:
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. The most expressions I use, are from CFX-Pre stage. |
||
May 13, 2021, 14:13 |
|
#6 | |
New Member
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5 |
Quote:
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 |
||
May 13, 2021, 19:52 |
|
#7 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144 |
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
May 18, 2021, 17:54 |
|
#8 | |
New Member
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5 |
Quote:
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! |
||
Tags |
blade sections, iso-clip |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
how to split a surface in CFX POST | mohammad | CFX | 10 | February 7, 2018 03:11 |
Error reading profile data in expression in cfx post | banu | CFX | 4 | March 27, 2015 10:03 |
Turbine Blade Flutter additional Varialbles display error in CFX post | sagarparikh31 | CFX | 8 | January 27, 2015 08:22 |
CFX Air conditioning Simulation_expression help!!!! Urgen!!! | yin2 | CFX | 6 | March 31, 2009 00:34 |
creating expresions in cfx build or cfx post | alex | CFX | 1 | August 22, 2002 14:01 |