CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

How to split air blade in CFX Post without loosing accuracy

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 8, 2020, 06:32
Default 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
JonasII is on a distinguished road
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.
Attached Images
File Type: jpg Iso clip power_002.jpg (86.8 KB, 16 views)
File Type: jpg iso clip_003.jpg (86.8 KB, 13 views)
File Type: jpg From Iso Clip_004.jpg (80.3 KB, 11 views)
File Type: jpg mesh regions_005.jpg (96.3 KB, 8 views)
File Type: jpg From mesh region_006.jpg (74.4 KB, 6 views)
JonasII is offline   Reply With Quote

Old   May 12, 2021, 14:54
Default The problem solved
  #2
New Member
 
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5
JonasII is on a distinguished road
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!
JonasII is offline   Reply With Quote

Old   May 12, 2021, 17:10
Default
  #3
Senior Member
 
Join Date: Jun 2009
Posts: 1,865
Rep Power: 33
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   May 12, 2021, 19:38
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   May 13, 2021, 13:45
Default
  #5
New Member
 
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5
JonasII is on a distinguished road
Quote:
Originally Posted by opaque View Post
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.

Quote:
Originally Posted by opaque View Post
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 is offline   Reply With Quote

Old   May 13, 2021, 14:13
Default
  #6
New Member
 
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5
JonasII is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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
JonasII is offline   Reply With Quote

Old   May 13, 2021, 19:52
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   May 18, 2021, 17:54
Default
  #8
New Member
 
Ivan Shvolko
Join Date: Dec 2020
Location: Minsk
Posts: 7
Rep Power: 5
JonasII is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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!
JonasII is offline   Reply With Quote

Reply

Tags
blade sections, iso-clip

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 17:08.