CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] 3D Wind turbine mesh

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

Like Tree2Likes
  • 1 Post By PSYMN
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   December 16, 2011, 06:24
Default 3D Wind turbine mesh
  #1
New Member
 
luxingzhe
Join Date: Feb 2011
Posts: 25
Rep Power: 6
luxingzhe is on a distinguished road
Dear All

I am planning to use sliding mesh model to simulate my wind tubine. i build the geometry in gambit, exported step file, and imported into ICEM for mesh. you can see from the step file that there are two parts( one is going to be stationary and the other is going to be rotating). I meshed the whole domain in ICEM, defined boundary condition, specially defined interfaces between the two domains. i ended up with 2.8 and 3.6 million elements for two different blocking strateries. however, i have problem reading the mesh in fluent, it gives me this error when building mesh in fluent : access violation. can anyone solve this problem for me?

Best Regards,
luxingzhe is offline   Reply With Quote

Old   December 16, 2011, 06:31
Default
  #2
New Member
 
luxingzhe
Join Date: Feb 2011
Posts: 25
Rep Power: 6
luxingzhe is on a distinguished road
Quote:
Originally Posted by luxingzhe View Post
Dear All

I am planning to use sliding mesh model to simulate my wind tubine. i build the geometry in gambit, exported step file, and imported into ICEM for mesh. you can see from the step file that there are two parts( one is going to be stationary and the other is going to be rotating). I meshed the whole domain in ICEM, defined boundary condition, specially defined interfaces between the two domains. i ended up with 2.8 and 3.6 million elements for two different blocking strateries. however, i have problem reading the mesh in fluent, it gives me this error when building mesh in fluent : access violation. can anyone solve this problem for me?

Best Regards,
Simon, it would be great if you can have a look at my problem.
luxingzhe is offline   Reply With Quote

Old   December 20, 2011, 17:17
Default
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hello, I had time for a quick look.

I noticed some penetration errors, but they were no big deal because you planned to have a sliding interface. However, while investigating the area I found that mesh from both sides was projecting to the same part...

See these pics...
Luxingzhe_01.jpg
Luxingzhe_02.jpg

Then I checked quality, I found some skew issues upstream of the leading edge. But for some strange reason, I had display problems when ever I turned on the blocking display... Under normal circumstances, I would have checked with a scan plane thru the problem area and then adjusted the edge distributions to match more closely between parallel edges in order to avoid the serious skewing of the mesh.

I think the edge display issues are related to how you did your blocking. You have put separate blocking in the same model and mixed up the index control... I would probably block the two halves separately (same model, 2 blockings). First block the blade and everything inside the disk. Then in a separate blocking on the same geometry, block everything outside the disk. You can load both into the same model as two sub-topologies, but you don't even need to. You could just merge the meshes later. Dealing with both topologies together like this must have been quite a hassle. Try it separate and you can make better use of index control, scan planes, etc. This would make it much easier to diagnose and tweak the blocking to get exactly what you want.

You said a simpler model had worked for you... Was it similar in that it had two zones blocked together like this?

Also, looking at the mesh topology of your blade, you have rounded tips, which would prompt me to try and put an ogrid in to capture that shape also... As it is, you will not be able to avoid some poor quality there (survivable, but poor).
luxingzhe likes this.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   December 20, 2011, 17:58
Default
  #4
New Member
 
luxingzhe
Join Date: Feb 2011
Posts: 25
Rep Power: 6
luxingzhe is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Hello, I had time for a quick look.

I noticed some penetration errors, but they were no big deal because you planned to have a sliding interface. However, while investigating the area I found that mesh from both sides was projecting to the same part...

See these pics...
Attachment 10502
Attachment 10503

Then I checked quality, I found some skew issues upstream of the leading edge. But for some strange reason, I had display problems when ever I turned on the blocking display... Under normal circumstances, I would have checked with a scan plane thru the problem area and then adjusted the edge distributions to match more closely between parallel edges in order to avoid the serious skewing of the mesh.

I think the edge display issues are related to how you did your blocking. You have put separate blocking in the same model and mixed up the index control... I would probably block the two halves separately (same model, 2 blockings). First block the blade and everything inside the disk. Then in a separate blocking on the same geometry, block everything outside the disk. You can load both into the same model as two sub-topologies, but you don't even need to. You could just merge the meshes later. Dealing with both topologies together like this must have been quite a hassle. Try it separate and you can make better use of index control, scan planes, etc. This would make it much easier to diagnose and tweak the blocking to get exactly what you want.

You said a simpler model had worked for you... Was it similar in that it had two zones blocked together like this?

Also, looking at the mesh topology of your blade, you have rounded tips, which would prompt me to try and put an ogrid in to capture that shape also... As it is, you will not be able to avoid some poor quality there (survivable, but poor).

Thanks for the reply, really appreciate that.
first of all, what do you mean by same model, two blocks. is it like you build a block around the blade and then build a bigger block for the inner domain, then ICEM will ask you whether you wanna merge them? (i will look into that and come back to you as soon as possible)

then, about the simper model, yes, i used the similar blocking strategy, that's why i decided to apply the strategy on my real model. the only differences are the model is smaller and the blade is cylinder which is much simper. i used the same blocking strategy, namely first block them together first, then split the whole block into two separate blocks (inner one and the outer one), then manipulate the two blocks separately. it is working fine~~that's why i have no idea why there is problem with building the mesh in fluent.

By the way, i sent you the one with different blocking strategy, namely build Ogrid around blade. i have the similar problem.

Regards,
luxingzhe is offline   Reply With Quote

Old   December 20, 2011, 18:33
Default
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
OK, so it is likely that doing it all in one model isn't the reason for your errors in Fluent (check the projections and mesh quality for that), but doing it as two separate blocking files will keep your index control much simpler and make it easier to diagnose and improve your mesh quality, projections, etc.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   December 21, 2011, 07:22
Default
  #6
New Member
 
luxingzhe
Join Date: Feb 2011
Posts: 25
Rep Power: 6
luxingzhe is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
OK, so it is likely that doing it all in one model isn't the reason for your errors in Fluent (check the projections and mesh quality for that), but doing it as two separate blocking files will keep your index control much simpler and make it easier to diagnose and improve your mesh quality, projections, etc.
hi Simon

i tried again, i think the problem must be the mesh, i got a few bad elements around the blade tip, which made the whole mesh unreadable. However, do you have better ways to block it? it would be great if you can figure out a better way of blocking for this model, i have been struggling for trying to mesh it nicely using ICEM.

Regards,
luxingzhe is offline   Reply With Quote

Old   December 22, 2011, 13:14
Default
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
It would probably be fairly straight forward, I just don't have time right now... I'll get back to it if I can.
luxingzhe likes this.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   December 26, 2011, 19:41
Default
  #8
New Member
 
luxingzhe
Join Date: Feb 2011
Posts: 25
Rep Power: 6
luxingzhe is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
It would probably be fairly straight forward, I just don't have time right now... I'll get back to it if I can.

hi, simon. i have to send you another message about the periodicy. I followed the right procedures seting up the periodicy in ICEM, and the mesh check shows no problems. but why doesn't Fluent allow me to set up the periodic zones?
i am looking forward to your reply.

Regards,
luxingzhe is offline   Reply With Quote

Old   December 28, 2011, 13:41
Default
  #9
New Member
 
luxingzhe
Join Date: Feb 2011
Posts: 25
Rep Power: 6
luxingzhe is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
It would probably be fairly straight forward, I just don't have time right now... I'll get back to it if I can.
Just to let you know that the problem is solved, i am now playing with Fluent, but it shows there are some elements with poor quality, which i hope doesn't influence the results too much.
Now i feel i am a little bit addicted to the Hexa volumn mesh from ICEM, thanks for the help anyway and have a nice vacation!
luxingzhe is offline   Reply With Quote

Old   February 24, 2012, 00:26
Default appreciate ur help
  #10
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by luxingzhe View Post
Just to let you know that the problem is solved, i am now playing with Fluent, but it shows there are some elements with poor quality, which i hope doesn't influence the results too much.
Now i feel i am a little bit addicted to the Hexa volumn mesh from ICEM, thanks for the help anyway and have a nice vacation!
Hi Luxingzhe,

May i know how u make it to able to import to fluent? i meshed the similar things(periodic boundary), somehow i get the access violation error when i import it to fluent. I did export to CFX version, and it works.

Regards,
LOH AC
Lacerlacer is offline   Reply With Quote

Old   February 24, 2012, 13:32
Default
  #11
New Member
 
luxingzhe
Join Date: Feb 2011
Posts: 25
Rep Power: 6
luxingzhe is on a distinguished road
Quote:
Originally Posted by Lacerlacer View Post
Hi Luxingzhe,

May i know how u make it to able to import to fluent? i meshed the similar things(periodic boundary), somehow i get the access violation error when i import it to fluent. I did export to CFX version, and it works.

Regards,
LOH AC
Not sure about your problem. did you mesh the model in ICEM, if you did, take very care attention to the periodicity (my problem regarding importing mesh into Fluent was due to periodicity), if you are sure there's no problem regarding the periodicity, then probably because of the elements type (Fluent doesn't support some specific types of elements) or the mesh quality. Still, if you meshed your model in ICEM, make full use of the mesh check, it almost could tell you everything. Hope it helps.

good luck
luxingzhe
luxingzhe is offline   Reply With Quote

Old   February 25, 2012, 07:18
Default
  #12
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by luxingzhe View Post
Not sure about your problem. did you mesh the model in ICEM, if you did, take very care attention to the periodicity (my problem regarding importing mesh into Fluent was due to periodicity), if you are sure there's no problem regarding the periodicity, then probably because of the elements type (Fluent doesn't support some specific types of elements) or the mesh quality. Still, if you meshed your model in ICEM, make full use of the mesh check, it almost could tell you everything. Hope it helps.

good luck
luxingzhe
Hi LuXingzhe,

Thanks for the reply. I am using ICEM CFD and periodicity for the mesh. I checked the mesh also, all 0.3 above, no negative and bad element. My mesh is all hexa elements. May u describe how u check regarding the periodicity problem? periodicity lead to bad element? Really thanks alot for ur input~

Regards,
LOH AC
Lacerlacer is offline   Reply With Quote

Old   February 25, 2012, 12:15
Default
  #13
New Member
 
luxingzhe
Join Date: Feb 2011
Posts: 25
Rep Power: 6
luxingzhe is on a distinguished road
Quote:
Originally Posted by Lacerlacer View Post
Hi LuXingzhe,

Thanks for the reply. I am using ICEM CFD and periodicity for the mesh. I checked the mesh also, all 0.3 above, no negative and bad element. My mesh is all hexa elements. May u describe how u check regarding the periodicity problem? periodicity lead to bad element? Really thanks alot for ur input~

Regards,
LOH AC
I suppose the strategy you used was this: block your domain, set the mesh parameters, pre-mesh, convert pre-mesh into unstructured mesh, then before you write fluent mesh file, go to mesh edit, where you can smooth your mesh, increase your mesh quality and of course check your mesh for some obvious problems.

hope it helps~~
luxingzhe is offline   Reply With Quote

Old   February 26, 2012, 00:51
Default
  #14
New Member
 
LOH AI CHOONG
Join Date: Dec 2011
Posts: 19
Rep Power: 5
Lacerlacer is on a distinguished road
Quote:
Originally Posted by luxingzhe View Post
I suppose the strategy you used was this: block your domain, set the mesh parameters, pre-mesh, convert pre-mesh into unstructured mesh, then before you write fluent mesh file, go to mesh edit, where you can smooth your mesh, increase your mesh quality and of course check your mesh for some obvious problems.

hope it helps~~
LuXingZhe,

Yaya, i did that. Mesh quality show 0.3 above. It should be good enough for fluent to process right? i am curious on the periodicity problem u mentioned. It suppose that we change one particular edge, then the block edges that subjected to periodic will change automatically right? I see that happened in my blocking.. U are trying to say that that automatic altering may lead to bad elements? or other things that u discover? Again~ really thanks for ur input. My University here dont have expert on that,i am totally in helpless ...

Regards,
LOH AC
Lacerlacer is offline   Reply With Quote

Old   May 15, 2012, 12:59
Default use mesh parameters
  #15
New Member
 
carlotta guerrini
Join Date: Oct 2011
Location: cranfield
Posts: 2
Rep Power: 0
carlotta is on a distinguished road
Hi everyone!
I'd like to know if there is the possibility for ICEM to use the curves and surface mesh set up from a previous mesh and use them for a new mesh with a different geometry (I;m using the same name for the same part). I need to do for slightly different geometries the same mesh. If you could help me I will really appreaciate.
Thanks
carlotta is offline   Reply With Quote

Old   May 16, 2012, 09:14
Default
  #16
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You can apply the properties from tetin file to another (so the mesh setup is already done), and you can apply the blocking from one to another... (easily associated the blocking to the new geometry)

You could keep the parts of the mesh that were the same, but we don't have a way to morph the mesh to fit a similar model. I think you can do that with RBFMorph.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   May 17, 2012, 05:40
Default
  #17
New Member
 
carlotta guerrini
Join Date: Oct 2011
Location: cranfield
Posts: 2
Rep Power: 0
carlotta is on a distinguished road
Thank you very much for the answer, unfortunately I need for similar geometry but not exactly the same. I will try with the program you suggested.
carlotta is offline   Reply With Quote

Reply

Tags
icem cfd, mesh

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
2D Simulation of Savonius Wind Turbine ravindersingh FLUENT 4 December 9, 2011 14:00
CFD analysis on wind turbine rotor Ken (Wind Turbine CFD Super Rookie) Main CFD Forum 42 July 18, 2011 22:11
Wind Turbine Blade Geometry SeanieB Main CFD Forum 0 November 27, 2009 11:18
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 01:34.