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

[ICEM] Dynamic Meshing of a 2D Airfoil

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

Like Tree4Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 8, 2010, 02:35
Default Dynamic Meshing of a 2D Airfoil
  #1
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
I am currently working on my Thesis that basically involves making a dynamic mesh for 2D Airfoil. I need to simulate 2D unsteady airfoil for a wind turbine. I need to know how to do the dynamic meshing in ICEM CFD. please help me with this if possible.

Thank you

Last edited by jola; January 5, 2012 at 12:01.
Anonymized_JL1 is offline   Reply With Quote

Old   March 8, 2010, 16:43
Default
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Can you post an image? Does it have any specific characteristics (such as a sharp trailing edge)?

Simon
PSYMN is offline   Reply With Quote

Old   March 9, 2010, 01:06
Default Dynamic mesh of a 2D Airfoil
  #3
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
Airfoil (NACA 0018) has blunt trailing edge. also it is an unsteady airfoil so I need to make a moving mesh. please let me know the steps to make a dynamic mesh for it in ICEM CFD. Please find the attachment of Image of Airfoil geometry.

Thanks Simon
Attached Images
File Type: jpg NACA0018.JPG (12.3 KB, 597 views)
File Type: jpg Trailing Edge.JPG (9.4 KB, 507 views)
Anonymized_JL1 is offline   Reply With Quote

Old   March 9, 2010, 11:27
Default Dynamic what?
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
The meshing is no problem...

But the mesh would just be a static mesh...

By dynamic, do you mean that the flow is dynamic around a static airfoil or do you mean that the flow causes the airfoil to flutter? Would you be looking at one way FSI then and also need a structural mesh?

The latter would probably require some sort of mesh morphing for small changes.

If you mean to look at large changes (such as a control surface rotating), then you could use ICEM CFD scripting to block it once and then adjust the angle in the script. Another option would be to put the airfoil in a circle that you could then rotate the static mesh around the centroid.

For solver directed mesh morphing, I recommend you go to the solver forum and ask that question there. For a while, we did have a mesh morpher in ICEM CFD (MOM3D or Optimesh) but we eventually decided that mesh morphing was most efficiently done in the solver and we should focus on providing only the initial mesh.

Maybe someone else in this forum will have some good info for you...
PSYMN is offline   Reply With Quote

Old   March 10, 2010, 01:57
Default
  #5
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
Yes Simon, I need to simulate 2 Dimensional Vertical Axis Wind turbine. wind is blowing over the 3 blades of a Vertical Axis Wind turbine in a streamline flow. I have gone through few papers and found that I need to put the airfoil in a circle that will be rotating and this will be again surrounded by a static mesh this is the same what you suggested me. Please find the link this is what I need to do http://www.youtube.com/watch?v=1eyEtzdHDEE

Thank you
Anonymized_JL1 is offline   Reply With Quote

Old   March 14, 2010, 17:12
Default Right...
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Right, so it is just like meshing a regular static domain, except that it is in a circle... Then the entire circle is set to rotate. The surrounding mesh has the equivalent circle cut out of it, but it does not rotate.

The solver handles the interpolation along that boundary wall.

If you mean to do this in 2D, I would guess it shouldn't be a problem... You could even mesh a single 120 degree periodic section and then copy rotate it to get the other 2.

If you mean to mesh the 3D model, that geometry could get a bit tricky... You could still take advantage of periodicity and only mesh one blade, but you may want to try a few more tutorials to get your practice up before taking on that geometry.

Simon
PSYMN is offline   Reply With Quote

Old   March 15, 2010, 08:56
Default in progress
  #7
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
I have started working on Geometry and Meshing as per your suggestion. I'll let you know further if I encounter any problem.

Thank you Simon.
Anonymized_JL1 is offline   Reply With Quote

Old   March 17, 2010, 09:02
Default Blocking of 2D moving Airfoil
  #8
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
Hi, I followed your suggestions but now I am experiencing some problem meshing 2D Airfoil with the application of periodicity function. The steps I followed are:-
1. Plotted the geometry of NACA 0018 airfoil surrounded by a circular farfield.
2. Did some blocking to split the geometry then associated Vertex-> Point and Edge->Curve.
Now the questions I have is:-
1. How to use periodicity feature to make Inner circle rotating?
2. Do I need to use "O" Grid feature to get the mesh around the airfoil?

Please have a look at the images and give me some more idea about it. I have also uploaded the Project file. Could you please write the steps for me to do it if you find some time.
Thanks for reading this
Attached Images
File Type: jpg Blocking1.jpg (96.8 KB, 460 views)
File Type: jpg Blocking2.jpg (95.6 KB, 388 views)
File Type: jpg Blocking3.jpg (89.9 KB, 410 views)
Attached Files
File Type: zip Airfoil.zip (53.7 KB, 169 views)

Last edited by Anonymized_JL1; March 17, 2010 at 09:31.
Anonymized_JL1 is offline   Reply With Quote

Old   March 18, 2010, 20:44
Default Not right at all...
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I might come back to look at your file later (perhaps someone else has time to help?)

I thought you wanted to have three airfoils all orbiting a central point? In which case you could mesh just 1/3rd of the circle (120 degrees) with the airfoil out the appropriate distance from the center (just like in that Youtube video you sent) and then rotate it about the center. In that case, yes, you would want periodicity.

How ever, you just have an airfoil at the center of a circle... Do you intend to roate it about its center? There is nothing in this example to make periodic with anything else.

Also, it looks like you have not even tried to fit the edges to the geometry here... Not sure what is going on, but the pics don't look right at all.
PSYMN is offline   Reply With Quote

Old   March 18, 2010, 21:24
Default Airfoil Mesh
  #10
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
Hello Simon,
I am sorry about this post actually I am new to ICEM and meshing thing, now I am learning it. I exactly need to do the same what I had sent you on youtube before. I tried to do Hex meshing but found it complicated so I switched to Tet meshing. Here I have completed the Tet meshing just for single Airfoil (initially I was trying to do it just for one airfoil) but wondering how to set up Periodicity now as you said I need to have at least two airfoil to introduce periodicity. I am now meshing 120 degrees of section then will go accordingly. please have a look at the Tet meshing am not sure if it is ok.

Thank you so much for your time.
Attached Images
File Type: jpg Tet Mesh.jpg (97.4 KB, 451 views)
Attached Files
File Type: zip air1.zip (12.4 KB, 88 views)

Last edited by jola; January 5, 2012 at 12:06.
Anonymized_JL1 is offline   Reply With Quote

Old   March 26, 2010, 11:18
Default there is no periodicity defined
  #11
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
Hello Dear,

I tried to mesh 120 degrees section of my wind turbine with the application of periodicity but when I check the mesh for periodicity it says "there is no periodicity defined". I have already set up periodicity in the global mesh parameters and than after the surface blocking I made the vertices periodic still I get the same error.
could you also please tell me how to define boundary conditions for this geometry.
please have look at the tetin file for this project.

Thank you for your help
Attached Images
File Type: jpg 120 degrees section of wind turbine.jpg (99.7 KB, 361 views)
Attached Files
File Type: zip Airfoil.zip (15.3 KB, 111 views)
File Type: zip Airfoil Mesh.zip (86.7 KB, 148 views)
Anonymized_JL1 is offline   Reply With Quote

Old   April 17, 2010, 00:03
Default Finally...
  #12
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I FINALLY made a "how to" movie to answer this frequently asked question about meshing a 2D airfoil with ICEM CFD Hexa Blocking... The movie is in three parts actually.

They are on the ANSYS YouTube site...

http://www.youtube.com/ansysinc

I know it is late, but I hope it helps...
madmax98, jessiehu99 and dandoon like this.
PSYMN is offline   Reply With Quote

Old   April 17, 2010, 00:40
Default
  #13
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
Hi Simon,
Thank you so much for providing us with a great Video of airfoil meshing. I am done with my rotating mesh of 2D airfoil and even I am now able to simulate it but having some problems regarding the mesh smoothing near the airfoils edges. it would be great if you could just have a look at what I have done just to check it.
I have attached tin file I am unable to send you the mesh file its out of the limit.

Thank you so much
Attached Images
File Type: jpg image.jpg (97.2 KB, 417 views)
Attached Files
File Type: zip final1.zip (50.1 KB, 338 views)

Last edited by jola; January 5, 2012 at 12:06.
Anonymized_JL1 is offline   Reply With Quote

Old   April 17, 2010, 01:08
Default
  #14
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
Simon I watched all three videos and I think now I can surely end up with a nice hexa meshing.

Thank you again
Anonymized_JL1 is offline   Reply With Quote

Old   April 19, 2010, 18:09
Default
  #15
New Member
 
Join Date: Apr 2010
Posts: 3
Rep Power: 7
mjb28 is on a distinguished road
Simon, Thankyou so much for creating those videos. I have been trying to work out to create a C mesh around my wind turbine aerofoil for the last week and you have made the videos at the perfect time for me. They really helped. Thanks again!
mjb28 is offline   Reply With Quote

Old   May 12, 2010, 05:14
Default
  #16
New Member
 
Join Date: May 2010
Posts: 5
Rep Power: 7
baggiovive is on a distinguished road
perfect time even for me! great job simon! thank you so much!
baggiovive is offline   Reply With Quote

Old   May 12, 2010, 07:40
Default
  #17
jsm
Senior Member
 
JSM
Join Date: Mar 2009
Location: India
Posts: 155
Rep Power: 11
jsm is on a distinguished road
Hi,

Generally for dynamic mesh problems, tri mesh is preferred to avoid the remeshing problem while solving. I dont know how effectively solver will take quad elements. This is my thought that sharing with you

with regards,
JSM
__________________
With regards,
JSM
jsm is offline   Reply With Quote

Old   May 22, 2010, 17:39
Default Hex Mesh 2D VAWT
  #18
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
Hi Simon,

With the help of your videos I am now able to make Hexa mesh of 2D Wind Turbine but now I am having trouble assigning the boundary condition in Fluent. I guess the problem is when I convert Structured Hexa mesh to Unstructured mesh, it automatically creates LINES under the Mesh tab in display tree and then Fluent considers those lines as a Boundary condition. so my question is how can I get rid of those lines and have the same BC as I assigned them in ICEM?

Attached is the Tin and Blk files.

Thank you.
Attached Images
File Type: jpg VAWT 120 degree.jpg (87.3 KB, 388 views)
File Type: jpg VAWT 360 degree.jpg (66.6 KB, 326 views)
Anonymized_JL1 is offline   Reply With Quote

Old   May 22, 2010, 17:43
Default Simon's reply to my Question
  #19
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
Anonymized_JL1 is on a distinguished road
I am glad you have made progress.


First, regarding this mesh, you really need the mesh around the airfoil to be much much finer or it simply won't capture your physics. That central Ogrid should have a lot more elements and a much smaller height at the airfoil (side 2). You also need to match edges and all that to get a smoother transition. I would also set the growth rates to no higher than 1.2. I also moved the verts around the Ogrid to have better internal angles (45 degrees is as good as you can get).



Smoothing wouldn't hurt either.



And you could probably also improve your quality at the trailing edge by actually chopping off (or rounding) the tip and associating the blocking with a geometry that is a better match. In this case, you have a blunt blocking struggling to fit to a sharp geometry and this inevitably results in poor quality.

Now to your question. I am not understanding why you want to get rid of those lines. Those line elements are good... Fluent needs them to hang the bocos on. In fact, you could use a few more. Are you copy rotating this mesh and then seeing the Geom part as "in the way"? It would be more effecient to send just the single sector to Fluent and user periodic bocos. I would take the "Geom" side cuves and put each into its own part, PER1 and PER2. Then on the output menu, select the solver and then apply bocos to those curve part names. Then when you get to fluent, you will be properly setup.

If I am not quite getting your question, please rephrase or add some screen shots so I can see the problem.

Simon Pereira
Product Manager
Attached Images
File Type: jpg VAWT smoothing.jpg (80.2 KB, 342 views)

Last edited by jola; January 5, 2012 at 12:08.
Anonymized_JL1 is offline   Reply With Quote

Old   May 22, 2010, 18:32
Default How to delete line elements
  #20
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Thanks for posting the Q&A so others could benefit...

I think I get your question now. You were copying the mesh before going to Fluent and then needed to get rid of those sides that end up between each section. I hope you understood the suggestion to use periodicity to your advantage, but that only applies if you were just planning to simulate this circular domain. If I think back to the youtube video you sent me at the start, you may be planning to rotate this circle within some larger domain... In which case, your copy/rotate plan may be a good one.

So, now that I get your original question, I can answer it.

After doing the copy rotate, you should merge the nodes along the boundary. User Edit Mesh => Merge Nodes => merge Nodes with a tolerance. Put a very small tolerance in (smaller than any element side) and turn on "ignore projections". You should make sure to do a check for single edges and make sure they are at the perimeter of the circle only and not along the 120 degree seams. Once your mesh is a nice connected disk, you can turn off the shells in the model tree and make sure the "lines" are on. (also turn off the curves to get them out the way) You should see lines elements on the screen. You will have your hub, your shroud and your three airfoils. You may also have your radial lines which were in the Geom Part. You can simply delete those lines. If you only have those shells in Geom, you can use the selection tool bar to select by part, or you could just select them with a window or what ever...

Make sure to run all the checks again at the end...

Then you can go ahead and mesh the surrounding domain... Put its shells in a different volume part (like FLUID2), then load both meshes into the same session. Just don't actually merge it node for node with this rotating one... Then output to solver...
dandoon likes this.

Last edited by jola; January 5, 2012 at 12:07.
PSYMN is offline   Reply With Quote

Reply

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
Airfoil Meshing Scheme in Gambit J. Weiler FLUENT 6 October 2, 2011 15:41
Dynamic meshing Manoj Kumar FLUENT 3 June 27, 2010 19:26
[GAMBIT] Meshing airfoil using .dat file problem creggie ANSYS Meshing & Geometry 10 June 27, 2010 19:24
[GAMBIT] Dynamic Meshing of a combustion chamber donarundas ANSYS Meshing & Geometry 1 December 2, 2009 08:13
help for dynamic meshing for incylinder combustion Ramesh K FLUENT 0 June 19, 2006 06:29


All times are GMT -4. The time now is 07:48.