CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] Dynamic Meshing of a 2D Airfoil (

Anonymized_JL1 March 8, 2010 02:35

Dynamic Meshing of a 2D Airfoil
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

PSYMN March 8, 2010 16:43

Can you post an image? Does it have any specific characteristics (such as a sharp trailing edge)?


Anonymized_JL1 March 9, 2010 01:06

Dynamic mesh of a 2D Airfoil
2 Attachment(s)
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

PSYMN March 9, 2010 11:27

Dynamic what?
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...

Anonymized_JL1 March 10, 2010 01:57

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

Thank you

PSYMN March 14, 2010 17:12

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.


Anonymized_JL1 March 15, 2010 08:56

in progress
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 March 17, 2010 09:02

Blocking of 2D moving Airfoil
4 Attachment(s)
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:)

PSYMN March 18, 2010 20:44

Not right at all...
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.

Anonymized_JL1 March 18, 2010 21:24

Airfoil Mesh
2 Attachment(s)
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.

Anonymized_JL1 March 26, 2010 11:18

there is no periodicity defined
3 Attachment(s)
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

PSYMN April 17, 2010 00:03

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...

I know it is late, but I hope it helps...

Anonymized_JL1 April 17, 2010 00:40

2 Attachment(s)
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

Anonymized_JL1 April 17, 2010 01:08

Simon I watched all three videos and I think now I can surely end up with a nice hexa meshing.

Thank you again

mjb28 April 19, 2010 18:09

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!

baggiovive May 12, 2010 05:14

perfect time even for me! great job simon! thank you so much!

jsm May 12, 2010 07:40


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,

Anonymized_JL1 May 22, 2010 17:39

Hex Mesh 2D VAWT
2 Attachment(s)
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.

Anonymized_JL1 May 22, 2010 17:43

Simon's reply to my Question
1 Attachment(s)
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

PSYMN May 22, 2010 18:32

How to delete line elements
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...

All times are GMT -4. The time now is 17:59.