Meshing of a closed wing
 

Hi everyone,

I already posted about this in another forum for fluent. The idea is to create a mesh around a closed wing (with a naca0012 crossection) within a cylindrical enclosure. Aftera more experienced person told me that the automatic mesher isn't capable of meshing this geometry, I thought about trying it in ICEM.

My strategy is as follows and based on the pdf and youtube tutorials:

1. create a box around the whole geometry and associate the edges on the side (cylindrical enclosure with wing imported from workbench) the cylindrical enclosre

2. create o-grid split around the wing (with playing around a scaling factor of 1.9 seemed to com close to the wing) with a split block command at the trailing edge

3. associate the new edges to the leading and trailing edge

4. next I try to cut out a block within the wing and move the outher ones to a new part (solid_wing).

5. associate edges of inner square to leading and trailing edge and delete blocks contained in the solid_wing. When trying to associate the small edges (going in x-direction) to the wing surface, the command doesn't complete for some reason.

Unfortunately, when I come to the meshing step, an error message pops up about empty spaces even though the pre-mesh works. Can anybody please tell me if my strategy is correct or doable at all, or point out what I am missing? I can't imagine ICEM not being able to mesh this kind of geometry compared to other geometries I stumbled upon in the forum.

In case the pictures aren't loaded correctly here are two links to pictures which are hopefully helpful to get my idea across:

http://dl.dropbox.com/u/15410418/CFD...wing-ogrid.jpg
http://dl.dropbox.com/u/15410418/CFD...wing-strat.jpg

Thanks in advance for any advice and best regards,

Lukas

post ICEM files (tin and blk)

There is a partial electiricity blackout at our labs since yesterday evening. The computers are not connected to the internet, so the whole Ansys stuff does not work because it's unable to connect to the license server.

But I have some of the files which I believe should be the correct ones.

Best,
Lukas

The computers were running again this afternoon and I managed to create a more suitable (hopefully) geometry with associations and assignments except for the deleting process and the inner triangle is a bit more skewed...is this a correct procedure at all I am following here?

difficult to block with this method... i tought about this one:
-Change your geometry by splitting to half (for symmetry)
-initialzed blocking in 2D , block like a simple airfoil.
-change 2D blocking to 3d using the rotate function:
It gave me this :
https://dl.dropbox.com/u/35161486/lukaz.png

Here is the link of the projec:
https://dl.dropbox.com/u/35161486/lukaz.zip
i hope it can help

Thanks a lot for your fast help.

The idea of this project was to read in a geometry file from the design modeler and mesh it according to certain points with a script file in icem so different geometries (e.g. not a circular alignment, but elliptical) could be used. Or can the 2D mesh be extruded around a not perfectly circular airfoil? But it seems that it won't be possible within a reasonable time frame.

This is going to be my last resort;) May I ask how your procedure was? And if anybody could give me a hint on how to set the meshing parameters in a sensible way, would be great (I have the pdf, but couldn't understand the different parameters 100%).

Have a nice weekend!

I have used the top down approach, but missed one important step. That is creation of O-block before merging the vertices, going to upload corrected version soon.

Step are:

1. creation of main block

2. Split the block at leading edge, mid chord and trailing edge

3. Create O -block for the closed wing (lower side)

4. split in o-block to create the 2nd rows of edges for upper side of wing

5. change the material inside the wing to solid

7. Merge vertices at the trailing edge of wing

8 . Make association to curves and points.

9. I also merged vertices at leading edge to make it more elegant. (not necessary)

10. adjusted the edges and vertices

11. Made another o grid for inside wing (throughout the domain)

https://dl.dropbox.com/u/68746918/closedwing.zip

http://img17.imageshack.us/img17/8324/15048013.png
http://img535.imageshack.us/img535/1415/68874729.png
http://img411.imageshack.us/img411/3658/68072877.png
http://img268.imageshack.us/img268/9896/31449150.png
http://img651.imageshack.us/img651/1223/71975849.png

The top down approach is well applicable to elliptical path or whatever. You can automate the process in ICEM by recording the script and which can latter used in standalone or batch mode. I recommend you to write the python script (or matlab for windows level execution) to handle the workbench and TCL script.

Here is the refined blocking. still needs corrections in geometry

http://img692.imageshack.us/img692/5756/25166215.png

Thanks a lot Far,

I will try to redo the steps and record them into a script file. Any advice on the meshing parameters by chance (reasonable max size, height ratio ...)?

Best regards,

Lukas

Hi

I wanted to do it through 3d blocking (top down approach) and I feel it was difficult case. I find it interesting because, I feel same blocking can be used for the S-type intake where we dont have the option for the axi-symmetric. So I made preparation for my next assignment. :D;) (kidding). But once you master the top-down approach then next case can be done within no time.

However, the strategy used by diamondx is better in terms of its ease of use and at the end you get the same blocking with both approaches. I would like to address you concerns about the usability of this approach (diamondx's) regarding the non axi-symmetric wing i.e if it is not following the circular path as diamondx used the rotate option. There are three options available, one of them is extrude along the curve. Where you just need to select the curve and its end point. But I am not sure, if t also works for the curved path.

You can define the size based on length of your object. For example if the length of any object is X and you specify the max size as Y. Then no of nodes are X/Y along that curve. You can also define the height of first layer and its growth ratio by specifying the first height and height ratio.

But I usually use the edge mesh parameters for ICEM HEXA and part mesh parameters for the tetra+prism meshing.

Thanks a lot, really appreciate your help guys!

I will try to implement both approaches and see how the mesh and simulations turns out. Why not using files/projects you used to help others?;)

Best regards,

Lukas

:confused: didn't pick you point :o

I just thought because you said you were preparing your next assignment;)....Maybe I understood your comment differently...

Hopefully the last issues about meshing:o:

Did define certain edges separately?
Do I have to define all the parameters in the Part Mesh Setup which contain a number?
Did you use the Calculate Mesh function? Because when I use it, it says something about a hole in the mesh...or is it because of wrongely set mesh parameters?

Thanks and best regards,

lukas

I do not use part mesh setup for hexa.

How did you get that nice mesh in your pictures or which function did you use? I try to get the flowfield around and behind the wing but it seems I'm mixing some meshing concepts here.

Best regards,

Lukas

Just used edge meshing parameters, nothing else. But I guess, nice looking mesh might be due to my 1GB graphics card :D

I almost got something similar by now even though I don't think this computer is close to your hardware ;)

How did you get the "plate" view of the mesh which you used for the pictures?

Best regards,

lukas

This is done with the help of scan plane. For this right click on premesh and you will get options including scan plane. Once you have scan plane panel in front of you, select any edge and you get the mesh plane perpendicular to that edge.

They can be, if I move to Zurich Switzerland;)

Good one!:D

I have a question about my mesh. The statistics are in the picture. Is this a qualitatively good mesh for fluent (According to other forums the element quality should be at least 0.1 or 0.5)? Another point is the amount of elements. What is a reasonable size for an inviscid/viscid case? Because I think with this amount of nodes/elements, even on a cluster it'll take some time to solve.

Every time I try to locally smooth the bad parts, the computer runs out of memory, makes an emergency save and shuts down ICEM. Even by trying to export to Fluent it gets into a "not responding" mode. Any suggestions or hints?

Best regards,

Lukas