CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)

 LittleBart May 5, 2011 15:39

Meshing a blade inside air volume

Hi there!

I'm trying to make a good-looking mesh for my wind turbine study. It's a blade and 120 deg sector of surrounding air. The airfoil is linearized with shorty lines in order to eliminate high-order NURBS surfaces problem, which I had suffered much from previously.

I want to mesh it in ICEM but not sure what strategy to use for blocking. Actually there are too many faces with different angles and locations to do this manually. Is there any techniques to associate inner o-grid block to the blade surface with minimum movements?

http://i20.fastpic.ru/thumb/2011/050...1d402c82f.jpeg http://i20.fastpic.ru/thumb/2011/050...bc4f62a5c.jpeg

 PSYMN May 6, 2011 09:31

If you take a look thru my posts, we already went thru this with someone else and I posted a lot of blocking images...

Once your blocking is right, you may be able to snap fit (one click) the surface projected nodes around the airfoil down to the surface...

 LittleBart May 6, 2011 10:52

I've made a block as 3D bounding box around the air volume, then snapped the vertex to the corner points and linearized two top edges of the block to match the external surface of the geometry (it is seen on the second pic).

But then when I'm trying to use o-grid split, it always shows me "o-grid did not succeed" message and I'm not sure what to do, how to make o-grid properly?

I'll definitely look your posts through (doing now)...

thank you...

 PSYMN May 6, 2011 11:36

Are you starting with a 3D block or just a surface block on the outside of the ff surface?

If you didn't start with a 3D block, try some of the hexa tutorials first before tackling this model or it will crush you :eek: ;)

 LittleBart May 6, 2011 14:59

started with "3D bounding box" block initialization. The external faces were ok, but still don't how to make o-grid inside. It looks like that on th pic attached when I'm trying.

http://xmages.net/storage/10/1/0/6/4...b_3b1b8c37.jpg

still can't find the mentioned thread with similar case .. can you remember may the topic or the threader's name or some clue...

 PSYMN May 6, 2011 16:03

Previous posts...

5 Attachment(s)
You have collapsed the 3D block down to a wedge...

Don't do that.

Leave it as abox with three corners on corners and the 4th at the mid point of the arc.

Then Create the Ogrid with faces at the flat ends of the cylinder and the symmetry planes.

==================================

The previous thread was talking about "wind turbines"... I probably recommended "shifted periodic"... Some of the images had the name "Zaqie" on them... (that should give you some search terms)

here are some screen shots that were part of the previously posted threads.

 LittleBart May 6, 2011 16:16

Many thanks. The pics are grate... I remember the second one from the meshing tutorial but shifted periodic is not clear to me yet. I'm working on that.

Will definitely try and post here.

 LittleBart May 13, 2011 06:33

Hello Simon and everyone who is interested in such a case!

Thanks to your instructions to Zaqie, I was able to deal with blocking of my geometry. But I'v faced some problems because of slightly different geometry than this of Zaqie's.

1. I have little bit different orientation of the blade because of small angles of attack and pretty twisted shape (angle difference between the root and the tip is deg). Because of that the strategy proposed for blocking has lead to some messy regions on the tip and on long-chord sections after I had snapped all edges of these splits to the curves.

http://i2.fastpic.ru/thumb/2011/0513...33ebd3a55.jpeg http://i2.fastpic.ru/thumb/2011/0513...14322aab3.jpeg

2. But still, this blocking topology allowed my to build and tune premesh and I'm pretty satisfied with that. That's how I learned edge settings and splitting skills :)

http://i2.fastpic.ru/thumb/2011/0513...564a95ed2.jpeg

But when I'm trying to calculate surface meshes it ignores the premesh and is trying to calculate according to the predefined edge params and global sizing. Furthermore, when I'm trying to change the global sizing for parts it seams to ignore that and still trying to calculate with very high density which I don't want to have. I left my comp for a day calculating the mesh and I got it after 15 hours of calculations and its sizing was about 1 mm for the air part when global setting 100. Global mesh coeff is 1.

So the question is how to force the settings I gained in the premesh to become settings of the surface mesher and volume as the next step?

Thank you,

LittleBart

 Ahmed May 14, 2011 00:02

 LittleBart May 14, 2011 05:01

Thank you for reply and for the tutorial, it really was really helpful!

But it doesn't really show the transition from premesh settings to mesh params. Or I'm just do not understand the concept of premesh itself. Is it really like separate from the mash-tab mash and I don't need to calculate surface and volume meshes if I have pre-mesh done?
Here little context to make myself clear. I'm doing this mesh for my blade study which I want to do in CFX and therefore I want to output the mesh into CFX-readable file with separate regions for BCs.
So, do I need to calculate volume mesh on the mesh tab or I can just make premesh in bocking tab and then just output it into CFX file.

My apologies once again for probably stupid question but I'm really very new in it.

 PSYMN May 15, 2011 20:37

Convert to unstructured mesh...

Yes, the premesh already has everything (surface and volume mesh), you just need to convert it into the right format for your solver. Check the quality while in premesh, make sure everything is good and then right click on Premesh to output to unstructured mesh...

Then do unstructured mesh checks, etc.

This unstructured mesh can then be output to CFX...

Simon

 LittleBart May 17, 2011 09:20

Hi !

Thanks Simon for help and patience! Little more question on unstructured mesh - will it preserve regions for inlet/outlet surfaces as separate 2D regions for CFX BCs ?

Btw, now I feel like ready for scripting, thanx to you :).

 PSYMN May 17, 2011 10:46

That is what PARTS are for...

If the blocking face is associated with (projects to) the geometry of part "INLET" then its premesh and subsequent unstructured mesh, will also be in the part "inlet". This is just the default behavior. When you output, the output will also have the faces in the inlet part ready for your bocos.

Simon

 LittleBart June 22, 2011 09:50

Hello everyone!

After long vacations I'm again face to face with my blade problem and again asking for your help. Thank to Simon now I can build relatively stable and adjustable unconstructed mesh for the blade. And now I'm trying to model the problem in CFX (13). Actualy, this problem is my old one, the one that made me turning to ICM CFD and master the Mesh Skill. Thats because I thought that the results I've received are bad because of the bad mesh quality.

In my previous problem I've made a blade geometry and meshed it with CFX Mesh. The CFX problem had the following parameters:
http://i23.fastpic.ru/thumb/2011/062...fc8511e0a.jpeg

CF:
Z - rotational axis, X -

Domain:
1. Air - fluid domain - ref. pressure = 1 atm; fluid - air; CF - rotational cf with 13 rad/s velocity (expected velocity of the modeled blade at 10 m/s wind).
2. Blade - solid domain (Aluminum).

http://i23.fastpic.ru/thumb/2011/062...131d1ed6b.jpeg

BCs:
1. Inlet - inlet surface of the air volume - Velocity = 10 m/s
2. Outlet - outlet surface of the air volume - Static pressure = 0 atm. (= ref. pressure)
3. External surface - wall - no slip wall (FF)
4. Side surfaces - domain interface Air/Air - rotational periodicity
5. Air/Blade - domain interface - fluid/solid - frozen rotor

That was the model. And these are the results:

http://i23.fastpic.ru/thumb/2011/062...3a7fe0d13.jpeg

But my main question is quality of the blade. In order to answer this question I've tried to evaluate the overall Lift Force of the blade and, as a result, Momentum or Torque. In order to compare this force with the one calculated with beam element theory.

I've calculated this with an expression

and got the value of 13.4 N
http://i23.fastpic.ru/thumb/2011/062...22397e026.jpeg

And now I've made the same procedure with new mesh and result is 12.5 N which is proximately the same.
to be continue...

 LittleBart June 23, 2011 03:51

yeaah.. I'll better repost it to the CFX section

 Far October 7, 2012 10:43

Quote:
 Originally Posted by PSYMN (Post 307719) Yes, the premesh already has everything (surface and volume mesh), you just need to convert it into the right format for your solver. Check the quality while in premesh, make sure everything is good and then right click on Premesh to output to unstructured mesh... Then do unstructured mesh checks, etc. This unstructured mesh can then be output to CFX... Simon
Is there any difference between the quality in pre-mesh and unstructured mesh (which is also created from that premesh)?

 BrolY October 8, 2012 03:44

I think the pre-mesh doesn't check the quality for quads.
But the quality for unstructured mesh does check the quality for quads, unless you specify not to.

 PSYMN October 9, 2012 17:53

Yea, depending on the metric, there may be some small differences that you will see, and some metrics are only available in one, but not the other. Or as BrolY says, the unstructured quality can include the quality of Quads or other element types.

The important thing is just to be reasonably confident that your mesh is good enough for your solver before you bother moving the files around.

 nkme2007 October 10, 2012 05:51

Hello All,

I want to do analysis of heat transfer from water flowing through pipes submerged inside concrete. I am modelling in GAMBIT and wish to analyse it on Ansys FLUENT.

Can anybody help me out, how to model and simulate?

Does any tutorials exist?

 PSYMN October 10, 2012 09:20

@ nkme2007

Quote:
 I am modelling in GAMBIT
You hijacked a bunch of different threads with your question, please don't do that. it is annoying. Particularly when you jump on threads for ICEM CFD or ANSYS Meshing (we don't know much about Gambit anyway)...

Just create your own thread or possibly find a Gambit thread with a similar question and replay to that.

But in the end, you probably won't get any help anyway because your question is too broad, you may as well say "how do I do CFD?" Try some Fluent tutorials and start on your project. CFD-Online helps those who help themselves.

 All times are GMT -4. The time now is 16:01.