CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Box in a Box (http://www.cfd-online.com/Forums/ansys-meshing/77377-box-box.html)

FabioT June 21, 2010 17:59

Box in a Box
 
Hi,
I need to mesh a building in a wind tunnel with ICEM 12.1.
Basically it is a box in a larger box.

How can I mesh so that, once I import in Fluid 12.1, he will consider the building rigid but will give me the pressure on the walls?

Thank you,

Fabio

FabioT June 21, 2010 18:00

Obviously it is a 3D problem.
If you have any tutorial explaing how to mesh something like that, please let me know.


thanks,

fabio

PSYMN June 22, 2010 10:11

Default
 
That is just the default situation. If you mesh with ICEM CFD (or pretty much any mesher), you will end up with shells on the walls of the building (all the boundaries of the volume actually). If you don't assign them a specific Boco, they will be assumed as walls. In Fluent, you can be more specific about the properties of the walls, but even there you can probably go with the default.

Now, if you wanted the opposite (a non rigid building that could flex with fluid structure interaction, that would take some more care ;)

Simon

FabioT June 22, 2010 13:12

1 Attachment(s)
Ok, thank you, but I still have some problems (it is the first time I use ICEM).

I've done the geometry and the blocks for the mesh, but i'm not really sure what is the best way to "Associate" after I split the blocks.
Should I do it with point by point or there is a more easy way?

Moreover I don't know how to associate the surfaces with the faces, because there are some internal faces between blocks that do not correspond with any geometrical part but only to another face of an adiacent block.

I hope you can understand what i've said: the attachment can help.

Thank you very much for any reply,

Fabio

PSYMN June 22, 2010 14:00

When you split a block, the new internal edges should be CYAN (blue) because the blocks on either side of the split are in the same blocking part (such as FLUID).

When I look at your image, it already looks wrong because all your internal edges are black, which means they are projected to surface. I am guessing that the only surfaces inside the volume are down in the tiny block in the middle of the base.

I suggest a start over ;)

1) Create block, apply. This will create a block perfectly aligned with your outer block.

2) Associate the outer edges with the curves of the large box. If we do this now, there will be fewer clicks than to associate these edges after we have split them.

3) Associate the corner verts to the corner points. This is not necessary, an experienced user could skip this step, but it helps newbies get all the corners properly.

4) Split the big block to capture the little block. This is two splits in X and Y and then 1 split just above the block in Z.

5) Zoom in and repeat steps 2) and 3) with the little block.

6) Delete the little block (Blocking => Delete blocks) (but not with the permanent option). This is probably the key step you were missing. This changes the blocking material for the inner block from FLUID (or whatever it was) to VORFN. As soon as the blocking detects a difference, it will immediately associate all the faces between those materials (the faces of your building) with the nearest part. This will give you shells in your building part and you should be all set.

6-alternate) you could chose to put the building into a different material instead of deleting that block. You could create a new material (SOLID) and "add blocking material to part". This would give the same result, except you would have the option to output the building mesh.

7) Setup mesh parameters.

8) Optionally, you could create an Ogrid around your building as a boundary layer.


Go and do some tutorials. They will get you going and save a ton of frustration. Start with something 2D for the basics, and then try a couple 3D ones.

Best regards,

Simon

FabioT June 22, 2010 16:52

Hi, I think i did it. I was going crazy because there was something wrong at the beginning...

I'm sure i will come up with some more questions sooner or later..

bye,

Fabio

PSYMN June 22, 2010 17:04

Tutorials...
 
Try some tutorials and you won't have any questions until later... (rather than sooner ;) )

Simon

FabioT June 23, 2010 12:21

Hi, thank you very much Simon!
I have done the mesh and I think it is fine.

I have now to import it in Fluent 12.1 but i am not really sure how to do it. Do I have to save the mesh in a particular format after i did it in ICEM?

What kind of mesh would you suggest?

Thank you again,

Fabio

FabioT June 23, 2010 13:19

3 Attachment(s)
By the way, this is what I've doneup till now.
My only doubt is the box in the middle: ICEM meshes also that part, but i don't want to consider it.

In the last post you told me that I should be fine, but I still don't understand why ICEM meshes also that.

I've already found how to import the whole mesh in Fluent.

Thank you,

Fabio

PSYMN June 23, 2010 14:28

Basic steps...
 
You really need to go thru a tutorial :eek:

Your first two images show that you were doing hexa blocking... But the 3rd image shows tetra (totally wrong process) and the cube wasn't even captured.

Are you trying to generate a tetra mesh or a hexa mesh? Even a basic tutorial will get you thru either.

Once you have an unstructured mesh (this step will be shown in every tutorial), you can go to the output tab. Select the solver first (you should probably pick Fluent). The next icon over lets you set up boundary conditions. The default setting is wall. Then output to Fluent... ICEM CFD will write out a fluent.msh file that you can read into the Fluent solver (or into TGRID or whatever).


All times are GMT -4. The time now is 10:44.