Brick mesh vs. tets 1

[Robert000]

Hi all,

I have some problems with brick meshing.

Anlyze type: Flotran CFD
Element: FLUID 142
Material: Air
Geometry: block in the middle bottom of the block boundary
Aim: to get accurate results of pressure coefficients (values+distribution)

Questions:

1. How is it possible to apply brick meshing?
2. What gives better results: bricks vs. tets?

Thanks a lot

Robert

 

[Stringmaker]

I'm having a tough time visualizing from you description what it is that you're trying to model exactly but to answer your questions in a general sense:

A1) Brick elements can be formed by either creating a mapped mesh of FLUID142 elements or by taking FLUID141 2-D elements and extruding these.

A2) I think the Ansys documentation sums this one up best:

"You will need to make assumptions about where the gradients are expected to be the highest, and you must adjust the mesh accordingly. For example, if you are using the turbulence model, then the region near the walls must have a much denser mesh than would be needed for a laminar problem. If it is too coarse, the original mesh may not capture significant effects brought about through steep gradients in the solution. Conversely, elements may have very large aspect ratios with the long sides along directions with very low gradients.

For the most accurate results, use mapped meshing. It more effectively maintains a consistent mesh pattern along the boundary. You can do this by issuing the command MSHKEY,1 (Main Menu> Preprocessor> Meshing> Mesh> entity> Mapped).

In some cases, you may wish to use hexahedral elements to capture detail in high-gradient regions and tetrahedral elements in less critical regions. As described in Creating Transitional Pyramid Elements in the ANSYS Modeling and Meshing Guide you can instruct ANSYS to automatically create pyramid elements at the interface.

For flow analysis, especially turbulent, you should not use pyramid elements in the region near the walls because it may lead to inaccuracies in the solution.

Wedge elements can be useful when a complex area can be easily meshed with triangles that are then extruded. For a quick solution, you can use wedge elements in the region near the walls. However, for accurate results, you should use hexahedral elements in those regions.

Wedge elements are considered to be degenerate hexahedral elements. When using the ANSYS MeshTool (Main Menu> Preprocessor> Meshing> MeshTool) to sweep triangles into wedges, you must select Hex elements."

Good luck,
-Brian

 

[Robert000]

I would like to compare lift and drag coefficients
on the simple shape model with values defined by standards.
After creating the mesh, I will define turbulent model
k-epsilon. Giving the velocity and boundary conditions will follow this step.

But my problem is in creating the brick mesh, because
"Volume 3 has an invalid topology for brick meshing" error
appears.

Volume 3 is creating by substracting the rectangular object
from the rectangular boundary.

How can I find a same example, or step by step method
of creating the brick mesh?

Thanks,

Robert

 

[meshparts]

Hallo Robert,

You must subdivide the area with the property of air into four (or three) trapezes. Then mapped meshing will work!

Regards,
Alex

PS: I would generate the geometry by the 'a' command, instead of 'rectng'.

 

[Robert000]

Hi Alex,

subdividing the area, not the volume into regular parts????

How could I do this, I don´t use it before.

Thanks

Robert

 

[meshparts]

Sorry, my explanation was for a 2D case. But in 3D it works the same. You just have to subdivide the sourunding air into 5 frustum of pyramids (one on top of the block). In the middle lies the block.

 

[meshparts]

Hi again,

Your problem is hopefully solved. Here the code:

aa=1
bb=1
cc=1

dd=0.25
ee=0.25
ff=0.25

/prep7

k,1,-aa/2,-bb/2,0
k,2,aa/2,-bb/2,0
k,3,aa/2,bb/2,0
k,4,-aa/2,bb/2,0

k,5,-aa/2,-bb/2,cc
k,6,aa/2,-bb/2,cc
k,7,aa/2,bb/2,cc
k,8,-aa/2,bb/2,cc

k,9,-dd/2,-ee/2,0
k,10,dd/2,-ee/2,0
k,11,dd/2,ee/2,0
k,12,-dd/2,ee/2,0

k,13,-dd/2,-ee/2,ff
k,14,dd/2,-ee/2,ff
k,15,dd/2,ee/2,ff
k,16,-dd/2,ee/2,ff

v,9,10,11,12,13,14,15,16 ! bloc in the middle
v,5,6,7,8,13,14,15,16 ! pyramid on the top of block
v,1,2,6,5,9,10,14,13 ! pyramid around the block
v,2,3,7,6,10,11,15,14 ! pyramid around the block
v,3,4,8,7,11,12,16,15 ! pyramid around the block
v,4,8,5,1,12,16,13,9 ! pyramid around the block

et,1,solid45
esize,0.1
mshkey,1
vmesh,all

Regards,
Alex

 

[Robert000]

Yes Alex, this is what I exactly need.

I tried another way of solution:
dividing the volume into blocks by working plane.
That means that I got 9 blocks.
After that I tried to mesh them.
The block in the middle was succesfully meshed,
but the same error (invalid topology) appeared for
the others. I don´t know why?

Thanks,

Robert

 

[meshparts]

If you are doing it right, it must work! The comand for dividing by workingplane should sound like this:

vsbw,all,delete

The keyword 'delete' is important!

 

[Robert000]

I create another cutting plane on the above
area of the rectangular object.
So I have now 17 blocks(9x2-1), 5 cutting planes
(rect. object is not meshed).
I use vsbw,all,delete and the brick meshing works now.

Thank you Alex.

Robert