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/)
-   -   [GAMBIT] 3D Mesh for complex structure (http://www.cfd-online.com/Forums/ansys-meshing/109310-3d-mesh-complex-structure.html)

Shinobi November 14, 2012 14:03

3D Mesh for complex structure
 
3 Attachment(s)
Hi guys,
I have a great problem with a complex structure. It is a very thin structure.
When I mesh this volumes wiht Hybrid volumes, I have this problem:
:confused:
WARN: Triangle meshing reached specified maximum number of mesh faces: 100000.
An incomplete mesh may have been generated. You can modify this behaviour
by changing the value of default MESH.TRIMESH.MAX_FACES.
WARN: Triangle meshing reached specified maximum number of mesh faces: 100000.
An incomplete mesh may have been generated. You can modify this behaviour
by changing the value of default MESH.TRIMESH.MAX_FACES.
No cells created, must be hole in surface meshERROR: TG_Mesh_Domain failed with error code 1.
ERROR: Tetrahedral meshing has failed for volume volume.85.
This is usually caused by problems in the face meshes.
Check the skewnesses of your face meshes and make sure
the face mesh sizes are not too large in areas of
small gaps.


How should work to solve the problem?

P.S. Model is an IGES import from Catia.

-mAx- November 15, 2012 03:05

If you read the errors, you should understand that Gambit is meshing a surface with more than the specified max limit
So you can increase this limit in defaults panel, or you can decrease the element size of your mesh.
If you are limited with your hardware, maybe you should consider your thin elements as baffle (shell).

Shinobi November 15, 2012 03:56

Quote:

Originally Posted by -mAx- (Post 392193)
If you read the errors, you should understand that Gambit is meshing a surface with more than the specified max limit
So you can increase this limit in defaults panel, or you can decrease the element size of your mesh.
If you are limited with your hardware, maybe you should consider your thin elements as baffle (shell).

Thanks for reply.
In menu MESH-->TRIMESH-->MAX_FACES I have modified value 100000 with -1 so Gambit insert automatically number of faces for each case.
To mesh without skewed elements, I must insert 1 as interval size during Tet/Hybrid mesh.
I set up BC but in fluent no convergency.
So I remember you that all volumes after import in GAMBIT
were mutually superposed. For this reason I have substracted the part of volume excess to volume that must be cut in the realization. So I can mesh them singly because if I unite them, I cannot mesh them for problems of healing.
To solve this problem I can use panel 'geometry cleanup' but GAMBIT creates several virtual_faces and convert volume in virtual_volume that I cannot connect.
Volumes cannot be converted in real volumes for ACIS error.
So I have volume disconneted and Fluent cannot converge.

I have a portable pc with processor Intel(R) Core(TM)2 Duo CPU P8400 @2.26 GHz 2.27 GHz with RAM 4GB and Hard disk 232 GB (124 GB are used). IN defaults of Gambit I can modify resource of software to increase his performance?
Can you tell me what do you mean thin elements as shell?
Thanks!
:-)

-mAx- November 15, 2012 04:11

Quote:

Originally Posted by Shinobi (Post 392197)
So I remember you that all volumes after import in GAMBIT were mutually superposed. For this reason I have substracted the part of volume excess to volume that must be cut in the realization. So I can mesh them singly because if I unite them, I cannot mesh them for problems of healing.

Can you developp that with pictures

Shinobi November 15, 2012 05:59

1 Attachment(s)
Quote:

Originally Posted by -mAx- (Post 392203)
Can you developp that with pictures

Ok, I describe you all phases.
I import Iges file with Heal Geometry and Make tolerant.
No selected options for stand alone Geometry (but also for them I have same problems) and no select virtual clean Up.
After import, not all volumes are recognized, so I must stitch faces.
(There are coincident faces).
Anyway I unite volume because in first analisys I can assume all volumes with same materials.
When I unite volumes as in picture, GAMBIT tell me:
WARN: Problematic geometry reported for volume volume.14.
WARN: There are output entities with badly checking geometry.
But it unites volumes.
I mesh
the single volume (volume 14) that remains. But I have this message:
Command> volume mesh "volume.14" tetrahedral size 1

Mesh of face face.315 contains 28 highly skewed elements (EQUISIZE SKEW > 0.97).

Mesh of face face.691 contains 47 highly skewed elements (EQUISIZE SKEW > 0.97).

Mesh of face face.365 contains 36 highly skewed elements (EQUISIZE SKEW > 0.97).

Mesh of face face.704 contains 36 highly skewed elements (EQUISIZE SKEW > 0.97).

Mesh of face face.274 contains 47 highly skewed elements (EQUISIZE SKEW > 0.97).

Mesh of face face.678 contains 44 highly skewed elements (EQUISIZE SKEW > 0.97).
WARN: Triangle meshing reached specified maximum number of mesh faces: 500000.
An incomplete mesh may have been generated. You can modify this behaviour
by changing the value of default MESH.TRIMESH.MAX_FACES.

Mesh of face face.578 contains 2 highly skewed elements (EQUISIZE SKEW > 0.97).
ERROR: Unable to allocate 4194304 bytes of dynamic memory
ERROR: Out of memory while meshing face.715.
ERROR: Out of memory while meshing volume.14.


So I change volume MESH-->TRIMESH-->MAX_FACES with -1 and re-mesh it. I have no problem for incomplete mesh but I go out of memory and GAMBIT crash.
:(
For this reason I chose not to join volumes to mesh every single volume.
But after I cannot connect mesh

-mAx- November 15, 2012 06:05

independantly to your skewness and max elements, are you importing solid parts?
Because in your description I don t see any step where you are extracting fluid domain
If you can try to export step or sat from catia (better quality with volume directly imported)

Shinobi November 15, 2012 06:39

3 Attachment(s)
Quote:

Originally Posted by -mAx- (Post 392229)
independantly to your skewness and max elements, are you importing solid parts?
Because in your description I don t see any step where you are extracting fluid domain
If you can try to export step or sat from catia (better quality with volume directly imported)

This is figure of import.
Yes they are all solid part.
First step is heat transfer ot that structure (I post here part of structure).
I assume a T_ext of outer face's stringers and T_int on internal face of frame. I suppose that I should not remove any fluid domain, or wrong?
I cannot try to export step or sat from catia, I have only that model.
Case in exam is similar to second image, third is the particular case post here, but without hole and pins because material is not alloy aluminum.

-mAx- November 15, 2012 06:43

are you not solving NS-equations?

Shinobi November 15, 2012 06:58

Quote:

Originally Posted by -mAx- (Post 392235)
are you not solving NS-equations?

Goal in first step is resolve a simple Fourier's law, but in 3D analysis. So I have laminar viscous.

-mAx- November 16, 2012 02:37

2 Attachment(s)
ok I import your igs file.
With a volume decomposition (splits) you are able to mesh it (without any errors)
I don't have time to mesh it full hexa and fine
:rolleyes:
Attachment 17004

Attachment 17005

Shinobi November 16, 2012 05:27

Quote:

Originally Posted by -mAx- (Post 392442)
ok I import your igs file.
With a volume decomposition (splits) you are able to mesh it (without any errors)
I don't have time to mesh it full hexa and fine
:rolleyes:
Attachment 17004

Attachment 17005

GREAT MAX!
:-)

A question:
I create brick to split and after move it to interested area or can be done more quickly?

-mAx- November 16, 2012 05:32

basically I united the radial part with the beam
then I splitted the volume with 2 planes for isolating the green and yellow beams
Finally, as you described, I created a brick, I placed it in the requested area and I splitted the remaining volume with the brick. It has created the blue and pink volume.

Shinobi November 16, 2012 05:42

Quote:

Originally Posted by -mAx- (Post 392463)
basically I united the radial part with the beam
then I splitted the volume with 2 planes for isolating the green and yellow beams
Finally, as you described, I created a brick, I placed it in the requested area and I splitted the remaining volume with the brick. It has created the blue and pink volume.

how can I put a plan?
I suppose a face, but it requires points.
Sorry but I am a noob with GAMBIT.

-mAx- November 16, 2012 06:07

yes I meant face >> http://aerojet.engr.ucdavis.edu/gamb...om_face_create

Shinobi November 16, 2012 06:55

1 Attachment(s)
Quote:

Originally Posted by -mAx- (Post 392475)

Creation of Plane between blue and green solid

a)create a face
b)translate face, but coordinates?
I have 4 points between blue and green solid, but that face doesn't include all green solid so I cannot split.

-mAx- November 16, 2012 07:05

use summarize tool >> http://aerojet.engr.ucdavis.edu/gamb...ck_query_total

pick desired vertex for knowing your translation vector.
Then create your face (it should be greater than your beam section, otherwise the split won't be correct.
Then move the generated face with your vector.

Shinobi November 16, 2012 07:30

Quote:

Originally Posted by -mAx- (Post 392491)
use summarize tool >> http://aerojet.engr.ucdavis.edu/gamb...ck_query_total

pick desired vertex for knowing your translation vector.
Then create your face (it should be greater than your beam section, otherwise the split won't be correct.
Then move the generated face with your vector.

Example.
I have a point A with coordinates (X1, Y1, Z1).
I create a face in (0,0,0).
When I move face, it moves in point A that is the center of figure will be point A?
When I move face, I don't have correct inclination of face so I must translate in other point?
Is that right?
Or is there a quicker way to do this?

-mAx- November 16, 2012 08:00

in your case:
*create 10000x10000 (YZ) surface
*move it with (17418 0 0)
*split

Shinobi November 16, 2012 09:38

Quote:

Originally Posted by -mAx- (Post 392505)
in your case:
*create 10000x10000 (YZ) surface
*move it with (17418 0 0)
*split

Perfect!!
Oh my good... it was very simple.
But now I have problem with brick :D
How can I insert him in interested area?

-mAx- November 16, 2012 09:48

create one and use move tool to reach interested area...


All times are GMT -4. The time now is 09:10.