|
[Sponsors] |
[ANSYS Meshing] Problem with meshing a complex Geometry (Hex) |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 22, 2012, 14:50 |
Problem with meshing a complex Geometry (Hex)
|
#1 |
New Member
Pete Drum
Join Date: Sep 2012
Posts: 6
Rep Power: 14 |
Hi everyone,
I just started to work with CFD Fluent and have a few Problems now with the meshing. I have to do a windenergypotential analysis for a building on my College campus. The Task is to make sort of a tutorial for other people, so that they have a better starting point. My Professor wants me to mesh the Geometry with Hexaeders. The Problem is now that the Geometry is very complex and there are still some tetraeders in the mesh, especially around the building, which is bad because that are the important zones. I have really no clue how to mesh the Geometry, so that the quality is good enough. Here is a photo of the actual meshing and the problem zones. http://imageshack.us/photo/my-images/96/bild6r.gif/ the big cuboid is of course the enveloping body. I did that with the boolean operation and sliced the Result in the middle, so that you can see the problem zones. I meshed that with Hexadominant, because there were no sweepable bodies available. Anyone an idea, how to solve that problem? Thank you very much |
|
October 23, 2012, 21:57 |
|
#2 |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 29 |
if you want to mesh it with hexa, you can get better control by using icem cfd.
It's difficult to get hexa in ansys meshing if you don't have sweepable bodies.... |
|
October 24, 2012, 04:02 |
|
#3 | |
Member
Join Date: Nov 2011
Location: Czech Republic
Posts: 97
Rep Power: 14 |
Quote:
|
||
October 24, 2012, 08:31 |
|
#4 | |
New Member
Pete Drum
Join Date: Sep 2012
Posts: 6
Rep Power: 14 |
Quote:
thanks for your answers. Yes I already heard that meshing with hexa in ansys meshing isn't working very good, but we dont have the possibility to use icem cfd. @sixkillers could you explain how to do that, in a more detailed way? I dont know how to slice the Building exactly - here is another picture of the geometry: http://imageshack.us/photo/my-images/196/geometryc.jpg/ Thank your very much! Edit: Referring to the first picture that i posted, how can I generate an Inflation Layer between the Building (Hexa) and the "Air" (Tetra)around the building?? Last edited by fluent_beiyo; October 24, 2012 at 10:41. |
||
October 25, 2012, 03:20 |
|
#5 |
Member
Join Date: Nov 2011
Location: Czech Republic
Posts: 97
Rep Power: 14 |
Hi!
Here are some tips: 1) Hexa dominant method in ANSYS Meshing isn't designed for CFD, but for FEA. 2) When you are doing external aero your computational domain (fluid domain) has to be large enough, so your final solution wont be affected by boundary conditions. What I see on the first picture is completely unacceptable. Your fluid box should be almost 10 larger that your build in each dimension. 3) As was mentioned earlier you have to divide your fluid domain into several swepable bodies to use method sweep. The most common way to do that is by using command slice (by surface) in DM. But before doing that I would simplify your building by merging several smaller faces into a larger one (command merge in DM). 4) For a sweep method boundary layer can be simply done by specifying bias factor and refining cells near a surface. 5) If you don't what to bother with creation of mesh too much. Just create your fluid domain in DM (again large enough) and load agdb file into ICEM CFD and create a tet mesh with hexa elements in core (chech Create Hexa-Core in ICEM). Definitely watch this two youtube tutorials: http://www.youtube.com/watch?v=SdUjp...feature=relmfu http://www.youtube.com/watch?v=C1Yw_...feature=relmfu |
|
November 8, 2012, 09:36 |
|
#7 |
Member
Tamil Nadu
Join Date: Oct 2012
Posts: 44
Rep Power: 14 |
Hi...
Mine is also a similar problem in meshing with GAMBIT. I want to model a building in GAMBIT 3D. Finally, aim of my project is to simulate the temperatures of the walls of building when water flows through pipes inserted in the ceiling (using Ansys Fluent). Is it possible to solve?? |
|
November 11, 2012, 09:33 |
|
#8 |
Senior Member
|
Hey
Are you still working on it. Any progress! I am working on it. Wanted to ask can you simplify some details (Fig. 4)? You want to mesh it inside or outside this domain? |
|
April 26, 2014, 05:55 |
FATAL error in meshing
|
#9 |
New Member
mechatronicstudent
Join Date: Apr 2014
Posts: 2
Rep Power: 0 |
hello everybody!
I'm new in ANSYS. I have some problems in modeling & meshing. I'm trying with : ANSYS15-x64 and in Mechanical APDL. my system is : Intel core(i5) 2.27 with 4G RAM. O.S : Windows 8-x64. I create this rectangle : wp x = 0 wp y = 0 width = 2 height = 1 I meshed it in default mode. with PLANE55 element. Then I could Extrude it in " Cylindrical " Active C.S & with SOLID278 with " Extrude Area by XYZ" tool. It meshed & Extruded exactly. MY PROBLEM IS : But when I'm trying to Extrude it in " Cylindrical-Y " Active C.S it happens this error : *** FATAL *** CP = 4.094 TIME= 12:30:54 An allocation was made with a negative length requested: -8 Filename:..\src\FEM_advFront.cpp Linenum:3032. I'll be so grateful if any one can help me. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[GAMBIT] Meshing complex geometry (Hull) | vmeertens | ANSYS Meshing & Geometry | 26 | March 29, 2010 11:24 |
[GAMBIT] complex geometry meshing | 1682333 | ANSYS Meshing & Geometry | 7 | August 31, 2009 13:44 |
Simulation of Flow through Complex 3D Geometry | EmersonKB | CFX | 5 | July 2, 2009 09:17 |
Meshing a complex geometry | AJG | FLUENT | 2 | June 29, 2005 09:39 |
unstructured vs. structured grids | Frank Muldoon | Main CFD Forum | 1 | January 5, 1999 11:09 |