CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ANSYS Meshing] Hex dominant method and local inflation

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   February 10, 2012, 05:59
Default Hex dominant method and local inflation
  #1
New Member
 
Carl Magnus Persson
Join Date: Feb 2012
Posts: 5
Rep Power: 5
carlp is on a distinguished road
Hi

I have this rather thin wall, and I am interested in the water content and temperature in that wall. I know that the big change will be through the wall and just small changes in the other directions. I want to have a structured mesh with cubes and due to a large geometry, i can't have the cells in the same size of the walls, thus i need to make the cells in the walls to "thin plates", not cubes. My idea is to make them with local inflation.

But even thou I only have straight lines in that part of the geometry, the mesh doesn't get cubic, and thus I have used Hex dominant method and that works. But when i use hex dominant method I can't use the local inflation no matter what. As fast as I choose the geometry to do the inflation, an "active" line appears that says: "no, invalid method". It also disappear when I delete the Hex dominant method.

Because of this I have also tried Method-Multizone with both hex core and hex dominant, but when that mesh is about to get generated it complain about bad cells and fail when "meshing the blocks".

Is there more ways to try to solve this? Why can't I do the inflation with a hex dominant method present?
carlp is offline   Reply With Quote

Old   February 11, 2012, 21:25
Default
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hexa Dominant was never intended for CFD. It puts isotropic hexas near the walls and junk in the middle. It doesn't work with prism, etc. Only use it for FEA (mechanical) applications. We should probably just hide it if you set the physics to CFD...

What you want is "Assembly Meshing" "Cutcel". You can use global inflation with Named selections to control where the prism is applied. It works very well at R14.0, but is different from the other "methods" in how you apply it. Look it up in the Help to find it.

The catch is that it produces a mesh with haning nodes and some poly's so it is only good for Fluent, CFX doesn't like it.
sara.om likes this.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   February 13, 2012, 15:55
Default
  #3
New Member
 
Join Date: Feb 2012
Posts: 13
Rep Power: 5
blacksoil2012 is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Hexa Dominant was never intended for CFD. It puts isotropic hexas near the walls and junk in the middle. It doesn't work with prism, etc. Only use it for FEA (mechanical) applications. We should probably just hide it if you set the physics to CFD...

What you want is "Assembly Meshing" "Cutcel". You can use global inflation with Named selections to control where the prism is applied. It works very well at R14.0, but is different from the other "methods" in how you apply it. Look it up in the Help to find it.

The catch is that it produces a mesh with haning nodes and some poly's so it is only good for Fluent, CFX doesn't like it.
Hi Simon,

Regarding your comment "Hexa Dominant was never intended for CFD", maybe this is true for ANSYS, but as far as I know, ANSA provides this option. That is, no matter what the surface mesh is, ANSA can generate hex core mesh, and also at the same time it can generate prism layers with subsequent hex core mesh. I feel this is a very good feature, since it not only provides us the boundary layer resolution for CFD but also can reduce volume mesh count by getting hex core. Do not know whether ICEM CFD has this function, but surely I am wishing Workbench Meshing can get this. Thanks!
blacksoil2012 is offline   Reply With Quote

Old   February 13, 2012, 21:44
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hexa dominant is different from hexa Core... TGrid and ICEM CFD each have a Hexa core option... Personally, I prefer the TGrid one.

I am not exactly sure how the ANSA algorithm works, but...

Hexa dominant starts at the surface and marches inward with isotropic hexas... If you have something with nice right angles, etc. it can produce hexas all the way across, but if you started with a pipe, or something like that, it will not be able to continue with hexas all the way to the middle.

In that case, if you are in Workbench, I suggest Cutcel. It will give you what you want and works nicely with inflation...
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   February 27, 2012, 04:50
Default
  #5
New Member
 
Carl Magnus Persson
Join Date: Feb 2012
Posts: 5
Rep Power: 5
carlp is on a distinguished road
I use fluent, and CutCell works good, maybe, it generates an acceptable mesh but:
Warning: "The model consists of a multibody part. The CutCell mesh may not accurately capture the geometry at the interface between two or more bodies."
but I have so far ignored it.

When I try global inflation, Error: "An error occurred while running the CutCell mesher. Please check the geometry or the mesh settings for problems". But not without the inflation, but if I use local inflation with the same settings it works but, it gets too small, even if I with total thickness och first layer thickness + size tries to force the inflation to be the size i want, it still gets to small.

(Total thickness - 5mm - 2 layers - no growth (1) gives two layers that have a total thickness of 1,3 mm, and i want it to be 10 mm. The thin walls are 25mm, so 5 layers in total at 5mm.)
carlp is offline   Reply With Quote

Old   February 27, 2012, 10:42
Default
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
What version are you using? It works well for me at 14.0, but it was still pretty new at 13.0...

Simon
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   February 27, 2012, 21:27
Default
  #7
New Member
 
Carl Magnus Persson
Join Date: Feb 2012
Posts: 5
Rep Power: 5
carlp is on a distinguished road
I'm using version 13...
carlp is offline   Reply With Quote

Old   February 28, 2012, 04:07
Default
  #8
New Member
 
Carl Magnus Persson
Join Date: Feb 2012
Posts: 5
Rep Power: 5
carlp is on a distinguished road
I've investigated the problem further:
1. I can't use global inflation, since then i can either choose program controlled and the inflation goes to the outer walls, or choose named selection and the wall, but the inflation is at the fluid side of the wall and not the inside of the wall (both with proper thickness).

2. It's not about the CutCell, i got the same problem with no other local method but inflation (and here it was very small). The same with method - multizone - Hexdominant, but here the inflation is almost 3 mm in two layers for both sides of the wall, leaving a 13mm thick cells in the middle (reasonable total amount of cells)

Thus, I think the problem lie in the geometry and/or the inflation itself (like that the mesh wants to fill large enough cells between the layers of inflation*). Any ideas? Can I suppress that for local inflation?

* http://www.kxcad.net/ansys/ANSYS/wor...thin_gaps.html
carlp is offline   Reply With Quote

Old   July 12, 2012, 08:02
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
CarlP,

For 1) ANSYS Meshing does not gives as many options as ICEM CFD or TGrid for setting up inflation (prism). ICEM CFD lets you decide which volumes it grows into, etc. but ANSYS Meshing only grows into the Fluid region... Perhaps the trick here would be to reassign the Solid region as a Fluid region and vice versa... ICEM CFD also has option (under Advanced Prism Meshing Parameters) for "Auto Reduction". This option compresses prism layers to avoid penetration across a small gap if the total heights would otherwise have overlapped...

For 2) Sorry, I don't really understand what you are saying. For cutcel with inflation, I suggest an upgrade to 14.0 (it was just too new at 13.0 and got a decade of work between 13 and 14, so it is really worth the upgrade). For Multizone with Hexdominant... Dont use hex dominant with CFD... MultiZone, another relatively new method, also got a ton of work between 13 and 14.0, (and again for 14.5 due out before the end of the year)... Probably more than any other method in ANSYS Meshing.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Reply

Tags
hex dominant method, inflation, invalid method, mesh

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
[ANSYS Meshing] Hex meshing producing poor quality elements on multibody part aarvay ANSYS Meshing & Geometry 8 March 16, 2012 16:29
discretizer - gmshToFoam Andyjoe Open Source Meshers: Gmsh, Netgen, CGNS, ... 13 March 14, 2012 05:35
Local stepping for steady state Mehdi Main CFD Forum 2 June 17, 2003 09:43
local timestep for agglomeration multigrid method Jian Xia Main CFD Forum 3 March 20, 2000 12:20


All times are GMT -4. The time now is 03:54.