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

[ICEM] Rigid sphere falling through air. Dynamic mesh

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

Like Tree2Likes
  • 2 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   June 28, 2010, 03:49
Default Rigid sphere falling through air. Dynamic mesh
  #1
New Member
 
Alexander Meier
Join Date: Apr 2010
Posts: 8
Rep Power: 7
alexmeier is on a distinguished road
Hi there

I'm trying to set up a problem in fluent.
I'd like to simulate a rigid sphere falling through air at standard conditions accelerated by gravity onely using a dynamic mesh and UDFs.
right now my problem is, that fluent can't read my mesh. I always get the same Error warning:

WARNING: cell 2 of thread 15 has NULL face pointer 3
ERROR: Build Grid: Aborted due to critical error.

Here is the mesh I wanted to use:



There is a region around the Sphere I have declared as new volume part when I have created the prism Layers. The reason for this is, that I want to move the boundary Layer and the Sphere in my simulation.

I have checked what happens, when I try to read in the same mesh in fluent, whiteout declaring the boundary Layer as new volume part. If i do so, there is no ERROR Warning.

For this reason I know, that there is something wrong whit this volume part declaration. but right now I can't think of any other possibility to realize my simulation.

Does anybody know what's wrong?


the Fluent User Manual says:

"If you create a single grid with multiple cell zones, you must be sure that each cell zone has a distinct face zone on the sliding boundary. The face zones for two adjacent cell zones will have the same position and shape, but one will correspond to one cell zone and one to the other."

I think that' why this ERROR occurs. But I don't understand how to realize this in ICEM?

Is there any other possibility to realize this Problem in Fluent?

thank you so much for your support.
Alex
alexmeier is offline   Reply With Quote

Old   June 28, 2010, 05:54
Default
  #2
jsm
Senior Member
 
JSM
Join Date: Mar 2009
Location: India
Posts: 155
Rep Power: 11
jsm is on a distinguished road
Hi

If you want separate fluid domain for prism elements, then specify side part and top part names also with new volume part. You can find these fields just below the new volume part. Then you will not get this error.
__________________
With regards,
JSM
jsm is offline   Reply With Quote

Old   June 28, 2010, 06:00
Default
  #3
New Member
 
Alexander Meier
Join Date: Apr 2010
Posts: 8
Rep Power: 7
alexmeier is on a distinguished road
Thx a lot. I'll give it a try
alexmeier is offline   Reply With Quote

Old   June 29, 2010, 09:05
Default more detail
  #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
JSM has the right solution, but I got this question a couple times recently (this week), and this is the longer explanation I typed out for them, so I thought I would post it here for others.

In Fluent, you can not have two different fluid volumes next to each other without a boundary between them. If you do that, you will get a "null pointer" error. This really means that each fluid volume should have a shell boundary and each shell should have a normal direction so bocos can be applied, but in your case, there isn't one between the tetras and the prisms.

If you had run your mesh checks, you would have had "uncovered faces" and "surface orientation errors".

There are two ways to avoid this error.

1) if you want the material in two different fluids, you need shells between them. You could get this from the "uncovered faces" check, or by using the "top" option when you put Prism into a different part. Then apply an "internal wall" boco to that internal part.

2) if you really just intended to have one fluid zone (but you had created the prisms first for your movement and therefore had the 2 parts as part of your mesh creation process), then you simply need another step to add all the volume elements to the same part. In the model tree, right click on the volume part you want to keep (perhaps (FLUID)) and choose "Add to Part". The message int he display window should say "select elements". (if it says select entities, then you should click the last icon in the selection toolbar so it changes to "select elements".) Then click the second last icon in the selection tool bar to select all the volume elements in your model. Now that all the volume mesh is in the same part, you can run the mesh checks and won't get the uncovered faces error, even after deleting the internal inlet face. You also won't get the null pointer error in Fluent.
hadikhayyamian and Yannian like this.
PSYMN is offline   Reply With Quote

Old   June 29, 2010, 09:06
Default Hexa option...
  #5
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
By the way, this model could be very easily scripted/meshed in ICEM CFD hexa and give you the very best quality mesh possible. Each iteration could be precisely controlled in terms of mesh distribution and would generate much more quickly for a faster solve.
PSYMN is offline   Reply With Quote

Old   June 30, 2010, 00:23
Default
  #6
jsm
Senior Member
 
JSM
Join Date: Mar 2009
Location: India
Posts: 155
Rep Power: 11
jsm is on a distinguished road
Hi Simon,

Normally I will not get uncovered faces error. If I get this error, I simply use Build mesh topology. This error will be removed automatically.
__________________
With regards,
JSM
jsm is offline   Reply With Quote

Reply

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
Regarding Negative volume detected in Dynamic mesh Vinay Morabad FLUENT 9 April 10, 2015 23:00
SnappyHexMesh for internal Flow vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 23 August 6, 2014 03:50
Dynamic Mesh on Pintle type injector. herntan FLUENT 15 January 4, 2012 04:31
air bubble is disappear increasing time using vof xujjun CFX 9 June 9, 2009 07:59
Dynamic mesh Phil FLUENT 1 June 15, 2003 04:57


All times are GMT -4. The time now is 07:41.