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

[ANSYS Meshing] 2.5D simulation in ICEMcfd

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 4, 2011, 01:05
Default 2.5D simulation in ICEMcfd
  #1
New Member
 
@p N
Join Date: Jan 2010
Location: United States
Posts: 27
Rep Power: 7
yvonne is on a distinguished road
Hi all!

I am trying to create a 2.5 D geometry of a centrifugal pump in ICEMcfd. following is the algorithm use:
  • Create the geometry
  • add parts: As Ill be using frozen rotor scheme, Ill need three domains--> Inlet(stationary), Rotating domain, Outlet(stationary). Corresponding to 3D setup, where we add surfaces to parts for creating bocos, Im adding curves for this 2.5D simulation.
  • I then add 2 interfaces (to separate the moving domain from the two stationary ones)
  • I mesh this.
  • I extrude the mesh in the z-axis by one layer thickness
After meshing generally (for 3D geometries) the domains will get created automatically, as ICEM will recognise the interface boundary. BUt thios is not happening in my 2D case.
In CFX-pre when I open the geometry it shows only one domain with 'interface' as a boco.
Im not doing pre-mesh or blocking as Im very new to ICEM. Is that the solution?
Kindly help!
yvonne is offline   Reply With Quote

Old   November 4, 2011, 01:13
Default
  #2
New Member
 
@p N
Join Date: Jan 2010
Location: United States
Posts: 27
Rep Power: 7
yvonne is on a distinguished road
I hope this info might help people facing the problem like me: (Reply from PSYMN- Simon Periera, Simon member)

Each zone or boco must be properly grouped for the solver.

If you have your fluid (Tetra/Prism or Hexa elements) in "GEOM", the solver wants to put them in a "fluid" or "solid" zone. But if you also have other element types mixed in (Shells, or lines), the solver needs to treat those as boundaries. It can't apply the same zone properties to all cells in the GEOM part, so it gives you that message.

Go back and make sure that you don't mix boundary conditions (surface and curve) with volumes in a single part and you will be successful.


Best regards,

Simon
yvonne is offline   Reply With Quote

Old   November 4, 2011, 21:57
Default
  #3
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
Yvonne that answer was for your other question... I forget the exact wording but it was something about multiple dimensions combined in "GEOM".

For Extrude (the subject of this question), you need to be a bit careful. Think about what you are starting with... Hopefully it is a surface mesh with shells in in various parts (these will become Fluids when you extrude them) and line elements around them in other parts (These will become shells that CFX can apply boundary conditions (bocos) to after you extrude them).

If you extrude, you can either enter a name or pick "inherited". If you pick inherited, the name of the new PART name is inherited from original 2D mesh. I would choose inherited for the sides so that they take the name of the line elements (INLET, INTERFACE, etc.). If I have one zone, I would name the volume (FLUID) and set the top to "inherited". But if I have multiple zones, it may be easier to set the fluid to inherited so that each zone would be in a separate part. But then you must go back and move the shells or volume elements to a separate part later. This is critical because the solver can't handle fluid zones and bocos (shells) in the same part or it will give that other error message that you asked me about...

The hassle of the previous paragraph is why I usually just export a 2D mesh in fluent mesh format and then read that into CFX. CFX will automatically extrude it to 2.5D without any hassle. I read that this was not working for you and I don't know why. My only guess is that maybe you didn't have it in the XY (Z=0) plane? Or maybe when you exported to Fluent you didn't specify that it was a 2D mesh?
__________________
-----------------------------------------
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   November 8, 2011, 01:22
Default
  #4
New Member
 
@p N
Join Date: Jan 2010
Location: United States
Posts: 27
Rep Power: 7
yvonne is on a distinguished road
Hi Simon,
Thanks a lot for your inputs I was able to simulate 2.5D model of a centrifugal pump.
What I did was the following:
  • As my geometry consists of 3 domains, I created the 3domains separately; i.e. 3 different ICEM files.
  • I followed the general 2.5D procedure: surface mesh followed by extrusion in the z-direction, separately naming the lateral faces which will be later initialized as symmetry.
  • Exported the 3 mesh files separately in .cfx5 format
  • Imported the 3 mesh files into CFX-pre
  • Created interfaces in CFX-pre and thus joined the 3 domains.
  • This worked for me and CFX simulated my 2.5D model.
Now, the problem Im facing is as follows:
There is a problem in the way CFX is calculating inlet and outlet areas. It is calculating the areas exactly an order of magnitude less than actual because of which the velocities calculated are an order of magnitude more; this results in a highly unrealistic value of pressure being calculated. Is there a way to rectify this problem? I checked out if I could write a CEL, but seems, CEL is just for post processing and for extracting calculated quantities.

Can you throw some light on this?
yvonne is offline   Reply With Quote

Old   November 8, 2011, 10:13
Default
  #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
You should probably take this CFX setup question over to the CFX forum...

My first guess is that it has to do with the scale of your model...

Or maybe it has something to do with the conversion from 2D to 3D...

Sorry, I have no experience with this particular problem.
__________________
-----------------------------------------
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
2.5d, ansys, fluent error, icemcfd

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
Why my simulation not agree with the wind tunnel experiment zhaowei CFX 4 July 11, 2015 03:36
Solar Radiation in OpenFOAM plainstyle OpenFOAM Running, Solving & CFD 15 July 8, 2014 04:43
Simulation of a complex wing in solidworks flow simulation niels1900 FloEFD, FloWorks & FloTHERM 6 April 20, 2011 10:44
Continuous vs interrupted simulation sega OpenFOAM Running, Solving & CFD 4 November 3, 2008 15:29
strange simulation error Ralf Schmidt FLUENT 2 May 4, 2007 13:02


All times are GMT -4. The time now is 00:24.