CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Mapping method in FSI

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 3, 2012, 08:52
Default Mapping method in FSI
  #1
Member
 
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Mina_Shahi is on a distinguished road
Dear Ansys users

i am simulating 2-way FSI with Workbench version 13. i created two models one for fluid flow in CFX and a second for structural vibration. and then linked these two in ANSYS WORKBENCH. in which displacement and pressere exchanged between two modules. But i am wondering that what kind of mapping method Workbench uses for transfering loads . because meshes on both sides of the interface connection are usually not matching.
i created both models and just linked them and every thing between is done by workbench automatically. does anyone know about mapping method using in workbench?
Mina_Shahi is offline   Reply With Quote

Old   January 3, 2012, 17:56
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
It's the same as the GGI mapping in CFX. The CFX documentation should say something about that mapping. An important point is that force is conserved.
stumpy is offline   Reply With Quote

Old   January 4, 2012, 04:32
Default
  #3
Member
 
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Mina_Shahi is on a distinguished road
Quote:
Originally Posted by stumpy View Post
It's the same as the GGI mapping in CFX. The CFX documentation should say something about that mapping. An important point is that force is conserved.
Thanks for the answer, but in the CFX documentation it is written :

Fluid-Solid interfaces are required at the bounding region between a fluid domain and a solid domain, but are often generated automatically. The mesh on these interfaces must be matching.

when you have both domains in CFX it is possible to have matching mesh but when the fluid part will be solving in CFX and Structure one in the ANSYS multiphyisics (ans both in the workbench package) then it is not always the case and you won't have always matching mesh and usually the mesh in fluid part is much finer.

Let me know what you think,

Mina_Shahi is offline   Reply With Quote

Old   January 4, 2012, 12:03
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
In the CFX 13.0 doc see:
// Modeling Guide // 5. Domain Interface Modeling // 5.4. Mesh Connection Options // 5.4.3. GGI (General Grid Interface) Connections

and

// Theory Guide // 3. GGI and MFR Theory

also see the MAPDL doc:

// Coupled-Field Analysis Guide // 3. The ANSYS Multi-field (TM) Solver - MFS Single-Code Coupling // 3.1. The ANSYS Multi-field solver and Solution Algorithm // 3.1.1 Load Transfer

Hope this helps!
stumpy is offline   Reply With Quote

Old   January 5, 2012, 06:26
Default
  #5
Member
 
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Mina_Shahi is on a distinguished road
Quote:
Originally Posted by stumpy View Post
In the CFX 13.0 doc see:
// Modeling Guide // 5. Domain Interface Modeling // 5.4. Mesh Connection Options // 5.4.3. GGI (General Grid Interface) Connections

and

// Theory Guide // 3. GGI and MFR Theory

also see the MAPDL doc:

// Coupled-Field Analysis Guide // 3. The ANSYS Multi-field (TM) Solver - MFS Single-Code Coupling // 3.1. The ANSYS Multi-field solver and Solution Algorithm // 3.1.1 Load Transfer

Hope this helps!
Thanks a alot, but one more question when you use workbench you don't know which mapping (global or blucket) it uses .
I just know that there are some folders which workbench makes (while doing FSI) and mapping method perhaps is available somewhere there, but i don't know exactly where, Can you please help me with that?
Mina_Shahi is offline   Reply With Quote

Old   January 5, 2012, 10:23
Default
  #6
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
In a completed run search for the ANSYS.mf file. This is the final input file to the structural solver. Near the end of this file you'll see a list of commands that start with "MF". You can look in the MAPDL doc for the details of each command. The mapping algorithm is part of the MFLC commands. There'll be two command for each FSI interface - one to map the displacement to CFX (this will use the NONC option) and one to map the force to ANSYS (this will use the CPP method).
stumpy is offline   Reply With Quote

Old   January 9, 2012, 07:54
Question
  #7
Member
 
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Mina_Shahi is on a distinguished road
Quote:
Originally Posted by stumpy View Post
In a completed run search for the ANSYS.mf file. This is the final input file to the structural solver. Near the end of this file you'll see a list of commands that start with "MF". You can look in the MAPDL doc for the details of each command. The mapping algorithm is part of the MFLC commands. There'll be two command for each FSI interface - one to map the displacement to CFX (this will use the NONC option) and one to map the force to ANSYS (this will use the CPP method).
Many thanks!

1- Is it also possible to change this item like NONC to CPP? OR VICE VERSA
2- in Ansys manuall it is written that :


CPP


Conservative: Uses a local conservative formulation while preserving the density profile (default for total force and wall heat flow). In the conservative formulation, total force (or heat flow) must be transferred across the interface from the CFX field solver to the ANSYS field solver.

Why local conservative and not global??? because in ansys documentation it mentioned that there are two method of interpolating: 1- globally conservative interpolation and 2- profile preserving interpolation .

Global or local conservative????
Mina_Shahi is offline   Reply With Quote

Old   January 9, 2012, 11:38
Default
  #8
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
I think the doc is wrong. The force transfer is locally and globally conservative.
stumpy is offline   Reply With Quote

Old   January 9, 2012, 11:54
Default
  #9
Member
 
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Mina_Shahi is on a distinguished road
Quote:
Originally Posted by stumpy View Post
I think the doc is wrong. The force transfer is locally and globally conservative.
Dear Stumpy

"" globally conservative interpolation " you can find it in ANSYS release 13.0 in the ANSYS Multi-field (TM) solver- MFS- Code coupling : for load transfer


What do you think? You think it is not correct??

Thank you !
Mina_Shahi is offline   Reply With Quote

Old   January 9, 2012, 12:48
Default
  #10
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
Best to check with ANSYS support.
stumpy 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
FSI Problem - Utilizing ALE method to map solutions natern OpenFOAM 1 November 7, 2011 18:00
Structural force in FSI mapping Fluent 12.0 benjamon FLUENT 1 October 24, 2011 10:32
difference in the trimming and mapping method guru STAR-CD 1 April 25, 2011 10:48
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19
Implicit method of FSI cjtune CD-adapco 0 March 12, 2003 13:07


All times are GMT -4. The time now is 12:40.