[Mina_Shahi]

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?

[stumpy]

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.

[Mina_Shahi]

Originally Posted by stumpy

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,

[stumpy]

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!

[Mina_Shahi]

Originally Posted by stumpy

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?

[stumpy]

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).

[Mina_Shahi]

Originally Posted by stumpy

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????

[stumpy]

I think the doc is wrong. The force transfer is locally and globally conservative.

[Mina_Shahi]

Originally Posted by stumpy

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 !

[stumpy]

Best to check with ANSYS support.