HI All

I am trying to simulate a coupled flow and structure problem with ANSYS+CFX (two way) coupling using MFX feature of ANSYS10.0

So far I am not much satisfied with it due to the following reasons:

-- It requires ANSYS classic knowledge and learing ANSYS apdl scripts needs a lot of time. In short it is not user friendly.

-- Secondly, convergence of Stagger iterations is really poor. I tried everything so far, i.e. varying time steps, under-relaxation etc. but there is no much success. In fact Stagger-iterations do not converge at all in my case.

Therefore I would like ask the following:

Is any user successfully using FSI feature of ANSYS10.0 for two-way coupling(Ofcourse not the people/developers from ANSYS)?

Can anybody share with me his/her expereince on ANSYS-CFX coupling with MFX e.g. convergence robustness, limitations, drawbacks etc?

Another question: which is the best commercial or freeware code for a FSI simulation.

many thanks in advance

VK

Hi Kumar,

You are at the moment using the most user friendly software.It gives you reasonable results for FSI.

Whats your problem with convergence.Post it.

Thanks

Regards

Rajit

Yes ofcourse CFX is most user friendly CFD code but not ANSYS classic with apdl.

My problem is convergence is that the Stagger iterations do not converge at all. Either I get negative volume message in CFX or the following messages from the two codes (If somebody wants to look into my case, I can send him the input files):

CFX=>

+--------------------------------------------------------------------+ | An error has occurred in cfx5solve: | | | | The CFX-5 solver exited with return code 1. No results file has | | been created. | +--------------------------------------------------------------------+

End of solution stage.

+--------------------------------------------------------------------+ | The following transient and backup files written by the CFX-5 | | solver have been saved in the directory | | D:\Daten\KV\Projects\FEC\FSI\PIPE_LANG_CADFEM\CFX\ run_004: | | | | 0_full.trn | +--------------------------------------------------------------------+

+--------------------------------------------------------------------+ | The following user files have been saved in the directory | | D:\Daten\KV\Projects\FEC\FSI\PIPE_LANG_CADFEM\CFX\ run_004: | | | | mon | +--------------------------------------------------------------------+

ANSYS=>>>>>>>>>>>>

*** ERROR *** CP = 2271.578 TIME= 23:11:23 One or more elements have become highly distorted. Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere. Try incrementing the load more slowly (increase the number of substeps or decrease the time step size). You may need to improve your mesh to obtain elements with better aspect ratios. Also consider the behavior of materials, contact pairs, and/or constraint equations. If this message appears in the first iteration of first substep, be sure to perform element shape checking.

Yes, ANSYS is good solution. And related to APDL languge in ANSYS try to compare it to programing language of other codes, for example - MSC PCL (in Patran). Feel difference... If someone have enough experience in programming then APDL will be no problem.

I AM really concern about this!but i am a pre-learner,

maybe we can communicate by e-mail.

Yes APDL is as simple as Fortran77 but for a beginer the problem is to know "what is what" and "who is who".

Anyway thanks for the response and let us not get ourselves involved in this discussion on simplicity of ANSYS-APDL. It would be great if someone can shed more light on convergense issues related to coupled simulations.

In my case I even tried to increase the number of stagger-iterations per time-step to 100 and made the numerical time step much smaller than the physical time scales. Still I see no success. That is why I was wondering if CFX users are currently intensively expoilting this feature of the code.

People who are interested and currently involved in FSI computations, I welcome all of you to have open discussion on this topic so that we all can benefit from this and remember the objective of these discussions is not to criticize any code or feature.

Can I ask you guys to post one or two working example (with input files) of FSI, ofcourse not the typical ANSYS examples of FSI.

many thanks

If elements are becoming distorted, then usually it's because they are moving too far in one iteration, because they are not good quality to begin with or the mesh stiffness is not appropriate. The first thing to do it to make sure you have a good quality mesh to begin with and that the fluids-only solution runs OK. Looks at the forces in the fluids-only solution and check they are reasonable. Next, make sure you have set up the mesh stiffness parameter to an appropriate value (see tutorial 20). It should not be a constant value. Next, consider the forces applied to the FSI boundary. How far do you expect it to move in one timestep? The distance it moves should be small relative to the geometry. The CFX Reference Pressure is not included in the forces transimitted to ANSYS by default. In general you'll need a converged fluids-only solution as the initial guess so you can avoid force spikes during start-up. hope this helps! Mike

Try to see 2-way coupling between Abaqus & FlowVision (http://www.capvidia.com/index.php?id=22)

Hi Mike

Thanks for a detailed reply.

As far my fluid mesh is concerned, the quality of the mesh is quite good. It is a hexa mesh with a minimum angle of 60 deg between the faces of cells, i.e. skewness is well controlled.

I start first with a steady state computation whose results, I use as an initial guess for the FSI simulation. From the steady solution, the force acting on the wall and pressure field in the domain look ok.

Mesh stiffness parameter is not constant, it is defined as:

stiffness = 1 / Volume of control volume

The movement of the boundaries in my case is mainly governed by a force acting on the structure side, I am interested to see how fluid affects this movement of the structure. From a transient analysis, without CFD, I observed that the maximum displacement (in one cycle) in the structure is around 2-3% of its dimension and I had 64 time steps in one cycle. Perhaps this movement is too much for the solver.

Reference pressure: I also expected that reference pressure should not be transmitted to ANSYS by defualt. Since I have an incompressible case, I am setting P_ref = 0 Pa.

From your remarks it seems all my settings are ok. Still, I attach my ANSYS input file with this post so that one can see if the settings are ok for the ANSYS solver.

*******************ANSYS INPUT FILE***********************

fini

/clear

/COM,ANSYS RELEASE 10.0 UP20050718 15:23:39 05/09/2006

!/input,menust,tmp,'',,,,,,,,,,,,,,,,1

WPSTYLE,,,,,,,,0

/PREP7

/TITLE Coupled FVM/FEM modelling

!****************************

!*** Craete keypoints********

!****************************

fsi_flag = 1

f_flag = 1

pi=4.*atan(1.)

r_inner=10*1.0e-3

r_outer=10.5*1.0e-3

rad=0.5*(r_inner+r_outer)

Length=400.0*1.0e-3

area_t=pi*(r_outer**2-r_inner**2)

dens_sol=4510.0

E_st=1.027e11

dens_liq=1000.0

Pratio=0.34

den_tot=(area_t*dens_sol+pi*r_inner**2*dens_liq)/area_t

!##########################

!##Geometry creation#######

!##########################

K,1,0,0,-Length/2,

K,2,0,0,Length/2,

!**********************

!*** Create axis line

!**********************

L,1,2

!*****************************

!*** Create arcs and surfaces*

!*****************************

circle,1,r_inner

circle,2,r_inner

ADRAG,6,7,8,9, , , 1

!#################################

!*****Geometry Finished***********

!#################################

!!!!!!!!!!!!!!!!!!!!

!*******************************

! Material Properties **********

!*******************************

ET,1,SHELL93 !**Element type

MP,EX,1,E_st !**Youngs Modulus

MP,dens,1,den_tot ! density

MP,NUXY,1,Pratio!Poisson Ratio

R,1,dth ! Real constant

!*

!******************************

!*Generate mesh

!*****************************

LSEL,s, , ,2, 9, ! select lines

LESIZE,ALL, , ,5, ! resolve above selected lines

lsel,none

lsel,s,,,11,12

lsel,a,,,14,16,2

lsel,a,,,1,

lesize,all,,,21,

MSHK,1 ! use mapped mesher

MSHA,0,2D ! use only quads

AMESH,ALL ! mesher executed

finish

!*********************

!!Transient Analysis

!********************

fcn=400.0

omega=2*pi*fcn

per_res=64

delt=1/(per_res*fcn)

n_per=16

f_max=1.5

nsteps=n_per*per_res

!*********************

!!FSI Analysis

!********************

/PREP7

ALLS

DDELE,ALL

*if, fsi_flag, eq, 1, then

mp,dens,2,dens_sol

mp,dens,1,dens_sol

totim=delt*nsteps

nsel,s,loc,z,Length/2

nsel,a,loc,z,-Length/2

d,all,ux,,,,,uy,uz ! D,ALL, ALL

nsel,all

alls

fini

/SOLU

ANTYPE,4 !Trasiente Analyse

EQSL,SPAR,,,,, 1.00000000

NLGEOM, 1

TRNOPT,FULL

NSUBST,1,10,1

resc,,none

nsub,1,10,1

nsel,none

! Apply Boundary condition

alls

esln

cm,FSIxx,elem

SF,all,FSIN,1

nsel,none

nsel,s,loc,z,-0.001,+0.001

*get,nnum,node,0,count

*dim, force,table,nsteps,1 ! TABLE fr Kraftverlauf definieren

*do,tt,0,nsteps,1

force(tt,0)=tt*delt

force(tt,1)=f_max*sin(omega*tt*delt)/nnum

*enddo

*vplot,force(1,0),force(1,1)

F,all,FY,%force%

kbc,0

autots,on

alls

DELTIM,delt,delt,delt

OUTRES,BASI,5

TIME,totim

!*** * MFS/MFX Aktivation

MFAN,ON,MFAX

MFCL,MFPS

! -> Simultane Berechnung 2-Weg Kopplung Struktur <-> Flssigkeit

!MFPSIMUL,group1,ANSYS,CFX,

!MFSORDER,group1,

! -> Sequenzielle Berechnung 1-Weg Kopplung Struktur -> Flssigkeit

MFTIME, totim

MFDT, delt, delt, delt,OFF

MFIT, 101, 1, 15

MFRELAX,DISP, 0.40000000 ,RELX

MFRELAX,FORC, 0.40000000 ,RELX

MFRELAX,TEMP, 0.40000000 ,RELX

MFRELAX,HFLU, 0.40000000 ,RELX

MFRELAX,HGEN, 0.40000000 ,RELX

MFRELAX,VELO, 0.40000000 ,RELX

MFRELAX,ALL , 0.40000000 ,RELX

MFRSTART, 0.00000000

MFPS, group1, ANSYS

MFPSIMUL, group2, CFX

MFSORDER, group1, group2

MFLCOMM, SURF,ANSYS,1,DISP,CFX,PIPE,Mesh Displacement,NONC

MFLCOMM, SURF,CFX,PIPE,Total Force Density,ANSYS,1,FORC,NONC

MFLI,

alls

finish

*endif !ENDIF FSI_FLAG

************ANSYS INPUT FILE ENDING************************

thanks for your help. VK

[mortazavi]

hi V. Kumar:
now in 2009 i have the same problem in fsi modeling...has your problem been solved???would you please help me now?
regards