
[Sponsors] 
September 22, 2011, 23:05 
Force can not converge

#1 
Member
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 10 
Hi all,
I am simulationg vibration of plate using FSI. When my case is running, it looks ok but I goe an error about force converge after some time step. How to control force converge in FSI simulation? Thanks in advance The output is like this MAXIMUM NUMBER OF EQUILIBRIUM ITERATIONS HAS BEEN MODIFIED TO BE, NEQIT = 26, BY SOLUTION CONTROL LOGIC. FORCE CONVERGENCE VALUE = 6252. CRITERION= 0.1013E01 MOMENT CONVERGENCE VALUE = 902.5 CRITERION= 0.7761E03 EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.5511E02 LINE SEARCH PARAMETER = 0.9994 SCALED MAX DOF INC = 0.5508E02 FORCE CONVERGENCE VALUE = 178.7 CRITERION= 0.5432E01 MOMENT CONVERGENCE VALUE = 1.747 CRITERION= 0.3133E02 EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1081E01 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1081E01 FORCE CONVERGENCE VALUE = 459.3 CRITERION= 0.7236 MOMENT CONVERGENCE VALUE = 18.97 CRITERION= 0.1127 EQUIL ITER 3 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.3077 LINE SEARCH PARAMETER = 0.5000E01 SCALED MAX DOF INC = 0.1539E01 FORCE CONVERGENCE VALUE = 927.6 CRITERION= 0.1883 MOMENT CONVERGENCE VALUE = 21.47 CRITERION= 0.3344E01 EQUIL ITER 4 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.9712E01 LINE SEARCH PARAMETER = 0.5000E01 SCALED MAX DOF INC = 0.4856E02 FORCE CONVERGENCE VALUE = 931.2 CRITERION= 1.310 MOMENT CONVERGENCE VALUE = 23.78 CRITERION= 0.7281E01 EQUIL ITER 5 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1393E01 LINE SEARCH PARAMETER = 0.1108 SCALED MAX DOF INC = 0.1543E02 FORCE CONVERGENCE VALUE = 831.4 CRITERION= 1.006 MOMENT CONVERGENCE VALUE = 20.60 CRITERION= 0.3555E01 EQUIL ITER 6 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1311E01 LINE SEARCH PARAMETER = 0.7095E01 SCALED MAX DOF INC = 0.9299E03 FORCE CONVERGENCE VALUE = 774.9 CRITERION= 0.9580 MOMENT CONVERGENCE VALUE = 19.67 CRITERION= 0.3672E01 EQUIL ITER 7 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.8859E02 LINE SEARCH PARAMETER = 0.6283E01 SCALED MAX DOF INC = 0.5566E03 FORCE CONVERGENCE VALUE = 727.2 CRITERION= 0.9256 MOMENT CONVERGENCE VALUE = 18.24 CRITERION= 0.2789E01 EQUIL ITER 8 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.6396E02 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.6396E02 FORCE CONVERGENCE VALUE = 161.4 CRITERION= 0.1909 MOMENT CONVERGENCE VALUE = 12.85 CRITERION= 0.4200E01 EQUIL ITER 9 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1331 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1331 FORCE CONVERGENCE VALUE = 0.6283E+05 CRITERION= 83.09 MOMENT CONVERGENCE VALUE = 1760. CRITERION= 7.059 EQUIL ITER 10 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1573 LINE SEARCH PARAMETER = 0.5441 SCALED MAX DOF INC = 0.8559E01 FORCE CONVERGENCE VALUE = 0.3131E+05 CRITERION= 87.41 MOMENT CONVERGENCE VALUE = 846.3 CRITERION= 3.895 EQUIL ITER 11 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.7290E01 LINE SEARCH PARAMETER = 0.9889 SCALED MAX DOF INC = 0.7209E01 FORCE CONVERGENCE VALUE = 5883. CRITERION= 3.142 MOMENT CONVERGENCE VALUE = 180.2 CRITERION= 0.1070 EQUIL ITER 12 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1671E01 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1671E01 FORCE CONVERGENCE VALUE = 336.2 CRITERION= 0.3233 MOMENT CONVERGENCE VALUE = 11.14 CRITERION= 0.2086E01 EQUIL ITER 13 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.3954 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.3954 FORCE CONVERGENCE VALUE = 0.3660E+06 CRITERION= 310.1 MOMENT CONVERGENCE VALUE = 0.1128E+05 CRITERION= 20.95 EQUIL ITER 14 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1732 LINE SEARCH PARAMETER = 0.8968 SCALED MAX DOF INC = 0.1553 1 FORCEDISTRIBUTED CONSTRAINTS DO NOT SATISFY COMPATIBILITY CONDITION FORCE CONVERGENCE VALUE = 0.4500E+05 CRITERION= 56.10 MOMENT CONVERGENCE VALUE = 2037. CRITERION= 2.005 EQUIL ITER 15 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1671 LINE SEARCH PARAMETER = 0.5095 SCALED MAX DOF INC = 0.8515E01 FORCE CONVERGENCE VALUE = 0.2581E+05 CRITERION= 115.5 MOMENT CONVERGENCE VALUE = 980.1 CRITERION= 3.614 EQUIL ITER 16 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1249 LINE SEARCH PARAMETER = 0.3520 SCALED MAX DOF INC = 0.4398E01 FORCE CONVERGENCE VALUE = 0.1696E+05 CRITERION= 68.74 MOMENT CONVERGENCE VALUE = 684.1 CRITERION= 2.620 EQUIL ITER 17 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.5225 LINE SEARCH PARAMETER = 0.9162E01 SCALED MAX DOF INC = 0.4787E01 FORCE CONVERGENCE VALUE = 0.1522E+05 CRITERION= 58.50 MOMENT CONVERGENCE VALUE = 624.2 CRITERION= 2.644 EQUIL ITER 18 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.5712E01 LINE SEARCH PARAMETER = 0.7985 SCALED MAX DOF INC = 0.4561E01 FORCE CONVERGENCE VALUE = 7083. CRITERION= 13.83 MOMENT CONVERGENCE VALUE = 319.0 CRITERION= 2.010 EQUIL ITER 19 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.3585E01 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.3585E01 FORCE CONVERGENCE VALUE = 6604. CRITERION= 8.681 MOMENT CONVERGENCE VALUE = 150.9 CRITERION= 1.513 EQUIL ITER 20 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.2946 LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.2946 FORCE CONVERGENCE VALUE = 0.2065E+06 CRITERION= 177.5 MOMENT CONVERGENCE VALUE = 6606. CRITERION= 11.36 EQUIL ITER 21 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1289 LINE SEARCH PARAMETER = 0.7385 SCALED MAX DOF INC = 0.9519E01 FORCE CONVERGENCE VALUE = 0.5226E+05 CRITERION= 80.58 MOMENT CONVERGENCE VALUE = 1557. CRITERION= 3.357 EQUIL ITER 22 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.3865 LINE SEARCH PARAMETER = 0.1790 SCALED MAX DOF INC = 0.6918E01 FORCE CONVERGENCE VALUE = 0.4413E+05 CRITERION= 149.3 MOMENT CONVERGENCE VALUE = 1294. CRITERION= 2.292 EQUIL ITER 23 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 1.864 LINE SEARCH PARAMETER = 0.5000E01 SCALED MAX DOF INC = 0.9319E01 FORCE CONVERGENCE VALUE = 0.3884E+05 CRITERION= 144.5 MOMENT CONVERGENCE VALUE = 1008. CRITERION= 1.913 EQUIL ITER 24 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.2576 LINE SEARCH PARAMETER = 0.6518 SCALED MAX DOF INC = 0.1679 FORCE CONVERGENCE VALUE = 0.3911E+05 CRITERION= 80.87 MOMENT CONVERGENCE VALUE = 1838. CRITERION= 4.715 EQUIL ITER 25 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.3611 LINE SEARCH PARAMETER = 0.1451 SCALED MAX DOF INC = 0.5240E01 FORCE CONVERGENCE VALUE = 0.3711E+05 CRITERION= 117.5 MOMENT CONVERGENCE VALUE = 1670. CRITERION= 3.896 EQUIL ITER 26 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1458 LINE SEARCH PARAMETER = 0.6567 SCALED MAX DOF INC = 0.9577E01 FORCE CONVERGENCE VALUE = 0.1696E+05 CRITERION= 43.84 MOMENT CONVERGENCE VALUE = 740.1 CRITERION= 2.085 

September 23, 2011, 12:48 

#2 
Senior Member
Join Date: Apr 2009
Posts: 531
Rep Power: 16 
That's the Mechanical solver that can't converge it's solution. Find out the fluid loads applied then try to repeat it using a nonFSI Mechanical only simulation. I can't help much on how you deal with convergence of the Mechanical solver, but the Mechanical only simulation may show something obviously wrong.


September 25, 2011, 21:17 

#3  
Member
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 10 
Quote:
I attached overall boundary conditions of Mechanical simulation. I used the default options of solver because I don't know how to deal with convergence solver. ( but I controlled force convergence in CFX solver). I did simulate only mechanical solver with just force load on the surface instead of fluid interface load. it works well. (there is no warning, no error) But I try to simulate mechanical with cfx (fsi), force is more and more diverge. it was converged but the level of converge criteria is increasing more and more with the below warning. ****************** Forcedistributedsurface identified by real constant set 12 and contact element type 12 has been set up. The pilot node 1397 is used to apply the force. Internal MPC will be built. The used degrees of freedom set is UX UY UZ ROTX ROTY ROTZ *WARNING*: Certain contact elements (for example 577&195) overlap each other. Please verify constraints (including rotational degrees of freedom) on the pilot node by yourself. The reasons for possible overconstraint are: *Certain contact elements (for example 577 & 195) overlap with other. *Certain contact pairs (for example 4 & 2) overlap with other. ************************************* anyone help me.. thanks Thanks Last edited by colopolo; September 26, 2011 at 05:27. 

September 26, 2011, 18:21 

#4 
Senior Member
Join Date: Apr 2009
Posts: 531
Rep Power: 16 
I think your Remote Displacements are generating MPC style contact elements. These are not valid with MFX, but this should have been caught by the Mechanical solver and it should have stopped with an error. Are you using an older version? In any case, in version 13.0 I think you can turn on beta features and then edit the details of the Remote Displacements and set the Behavior to Beam. This avoids the MPC contact elements.


September 27, 2011, 06:23 

#5  
Member
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 10 
Quote:
I am using version 13.0. Could you tell me how to modify remote displacements? my boundary condtion is Y moving is free and z roation is free. the otheres are 0. how to set the behavior to beam? please help me . Thanks 

September 27, 2011, 13:23 

#6 
Senior Member
Join Date: Apr 2009
Posts: 531
Rep Power: 16 
Turn on beta features then look in the Details view for the Remote Displacements. You should see something called "Behavior".


September 27, 2011, 19:35 

#7  
Member
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 10 
Quote:
I turn on beta feature in CFX_pre. then I check "behavior' of remote dispacement. I have two options  Deformation and rigid. I got an error using rigid option. so I use deformation option in behavior. I coud not find "beam " option in behavior. 

September 29, 2011, 17:57 

#8 
Senior Member
Join Date: Apr 2009
Posts: 531
Rep Power: 16 
The remote displacements are not in CFXPre, so it's no use turning on the beta features there. You need to turn them on in Mechanical. I think it's in the "Options" under "Appearance" or something.


September 30, 2011, 04:54 

#9  
Member
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 10 
Quote:
I did turn on beat feature in Mechanical. But I have no idea how to modify remote displacement of edge of plate. When you look at attached file, force is still diverge. I uploaded my file.. if you have time, I appreciate you check what I was wrong with my case. Very appreciate your help Last edited by colopolo; October 3, 2011 at 21:58. 

September 30, 2011, 14:54 

#10 
Senior Member
Join Date: Apr 2009
Posts: 531
Rep Power: 16 
On the main WB page you need "Tools > Options > Appearance > Beta Options" turned on. You should then see the option in the image...


October 2, 2011, 23:45 

#11  
Member
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 10 
Quote:
I changed option as your comments. then I am watching the convergence of forces. The convegence of force is still increasing and finally it did not converge. The purpose of this simulation is the critical flutter velocicy could be simulated using FSI or not. According to experiment, the flutter velocity occurred at certain velocity. So, I simulate this case as chaging inlet veloctiy and see the diplacement of plate. I expect that the displacement of plate is supposed to have large oscillation after critical velocity. I set up this case as follow steps; 1. adjust the natural frequency of simulated plate as same as experimetal condtion. 2. boundary condtion of Mechnaical solver  remote displacemendt with beam (beta) at edges of plate.  put the fluid interface on 4 faces of plate (interaction with fluid)  solve is direct solver and weak spring is program controlled.  large deflection is on.  put some value on beta damping ratio.  the others are used default option.  time step is 0.01 sec for 10sec (total time) 3. boundary condtion of CFX  inlet velocity : 15 m/s ( test velocity before occuring large amplitude of plate)  time step is 0.01 sec for 10 sec.  the others are a quite standard options (i think b.c. of cfx has no problems) The above steps is what I was done. I really have no idea what i am going to do with this simulation. If you have time to look at my file, please let me know what I did wrong setup . Any comments on the above my steps if I have something wrong with procedure Always, appecite you. Thanks. Last edited by colopolo; October 3, 2011 at 00:50. 

October 3, 2011, 14:46 

#12 
Senior Member
Join Date: Apr 2009
Posts: 531
Rep Power: 16 
Here's a few things to fix...
 The Point Masses may need to use the Beam (Beta) options too, since I think they end up creating MPC style contact elements in the background.  You should use a steady state fluid solution for initialization  The timestep looks too big. The mesh displacement monitor points were showing about 6 timesteps covered one oscillation. You should have about 20, so 0.03[s] would be a better timestep.  Split your interface into 4 separate interfaces to get a more accurate force along the edges  In CFX turn on Monitor Coefficient Loop Convergence so you can see how the mesh displacement are (or are not) converging within a timestep  I would recommend a minimum of 2 coefficient loops in CFX per coupling iteration  The under relaxation factor of 0.1 on FORC is way too small. You would need about 50 coupling iterations to allow reasonable convergence using such a small factor. Start with a value of 1 and watch your monitor points to see if this is stable (after turning on Monitor Coefficient Loop Convergence)  Make sure you use Double Precision when starting CFX. Hope this helps! 

October 3, 2011, 21:57 

#13  
Member
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 10 
Quote:
Very Thanks.. Finally, it works !! I am symply testing the case using single precision for just checking works or not. I really appreciate you to help me !! I will post the results of my case in sooner or later, with a question if I have. Have a good day! P.S. what is weak spring option? Do I need to use this option? The above file is what I modified. I am really sorry to bother you but if you have time to look at it, could you help me? please check my file and kindly let me know it looks ok or not. Last edited by colopolo; October 5, 2011 at 00:18. 

October 4, 2011, 23:03 

#14  
Member
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 10 
Quote:
I set up inlet velocity as 25 m/s which is larger than critical flutter velocity in this case. I got displacement of plate but it does not oscillate at all. I supposed that it should be oscillated. I attached a file and any commnents on this results are welcome. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Viscous force and coefficient viscous force  tobino  Main CFD Forum  0  February 20, 2011 22:06 
Userdefined force transfer across FSI interface  vivekcfd  CFX  7  March 10, 2010 21:43 
Urgently Need the code of Lift force and VM force  Kai Yan  Main CFD Forum  0  July 16, 2008 08:07 
DEFINE_CG_MOTION and pressure force  Teo Fumagalli  FLUENT  0  April 11, 2008 11:25 
pressure force and viscous force  CFD  FLUENT  0  March 7, 2006 02:03 