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

Force can not converge

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 22, 2011, 22:05
Default Force can not converge
  #1
Member
 
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 5
colopolo is on a distinguished road
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= 0.1013E-01
MOMENT CONVERGENCE VALUE = 902.5 CRITERION= 0.7761E-03
EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.5511E-02
LINE SEARCH PARAMETER = 0.9994 SCALED MAX DOF INC = 0.5508E-02
FORCE CONVERGENCE VALUE = 178.7 CRITERION= 0.5432E-01
MOMENT CONVERGENCE VALUE = 1.747 CRITERION= 0.3133E-02
EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.1081E-01
LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = -0.1081E-01
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 = 0.5000E-01 SCALED MAX DOF INC = -0.1539E-01
FORCE CONVERGENCE VALUE = 927.6 CRITERION= 0.1883
MOMENT CONVERGENCE VALUE = 21.47 CRITERION= 0.3344E-01
EQUIL ITER 4 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.9712E-01
LINE SEARCH PARAMETER = 0.5000E-01 SCALED MAX DOF INC = 0.4856E-02
FORCE CONVERGENCE VALUE = 931.2 CRITERION= 1.310
MOMENT CONVERGENCE VALUE = 23.78 CRITERION= 0.7281E-01
EQUIL ITER 5 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1393E-01
LINE SEARCH PARAMETER = 0.1108 SCALED MAX DOF INC = 0.1543E-02
FORCE CONVERGENCE VALUE = 831.4 CRITERION= 1.006
MOMENT CONVERGENCE VALUE = 20.60 CRITERION= 0.3555E-01
EQUIL ITER 6 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.1311E-01
LINE SEARCH PARAMETER = 0.7095E-01 SCALED MAX DOF INC = -0.9299E-03
FORCE CONVERGENCE VALUE = 774.9 CRITERION= 0.9580
MOMENT CONVERGENCE VALUE = 19.67 CRITERION= 0.3672E-01
EQUIL ITER 7 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.8859E-02
LINE SEARCH PARAMETER = 0.6283E-01 SCALED MAX DOF INC = 0.5566E-03
FORCE CONVERGENCE VALUE = 727.2 CRITERION= 0.9256
MOMENT CONVERGENCE VALUE = 18.24 CRITERION= 0.2789E-01
EQUIL ITER 8 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.6396E-02
LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = -0.6396E-02
FORCE CONVERGENCE VALUE = 161.4 CRITERION= 0.1909
MOMENT CONVERGENCE VALUE = 12.85 CRITERION= 0.4200E-01
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 = 0.8559E-01
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= 0.7290E-01
LINE SEARCH PARAMETER = 0.9889 SCALED MAX DOF INC = 0.7209E-01
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= 0.1671E-01
LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = 0.1671E-01
FORCE CONVERGENCE VALUE = 336.2 CRITERION= 0.3233
MOMENT CONVERGENCE VALUE = 11.14 CRITERION= 0.2086E-01
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 FORCE-DISTRIBUTED 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 = -0.8515E-01
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 = 0.4398E-01
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 = 0.9162E-01 SCALED MAX DOF INC = -0.4787E-01
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= -0.5712E-01
LINE SEARCH PARAMETER = 0.7985 SCALED MAX DOF INC = -0.4561E-01
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= -0.3585E-01
LINE SEARCH PARAMETER = 1.000 SCALED MAX DOF INC = -0.3585E-01
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 = -0.9519E-01
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 = 0.6918E-01
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 = 0.5000E-01 SCALED MAX DOF INC = -0.9319E-01
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 = 0.5240E-01
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 = -0.9577E-01
FORCE CONVERGENCE VALUE = 0.1696E+05 CRITERION= 43.84
MOMENT CONVERGENCE VALUE = 740.1 CRITERION= 2.085
colopolo is offline   Reply With Quote

Old   September 23, 2011, 11:48
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
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 non-FSI 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.
stumpy is offline   Reply With Quote

Old   September 25, 2011, 20:17
Default
  #3
Member
 
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 5
colopolo is on a distinguished road
Quote:
Originally Posted by stumpy View Post
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 non-FSI 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.
Thanks for your comments.
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.
******************
Force-distributed-surface 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
Attached Images
File Type: jpg fig1.jpg (35.7 KB, 36 views)
File Type: jpg fig2.jpg (61.7 KB, 28 views)

Last edited by colopolo; September 26, 2011 at 04:27.
colopolo is offline   Reply With Quote

Old   September 26, 2011, 17:21
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   September 27, 2011, 05:23
Default
  #5
Member
 
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 5
colopolo is on a distinguished road
Quote:
Originally Posted by stumpy View Post
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.
Thanks for your comments.
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
colopolo is offline   Reply With Quote

Old   September 27, 2011, 12:23
Default
  #6
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
Turn on beta features then look in the Details view for the Remote Displacements. You should see something called "Behavior".
stumpy is offline   Reply With Quote

Old   September 27, 2011, 18:35
Default
  #7
Member
 
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 5
colopolo is on a distinguished road
Quote:
Originally Posted by stumpy View Post
Turn on beta features then look in the Details view for the Remote Displacements. You should see something called "Behavior".
Thank you for your help,
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.
colopolo is offline   Reply With Quote

Old   September 29, 2011, 16:57
Default
  #8
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
The remote displacements are not in CFX-Pre, 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.
stumpy is offline   Reply With Quote

Old   September 30, 2011, 03:54
Default
  #9
Member
 
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 5
colopolo is on a distinguished road
Quote:
Originally Posted by stumpy View Post
The remote displacements are not in CFX-Pre, 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.
Thanks you. I misunderstood it.

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
Attached Images
File Type: jpg fig1.jpg (32.7 KB, 30 views)

Last edited by colopolo; October 3, 2011 at 20:58.
colopolo is offline   Reply With Quote

Old   September 30, 2011, 13:54
Default
  #10
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
On the main WB page you need "Tools > Options > Appearance > Beta Options" turned on. You should then see the option in the image...
Attached Images
File Type: jpg Beam_option.jpg (17.4 KB, 18 views)
stumpy is offline   Reply With Quote

Old   October 2, 2011, 22:45
Default
  #11
Member
 
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 5
colopolo is on a distinguished road
Quote:
Originally Posted by stumpy View Post
On the main WB page you need "Tools > Options > Appearance > Beta Options" turned on. You should then see the option in the image...
Thanks you !!

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 set-up .
Any comments on the above my steps if I have something wrong with procedure

Always, appecite you.

Thanks.
Attached Images
File Type: jpg error.jpg (54.3 KB, 11 views)

Last edited by colopolo; October 2, 2011 at 23:50.
colopolo is offline   Reply With Quote

Old   October 3, 2011, 13:46
Default
  #12
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
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!
stumpy is offline   Reply With Quote

Old   October 3, 2011, 20:57
Default
  #13
Member
 
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 5
colopolo is on a distinguished road
Quote:
Originally Posted by stumpy View Post
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!

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 4, 2011 at 23:18.
colopolo is offline   Reply With Quote

Old   October 4, 2011, 22:03
Default
  #14
Member
 
^^
Join Date: Aug 2011
Posts: 70
Rep Power: 5
colopolo is on a distinguished road
Quote:
Originally Posted by stumpy View Post
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!
running is ok but the result is something weird.

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.
Attached Images
File Type: jpg disp.jpg (31.6 KB, 13 views)
colopolo 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
Viscous force and coefficient viscous force tobino Main CFD Forum 0 February 20, 2011 22:06
User-defined 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 07:07
DEFINE_CG_MOTION and pressure force Teo Fumagalli FLUENT 0 April 11, 2008 10:25
pressure force and viscous force CFD FLUENT 0 March 7, 2006 02:03


All times are GMT -4. The time now is 06:52.