Learning Forum

[Frederik Zemlin]

Hi,

I'm having trouble eliminating rigid body motion in my analysis. The solver fails always at 17% progress. The model is of a quarter symmetric BGA where the PCB has a fixed support and the cut faces have frictionless supports assigned. The load is a thermal condition applied to all bodies. All contacts are bonded, except for three rough ones with the coating on top. Formulation for the bonded contacts is set to augmented lagrange and the stiffness is updated every iteration. Running the contact tool reports no open contacts, all are closed and look normal. I have weak springs enabled.

The solver reports the following error:

 

*** WARNING ***                         CP =    3018.578   TIME= 19:39:20
 Material number 2519 (used by element 2005418) should normally have at 
 least one MP or one TB type command associated with it.  Output of     
 energy by material may not be available.                               

 *** NOTE ***                            CP =    3018.594   TIME= 19:39:20
 The step data was checked and warning messages were found.             
  Please review output or errors file (                                 
 E:\BGA_model\_ProjectScratch\Scr00BE\file0.err ) for these warning     
 messages.                                                              

 *** NOTE ***                            CP =    3018.594   TIME= 19:39:20
 This nonlinear analysis defaults to using the full Newton-Raphson      
 solution procedure.  This can be modified using the NROPT command.     

*** ERROR ***                           CP =    3152.953   TIME= 19:41:34
 The value of UZ at node 957648 is 1.862045956E+11.  It is greater than 
 the current limit of 1.E+09 (which can be reset on the NCNV command).  
 This generally indicates rigid body motion as a result of an           
 unconstrained model.  Verify that your model is properly constrained.  

 *** ERROR ***                           CP =    3152.953   TIME= 19:41:34
 *** MESSAGE CONTINUATION ---- DIAGNOSTIC INFORMATION ***               
 If one or more parts of the model are held together only by contact    
 verify that the contact surfaces are closed.  You can check contact    
 status in the SOLUTION module for the converged solutions using        
 CNCHECK.                                                               

 *** WARNING ***                         CP =    3152.953   TIME= 19:41:34
 The unconverged solution (identified as time 1800 substep 999999) is   
 output for analysis debug purposes.  Results should not be used for    
 any other purpose.   

 

 

Thanks in advance.

 

Frederik

[Ashish Khemka]

Hi Frederik,

The error message indicates rigid body motion. You can create a named selection for node number 957648 and check which body is unconstrained.

Regards,

Ashish Khemka

[Frederik Zemlin]

Hi Ashish,

Thanks for the response. The body in question should be fully constrained as it has bonded contacts to adjacent bodies. I have tried adding an edge blend as the node sits on a corner but it didn't help.

best regards,

Frederik

[Ashish Khemka]

Hi Frederik,

Try running a quick modal analysis to see if you find any rigid body modes.

Regards,

Ashish Khemka

[Frederik Zemlin]

Hi Ashish,

the modal analysis has no free body modes. I think I found the cause for the rigid body motion, a material had a wrong very large CTE assigned. But get an error now that the solution doesnt converge at time step 1250.

best regards,

Frederik

[Ashish Khemka]

Hi Frederik,

Can you please share the snapshot of the solver output?

Regards,

Ashish Khemka

[Frederik Zemlin]

Problem has been solved. Had to set the normal stiffness to 0.01 and solver to direct.