Convergence issue in trim rigidity analysis

[kk10CAE]

Hi,
Myself Krishna, I am facing a convergence issue in non linear static analysis in abaqus please find detailed description below

Analysis objective:-
To find maximum displacement & von mises stress on a curved trim surface applied with 22N force over a applicator(flat circular plate) in vertical direction.

Software used:- ABAQUS 6.10

Analysis performed:- Non linear static analysis

Description:-
Trim assembly modeled as shell & applicator as rigid with rigid body.
Trim mounting locations are encastred.
Loading location is center node of rigid body on rigid.
Surface to surface contact with applicator as master & trim surface as slave
At loading location, fixed boundary condition was applied as 12456 & 3rd direction kept free.
Cload of 22N applied on loading location(node # 1) of applicator on vertical direction towards trim surface.

Problem:- facing convergence issue.

Error message on .MSG file:-
***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE 1,D.O.F. 3. THIS NODE HAS NO STIFFNESS IN THE SPECIFIED DIRECTION AND IS NOT COUPLED WITH THE REST OF THE MODEL.
               CONVERGENCE CHECKS FOR EQUILIBRIUM ITERATION     4
 AVERAGE FORCE 6.032E-08   TIME AVG. FORCE  1.000E-02 
LARGEST RESIDUAL FORCE  -8.594E-03   AT NODE 1   DOF  3 
LARGEST INCREMENT OF DISP 5.041E-14   AT NODE 3034 DOF  3
 LARGEST CORRECTION TO DISP. -6.908E-14   AT NODE 2674   DOF  2
THE FORCE IS ZERO EVERYWHERE BUT THE FORCE  RESIDUAL OR THE DISP. CORRECTION IS NON-ZERO

 AVERAGE MOMENT 9.472E-13   TIME AVG. MOMENT 2.920E-02 (FROM FORCE FIELD)
 LARGEST RESIDUAL MOMENT 5.383E-11   AT NODE       1172   DOF  4 
LARGEST INCREMENT OF ROTATION  7.066E-15   AT NODE 2664   DOF  6 
LARGEST CORRECTION TO ROTATION 8.213E-15   AT NODE 2674   DOF  4
          THERE IS ZERO MOMENT EVERYWHERE 
 ***NOTE: THE SOLUTION APPEARS TO BE DIVERGING. CONVERGENCE IS JDGED UNLIKELY. 
 ***ERROR: TOO MANY ATTEMPTS MADE FOR THIS INCREMENT

"Please suggest me ideas to fix this issue"

 

[corus]

It's not restrained in the 3 direction.

 

[kk10CAE]

@corus - 3rd DOF of applicator released intensionally, so that it will move in that particular location & press the trim below

 

[kk10CAE]

Actually this issue was sorted using following controlcards

*CONTACT CONTROLS, AUTOMATIC TOLERANCES, STABILIZE
*CONTROLS, PARAMETERS = TIME INCREMENTATION
, , , , , , 25, , ,
*CONTROLS, ANALYSIS = DISCONTINUOUS

Need to study about above mentioned cards.
If any one have idea about those, please let me know

 

[adfergusson]

How did you create your geometry? I have a suspicion that your parts may not actually be in contact. If the parts are not fully in contact then a rigid body motion will be required for them to come into contact. Such a motion will lead to a stiffness matrix that is singular so the system cannot be inverted for a solution, which is probably why you're getting a 'numerical singularity' message. A way you can check for this is to use displacement control rather than load control. If the model then runs then it is likely that you've got issues with your parts not being in contact/rigid body motion. In this case, either put them in contact or use contact stabilisation to allow you to use load control.