numerical singularity problem

[brendanpeach]

Hi
I'm currently modelling a train track insulated joint bar with abaqus and i can't fix a problem i keep encountering. The job keeps re-attempting the first increment of the first step because of problems.

The model consists of two rail sections with and end post in the middle and two 6 hole joint bars bolted across the join. The rail sections have tie constraints to the end post. I've experimented with the joint bar interactions and have found that i seem to get more progress with the joint bars tied to the rail face rather than a no friction contact. the joint bars and rail all have interactions with the 6 bolts, no gaps exist between the bolts and the bolt holes. the bolts are currently modelled as deformable parts with the normal properties of steel.

The warnings i get are along these lines:
***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING ELEMENT
BOLT2.1 D.O.F. 1 RATIO = 3.08682E+011.

***WARNING: THE SYSTEM MATRIX HAS 27 NEGATIVE EIGENVALUES.

CONTACT PAIR (ASSEMBLY__PICKEDSURF618,"ASSEMBLY_NEG BAR HOLE 5") NODE
BOLT5.229 IS OVERCLOSED BY 3.32517 WHICH IS TOO SEVERE.

***NOTE: SEVERE CONTACT OVERCLOSURES EXIST. CONVERGENCE IS JUDGED UNLIKELY.

As you can see the problem seems to be with the bolts. with the numerical singularity problems i am getting problems with D.O.F 1,2 and 3.

Any help would be appreciated.

 

[rstupplebeen]

brendanpeach,

With contact I usually find that the convergence problems are due to rigid body motions. Basically on the first time step the part moves to infinity 3E11. This can be solved with weak springs or the addition of damping to the system. I can not remember the exact buzz word (viscus damping??) for the damping but with the help this should get you there. It is in the contact or solution controls. The damping is a newer feature that will reduce the influence before convergence completes. You should check out the energies in the system to see if the energy is providing too much error for your system. Hope this helps.

Robert Stupplebeen

 

[xerf]

Have you tried to set the initial time increment to a small value ?

 

[brendanpeach]

xerf:
the total time is set to 1 and my initial time increment is 0.1, but having said that the model has attempted the first step a couple of times, taking the increment down to like 0.005, so i don't think that's it.

rstupplebeen:
i have tried applying contact controls, i think i set a control on so that it moves nodes to prevent overclosure. i'll look into putting dampers on the bolts, maybe i could fix boundary conditions as well? i don't understand how the pins could be moving to infinity..

i replaced my 6 bolts last night with analytical rigid body pins and the system solved! the stresses seem a bit low but i haven't had a good look at the deformation scale etc. this still doesn't fix my initial problem. i initially modelled the bolts with cylindrical parts and placed the bolt load on them but thought that maybe the bolt load is causing them to buckle. so then i added the bolt head and nut to distribute the bolt force over the joint bar.

sound like i've made a fundamental error without realising??

 

[xerf]

dt=0.005 could be considered a large time increment, for contact cases. I had simulations that needed 1.e-9 to achieve convergence.

ABAQUS tries to reduce the time increment only a limited number of times, I think the default setting is 4 or 5 time and then it aborts if the solution does not converge. If your load magnitude is significant then 0.005 of it might generate a significant amount of inter-penetration of the contact surfaces, especially if the mesh is inadequate.

You should try a smaller initial increment, say 0.001.

 

[rstupplebeen]

*CONTACT CONTROLS, STABILIZE was what I was trying to remember. I found this article in the archives

http://www.eng-tips.com/viewthread.cfm?qid=194276&page=3

I would check out that link and help for this command. Good luck.
Rob Stupplebeen

 

[bassmanjax]

I agree with Xerf - depending on how close the parts are at the start, you may well need a very small starting increment to get things going.

Regards

Martin Stokes CEng MIMechE

 

[ysg519]

brendanpeach,
Please let me know how you resolved this problem. Did xerf's advice on changing time to 1.e-9 help? My error is shown below. Thanks


***NOTE: SEVERE CONTACT OVERCLOSURES EXIST. CONVERGENCE IS JUDGED UNLIKELY.


INCREMENT 1 STARTS. ATTEMPT NUMBER 5, TIME INCREMENT 3.906E-03


***WARNING: THE SYSTEM MATRIX HAS 2 NEGATIVE EIGENVALUES.
EXPLANATIONS ARE SUGGESTED AFTER THE FIRST OCCURRENCE OF THIS MESSAGE.


***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE
CEBAF_ASM-3-1.41 D.O.F. 1 RATIO = 4.22608E+10.