convergence issues in three-point-bending 1

[isok89]

Hello,



I am trying to simulate a three-point bending test by contact modelling in Abaqus using the implicit integration scheme.
The set-up is as follows:

- Contact pairs, surface to surface
- Applying load on rigid plate
- time step 1

Whatever I do, I can't get it converged, at 0.85 timestep, this value has been haunting me for days, the job aborts and in the message
file I get an error message about 'maximum contact force error, maximum penetration error'.
The nodes that are creating all the fuss are located on the corner radii.

I tried all of the following:

- Increase contact stiffness by factor 10 - 99
- Use Lagrange Multiplier
- Use default settings in contact control for stabilization
- Unsymmetric solver
- Mesh refinement at corners
- Frictionless/friction

This is output from the message file:

MAX. PENETRATION ERROR 343.443E-12 AT NODE SEC41A-1.130 OF CONTACT PAIR
(ASSEMBLY_SLAVESURFACE,ASSEMBLY_MASTERSURFACE)
MAX. CONTACT FORCE ERROR 3.91508E-06 AT NODE SEC41A-1.2547 OF CONTACT PAIR
(ASSEMBLY_SLAVESURFACE,ASSEMBLY_MASTERSURFACE)
THE CONTACT CONSTRAINTS HAVE CONVERGED.

AVERAGE FORCE 61.6 TIME AVG. FORCE 6.97
LARGEST RESIDUAL FORCE 86.9 AT NODE 2851 DOF 2
INSTANCE: SEC41A-1
LARGEST INCREMENT OF DISP. -0.434 AT NODE 2823 DOF 2
INSTANCE: SEC41A-1
LARGEST CORRECTION TO DISP. -0.174 AT NODE 2823 DOF 2
INSTANCE: SEC41A-1
FORCE EQUILIBRIUM NOT ACHIEVED WITHIN TOLERANCE.

AVERAGE MOMENT 17.6 TIME AVG. MOMENT 295.
LARGEST RESIDUAL MOMENT 35.6 AT NODE 2851 DOF 6
INSTANCE: SEC41A-1
LARGEST INCREMENT OF ROTATION -0.136 AT NODE 2851 DOF 6
INSTANCE: SEC41A-1
LARGEST CORRECTION TO ROTATION -5.217E-02 AT NODE 2851 DOF 6
INSTANCE: SEC41A-1
MOMENT EQUILIBRIUM NOT ACHIEVED WITHIN TOLERANCE.


Would greatly appreciate any help

 

[IceBreakerSours]

The implicit solver is not having any trouble with contact.

..
THE CONTACT CONSTRAINTS HAVE CONVERGED.
..
FORCE EQUILIBRIUM NOT ACHIEVED WITHIN TOLERANCE.
..
MOMENT EQUILIBRIUM NOT ACHIEVED WITHIN TOLERANCE.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Dave442]

There is an example of a three point bend test in the Abaqus Example Problems Guide:

2.1.16 Progressive failure analysis of a thin-wall aluminium extrusion under quasi static and dynamic loads

Although it is not a static analysis and also includes damage and failure, it might help you figure out your boundary conditions, interactions etc..

 

[isok89]

I solved the issue however within a static general step, once yielding occurs, converging stops. I assume the algorithm in static general can't handle the zero slope. Am I wrong in my assumptions? I have tried with static riks and now
I do get plastic strains and stresses beyond first yielding.


I can't get beyond first yield stress in the static general step.

 

[Mustaine3]

Zero slope is a problem.
The applied load is increased, but the resistance (stresses) can't increase. Then it is hard to find a equilibrium.

 

[isok89]

I used displacement control and the results are nice. I am tracking the load by extracting the reaction forces of
my supports, but I'm not sure how good of a representation this is of my actual load. Is there a better way to determine my actual load in the three point bending test?

 

[Mustaine3]

No, reaction force is the way to go.

But be aware, that with displacement control and zero slope in the plasticity data, the solution might not be unique. When yield stress is reached, there are is not the one strain for the stress. So again, use a positive slope in your plasticity data.

 

[isok89]

I am tracking the reaction forces and conducting a mesh convergence study right now.
However as my mesh density increases I have to track numerous nodes.


Is it possible to have a reference node for multiple nodes? Like I select nodes from my deformable part and I
assign a reference node towards it and I can make a set of this reference node in history output. Basically this reference node will have the average value of my selected nodes.

 

[Dave442]

You can tie the degrees of freedom for a node set to a reference point using *Equation.

 

[isok89]

I am having trouble now with applying Riks method, I have tried different arc length factors but I'm having convergence issues prior to collapse load. With displacement control static general everything went fine and I validated the model.
Isn't Riks just an improved procedure of displacement control, with the arc length method?

The error message is as follows:

AVERAGE FORCE 1.885E-04 TIME AVG. FORCE 1.885E-04
LARGEST RESIDUAL FORCE 3.052E-07 AT NODE 63 DOF 2
INSTANCE: APPLICATOR-1
LARGEST INCREMENT OF DISP. -1.119E-04 AT NODE 31428 DOF 1
INSTANCE: BEAM-1
LARGEST CORRECTION TO DISP. -1.266E-06 AT NODE 31428 DOF 1
INSTANCE: BEAM-1
DISP. CORRECTION TOO LARGE COMPARED TO DISP. INCREMENT

AVERAGE MOMENT 5.647E-05 TIME AVG. MOMENT 5.647E-05
LARGEST RESIDUAL MOMENT -5.980E-10 AT NODE 732 DOF 6
INSTANCE: BEAM-1
LARGEST INCREMENT OF ROTATION 2.126E-06 AT NODE 597 DOF 6
INSTANCE: BEAM-1
LARGEST CORRECTION TO ROTATION 2.404E-08 AT NODE 597 DOF 6
INSTANCE: BEAM-1
ROTATION CORRECTION TOO LARGE COMPARED TO ROTATION INCREMENT

NUMBER OF EQUATIONS = 222834 NUMBER OF FLOATING PT. OPERATIONS = 3.12E+10

CHECK POINT START OF SOLVER

CHECK POINT END OF SOLVER

ELAPSED USER TIME (SEC) = 3.2000
ELAPSED SYSTEM TIME (SEC) = 0.0000
ELAPSED TOTAL CPU TIME (SEC) = 3.2000
ELAPSED WALLCLOCK TIME (SEC) = 3

1 SEVERE DISCONTINUITIES OCCURRED DURING THIS ITERATION.
1 POINTS CHANGED FROM CLOSED TO OPEN

CONVERGENCE CHECKS FOR SEVERE DISCONTINUITY ITERATION 31

MAX. PENETRATION ERROR 382.994E-09 AT NODE BEAM-1.31451 OF CONTACT PAIR
(ASSEMBLY_SLAVE,ASSEMBLY_MASTER)
MAX. CONTACT FORCE ERROR 5.92057E-03 AT NODE BEAM-1.31451 OF CONTACT PAIR
(ASSEMBLY_SLAVE,ASSEMBLY_MASTER)
THE ESTIMATED CONTACT FORCE ERROR IS OUTSIDE OF CONVERGENCE TOLERANCES.

I have tried mesh refinement at the slave surface, but to no avail. Riks method doesn't allow me to implement
automatic stabilization from contact controls. However my static general displacement controlled model convergences even without contact stabilization.