Common Errors and Warnings in Convergence Problems-Abaqus

ERROR: TOO MANY INCREMENTS NEEDED TO COMPLETE THE STEP

• Check the message file for any warning messages, such as numerical singularity or zero pivot warnings, that may be causing slow convergence
• If there appear to be no convergence issues, then you may need to increase the limit to the number of increments for that step

ERROR: TOO MANY ATTEMPTS MADE FOR THIS INCREMENT –ANALYSIS TERMINATED

• This is just an error message which gives reason for why Abaqus finally aborted
• Do not modify the solver controls to increase the number of allowable attempts per increment
• Check the message file for warning messages that could cause convergence difficulties
• Check the model definition, and make sure that the model can actually withstand the applied loads

ERROR: TIME INCREMENT REQUIRED IS LESS THAN MINIMUM SPECIFIED-ANALYSIS ENDS

• Again, this is just an error message which gives reason for why Abaqus finally aborted-it is not a suggestion by Abaqus to reduce the minimum allowable increment size
• Check the message file for warning messages that could cause convergence difficulties
• Check the model definition, and make sure that the model can actually withstand the applied loads

WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES THE STRAIN TO CAUSE FIRST YIELD AT 500 POINTS

• Indicates excessive plastic yielding in the given increment
• Possible causes would be:

         ·         Excessive or unrealistic loading (inconsistent units, for example)

         ·         Incorrect or insufficient stress-strain plastic data

         ·         Insufficient mesh refinement

         ·         Unstable deformation, such as buckling 

NOTE: The factor ‘fifty’ mentioned in the warning message cannot be modified

WARNING: ELEMENT 441 IS DISTORTING SO MUCH THAT IT TURNS INSIDE OUT  

•  Possible causes would be:
  ·         Insufficient mesh refinement
  ·         Hourglassing in first-order reduced integration elements
  ·         Inconsistent units for material properties and/ or loads
  ·         Excessive or unrealistic loads
  ·         Adjusting slave nodes of severely overclosed surfaces for contact pairs or tie constraints
            (initial overclosures)

WARNING: THE SYSTEM MATRIX HAS  9 NEGATIVE EIGENVALUES

•   Possible causes would be:

            .          Some form of loss of stiffness suggesting that the stiffness matrix is assembled about a 

                       non-equilibrium state: 

                                   .    Geometrical instability: buckling, compression 

                                   .    Material instability: inappropriate hyperelastic material models, onset of perfect

                                        plasticity 

            .        Numerically, the use of Lagrange multipliers in certain cases may also lead to these

                     warning messages 

            .        Use of 3D second-order elements as contact (slave) surfaces

•  Typically, these warning messages do not appear in converged iterations

                  .          If they do, ensure that the solution is physically acceptable

WARNING: SOLVER PROBLEM. NUMERICAL SIGULARITY WHEN PROCESSING NODE 1 D.O.F. 3 RATIO=3.141E+15

•  Typically suggests an unconstrained rigid body motion
•  Even if the analysis runs to completion with these warnings, the results may not be accurate

WARNING: SOLVER PROBLEM. ZERO PIVOT WHEN PROCESSING NODE 1 D.O.F.1

• Typically suggests an overconstraint
• Even if the analysis runs to completion with these warnings, the results will not be accurate

Helping Abaqus Find a Converged Solution

Understand the physics of the problem:

• It is vital to understand the physics behind any problem. For example:

·         How does the actual structure behave for the applied loading

·         How is the structure constrained at different locations

·         How are the different components connected to each other

·         What is the nature of the loads acting on the structure

• We make many assumptions and approximations in any analysis, which have to be reasonable and justifiable. For example:

·         Is the chosen material model appropriate?

·         Are the element types properly chosen

·         Is the mesh size appropriate

·         Is contact properly defined (choice sliding algorithm, friction coefficient, surface behavior etc.)

Build up the model slowly:

•  The most important way to help Abaqus find a converged solution is to build up the model piece by piece

·         Do not put every complexity and detail directly in the first attempt-it probably will not work

• Start with the simplest model possible-perhaps one with contact but no plasticity, friction, or nonlinear geometry-this would give valuable insight into how the model behaves

• Add complexities (friction or plasticity) one at a time. Doing this will limit the number of questions to consider if a convergence problem arises.

• Although it might seem as if this process will increase the time needed to perform the analysis, in fact it often reduces the time because debugging a large model with convergence problems can take days or weeks.

Provide reasonable values:

•  Make sure that the units of the material properties (especially density) are consistent with the geometry and loads in the model.

• Make sure that the material properties provide sufficient stiffness to resist the applied loads, or plan accordingly and use the appropriate analysis techniques.

• Give reasonable values for the minimum increment size and the maximum increment size (or use the defaults).

• Use the message file or job diagnostics to identify the proper cause(s) for nonconvergence

Reasons for cutback in load increment of a convergence problem-Abaqus

The reasons for cutback in load increment of a convergence problem in Abaqus are divided into three categories. They are as follows

Algorithmic cutbacks

• Divergence

•  Too slow convergence

• Too many iterations

Stiffness/residual calculations

• Element distortion

• Material model calculation problems

Contact

• Too many severe discontinuity iterations

• Too severe penetration

Causes of convergence problems

The most common cause of convergence problem in nonlinear simulations is inadequate FE modeling.

Examples of inadequate FE modeling include:

• Defining conflicting constraints between boundary conditions, contact conditions, and /or multi point constraints

• Not adequately constraining the model-allowing rigid body motions

• Having incomplete (or inadequate) material data

• Using an inappropriate element for the problem

Another common cause of convergence problems is that the physical system is very unstable, making it very difficult to find an equilibrium solution.

Examples include:

• Buckling of thin-walled, cylindrical shell structure

• Snap-through with contact changes

• Compression of highly confined, incompressible materials (rubber)

• Development of local instabilities occur

In these cases it is important that the correct element type and analysis techniques be used; otherwise, it can be very difficult to obtain a solution.

Symptoms of convergence problems in Abaqus

The symptoms of almost all convergence problems can be found in the message(.msg) file. The printed output(.dat) and status(.sta) files may also provide hints about certain issues

The following message in the message file,

***WARNING: THE SOLUTION APPEARS TO BE DIVERGING

is not the cause of a convergence problem-it is a reason for Abaqus to cut back the increment size.

However, such a warning might be the symptom of a convergence problem in the model.

It also might be because too large an increment was used.

The following are some warning messages that appear in the message file and which may be symptoms of a convergence problem

***WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES THE STRAIN TO CAUSE FIRST YIELD AT 7 POINTS

***WARNING: THE SYSTEM MATRIX HAS 3 NEGATIVE EIGENVALUES

***WARNING: ELEMENT 441 IS DISTORTING SO MUCH THAT IT TURNS INSIDE OUT

***WARNING: THE SOLUTION APPEARS TO BE DIVERGING

***WARNING: OVERCLOSURE OF CONTACT SURFACES SURF_A AND SURF_B IS TOO SEVERS—CUTBACK WILL RESULT

***WARNING: SOLVER PROBLEM. ZERO PIVOT WHEN PROCESSING NODE D.O.F.1

***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE 15 D.O.F 2 RATIO-3.14159E+15