AdvancePipeliner

For lateral buckling analysis of a HP/HT pipeline, I wrote a FORTRAN subroutine to model cohesive/break out behavior of clay type soils under large lateral displacement of the pipeline. I wrote this subroutine under Abaqus 6.6 with Intel FORTRAN 8.x, and when I tried to reuse it under Abaqus 6.7, I found that it didn't work out as it did before. After a quick survey, I found that the problem probably is not from my subroutine. It is from new Abaqus 6.7 approach to contact problems and is well described in SIMULIA support website (MySupport). Following is the explanation of SIMULIA for changes in Abaqus 6.7 contact approach. I just copied it from SIMULIA MySupport to let Google to index it. It also addresses other contact difficulties in Abaqus 6.7.

Several key contact modeling features were enhanced in Version 6.7 of Abaqus/Standard. These notes discuss some of the differences and may help your understanding of why analyses behave differently between versions.

Symptom

The first iterations of an increment are the same in the message file. After several iterations though, the iteration printout becomes different. What changed between versions In Version 6.7, the default handling of severe discontinuities (changes in contact open-close and/or stick-slip status) during solution iteration changed. Prior to Version 6.7, the default behavior was to iterate until no severe discontinuities occurred and equilibrium tolerances were satisfied. The Version 6.7 default approach allows an increment to be accepted as converged if any changes in contact status are small enough. Treating severe discontinuities in this manner is generally more effective than the traditional approach and can improve convergence. See Section 11.3, “New default approach to the handling of severe discontinuities in Abaqus/Standard,” in the Version 6.7 Abaqus Release Notes. The Version 6.7 default approach is known as the “Convert SDI” algorithm and is included in the analysis step definition by using *STEP, CONVERT SDI=YES; the default in Version 6.6 was CONVERT SDI=NO. Be aware that the “Convert SDI” algorithm changed somewhat in Version 6.7. Instead of converting overclosure and opening errors to residual forces and only checking those, Abaqus/Standard now directly compares overclosure and opening errors to the displacement increments. It also estimates contact force errors, and compares those directly to the average forces instead of converting them to residuals. The CONVERT SDI=NO parameter may also introduce differences in some cases because of a few minor changes in the Version 6.7 time stepping logic. For softened, penalty, and augmented Lagrangian contact in Version 6.7, a severe discontinuity iteration is triggered whenever a point closes or opens with CONVERT SDI=NO; this was not the case in Version 6.6. Associated keyword options No particular option, the default behavior has changed. Resolving the different behavior To revert back to the Version 6.6 default algorithm, in which a new iteration is forced if severe discontinuities occur during an iteration, specify *STEP, CONVERT SDI=NO in the first general step of the analysis or in the step where the difference appears. The CONVERT SDI option is propagated to the next general steps.

Symptom

Version 6.6 converges, but Version 6.7 does not. In some cases, Version 6.7 can’t complete the first increment and the status file may look like: STEP INC ATT SEVERE EQUIL TOTAL TOTAL    STEP   INC OF    DOF    IF DISCON ITERS ITERS TIME/ TIME/LPF TIME/LPF MONITOR RIKS ITERS              FREQ 1   1   1U    4     0     4  0.000    0.000  0.1000 1   1   2U    4     0     4  0.000    0.000  0.02500 1   1   3U    4     0     4  0.000    0.000  0.006250 1   1   4U    4     0     4  0.000    0.000  0.001563 1   1   5U    4     0     4  0.000    0.000  0.0003906 THE ANALYSIS HAS NOT BEEN COMPLETED A similar pattern can happen in the middle of the analysis as well. What changed between versions As noted above, the default step definition in Version 6.7 is *STEP, CONVERT SDI=YES; the default is CONVERT SDI=NO in Version 6.6. As part of this, the check to determine whether residuals are increasing has changed. See Section 11.3, “New default approach to the handling of severe discontinuities in Abaqus/Standard,” in the Version 6.7 Abaqus Release Notes. Associated keyword options No particular option, the default behavior has changed. Resolving the different behavior If contact solution controls (e.g. *CONTACT CONTROLS, AUTOMATIC TOLERANCES) or solver solution controls (e.g. *CONTROLS, PARAMETERS=FIELD) were introduced to aid convergence in Version 6.6, first try removing these. If the solution differences remain, try one of the following:

1. Insert*CONTROLS, PARAMETERS=TIME INCREMENTATION 6,
2. Insert *CONTROLS, ANALYSIS=DISCONTINUOUS
3. Specify *STEP, CONVERT SDI=NO

Items (1) and (2) may be preferable to (3) because the total iteration count for the problem will very often be smaller with the default CONVERT SDI=YES. The symptom is quite recognizable so the remedy is straightforward. If you still see a cutback after 4 iterations during each attempt, make either correction (1) or (2). Both of these increase the number of iterations (without SDIs) after which the check is made whether the residuals are increasing in two consecutive iterations. With the option ANALYSIS=DISCONTINUOUS the number is 8. In correction (1) sometimes more than 6 iterations may be needed. Please make additional runs using the appropriate options below before reporting the trouble. As noted, the options can be specified in the input file or in the abaqus_v6.env file. A particular problem may require several options in combination for a successful run in Version 6.7. Symptom Differences in the message files of the Version 6.6 and Version 6.7 runs can be seen from the start of contact. Specifically:

• The largest residual forces are different
• The numbers of contact openings and closures reported are different

What changed between versions The contact penalty stiffness computed from the underlying element material properties has been modified to improve robustness and deliver more consistent results upon small changes to a model; see the first paragraph of the description in Section 11.6, “Modifications to the representative underlying element stiffness and linear penalty stiffness in Abaqus/Standard” in the Version 6.7 Abaqus Release Notes. For self contact and/or slave faces formed on second order elements in Version 6.6, the contact penalty stiffness was further reduced in the code by a factor of 10, 100, or 1000. Such additional factors have been removed in Version 6.7. See the second paragraph of the description in Section 11.6, “Modifications to the representative underlying element stiffness and linear penalty stiffness in Abaqus/Standard” in the Version 6.7 Abaqus Release Notes. Associated keyword options *SURFACE BEHAVIOR, AUGMENTED LAGRANGE or *SURFACE BEHAVIOR, PENALTY or *CONTACT PAIR, TYPE=SURFACE TO SURFACE without *SURFACE BEHAVIOR (it uses *SURFACE BEHAVIOR, PENALTY by default). Resolving the different behavior To revert to the Version 6.6 penalty stiffness behavior, include the following in your abaqus_v6.env file :

import os os.environ["ABA_STD_CONT_V66_UNDERLYINGSTIFF"]="1" mp_environment_export = mp_environment_export + ('ABA_STD_CONT_V66_UNDERLYINGSTIFF',)

The last line must be entered on one line and may be necessary when using multiple CPUs on some platforms. Please always specify the environment variable names using capital letters. You may also try successively changing (usually reducing) the contact penalty stiffness using:

*SURFACE BEHAVIOR, [AUGMENTED LAGRANGE | PENALTY] ,,<scale factor1> *CONTACT CONTROLS, STIFFNESS SCALE FACTOR=<scale factor2>

If this approach is used, it is recommended to try changing the stiffness by order of magnitude scale factors (0.1, 0.01, etc.). The actual scale factor will be the product of <scale factor1> and <scale factor2> if both are used.

Symptom

When the model has element-based slave contact surfaces with the underlying  elements being second order, there are differences in the Version 6.6 and Version 6.7 message files from the start of contact. What changed between versions In Version 6.6, the supplementary constraints on quadratic slave faces were always on. In Version 6.7, there is a special selective scheme that generally imposes less supplementary constraints than in Version 6.6. The selective scheme can improve convergence behavior. See the last bullet in Section 11.7, “Algorithmic changes for contact in Abaqus/Standard” in the Version 6.7 Abaqus Release Notes. Associated keyword options No particular keyword, the default behavior has changed. Resolving the different behavior To recover the Version 6.6 supplementary constraint behavior, set the SUPPLEMENTARY CONSTRAINTS parameter to YES: *CONTACT PAIR, SUPPLEMENTARY CONSTRAINTS=YES Note that the default value in Version 6.7 is SUPPLEMENTARY CONSTRAINTS=SELECTIVE.

Symptom

For augmented Lagrangian contact, the message files start to differ after the first contact augmentation. An augmentation is flagged with the line THE CONTACT CONSTRAINTS WILL BE AUGMENTED in the Version 6.7 message file. In Version 6.6, the warning CONTACT HAS NOT YET CONVERGED is issued. What changed between versions The augmentation is more uniform in Version 6.7; see the second bullet in Section 11.7, “Algorithmic changes for contact in Abaqus/Standard” in the Version 6.7 Abaqus Release Notes. The augmentations must indeed be executed during analysis for the differences between versions to appear; usually, the augmentations are not executed. Associated keyword options *SURFACE BEHAVIOR, AUGMENTED LAGRANGE Resolving the different behavior To recover the Version 6.6 behavior, include the following in the abaqus_v6.env

file:

import os os.environ["ABA_STD_CONT_V66_AUGM"]="1" mp_environment_export = mp_environment_export + ('ABA_STD_CONT_V66_AUGM',)

The last line must be entered on one line and may be necessary when using multiple CPUs on some platforms. Please always specify the environment variable names using capital letters.

Symptom

A *DYNAMIC contact problem runs differently. What changed between versions The contact constraints are skipped during dynamic impact computations for contact pairs with softened pressure-overclosure behavior, augmented Lagrange, or penalty constraint enforcement methods in Version 6.7. Such contact constraints were present in Version 6.6 for other than finite sliding surface-to-surface formulations. Associated keyword options *SURFACE BEHAVIOR, AUGMENTED LAGRANGE *SURFACE BEHAVIOR, PENALTY *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=[EXPONENTIAL | TABULAR | LINEAR] Resolving the different behavior There is no way to revert back to the Version 6.6 approach.

Symptom

A contact problem using the finite sliding surface-to-surface formulation runs differently between Versions 6.6 and 6.7. What changed between versions The finite sliding surface-to-surface formulation has undergone major changes. By default, the contact constraints are now centered at the nodes of the slave surface instead of at a number discrete points on the slave surface facets. Many improvements were made in the search algorithms, and smoothing conditions were added at the edges of master surfaces as well as between master surface facets. Finally, the default penalty stiffness was changed. Associated keyword options *CONTACT PAIR, TYPE=SURFACE TO SURFACE (no SMALL SLIDING) Resolving the different behavior Not all of the changes can be reverted to Version 6.6 behavior. Use: *CONTACT PAIR, TYPE=SURFACE TO SURFACE, CONSTRAINT POSITION=FACE CENTERED to return the position of the contact constraints to the slave surface facets.