نحوه حل مشکل Abaqus - Too many attempts made for this increment
نحوه حل مشکل Too many attempts made for this increment در نرم افزار آباکوس (Abaqus)
Debugging Abaqus/Standard divergence with too many cutbacks in the last attempted increment
Question
My Abaqus/Standard analysis has terminated because too many cutbacks were taken in the last time incrementthat was attempted. How can I correct this?
Answer
(The following applies to all versions.)
Possible sources of the problem include:
• Failure to determine the contact state: Identified by termination after too many severe discontinuity iterations (SDIs).
These difficulties are generally caused by problems with the contact definitions. Consider the following:
o If the termination occurs in first increment, possible causes include excessive overclosures.
o If the termination occurs after the first increment, possible causes are contact chattering (slave surface contact state alternates between opened and closed repeatedly so that the maximum number of SDIs is reached). Look at the causes of contact chatter for additional information.
• Failure to achieve equilibrium: Identified by force/moment residuals and displacement/rotation corrections not getting smaller; termination error indicates divergence. Consider the following items in diagnosing the problem:
o Contact-related issues.
o Excessive element distortion warnings: normally occurs only after the analysis simulation has partially completed, unless the initial model was incorrect.
o Hourglassing (deformed mesh goes into a regular pattern that clearly is not physical; normally seen easily in deformed mesh plots).
o Excessive yielding, generally associated with a message that the current strain increment exceeds the strain to first yield by more than 50 times.
o Large elastic strains when using an elastic material model in a geometrically non-linear analysis.
Large elastic strains should be modeled with the hyperelastic or hyperfoam material models; elastic material models are intended for elastic strains that remain small (
o Is the material response incompressible or nearly incompressible? (Frequently elastic-plastic materials are nearly incompressible.)
o Possible unconstrained rigid body motion indicated by the presence of NUMERICAL SINGULARITY warnings and very large displacement corrections.
o Overconstraints frequently indicated by zero pivot messages in the message (.msg) file.
o Local instabilities such as wrinkling or material localization developing during the analysis.
o Analysis ends in a core dump; analysis does not complete and output files end in the middle.
o If the analysis seems to be approaching a load maximum and negative eigenvalue messages appear during the iterations of the last increment, the analysis may be reaching a global instability.
o Very small displacement correction, but the tolerance on the residual force is not satisfied.
This is probably due to numerical precision issues such as having all the coordinates in the model be very large compared to the size of the model or using units in which typical mass-, force-, or energy-like quantities are very small or large. If the displacement corrections are truly small relative to the displacement increment, the increment has probably converged. The tolerance on the force residual can be relaxed in this case.
o Follower loads (including distributed pressures) in analyses including non-linear geometric effects.
و اما اگر در نخست?ن گام حل به مشکل برخورد نمود?د:
Source of convergence difficulty in the first increment of an Abaqus/Standard contact analysis
Question
My Abaqus/Standard contact analysis terminates in the first increment after too many severe discontinuity iterations. What might be causing this?
Answer
(The following applies to any version.)
One or more of the contact pairs in the analysis may have an excessive initial overclosure. The overclosure may be a feature of the model, or it may be the result of a modeling error. In either case, an excessive overclosure may cause the analysis to terminate prematurely. In this section some common sources of excessive initial overclosures are discussed.
1. In the case of an overclosure that is a feature of the model, as with an interference fit analysis, the overclosure may be too large to resolve in one increment.
To help with the diagnosis, print information about the overclosures during the datacheck and solution phases:
o Abaqus/CAE: Job Module : Job Manager : Edit ? General ? Preprocessor printout ? Print contact constraint data
Step Module : Output ? Diagnostic Print... ? Contact
o Input file: *PREPRINT, CONTACT=YES
*PRINT, CONTACT=YES
The solution in this case is to use the *CONTACT INTERFERENCE option to remove the overclosure. Sometimes resolving the overclosure over several increments is required. Adjusting the solution controls to increase the maximum number of severe discontinuity iterations allowed in an increment may also be needed to overcome this difficulty.
Sometimes small overclosures (relative to element dimensions) can be removed by adjusting the slave nodes in the contact pair:
o Abaqus/CAE: Interaction Module : Interaction Manager : Edit ? Slave node adjustment
o Input file: *CONTACT PAIR, ADJUST=[Node set label | Adjustment value]
2. The master surface normals may be pointing away from the slave surface.
Use Abaqus/Viewer to check the normals on the master surface.
The solution in this case is to redefine the master surface so the normals point towards the slave surface, assuming the surfaces are open.
3. The model may be permitting a rigid body motion (VERY large overclosures detected; sometimes on the order of 10**15), typically due to loading a body with forces when there are insufficient boundary conditions or insufficient active contact constraints to remove rigid body motion.
You will, in most cases, also see messages about NUMERICAL SINGULARITIES in the message (.msg) file. Print overclosure information during the solution (as described in Item 1) to diagnose the problem.
This case can be resolved with different approaches:
o Use boundary conditions to move the bodies until they are just in contact (do this in a "dummy" step). In the next step remove these boundary conditions and replace them with forces that maintain the contact (this is the recommended technique).
o Add soft springs to the model in the directions of the rigid body motion. The degrees of freedom (dofs) requiring springs can be seen from the dofs associated with the numerical singularity messages. The stiffness of the springs must be small enough that the forces in the springs are negligible compared to typical forces in the problem.
o Use contact stabilization (*CONTACT CONTROLS, APPROACH (Version 6.1 or later) or *CONTACT CONTROLS, STABILIZE(Version 6.5 or later)) to stabilize the motion (using damping effects) when, at some point in the analysis, contact is meant to prevent rigid body motion. (If this is not done carefully, the viscous forces can dominate the solution. Print out the forces due to viscous effects applied with these options using the VF output variable. Additionally, output variable ALLSD measures the energy dissipated by viscous damping; the ratio of this quantity to the elastic strain energy or other appropriate general energy measure should be small.)
If the analysis converges in an iteration during which NUMERICAL SINGULARITIES appear, check the solution carefully. Abaqus/Standard attempts to fix the solution, but sometimes this fix will not give a correct solution. You should remove the cause of the NUMERICAL SINGULARITIES instead. If numerical singularities only occur in iterations prior to the iteration which converges, the solution should be correct; however, you should always check that this is so.
4. Contact chattering: the contact state changes from one iteration to the next so that the maximum number of SDIs (severe discontinuity iterations) is reached. Read Causes of contact chatter for additional information.
For more information see:
• 'Contact interaction analysis: overview'
o Section 34.1.1 of the Abaqus 6.11 Analysis User's Manual
o Section 35.1.1 of the Abaqus 6.12 Analysis User's Manual
• 'Commonly used control parameters,' Section 7.2.2 of the Abaqus 6.11 or 6.12 Analysis User's Manual
• 'Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs'
o Section 34.3.5 of the Abaqus 6.11 Analysis User's Manual
o Section 35.3.5 of the Abaqus 6.12 Analysis User's Manual
• 'Contact formulations in Abaqus/Standard'
o Section 36.1.1 of the Abaqus 6.11 Analysis User's Manual
o Section 37.1.1 of the Abaqus 6.12 Analysis User's Manual
• 'Common difficulties associated with contact modeling in Abaqus/Standard'
o Section 37.1.2 of the Abaqus 6.11 Analysis User's Manual
o Section 38.1.2 of the Abaqus 6.12 Analysis User's Manual
