What is too many attempts error in Abaqus? How to solve it?
In Abaqus, the “too many attempts” error typically refers to a convergence issue encountered during the solution process of an analysis. It is one of the most famous errors in the Abaqus. This error could occur in analyses using the Standard solver. Abaqus uses an iterative algorithm to solve complex problems, and convergence is achieved when the solution reaches a stable state. The error message “too many attempts” indicates that Abaqus has exceeded the maximum number of attempts allowed to reach convergence. This means that the solution is not converging within the specified tolerance limits even after a significant number of attempts. Now, you might say, “What is attempt?” or “What do you mean by the iterative algorithm?” To answer your questions, you need to understand how the Standard solver works and the Attempt concept in the Standard solver. Knowing these concepts helps you better understand the “Too many attempts error” and how to solve it. Our recommendation is to read this article: “A Clear Guide to Abaqus Step, Increment, Iteration, Attempt Concepts” or watch its video: https://www.youtube.com/watch?v=XEvuQeG9UiI
When this error occurs, it suggests that the analysis setup or model may have issues that prevent convergence. Some common reasons for encountering the “too many attempts” error in Abaqus include:
- Incorrect boundary conditions: If the applied loads or constraints are not properly defined, it can lead to convergence problems. Check if the boundary conditions are correctly assigned and consistent with the problem you are trying to solve.
- Material model or properties: Certain material models may require careful parameter selection and may be sensitive to certain conditions. Verify that the material properties and constitutive models are appropriate for the analysis and that they are defined correctly.
- Numerical instability: The analysis may involve elements or conditions that lead to numerical instability, such as severe mesh distortion, very large or small element sizes, or excessively high deformation. Review the model and make necessary adjustments to improve stability.
- Insufficient convergence tolerance: The convergence criteria set for the analysis may be too strict, leading to premature termination of the solution process. Consider adjusting the convergence tolerance to a more suitable value.
Generally, you can say: “Too many attempts made for this increment”; means the solver attempted several times to calculate the equations for this increment, but the convergence conditions were not satisfied; so, you either look into the “Increment size” again and modify it or look somewhere else to overcome this Error.
Methods of solving the “Too many attempts made for this increment” error
In problems you are having contacts and interactions, you could use the methods below:
- Use a smaller mesh size so you can have a greater number of elements (fine mesh) in surfaces that are in contact with each other. Like the picture below demonstrating an extrusion process, using a fine mesh in the curvature surface will give you a smooth curvature and increase the chances of avoiding the Too many attempts error.
- You can create a Step between the Initial step and the main step (loading step) to define the contacts properly. This extra step will help to apply the contacts before loading conditions to probably avoid the error. In this step, you must pick a point from each part of the assembly and fix all its degrees of freedom and in the loading step deactivate them and apply the loading conditions.
- If the two previous methods didn’t work out for you, you can change your solver from Standard to Explicit and apply the proper changes in the Interaction and Load modules due to the Explicit solver. Oh, don’t forget to define the Density if you’re using the Explicit solver.
In problems having large deformation, such as forming you can use the following methods:
- Using smaller meshes in regions having large deformations.
- Check the strain value (Total strain); if it is greater than the maximum value in the plastic area in the stress-strain curve, it means the model is entering the damage area, and that means you must define the damage model in the material properties of the model. This leads to accurate results and most probably avoids the Too many attempts error.
- Using the Explicit solver instead of the Standard solver along with the ALE Adaptive Mesh method.
How can I change the allowed number of severe discontinuity iterations?
Severe discontinuity iteration is detected contact changes (for example, chattering) in the current iteration, which cause convergence issues, and it’s a common thing in the contact field. The ABAQUS/Standard will iterate until there are no more severe discontinuities, or they will be small enough.
You would be able to increase the maximum number of the severe discontinuities iteration by using the keyword “*CONTROLS, PARAMETERS=TIME INCREMENTATION,,,,,24” (see figure 1) or through the graphical interface (see figure 2 and 3). Go to the step module, then proceed according to figure 2. Then choose the desired step and select “Edit” (figure 3). According to figure 3, go to the “Time Incrementation” tab, the first More option, and change the IA from the default 5 to any number you want.
Figure 1: change the number of allowed severe discontinuity iterations through the input file
Figure 2: select the General Solution Controls then Manager
Figure 3: change the number of allowed severe discontinuity iteration
