One or more elements have become highly distorted. Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere. Try incrementing the load more slowly (increase the number of substeps or decrease the time step size). You may need to improve your mesh to obtain elements with better aspect ratios. Also consider the behavior of materials, contact pairs, and/or constraint equations. If this message appears in the first iteration of first substep, be sure to perform element shape checking.
If you are working with models that involve elastic-plastic material properties, you may encounter an error message related to “element distortion”. This message is a numerical representation of the model’s behavior and may or may not reflect real-world phenomena accurately. To troubleshoot this issue, you should follow these steps:
1、Check the maximum stress in the model at the last converged time step.
Check the stress levels in the model at the last converged time step and compare them to the yield and ultimate stress as defined on the stress-strain curve within ANSYS. If the stress levels are close to or above the yield stress, the component may be approaching or at plastic collapse. This indicates that the model may have reached its maximum load capacity under the defined loads and boundary conditions.
2、Verify that the model behavior is realistic.
Ensure that the model’s behavior is realistic and that there are no poorly defined boundary conditions, loads, or contacts causing element distortion. For example, a contact pair that should slide may be defined as bonded, which can prevent sliding and result in artificial distortion of elements and fictitious plastic strains.
3、Make sure large displacements are turned ON.
It is essential to turn on large displacements. The mechanical stiffness of the model depends on material properties, contacts, and geometry. Large displacements refer to changes in model stiffness due to geometric changes, and ignoring geometric non-linearity can lead to convergence difficulties and erroneous results when dealing with plasticity.
4、Modify the mesh
Modifying the mesh can help to fix the issue. Try refining the mesh in the problem area by changing element sizing, order, or type, using surface meshing, or using slices for better mesh transition. By combining these methods, you can efficiently obtain a mesh that allows you to get over the convergence issue.
5. Apply the load more “slowly”.
In transient analysis, time is a modeled physical phenomenon, where the load steps are referred to as time steps. By applying the load incrementally, we can help the model converge more smoothly. For example, we can define the time steps as shown in Fig 2 below. The initial time step is 0.10, and the model will first try to solve for 0.1*Total load. If this fails, the algorithm can reduce the time step factor to as low as 0.05 (Minimum Time Step) to improve convergence. If convergence still isn’t achieved, the solution will crash with an error message.
6. Increase the maximum number of equilibrium iterations.
The number of iterations is the maximum number of attempts the model will make to reach a converged solution at a given load. By default, this is set to 26 within ANSYS, but it can be increased. We recommend changing it to 50 to allow the model more iterations before deciding to bisect. In Workbench, the maximum equilibrium iterations can be changed by adding an APDL command snippet under “Static Structural” or where the loads are defined, as shown below:
The above command would set the iterations to 50. This can be confirmed by checking the solve.out file where you should see the following text:
USE A MAXIMUM OF 50 EQUILIBRIUM ITERATIONS EACH SUBSTEP
7. Use Linear Material Properties.
Linear material properties should be used as a last resort, and only if the localized stress/strain response in the problem area is not relevant to the overall objective. In some cases, it’s possible to assign linear material properties only to a small slice of the component in the region of interest. Alternatively, you can create a named selection and assign linear material properties to it using a command snippet.
By following these practical solutions, you can improve convergence and overcome element distortion error in structural simulations. If you encounter any issues or have any questions, please feel free to ask them in the comments, and we’ll do our best to help.