If you are looking to the peak stress at crack tip, I think you are wasting time: the solution does not converge (peak stress=Inf).

Instead, to get the Stress intensity Factor (SIF) use a very fine mesh, with a ratio element size/crack length of about 1e-4-1e-5 or less and take the stress values in the region just in front of the crack tip, not too far away, where the SIF is almost constant. A linear interpolation could be used to estimate SIF value.

Hi Jamal,

if you are referring to sensitivity to the peak stress, Denis' answer is right of course.

However I was wondering if you are considering the "influence" of the mesh rather than its "sensitivity". I did an investigation last year, simulating the propagation of a laser ultrasound field in a standard and defected model and using ABAQUS explicit solver. I wanted to observe the difference between the displacement pattern collected from a particular point of the model, quite far from the ultrasound source.

After some simulations I realized the mesh was influencing my results. I'm not referring to the element size or to the element type, but a slightly different mesh arrangement produced different patterns even when I simulated the ultrasound wave propagation two times in the standard model.

I decided to use three different meshing approaches, in order to understand what was going on.

As far as the first approach is regarded, it was the common approach; two completely independent models were used to reproduce the safe and the defected sample. Observing the differential pattern, obtained from the difference between the two simulated displacement patterns in the standard and defected model, a high-frequency noise seemed to be added to the signal. Such high frequency component was not expected because of the average element size. The reason for this was identified in the presence of small differences between the meshes of the two models (with and without defect). In 3D models the internal structure of the mesh can change, even if the mesh on the surface may appear equal. A solution for this fact was searched with the second and the third approach.

In the second approach only the defected model was initially created and meshed. After having simulated the ultrasound propagation in the defected sample, the defect (a cylindrical hole) was filled with a solid cylinder, representing a new part in the numerical model. This part was joined to the main part using an ABAQUS tie constraint condition. The tie constraint allowed me to fuse together the two regions even though the meshes created on the surfaces of the regions were dissimilar. In this way the standard sample was reproduced and the ultrasound propagation was simulated. This didn't solve the issue, plus adding further complications.

Finally, a model with a partitioned volume was created in the last approach. The partition of the volume was used to divide the defected region from the rest of the model, extruding a circular perimeter drawn on the surface of the 3D model. It represented a solution to have a single part with two different volumes. Initially the whole volume was meshed and, after having simulated the ultrasound propagation in the standard sample, the mesh of the cylindrical region (filling the hole) was cancelled. The not-meshed volume is automatically excluded from the analysis. This approach removed the necessity of any constraint condition, ruling out any problem related to the numerical algorithm that creates the interaction between dissimilar meshes of the tied surfaces.

The last approach eliminated the unwanted high frequency noise coming from the differences between the mesh of the standard and the defected model. A figure showing a comparison between the different displacements and their spectra is in attachment to this answer.

Hope this step by step description can give you an idea of how remove the influence of the mesh in your simulation, if it is what you are looking for.

Best wishes with your research,

Carmelo

Interesting..