Learning Forum

[Fahadmasqsododo]

I am using explicit dynamics and i am facing an error of "time step is too small" . i have tried changing mesh size and i have tried changing maximum time step but i am unable to overcome this error but on the other side when i use a big size element mesh without using Automatic Meshing so now the remaining clock time starts increasing and increasing can i get an answer that how my remaining clock time should start decreasing instead of increasing. i am performing impact analysis on canopy of an aircraft upon bird hit strike.

[Ashish Khemka]

Please see if the following links help:

solver error time step too small ÔÇö Ansys Learning Forum
Error !!!! Time Step too small ÔÇö Ansys Learning Forum
Time step is too small error ÔÇö Ansys Learning Forum

Regards Ashish Khemka

[Chris Quan]

If you are using Lagrange elements in impact analyses, you must have proper failure model applied to the materials in Engineering Data so the materials could damage and fail during the impact loading. Otherwise, material strength will be over-predicted by the analysis.
Erosion model should also be activated under Analysis Settings in Mechanical GUI to remove any elements that are distorted by the high impact force.
For a typical bird-strike analysis, bird has a very low material strength, comparing with the aircraft. It deforms very severely, even under a low impact loading. So the bird is best modeled by either SPH particles or multi-material Euler solver to avoid the possible time step problem caused by mesh distortion.

[Fahadmasqsododo]

can you tell me how to use SPH particles or Multi material euler solver in ansys?

[Fahadmasqsododo]

can you tell me how to use SPH particles or Multi material euler solver in ansys?

[Chris Quan]

To use SPH particles and multi-material Euler solver in Explicit Dynamics system, you need to get the recent ANSYS releases.
To use multi-material Euler solver, you need to change the Reference Frame of the geometry body to Eulerian (Virtual). See the picture below. Then you need to look at the Euler Domain Controls under Analysis Settings to verify or modify the Euler domain settings. 3D mutli-material Euler solver has been available in Explicit Dynamics system for many years. 2D multi-material Euler solver is only available since the 2022R1 release.
To use SPH particles, you need to change the Reference Frame to Particles and use Particle meshing method under Mesh to generate SPH particles. SPH particles is not available to 2D analysis. It is only available for 3D analysis.