Hi，

As far as know, the time increment can not be set by the user in dynamic explicit analyses. You may try 'mass scaling'?by setting a longish target time increment when edit mass scaling, the analysis time could be shortened I think.

Best,

Luping

Mass scaling is a good option as suggested by Luping Wang. But be careful, this may lead to incorrect results. The other option is to verify which element control the time step. If there are small elements in the model try to re-meshing to reasonably large size will improve the time step.

Solution time step on explicit FE simulations are governed by the size of the smallest element in your mesh. So, in short, check the size of your mesh and ask yourself the question: "do the elements really need to be that small?"

Thank you for all your answers.

All the elements in my mesh have approximately the same size, but I will inspect it again to see if I can make it coarser.

I would like to try this mass scaling option. Ravi shankar Badry, could you tell me more about how it may cause incorrect results and how to prevent that?

Best,

Sálvio.

When mass scaling option is invoked, programs add fictious mass to nodes/elements, so that the time step will increase. This additional mass added to the solution, may slowdown stress propagation speeds at respective elements, hence the results will be different from actual solution.

Hi, the step time increment in ABAQUS Explicit is based upon the Characteristic length of the smallest element. And the step increment should be less than the Stability limit to achieve good results. Thus, the Stability limit is the most important consideration and the factor to be determined in an Explicit analysis.

There are ways by which we can increase this time increment.

1. Firstly, as told, the stability limit is based upon the dimensions of the smallest element length. The stability limit is the ratio between Characteristic length of the element and the Wave speed. Imagine you have a large number of well shaped elements and one poorly shaped element with one edge very small. It is the this small length which will be considered in Explicit analysis. Hence, it is better to have a uniform refined mesh throughout your entire model.

In the status file, see the list of the 10 controlling elements and see if their meshing can be improved.

2. Secondly, you can employ a concept called as "Mass Scaling". The ABAQUS Status file will give you a list of the top 10 elements which are increasing the simulation time. Choose these 10 controlling elements and increase their mass. Why increase their mass? , because Stability Limit is based upon the Wave speed and the Wave speed is a function of mass. The wave speed is the square root of the ratio between Young’s modulus and Density. (Note : It is dilatational wave speed)

Thank you Vishakh Rajendran , that was a very useful explanation. I have not tried this yet because I just switched to other tasks for a while, but I will try this when time comes and let you know how it worked.

Best,

Sálvio.

Thanks, do let me know Salvio Aragao Almeida Junior