How to decide initial size increment in Abaqus Dynamic Implicit?

I am using Dynamic Implicit to model a rolling problem. But I am not really sure what to choose as Initial increment. The default suggestion by Abaqus is the step time.

It really depends on two things:

1. What do you hope to get out of the analysis?
2. How much discretization do you need to integrate the equations?

For the first item, if you need 100 snapshots of stresses during the rolling process, then try the step time divided by 100 as your initial and maximum time increment. If all you need is the final deformed state of the structure, then you might be able to get away with the step time.

However, Abaqus might reduce your initial increment if it can't integrate the equations. This gets us into the second item. Many of the models in Abaqus (e.g., the material response) require a certain level of time discretization to converge to an acceptable solution. Abaqus will (try to) reduce the time increment to the maximum value that will allow it to integrate the equations. Once you know what this maximum time increment is, best practice is to perform a convergence study by reducing the time increment and checking that your quantities of interest do not change very much. That is, you need to confirm that the time increment selected by Abaqus is accurate enough for your purposes.

Note, Abaqus may not be able to converge to an acceptable solution using the step time as the initial time increment. In that case, I usually reduce the initial time increment by a factor of ten until Abaqus converges to a solution. The convergence study is still needed after that.

Once you have experience with the material, the loading, the contact algorithms, etc..., you'll be in a better position to pick the initial time increment. However, the step time isn't a bad first guess if you know absolutely nothing at all about the system's response. If nothing else, the analysis will break early.

By default Abaqus decides time increments adaptively. The initial time increment is typically a guess. If the guess is too large to solve the equations for the first time increment, it guesses smaller and repeats the process. If the guess could be larger and the equations still solve well, it increases the guess.

If your simulations run in a reasonable time frame, don't worry about the time increment. If you have to run a bunch of similar simulations and would like to speed things up a little, open up the monitor while your simulation is running and watch how Abaqus adaptively sets the first increment. Write down what it settles on, and use that as the first increment size for future simulations. This will save time because Abaqus can jump straight to the right answer without a ton of guessing.

If you have to choose a fixed time increment scheme, the proper time increments depend on a lot of factors, including the physics you are trying to simulate and the non-linearity of your problem with respect to time.