# Physical meaning of increment in static problem in abaqus

When we use Abaqus to solve the static problem, one step is to set:

Time period, the number of increments and increments size.

But since the static problem is not time-dependent, there is no time, which means the above time is virtual time. Then I was wondering how we look at those parameters in the static case.

Can we think that way: The Time period is the real/physical total deformation time for the static problem and is scaled to 1. And its substep which from Time period/number of increments comes from the sub deformation which is also scaled.

"Statics" usually is defined as meaning that the acceleration of the structure is too small to cause significant inertia forces, i.e. the "mass $$\times$$ acceleration" terms in the equations of motion can be ignored.

However the response of the structure may still change with time when the acceleration is negligible, if the material behaviour is nonlinear and time-dependent.

For example in a creep analysis, the amount of creep strain is time-dependent, and may eventually cause structural failure even when there is no change in the external loads. In this type of analysis, time is a real physical quantity, not an arbitrary scale factor between 0 and 1.

Even if the material behaviour is linear, in a coupled thermal - structural analysis the changes in the temperature distribution depending on the thermal conductivity and specific heat of the material are modelled in "real time", and produce corresponding real-time changes in the thermal stress in the structure.

• Thank you very much. Your answer is very clear. – yuxuan Apr 6 '19 at 18:57

In linear static formulation of FE problem the equations do not include time, so the time you enter is not used.

If, however, you are doing an implicit time dependent analysis, the time and time-steps are used to advance the solution in time. Note that each step is still a static solution of the system.

If there is a material non-linearity then the solver will have to converge in small steps towards the solution (using for example the Newton method or line search), but it is not related to the time you are asked to enter.

Hope it helps!

• abacus is not a FE program – joojaa Apr 5 '19 at 15:46
• @joojaa I think you are wrong. It was bought by Dassault and changed its name to Simulia, but other than that its the same software. – hdrz Apr 5 '19 at 16:28
• sorry your right, temporary brain damage ;) – joojaa Apr 5 '19 at 17:21
• +1. hdrz, @joojaa as possible users of Abaqus, I wonder if you've seen this question and/or if you might know the answer to it? mattermodeling.stackexchange.com/q/2055/5 – Nike Dattani Nov 14 '20 at 3:36

Static analysis is an ideal scenario, no real event is actually static- either quasi-static or dynamic.

It is based on the assumption that all loads are applied slowly and gradually until they reach their full magnitudes.

So when you have some (pseudo) time steps, what you are basically doing is discretizing the steps of load application.

While the other answers make some good points the only one really addressing the issue is Schneider's response. The time increments in a static problem in abaqus means that the total load, say for example 10 N, is divided into chunks of say 1 N each (if you have 10 substeps), and the software adds 1 N each time the previous substep has converged. This is done because it is easier for the solver to converge with small loads.