## General Mechanical

#### force convergence plot

• m.caragiuli
Subscriber

Hi

I have a doubt about the trend of a static structural simulation. Boundary conditions include a force applied to a body and a fixed support.

nonlinear control outputs include the force convergence 0,5%tolerance and 1e-2 N minimum reference.

The following picture represents the force convergence plot after hours of simulation.

I'm not sure about the validity of this trend, I mean is it normal that the force convergence starts already below the force convergence criterion? Moreover if the minimum reference is 1e-2 N why does the force convergence start at 1,7e-4N?

Thanks for the attention!

• peteroznewman
Subscriber

This is a good outcome. Don't worry about the Force numbers. ANSYS has figured that out for you.

It looks like you had Initial Substeps set to 10 and maybe Minimum Substeps set to 10, so you ended up getting to full load in 20 iterations.

If you want to try to spend less time waiting, you can reduce the Initial Substeps to 4 and Minimum Substeps to 1. Then if you are lucky it will get to full load in 3 or 4 iterations since it will increase the time increments after a successful first iteration at 0.25 time increment.

• m.caragiuli
Subscriber

Hi Peter,

yes, it works in a smaller time as you said!

Just a few questions...

You understood I had Initial substeps set to 10 and you saw it because simulation starts just above 0 and ends at 1 so ten steps of 0,1 and this means 10 initial substeps. Then you said that Minium Substeps are set to 10, how did you say that? Maybe it is because the time increment keeps constant during iterations and simulation ends in 20 iterations?

Last question. You say don't mind about the force numbers, why? Shouldn't the plot starts above the force convergence criterion? Why the force value at which the plot starts doesn't correspond to the applied force?

Thanks!

• peteroznewman
Subscriber

I said Initial substeps because the first point was at time=0.1.

I guessed that the minimum substeps was 10 because the solver did not increase the time increment as I would expect if the minimum substeps was 1.

It's an internal calculation of force imbalance, not applied force.

• m.caragiuli
Subscriber

Peter one more question, please. From the force convergence plot I can see green lines in correspondence of a converged substep. They are 9, maybe the first one is hidden by the graph or is neglected since the plot already starts in convergence, however are they related to the initial substeps that are mandatory or to the minimum substeps?

• peteroznewman
Subscriber

If you have a minimum of 10 substeps, then you will get a minimum of 10 green lines.

If your initial substeps is 100 and your minimum was 10, you can get anywhere between 100 and 15 green lines because the solution control logic automatically increases the time increment from 0.001 to 0.1 exponentially as each substep converges by a factor of 1.5 or 2.

• m.caragiuli
Subscriber

Sorry Peter, the last part is not very clear. If initial substeps are 100 the initial time increment is 0.01 and if minimum substeps are 10 it means that the solution increases the time increment from 0.01 to 0.1. How do you know the exponential convergence factor?

• peteroznewman
Subscriber

ANSYS increases the time step by a factor of 1.5 (or more) each substep.

That is exponential growth. Try it out.

• m.caragiuli
Subscriber

Peter I'd like to ask you something related to the force thus I don't know if I can continue my question here or on a new topic. Let me know. The question is the following: if I perform a simulation of a body fixed to the ground and subjected to a load, is it better to set only a force convergence criterion or two convergence criteria such as the displacement and the force ones? I know that to converge a simulation should satisfy all the criteria assigned, thus the more the criteria the more difficult is the convergence, but the more accurate will be the result. Is it true?

• peteroznewman
Subscriber

Nyla, you can keep asking questions related to this topic for as long as you want. Once you click a post with Is Solution, then the discussion is marked as Solved and some people will stop looking at it, even when new questions are posted.

ANSYS automatically includes all convergence criterion that apply. I have never had to turn any off.  Only one time, I had a model done outside that had shell elements and the analyst had to turn off moment criterion to achieve convergence. It is very rare to have to turn any of them off.

• m.caragiuli
Subscriber

ok, so should I keep all the criteria on? Because by applying a displacement for instance I thought that moment convergence wasn't necessary to be turned on.

• peteroznewman
Subscriber

There is no moment convergence on a solid model.

Don't change anything from the defaults on the Convergence Criteria. Resolving a convergence issue is almost always done by improving elements including keyops or modifying contact details.