

March 31, 2020 at 6:18 pmm.caragiuliSubscriber
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 1e2 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 1e2 N why does the force convergence start at 1,7e4N?
Thanks for the attention!

March 31, 2020 at 6:33 pmpeteroznewmanSubscriber
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.

April 8, 2020 at 7:12 amm.caragiuliSubscriber
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!

April 8, 2020 at 2:41 pmpeteroznewmanSubscriber
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.

April 8, 2020 at 3:14 pmm.caragiuliSubscriber
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?

April 8, 2020 at 7:58 pmpeteroznewmanSubscriber
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.

April 9, 2020 at 2:04 pmm.caragiuliSubscriber
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?

April 9, 2020 at 4:56 pm

April 15, 2020 at 4:21 pmm.caragiuliSubscriber
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?
Many thanks for your clarification!

April 15, 2020 at 5:28 pmpeteroznewmanSubscriber
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.

April 15, 2020 at 5:35 pmm.caragiuliSubscriber
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.

April 16, 2020 at 12:43 pmpeteroznewmanSubscriber
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.

 You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from lifesaving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 How to calculate the residual stress on a coating by Vickers indentation?
 An Unknown error occurred during solution. Check the Solver Output…..
 Saving & sharing of Working project files in .wbpz format
 Solver Pivot Warning in Beam Element Model
 Understanding Force Convergence Solution Output
 whether have the difference between using contact and target bodies
 Colors and Mesh Display
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 Massive amount of memory (RAM) required for solve
 What is the difference between bonded contact region and fixed joint

1932

1720

927

688

378
© 2022 Copyright ANSYS, Inc. All rights reserved.