

April 5, 2020 at 6:24 pmj.drozdowskiSubscriber
Hello.
I'm trying to solve some example for MNA analysis.
It is a thin shell supported in the bottom and loded from the top.
I would like to get stability path of one particular node on the top of the shell. I got a converged solution and the maximum value of translation is similar like in example. So guess it is correct.
The chart form example I would like to obtain looks like that:
1) First question is how to retrieve tabular data with more density than it is shown by default ? For example i would like to have tabular data for every 0,05s increment not just for 0,2s substep.
I know how to retrieve those values from the chart manually by i don't how to increase density of tabular data. Because of lack of tabular data my chart in excel is very edgy,
2) Second question is it possible to draw stability path automaticly in Ansys ? I would like to obtain chart like that:
Vertical axis  load increment for example 0,1 0,2 0,3 0,4 etc.
Horizontal axis  Translation of chosen point. 
April 5, 2020 at 6:48 pmpeteroznewmanSubscriber
To get more points, under Analysis settings, turn on Auto Time Stepping, then type 20 for Initial, Minimum and Maximum substeps. That way, each step will be 0.05 s.
If your end time is 1 second, then the Y axis you want is simply Time. You can Probe the Deformation of the point. Then you can make a chart and make the deformation the X axis and Time the Y axis and you will have the chart you want.

April 6, 2020 at 12:17 pmj.drozdowskiSubscriber
Hello.
I tried your solution. It has converged and i got density that i was looking for but results looks completely different. Maximum deformation is around 15000mm. So I guess it is wrong. I thought that If I'm decreasing size of substep I'm just telling to solver to divide load into smaller portions in every substep and i'm increasing amount of iteration.
But why it is so influencing the final result ? 
April 6, 2020 at 12:56 pmpeteroznewmanSubscriber
Under Analysis Settings, change Large Deflection to On.
Also, change your Initial, Minimum and Maximum Substeps to 100.

April 6, 2020 at 1:27 pmj.drozdowskiSubscriber
Ok, I tried that. Now i got directional deformation of my chosen point close to 4 mm (which is correct answer). Process failed at 52nd substep. I got green check mark at Directional deformation and Total Deformation results but the rest is marked red. I got also some strange pick on the deformation chart.
How to interpret that ? 
April 6, 2020 at 5:21 pmpeteroznewmanSubscriber
A nonlinear solution of a Static Structural analysis that fails to converge will always extrapolate to the final load, 4 mm in your case, and show the nonconverged result plot. I don't like when it does that. I always go to the Tabular Data window and pick a row before the last row and Retrieve this result. But in your case, I think you want to go back to t=0.47 s for a stable result.
Here is where multistep solutions become very useful. A lot starts to happen after a displacement of 4*0.47 = 1.88 mm. If your applied load was not 4.0 then substitute the value you had for the displacement.
Under Analysis Settings, change the Number of Steps from 1 to 3.
On the Displacement boundary condition, make the displacement for Step 1 equal to 1.88 and the displacement for Step 2 = 2.2 mm and the displacement for Step 3 = 4 mm.
Under Analysis Settings, set the Current Step to 2.
Change the Initial and Minimum substeps to 1000 and the Maximum to 2000.
Now you will get some very small steps when the structure goes critical and starts to buckle and collapse.
Do the same for Step 3.

April 7, 2020 at 6:21 pmj.drozdowskiSubscriber
Hello Peter.
Thank you for your advices. It change my understanding what is happening during solution.
I tried 3 steps and two last divided by 1000. It took a lot of time and crash around 1,23 s.
I played a bit with this values and I succeed to get chart that i wanted. I just have two more questions.
In my example I'm increasing linear load on the top ring during solution until it achieve 50 N/mm.
In my first try which I already show you with 1 load step from 0 to 50 N/mm divided automaticlly into 4 substeps the solution has fully convereged and i got stress map like this. The construction yielded just in some spots.
In the second try with 3 steps divided into more substeps at time 2,7 s load get to the max value 50N/m and collapse.
The same construction the same load but applied in smaller portions and actually whole cross section yielded. Below the last converged step with reasonable results.
Could you please tell me:
1) The unconverged fully solution doesn't mean that the solution itself is wrong. We just have to conclude that the construction is to weak and just collapse under the load ? True ?
2) If above is Yes, why solver converged the first try without any problems and the yield zone under the same maximum load is much smaller ? The only difference was quantity of substeps.
Regards. 
April 7, 2020 at 9:27 pmpeteroznewmanSubscriber
1) Just ignore the unconverged result at full load, it is for diagnostic purposes only. I always pick the last converged substep to look at results. Those results can be used. A material that has plasticity can go fully plastic and there is no ability to carry a higher load. If that was loaded with a force, then there will be no more converged increments because the structure cannot support higher forces. If the structure was loaded with a displacement, then the solution can continue and the reaction force will be less after the ultimate load is reached.
2) Nonlinear models can be very sensitive to the conditions of the model. Taking large steps, the solver can sometimes jump over an instability that smaller steps will find. The best way to reduce this sensitivity is to create a small flaw in the perfect cylindrical geometry. This is often done by adding a tiny amount of the deflected shape of the linear eigenvalue buckling solution, or one of the modes of a modal solution. That makes the collapse load much lower than it is for the perfect cylindrical geometry, but the forcedisplacement curve will be very repeatable over a large range of load increment size and element size.

 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

1970

1720

935

708

391
© 2022 Copyright ANSYS, Inc. All rights reserved.