Non-linear analysis(arc-length) in snap through element like key board button

[Anonymous]

Hi,I'm a master student and trying to fit measured data with simulation data using FEM in snap-through object.I have already measured data using (Displacement load measuring instrument),but I can't solved snap-through analysis, though I tried many methods or parameter or do other things) So Could you help me or give me the way to solved this model?

I wanna get the snap through data like this ↓↓
https://www.lancemore.jp/ls-dyna/example_054.html

Set up
・Model is a part of spherical shell like a dome
・Model detail:diameter is 30mm,Height is 4mm,Spherical shell has an edge ring to easily to snap buckling.
・loads:The model in center of vertical point is 15N loaded
・Material:Material is ABS/
・Constraint:I constrained the edge diameter of this model.
・Analysis method is Non-linear analysis(arc-length method is On/Intermediate OutPut is On)


Trying 1st
・Setup
　・Idealization is solid!
　・Result:Fatal ERROR E5089 Maximum Number Of Controlled INCREMENT REACHD
　・What I did: I changed maximum number of controlled increment steps(40→80→180) to rewrite NLPCI of Nastran File.
　・Figure:Step 30 is not work
　　・1,As load scale is increasing,displacement is decreasing.....why?
　　・2,Why this drop point is occurred?
　　・3, Analytics of process is finished 8.5%.This is a result of divergence.

  ・Figure:Step 200 is absolutely fatal (why the curve is so nosy????)

Trying 2nd
　・Setup
　　・Import spherical shell surface model from rhinoceros.
　　・Idealization is shell model and thickness is 0.5mm.
　・Result :

Trying 3rd
　・Setup
　　・model slightly changed to be easely snap through
　　・Idealization is shell model and thickness is 0.5mm.
　　・actually In this phase model is different model from realistic product,but I wanna check whether or not snap thorough phenomena can solved or not in Autodesk Nastran.
　・Result:Fatal ERROR E5076 Maximum Number of Bisection Permited reached
　・What I did: I changed maximum number of bisection (default→60)

So What I should I do?Could you give me some advise?I can't find which part is not working.Probabry 3D model is not good.....?

Supplemental Study
I thought Arc length method is advanced method of Newton rapson method(control parameter is not force/displacement but arc length(by Riks or CRIS).so I need to adjust convergence error more loosely ?but I didn't get error of E5076：MAXIMUM NUMBER OF BISECTIONS.So I completely trouble with this problem.

[Roelof.Feijen]

Hello @Anonymous ,

To be honest I am not sure where I should start.

The solid model (snapthrough_model.ipt) is not useful in this case. I didn't even take a look at it.

The first shell model (snapthrough_model_shell.ipt) is a good approach. The second one (snapthrough_model_shell_more.ipt) does contain Generic material properties.

I finally created my own model, because I have some doubts about your geometry and just to show you that it's possible to do a nonlinear analysis with arc-length method in snap through and snap back effect.

I have some suggestion:

Use a shell element, which is better able to calculate the deflection than the solid element does.

You will also need to use a finer mesh than you do now. Linear elements should be sufficient enough.

The edges in your shell model (snapthrough_model_shell.ipt) are fully fixed according to the cartesian coordinate system. In my opinion you need a cylindrical coordinate system and only constrain the translational directions. In that way the edge is able to rotate. See this article how to create a cylindrical coordinate system.

The Maximum Displacement versus Load Scale Factor - XY plot:

In a nonlinear analysis the Scale of the Load normally always increases. Example, we start by step 0 - 0%, step 1 - 10%, step 2 - 20%, step 3 - 30% .... end at step 10 - 100%.

Unlike the Newton-Raphson method, the Arc-length method uses an extra constraint and allows the solver to reach the convergence with lower applied load and find the equilibrium.

This property of this method makes it possible to trace the behavior after a limit point is reached, even though that the stiffness matrix is ​​not positive definite.

The Scale of the Load can increase and decrease during the analysis.

The Maximum Displacement versus Load Scale Factor - XY plot shows the load scale from minimum to maximum. Not following the order of the load steps step 1,2,3,4 ....1000. So step 0 - 0%, step 1 - 10%, step 2 - 20%, step 3 - 15%, step 4 - 5 %, step 5 - minus 4%, step 6 - minus 8 %, etc. That's why this XY plot looks so strange in this case.

Use the FNO Reader to create your own XY plot in this case.

I have create a video with Autodesk Screencast that shows you the whole procedure.

When using arc-length method be sure to use enough iterations. I start most of the time with 500 iterations. I 'll stop the analysis when I think it's done and merge the intermediate results with the FNO Reader.

The load is also much bigger than it can handle. That doesn't matter in, because arc-length method will scale the load as you will see during the analysis and in the end when a XY plot is created.

I attached my ipt file. The only thing you need to do is generate the nastran file, modify the arc-length settings in the nastran file and hit "Run nastran file".  Hope this helps. 

[TomaszRedRooster]

Hi Roelof.

I've made exactly same analysis with with shell model like your and perfectly same settings but I got only 15 increments when analysis completed and not 127 like you. Do you know what may be a reason?