Nonlinear buckle test only works up to a certain pressure

[sakkie.coetzee]

VERY new to NASTRAN, so please bear with me if my terminology is not up to scratch. Using NASTRAN 2021.

I'm testing a thin wall aluminum pressure vessel for deformation under pressure.  Nonlinear buckle.

To do this test of course you have to "teach" the program the material properties.

This I've done using data from a tensile tester, and I've converted the values from mechanical to true.

The program calculated the Yield strength from the known Elastic modulus and  Poisson's Ratio.  From that point I added the calculated values into the plastic deformation range, right up to the Ultimate Tensile Strength.

From history I know what the deformation should be, and when I do the test up to roughly 60% of the real world test pressure, everything works out fine.  The deformation comes out slightly lower than what I expect, but that's a different concern for another discussion.

As soon as I enter a pressure above the 60% mark, I get an error code.

E5076 Maximum number of bisection permitted reached.

I need ideas on where to go correct the model please.

Wish I could share the part, but it's company IP......

[John_Holtz · Accepted solution]

Hi @sakkie.coetzee . Welcome to the Inventor Nastran forum.

I have some questions or comments to make sure everyone understands your setup.

"Nonlinear buckle."

• Does this mean that you have set the analysis type to "Nonlinear Buckling"?
• Does this pressure vessel have an internal pressure or an external pressure?
• Will it really buckle due to the load? In other words, is a buckling analysis the correct analysis type because it will buckle (like a Euler thin column will buckle.)

"The program calculated the Yield strength."

• Just to be clear, you are referring to the program that measured your data. Correct? Nastran does not calculate a yield strength. The yield stress is a value that you enter.

"As soon as I enter a pressure above the 60% mark, I get an error code."

• The lack of convergence can be caused by any number of issues. Pick a reason, any reason. 😊
• Has the model yielded? Any stresses unreasonably large?
• Is the stress-strain curve always increasing? (Simulations generally do not like it when the stress-strain curve decreases.)
• Is the model becoming statically unstable to the 60% mark? 
• Is the mesh fine enough to have a small change in stress over the area of each element?
• Is the number of steps (entered in the Nonlinear Setup in the model tree) large enough to have a small and smooth transition of results from one step to the next?

This article may have some information that would help. See Understanding convergence in a Nastran nonlinear analysis. (I see the table or figure with the 29 lines is formatted incorrectly. It may or may not be fixed by the time to read the article.)

[sakkie.coetzee]

@John_Holtz   Hi John, thanks for the reply.

I was pretty certain that further clarification would be required, so here goes.

• Analysis type set to Nonlinear Buckling
• Internal pressure, with the sides inward domed, very much like a soda can bottom.
• The test conducted has two stages.  The first point is to test for the amount of deformation at a set pressure.  This pressure is well into the plastic deformation range.  The second test is test for buckle strength, testing to destruction.
• Your question around the yield strength.  In the stress/strain table, NASTRAN enters two data points, 0,0 and a calculated value from the Elastic Modulus and Poisson's Ratio.  This second value as I understand the explanations are the Yield Strength point on the S/S curve.  Yes it does not calculate YS, rather, it uses the given value and determines it's point on the curve.  Correct?

As for the rest of the questions?  😁  ....those are the ones that I was really looking for.  Where can I go scratch? I'll go through the list and experiment with the settings.  To speed up the test, I DID make the mesh very course, and there is some very real deformation taking place even at the first pressure.

Again, thanks for the guidance.  Looks like I've got a busy weekend ahead!!!

[John_Holtz]

Hi again @sakkie.coetzee 

The second point on the stress-strain curve is calculated from the elastic modulus and entered yield stress. It is not using Poisson's ratio. (modulus = stress/strain, so strain = stress/modulus. strain @ yield = stress @ yield/modulus.)

Is it possible that the domed sides are "buckling" out at the 60% pressure that is applied? (I am not sure if that is buckling or a snap-through.) It is very difficult for a static analysis to transition from one static position to a completely different static solution because the change in stiffness is so drastic between the two states. If this is the difficulty with the convergence, the solution is not to use a nonlinear buckling analysis. If it can be solved as a static analysis, the solution is to perform a nonlinear static analysis and activate the arc-length. 

Here are some more things to review:

• What is a nonlinear buckling analysis in Nastran. It does not do what most people thing it does.
• Offline Help. The "Solver 2021 User's Manual.pdf" is mainly focused on editing the Nastran file, but it also includes some good information about some of the settings and calculations. The "Nonlinear Analysis Handbook" also has lots of good suggestions.

[sakkie.coetzee]

Thanks again @John_Holtz 

At the moment I'm not yet testing to destruction.  I'm only testing to the intermediate pressure, but as said, even this is well into the plastic deformation range of the S/S curve.

I've gone through a couple of setups, and it looks like the main problem WAS the increments being too big.  The deformation per increment was still managable up to a certain pressure, but as soon as more severe deformation happens, the analysis failed.  I've had to up the increments to 1000.  It's been running for well over 4 hours, and it's at 760/1000 increments, but still carrying on.  It's already gone past the 60% mark.  Even at these very small increments, it still goes through  10-13 iterations per increment.  In the early stages of the test it only did 2 - 3 iterations per increment.

I'm holding thumbs that it will carry through to the end this time.

Thanks for all the guidance.  You have no idea how much it helped.

[sakkie.coetzee]

@John_Holtz 

Running time, 11 hours 30 minutes!!!!!  BUT IT WORKED!!!

Deformation expected 2,0 to 2,2mm in real life at test pressure.

FEA predicts 2,04mm

I shouldn't be surprised, but I can hardly believe how incredibly accurate it is!!!