# Why Ansys can't create negative curve force or pressure-displacement ? is there a way to do this?

OguzhanA
Member

I have a buckling analysis about cylinder. I analyzed it using stabilization setting. But my result isn't what I want. Theoretically , Cylinder behavior curve should be negative slope(figure-1). But in My result ,curve is positive slope(figure-2) . Critical Buckling Load can be true,but ı think behavior is failed.

figure-1

figure-2

I will be glad if you give an idea!

Regards

## Comments

Hi,

Please refer the following steps for buckling analysis:

Regards,

Ashish Khemka

thank you @akhemka but this does not contain the answer to my question.

Hi @OguzhanA ,

What I meant to indicate is that you might need to perform a post-buckling analysis if you have already crossed the first point (pt. A) on the force deflection curve. To have a force deflection curve with negative slope you may try prescribing displacement boundary condition rather than force to have a stabilized solution. The reaction force on displacement b.c. can be used to generate the load-deflection curve then.

Regards,

Ashish Khemka

thank you @akhemka how can I use displacement for cylinder face ?

Regards

You can use Stabilization with a Pressure Load.

Hi @OguzhanA ,

Did the suggestions above help you?

Regards,

Ashish Khemka

@akhemka I just got strain line with stabilization. Because I dont know how can I apply displacement instead of pressure. Do you have an idea?

Regards

Oguzhan

Hi @OguzhanA ,

You can apply the diplacement and track the force reaction to generate the force deflection curve.

Regards,

Ashish Khemka

@akhemka how can I apply displacement for cylinder face ?

Regards

Hi OguzhanA,

The answer you are looking for is the ARCLEN command.

Issue ARCLEN,ON in a static structural environment command snippet if you are in the mechanical application. Using the default settings of the command is advised and works for most cases.

There is a related comman, ARCTRM, but you should not need to utilise this command.

For your analysis, I believe you will need nonlinear geometry active, NLGEOM command, I am not sure if the ARCLEN command automatically turns this on or if you will have to do this separately.

Thanks for comment @BenjaminStarling . I tried Arclen but I didn't see negative curve . You can try this simple example. Cylinder Height:1250 mm Thick: 1 mm Radius:1000 mm , Bottom and Top edge fixed. Material: young modulus=210 000 Mpa and Poisson=0,29 and external pressure

Like this

Thank you

Regards

Oguzhan

If you aren't seeing a negative curve there may be other issues with the model or the specific example. However, using the arc length method is the only way to get a negative slope on the force deflection curve. Stabilisation will not acheive this for you. I will look into the example you have provided and get back to you.

thank you @BenjaminStarling, I'm waiting for your answer.

Regards

Oguzhan

Hi Oghuzan,

I have acheived steady convergence through the negative curve of the force-deflection curve, this is shown below by the negative time increment, however I will be stopping the analysis here as disk space and time are an issue for me at the moment. Whether this analysis ultimately shows what the theory says it should, I am not sure.

To acheive this I made the following changes to the test case you described.

image below of my point load to introduce assymetry

I am using 2020R2, so you may see differences if you are using a different version, or the academic version.

My final comment is to persist with using arclen, I have seen that you have been asking this question for a while now and have been led to use stabilisation. Stabilisation cannot model the negative curve at all, and the arc length method is 100% required.

If I have time later on I may pick this up again and solve to completion.

Hello @BenjaminStarling thank you for answer. I will try this settings now.But I have only two questions.

1-How much pressure load did you apply?

2-For arclen command, just write "arclen,on" or "arclen,on,max,min"

Regards,

Oguzhan

Hi Oguzhan,

I solved this to near completion. I ended up with non convergence at around 0.92, after reaching 0.97. The point load ended up causing further assymetry, final result shown below. The max deformation is occuring where I have applied the point load. This may not be the result you are seeking, so I would probably return to using the buckled shape.

1 - I applied 0.02 MPa.

2 - I used "arclen,on". however based on the non convergence you may need to play around with the

MINARCvalue to get through to convergence.For my own understanding, is it expected that this structure ever becomes stable again? if it is not, the solve will never reach convergence, however you can still plot the force deflection curve for part of the buckling process.

Hi @BenjaminStarling ,I am sharing an experimental chart and expect the behavior to be close to that. Where do you think we could go wrong?

Regards,

Oguzhan.

Hi Oghuzan

What units is that graph in? is that for the same case you have provided for me to model?

To me it appears that the structure isn't really stable, even towards the end of the loading history, this is evident in the orange curve where the gradient is consistently changing (and going backwards in terms of deflection). Also not sure what is going on with the yellow curve. the grey curve in particulary would indicate that you need an extremely small value for the

MINARCvalue, and very small time steps, to achieve such a sharp change in gradient. The blue curve would be the most ideal to recreate, as it has smooth changes in gradient which would not require a really small value ofMINARCto capture.That being said, I think we are expereincing non convergence before we are even close to the second change in stiffness behaviour. I will have time this weekend to investigate further. It may just be that further reductions are required in time step sizes.

Do you have any papers/references to this type of analysis or any theory that you can share with me such that I can get a better understanding of what we may be missing?

Of course, I started this work because of an article. I can share the article with you. There are experimental studies and there is another program, abaqus program solution, but only for the part up to the initial torsional load. I am sharing the article link and abaqus solution link with you. But in the experimental data, we noticed that the pressure values in the article are 10 times bigger. There was probably a mistake.

https://www.youtube.com/watch?v=02bB_o50V_g

Regards

Oguzhan

Hi Oghuzan,

I watched that video you linked, and found it contains everything you need to proceed with this analysis. Below are all my thoughts in no particular order.

SECDATAcommand, however I do not think this is consequential to your analysis.MINARCvalue, I would recommend you use the same value. It may not translate between solvers to be the same variable, but in either instance, it is an incredibly small value.MINARCvalue as I mentioned above will help the solve get further before non convergence. He acheives far greater displacement with the GNIA case, however we don't have much to compare with this case without having a similar imperfection introduced to the structure.