Highly nonlinear explicit analysis using shell elements

[AmyLovisa]

Hi everyone,

I am having a great deal of difficulty with a model I have been working on for a long time now. I am modelling corrugated roof cladding (waveform profile) that is only 0.42 mm thick and made from high strength steel. There is a small hyperelastic dart compressing against the top crest of the cladding which leads to the cladding buckling. The model involves large membrane and bending stresses. There is nonlinear contact, nonlinear material properties, nonlinear loading, and large displacements and deformations. An Explicit analysis runs well but the results show the model behaving significantly more stiff than its experimental counterpart. I have tried every available shell element in the Explicit library (continuum elements are not feasible for run time). I have tried different section controls and integration types all with little effect on the result. I am now modifying the material properties for the through thickness specifically in an attempt to improve the results. I feel the transverse shear is the primary cause of the inaccuracy.

Has anyone else come accross this problem before?

You help is greatly appreciated....and needed!!

Thanks

 

[corus]

A model that shows greater stiffness than expected may be due to the number of elements you used. Too few then the stiffness increases. Alternatively, it may be due to boundary conditions where assumed fixed restraints (for example) provide greater stiffness than in reality.

 

[loki3000]

perhaps you could upload the inp file?

 

[AmyLovisa]

Hi Corus,

Thanks for your input. After your suggestion I once again checked the boundary conditions and couldn't see any fault. They match the experimental well. I even released the boundaries so one region is now free to rotate in a bid to reduce the bending in that direction. Still no improvement. I truly do think the large bending stresses right at the compressing epdm dart is causing trouble. I am trying now to include some solid elements to accommodate for some of the bending, but I can only incorporate a few without excessive run times resulting.

Hi Loki3000, thank you for your interest. I will attach my latest input file (I have lost track of what revision number this is). Just as a note, the quarter model is not ideal as there is some eccentricity in the location of the longitudinal boundaries. I do have a fully constructed model that accounts for that eccentricity but have simply been using the quarter model to increase the turnaround of the analyses so I can hopefully identify the issue more quickly.

I really appreciate the input! I am running out of ideas!

Thanks,
Amy

 

[rstupplebeen]

Amy,

I ran your model and in the last time step reported the elastomer goes unstable. I believe due to the large compression the aspect ratios of the elements became excessive. This can probably be alleviated with mesh modification. I typically try to skew the element shape to be the opposite of what the loading will cause.

On one of the free edges you have 2 lines of nodes fixed is that to model a clamp? If this is still abnormally stiff I would check out Corus's suggestion of relaxing the fixed constraint. Even under the best clamping conditions there is some compliance in the system often arising from localized grip slip.

I hope this helps.


Rob Stupplebeen

http://www.optimaldevice.com

 

[corus]

I too noticed the two lines of fixed restraints. It may be useful to assess the effect of removing some of those restraints, whilst preventing rigid body motion. Alternatively, those restraints maybe due to bolting on to another material so perhaps elastic supports might reduce the overall stiffness. You'll need to determine a stiffness for the supports though.

 

[AmyLovisa]

Hi Rob and Corus,

Thank you so much for your input. Especially for taking the time and resources to run the model. I will modify the elements in the hyperelastic material to avoid the excessive distortions.

You are correct, the two lines of nodes are restrained to simulate a clamp. Two 6 mm steel plates clamp the edges. They are clamped under great compressive force thanks to 12 high tensile bolts (which are great fun to do up). I cannot see any movement during the experiments but I have not measured the movement itself at the boundary. I will run an analysis with that boundary relaxed and see how it affects the results. Hopefully it reduced the stiffness significantly!

Thank you again for your help,
Amy

 

[AmyLovisa]

Hi Rob and Corus,

Yep, you were 100% right. Even though the boundaries appear very rigid, they must be somewhat relaxed. I just tried the model with the boundaries free to translate in the y direction with only the line of symmetry preventing translation in the y. There is no way the conditions in the experimenta are that relaxed so I was hoping the model would produce results that are now too soft, and it did! The magnitude of the reaction force is considerably improved. I just need to work out exactly how elastic those supports should be.

So simple. I spent far too long thinking it was something complex (far far too long)

Thank you again for your help.

I should have asked sooner.

Amy

 

[IceBreakerSours]

Fixing the nodes, as pointed out by corus and rstupplebeen, is a 'strong' constraint. I don't know if you are familiar coupling constraints but you might want to look in to *Distributing Coupling; it might do the trick by constraining the motion of the coupled nodes in an average sense.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[corus]

If it's bolted down then you could model the bolted joints themselves with some bolt preload. In theory the bolt preload can be calculated from the applied torque but in practice this can vary considerably. The bolt stiffness might give you the flexibility you need.