Thin film wrinkling

mdsimulationgroup

Hello,

I'm relatively new to FEA but was hoping I could get some insight on simulating wrinkling in thin films under tension.

I have a material that is 25 microns thick, 1.15 cm wide and 25 cm long. It is isotropic (or at least I'm assuming it is ) with a modulus of 2.5 GPa, Poisson's ratio of 0.333.

Under tension of about 8 to 10 N we are seeing wrinkles form.

I would like to model this phenomenon but I am unsure of the type of model to use and the boundary conditions.

I have tried "Static 3D" and "Shell / Membrane" with the appropriate thickness. Then had a fixed support on the base and a force on the other end but the material only deformed like a tensile sample and was very uniform. I'm guessing I'm missing something.

Any help would be greatly appreciated!

Thanks,
Frank

mdsimulationgroup

Attached is the input I've tried.

Victor

Since displacement isn't proportional to load, you will need nonlinear analysis (Nonlinear static 3D and CCX solver). It probably needs an initial imperfection too, like some nodes moved a little.

I couldn't find any wrinkling that way but I wonder if the elements are too big to capture it or maybe the phenomenon requires plastic yielding or non-linear elasticity?

I would use hex20 with only 1 or 2 elements in the thickness direction instead of 16 hex8's.

Mishal

I know that Calculix only supports brick/solid elements and so any plate is then changed into brick/solid elements by the solver. Apart from my mathematical knowledge of brick/solid elements I have not used them very often, however from what I gather they are very robust elements and work well with poor aspect ratios also. Would the mesh presented in the image still perform well? I assume using hex20 would substantially improve results compared to plate/shell elements and other solid elements with fewer nodes.

disla

Hi Mishal,

Without forgetting the need to perform a convergence study, one general hint to foresee the required mesh density is to ask oneself ; how do I expected the Stress field will be?. Then put more elements where you expect more variation.
Looking at your plate, it seems a pure traction problem. That is to say, uniform stress across the plate so it has no sense to refine. Example



If you have some bending along the plate involved, Stress will vary along the plate. So, put elements along the plate and across the thickness.



Returning to pure traction, If your supporting base is fixed, then some stresses may emerge close to the support due to Poisson Ratio. That suggest mesh should be more dense close to the support and then you can could make It coarser as it goes away.

Victor

The problem here is to find wrinkling so the elements need to be small compared to the wavelength of the wrinkles which is a bit unknown. Maybe it's too coarse?

The CCX manual has an example of wrinkling due to shear in section 5.16 Wrinkling of a thin sheet.

Maybe it's necessary to clamp both ends, like this



According to that paper (https://www.sciencedirect.com/science/article/pii/S0020768311003040) it should show up with linear buckling analysis, so that's probably a good thing to do first because it's much more reliable at getting *something*.

mdsimulationgroup

Hi Victor,

How do I set up "linear buckling analysis"?

Thanks,
Frank

Victor

1. Set analysis type to Bucking 3D
   
2. Choose a Number of modes. I normally use 3 or 4 to get a sense of what else is around even though only the first mode would actually occur.
   
3. Set Shift point to something less than the lowest buckling factor. Maybe just use 1 to start with then reduce it later to make sure there are no lower modes it missed.
   
4. Solve!
   

I just tried it and it looks like it's wrinkling near the support but needs finer mesh to capture it better.

mdsimulationgroup

I was able to use the linear buckling to get winkles....am I able to use the modes to find the needed displacement or force to cause the winkles?

Victor

The critical load is buckling factor times applied force.

You can adjust the mesh according to the mode shape and a scaling factor using Mesh tools -> Transfer displacements from solution.