Discrepancy between Shell and Continuum elements 1

[jongyonkim]

Hi,

With ABAQUS/Explicit, I'm modeling the mechanical bending behavior of a 100mm x 100mm x 0.5mm flat sheet of Silicon. I apply the force in the center and see where it breaks (when Mises stress = yield stress).

Since the plate is sufficiently thin relative to other dimensions, I decided to model it as a shell. (I read in the manual that the ratio of the relative dimension should be around 1/15...in this case it is 1/200, so it holds). I also turn on Nlgeom to account for the excess bending.

I get drastically different results from using the 3D continuum (Explicit element C3D4, with section type: "solid, homogeneous") geometry and the 2D shell (Explicit element S4R, with section type: "shell, homogeneous") with specified shell thickness - for one, the Mises stress distribution differs on 3-6 orders of magnitude at a given displacement of the center as the force is applied in the center. ALLWK is also much higher in the shell (for some reason) than in the continuum per displacement.

I am wondering why this is the case.

Thank you.

 

[xerf]

The linear elements do not give good accuracy for bending problems because are too stiff (this is known drawback of linear elements). I think the linear triangular elements (for 2D) and the linear tetrahedron elements (for 3D) are the worst (by far) with respect to accuracy.

You should try using second order elements (e.g., C3D10) if your problem includes significant bending.

 

[jongyonkim]

Hi Xerf,
Thanks for the tip.

I must use "Shell" type and prefer "Dynamic, Explicit" step for my analysis, because the flat sheet is just a reference case for a more complicated "sheet" composed of many thin structures.

I tried to compare the shell (Explicit element library, Shell family, linear geo order, Quad S4R) result with the continuum (Explicit element library, 3D stress family, quadratic geo order, Hex C3D8R) result to see if they matched up. I am assuming the continuum result is more accurate , but I am not sure now (bad choice of element for continuum above?). The element controls are both set to default with second-order accuracy on.

Results show that the structure will fail much earlier with the shell type, and the structure will need unrealistically severe deformation before it fails (Mises stress = Yield stress). I am guessing that my continuum model definition is wrong (but the shell definition better be right!).

Am I using the correct Element Type for the Shell? For some reason, for the shells, the explicit library supports only linear geo order (S4R). Is this sufficient to model a thin plate undergoing severe bending and its stress distribution? Should I stick to "Dynamic, Explicit" or move on to other analysis types?

Thanks again.

 

[xerf]

This might be useful for you:
ABAQUS Benchmarks Manual (v6.6) ->
2.3.5 Performance of continuum and shell elements for linear analysis of bending problems

 

[jongyonkim]

Thanks Xerf,

I realized that my mesh quality was poor for the continuum plate (only one-element thick! or 2 nodes to define thickness), which gave much lower Mises stress result than predicted.

I made the thickness of the continuum plate 5 elements thick, and now it is giving reasonable results. However, it is still below (20% less than 5-integration point Simpson's). If I use 3-integration point Gaussian method, I get almost the exact result.

However, I am confused between which method (Simpson's and Gauss's) is more appropriate/accurate for my simulation. In the ABAQUS reference, it says that Gauss should not be used if I am interested in the outer surface behavior of the structure. I clearly need the overall stress level for this simulation (failure is when Mises stress = yield stress), so I guess a 5-integration point Simpson's will work fine for my simulation. (I can't seem to get continuum match up with Simpson's though...)

I just want to check before I make my final decision about accuracy. Thank you very much.

 

[xerf]

The most accurate stress values are obtained at the integration points. If you need the stress values at some locations other than the integration points, these values will be approximated based on the stress values obtained at the integration points.

For the Gauss quadrature all the integration points are inside the integration domain. For example, for a 1D domain [a,b], the integration points are a<x_i<b.

Simpson's integration rule uses points on the boundary, that is it uses a and b as locations for some of the integration points.