Discussion Forum

Hello Pasquale,
The very-soon-to-be-released version 4.4 brings significant ease-of-use improvements when coupling shells and solids. If at all possible, I would recommend you wait a few days for 4.4 to be available to start work on this.
Best,
Jeff

Hi,

For a thin shell there might be a shortcut:

If the shell thickness is small when compared to the solid thickness, then the fact that the true shell midsurface is placed above the solid face can be ignored. In this case you could just model the shell on the boundary which is the face of the solid. In such an approach, you can simply change the name of the displacement degree of freedom in the shell interface from say u2 to u. Then both the Shell interface and the Solid interface have common degrees of freedom.

The relative error in the bending stiffness of the section when using such an approach is of the order 2*shell_thickness/core_thickness, so the shell should be relatively thin.

If you want to use the more correct approach in version 4.3b or earlier, then you need to map the results in the shell onto the solid boundary by an extrusion coupling operator, and then prescribe the displacements on the solid based on the values from the shell. The expression for u (in the solid) would then look something like genext1(u2+arx*shell.d/2)

Regards,
Henrik

Hi Henrik,
you was very useful.

Your approach is very fast and simple. I want just a clarification about the error i do using this approach.

In my case I have a 33mm core and a 3mm skin, applying your equation the result is 0.182
In which sense 0.182 represents the error? it's a percentage error or is the indication that the error i do is in the order of 10^-1?

thanks for your help.

Hi,

With your numbers, you will underestimate the section bending stiffness with ~18% if you use the true geometry of the core. The bending stiffness is essentially proportional to the square of the distance between the shells, so the error approximation better than just 'order of magnitude'.

If you however increase the core thickness in your model to 36 mm, you will get a rather accurate bending stiffness. In the other hand, you will overestimate the shear stiffness with 10%, since it is proportional to the core thickness.

Depending on the type of effects you are investigating in your analysis, different approaches will be more or less useful. You could for example use a 36 mm core with a 10% reduction in elastic properties to compensate.

Regards,
Henrik

Hi Henrik,
thanks for your help.

The task of my analysis is to simulate a 3 point bending test.
I have simulated just half panel, applied a simmetry condition and a load edge, a pinned edge constrain.

Which approach do you suggest in this case?

If I want develope the correct approach which steps I need to follow? there is a guide I can read?
I have found no topics in the forum or in comsol help.

Best regards,
Pasquale.

Hi Pasquale,

Which approach you should use must be determined by judging several factors

- Aspect ratio of the specimen (bending or shear dominated?)
- Accuracy requirements
- Is it OK when you present the results to have used 'tricks'?

Also note that with the dimension you have, it is actually possible to use solid elements also in the skin.

There are no examples in the Model Library which would guide you here.

Regards,
Henrik