doubt connection beam elements and shell

[Francesca Pistorio]

Hello, everyone!
I'm Franciscan and I'm writing because I need advice about a doubt I can't solve.
I need to model in ansys (especially I am using apdl) a mems gyroscope and I started with a really simple design, so as to simplify my problem as much as possible. It is a simple plate suspended through 4 beams to "l" . I attach an image at the bottom for greater understanding.

Since the structure is thin enough, I had in mind to use shell181 elements to shape the central plate and beam188 elements for beams. The beam 188 helmets and shell 181 both have 6 degrees of freedom, so I thought that, to connect them together, it would be enough to share the node to the interface. However, I fear that my analysis is incongruent, since shell elements do not have rigidity around the perpendicular axis on the plane where they lie.

despite this "dubbio", I tried to perform a modal analysis in order to determine the own frequencies of the structure. the problem is that, using few elements to build the mesh of the central plate, the results that I get are quite close to the theoretical ones. a much more fine mesh instead, leads drastically to a greater error. I can't explain this, but I would have expected the opposite. that is due to the wrong connection between beam and shell?

attached I insert my code apdl. I hope someone can give me advice.

Thank you and a dear greeting.

Franciscan

 

[Onda]

normally you do not tie a beam element to a shell only for a knot but you use a rigid element that binds a series of shell knots to the beam element node.
I would think that when the mesh size decreases, your structure becomes softer and lowers the frequencies. this because the beam on the knot of the big element, transmits its stiffness to much of the large shell. while the same beam connected to a smaller shell has less influence.
Therefore, the best thing would be that your shell near the beam had a similar size to that of the beam itself (real size) and that you connect the three remaining shell knots to the node connected with the beam with a rigid element.
Let us know

 

[Francesca Pistorio]

First of all, thank you for the answer.

I tried to solve the problem in another way (but I will immediately try what he suggested to me now). Basically, since the incorrect value of the calculated frequencies is caused by the fact that the shell elements have a dofs "fittizio" (the rotation around the normal axis on their plane), I imposed on the interface of the "constraint equations". In this way I impose that the degree of freedom of rotation z of the node to the interface is coupled to the degrees of freedom in the plane (ux and uy) of adjacent shell elements. my goal is to give "rigidity" to the shell elements...

in this way I solved the problem of frequencies: the results are correct, they no longer decrease when the fineness of the mesh increases, they respect the analytical calculations. the problem now are modal forms: the first and second way are reversed with respect to what expected from the theory. I can't really explain it. . .

Any suggestions? Can I miss something?

(I will also try your suggestion)

 

[Onda]

Why don't you put the ways that come and what you'd expect?
It's weird that you have the inverted ways. . explain better

 

[Francesca Pistorio]

the structure, for the measures I deliberately given, should deform in direction x at the lowest frequency and in direction y at the lowest frequency. attached instead place what I get from the simulation: the lower frequency deformation is instead in the direction y. this fact I do not explain to me from the analytical calculations. . .
I also tried to perform two other simulations, using only shell elements or only solid elements respectively, so that I could make a comparison. what I get this time reflects analytical calculations, both in terms of modal deformations and of own frequencies.

It's like the rigidity I get by imposing the bond equations is not the correct one. I don't know if that makes sense.

I thank you anyway for the help and interest you are giving me!

 

[Onda]

Have you checked the beam elements section orientation? Could it be that sections if not bisimmetric, have been misguided and therefore are you with incorrect stiffness in the direction?

 

[Francesca Pistorio]

After several attempts, I was rekindled to solve the problem, thank you. was caused by the wrong orientation of the elements. thanks really for the suggestion