Frequency analysis with beam and solid elements

[ekyr01]

Hi,

I have carried out a frequency analysis of a simply supported beam by comparing the results between beam and solid elements. The beam elements match the solutions with my hand calculations. However, solid elements do not give very close solutions. Does anyone knows what the problem is with solid elements?

Thanks a lot.

 

[testing]

You're going to have to provide more details. What are the dimensions of the beam? Did your hand-calcs use Euler-Bernoulli or Timoshenko theory? If your slenderness ratio is <10, I'd expect that to be the issue if you used EB type beam elements.

 

[ekyr01]

The dimensions of the beam are 100x100x700 mm. The hand calculations were based on Euler - Bernoulli theory. Is this the issue?

 

[burningDiesel]

The beam elements should EXACTLY match the solutions by hand.
And if this is a simple supported structure and your model is good, the solid elements should give a more precise answer.
But, as mentioned, if the beams are slender, difference should be small.
For thick beams, eg. check with roark formulas for stress and strain.

 

[ekyr01]

Hi sdebock. Beam elements gave me exact solution. Solid elements gave me another solution about 30% difference. In my 3D model, I have restrained x,y and z directions apart from rotation in the x axis (horizontal) and in the other size of the beam, I have restrained it in the z axis (translation and rotation) and the translation in the y axis. However, the solution matches with quadratic only elements not linear. Am I doing something wrong?

 

[burningDiesel]

are you looking at stress or force? how refined is your mesh?

 

[ESPcomposites]

It seems like the solid elements are not dense enough to create a converged solution. I am guessing the FEM frequency is too high, meaning that the elements are effectively "too stiff". It wasn't clear if you referring to two solid element meshes (one with first order and another with second order elements)? If so, it would likely be that the second order element mesh has converged but that the first order element mesh has not. Note that convergence is relatively slow when modeling bending phenomenon with solids through the thickness (specifically first order though).

Brian

http://www.espcomposites.com

 

[ekyr01]

Even shell elements do not match with beam elements and hand calcs.

 

[testing]

You said the beam dimensions are 100x100x700 mm. Does this mean the cross section is 100x100 mm and the length 700 mm? If so, redo your hand calcs with Timoshenko theory and see if they match the solid shell. Also, redo the beam elements with the shear deformable (Timoshenko) beam elements. Check the documention for beam elements to figure out which is which. If I remember right, B33 is E-B and B31 would be Timoshenko. If the alternate hand calcs and beam elements match your solid/shell results, you have your answer