Plate Deflection: FEM vs. hand calculation 1

[flyforever85]

I'm trying to compare the FE results with a hand calculation but I'm not having great luck yet.
I have a plate, 300 mm x 300 mm, (aluminum 72,000 MPa, v=.33), thickness 3 mm. An homogeneous pressure of 0.005 MPa is applied all over the plate. THe plate is fixed at every edge.

The FEM model gives me a max deflection of 1.81 mm at the center of the plate while a formula from Bruhn gives me a max deflection of 0.92 mm (the formula is wmax = (alpha x q x a^4)/(E x t^3) where q is the pressure, a is the edge length. alpha depends on the boundary condition and for a fixed edge it's 0.0438

Thogths?

 

[FEA way]

Strange, my FEM result (from Abaqus) is 0.2825 mm while analytical result (from Roark's) is 0.2875 mm. Roark's gives the same equation but alpha equals 0.0138 since it depends on a/b ratio. Double check all your units and input values.

 

[karachun]

Timoshenko, Voynovsky-Kriger Theory of plates and shells, page 202 give alpha = 0.00126 for square plate.
Link

 

[flyforever85]

I have another question:
I made a model in FEM of an aluminum (2024) plate, 300 x 300 mm2, thickness of 1 mm. The plate has rivets at three edges and the fourth is free. An homogeneous pressure of 0.0336 MPa is applied all of the surface. I used a plastic curve to model aluminum. I get a displacement of 86 mm at the center of the plate! Stress is only 361 MPa. I cant' understand if in reality the plate would deform that much or I'm missing something.

There are the values I used for the plastic curve
e s
0 0
0.00457 331
0.01524 376
0.03549 409
0.1 448

 

[FEA way]

Can you attach some pictures showing this model (with visible boundary conditions) and its results ? It seems that there's some serious mistake in the input data.

 

[flyforever85]

Sorry my bad.
There are the data:
length = 1050 mm
height = 300 mm
thickness = 1 mm
Pressure = 0.0336 MPa

Now, the plate is riveted on the bottom edge and the two lateral edges but free to move on the top edge (easy to see that from the deformed picture). The plate is also riveted vertically to create three subplates. You can simplify the model with a single plate 300 mm tall and 1050/3 mm long and apply a third of the pressure. The mid subplate was modified with a stringer so forget about the deformation in that area.

Thank you

https://files.engineering.com/getfile.aspx?folder=80b53040-5898-4b45-b2ee-43434f305e5e&file=1.png

https://files.engineering.com/getfile.aspx?folder=0b798659-1e28-4de9-a65d-fa7128f4345c&file=2.bmp

 

[flyforever85]

I can't find an explanation to the fact that if I use the same model with both linear and non linear analysis, with the latter the displacements increase by almost 15 mm. I would assume they stay the same

 

[ESPcomposites]

Items to consider for nonlinear geometry

1. For a linear analysis, the assumption is sin(theta)=theta (small deformation assumption). However, as this assumption changes, so can the result. This will also depend if the force is a "follower force" or not (meaning the angle of the force changes with the deformation).

2. There is something called "stress stiffening" (incorporated by the geometric stiffness matrix - aka differential stiffness matrix). The classic example is the membrane of a drum. As it deforms out-of-plane, it becomes more and more difficult to increase the out-of-plane deformation. The geometry changes, the membrane (in-plane) stresses increase, and the out-of-plane deformation becomes more difficult to increase. The opposite case is a that of a column with an imperfection/perturbation. That said, I don't understand why your case shows an increase of deformation (I would have expected a reduction - though I have not looked at it closely).

Brian

http://www.mystran.com

 

[SWComposites]

What nonlinear solution are you running?

 

[flyforever85]

THank you all for your answers.

SWComposites: I'm using SOL 106.

 

[dmapguru]

Two possible reasons for larger displacements are: 1. you said you have an elastic-plastic material behaviour. Does the material reach yield stress? The other reason for a larger displacement often overlooked is you said you have a pressure defined over the plate. As the modal deforms, the displacements are updated and the panel surface area increases. The pressure does not change, so the total load on the panel increases. Inspect the OLOAD summary for the applied load.

If you want us to look further, please provide the input file.

DG

 

[flyforever85]

I found the solution of the problem: I didn't use the parameter FOLLOWK and LGDISP for large displacements. Because of that, the stiffening effect of the deformation was not taken into account by nastran. The deformation went from 214 mm to 15 mm... I'd say a huge change!