# Plate deflection theory vs FEA: same problem, same parameters, different results

1. Sep 5, 2010

### roy_lennon

Hello. I'm trying to simulate a plate deflection using finite element analysis software ALGOR. Previously I made analytical calculations and I got the maximum deflection like this: (My plate is simply supported on all edges, so I used Navier's Method. Got the theory from Szilard's Theories and applications of plate analysis)

w(x,y) = (16p/[$$\pi$$^6]D) $$\sum$$$$\sum$$
(sinm$$\pi$$/a)(sin n$$\pi$$/b)/[mn[(m/a)^2+(n/b)^2]]

where
p = gC = (9.81m/s^2)(11 kg/m^2) = 107.91
D = Eh^3/12(1-v^2) = (72 GPa)(0.005 m)^3 / 12(1-0.17^2) = 772.32
a = 0.11 m
b = 0.09 m

both sumations go from m,n = 1 to infinity, only for odd numbers.

My plate dimensions are: 110 mm x 90 mm x 5 mm
Young Moudulus: 72 GPa
Poisson's ratio = 0.17
Density = 2.2 g/cc

with this method I get a maximum deflection of 54.82 nm. I also tired Levy's Method and got the same value.

Now, I go to ALGOR import the plate from SolidWorks, write in all the material parameters. set the boundary conditions to all four edges fixed, turn in the gravity in -z and then run the simulation and I got maximum displacement in the center of the plate of 30 nm.

I have made the simulation many times, and I'm sure I've all the right values and still I dont know why this value is different from the one I got using analytical models.

I would be REALLY greatful for any help you can give me.

Thanks!

rgm

2. Sep 5, 2010

3. Sep 6, 2010

### JolileChat

Roy,

For the analytical method, you said your plate is simply supported on all edges.
For the FE method, the plate is fixed on all edges.
Do you confirm that?

4. Sep 6, 2010

### roy_lennon

@John.phillip: I've tried different ways to do this:

-Element type: Plate
-Mesh type: plate/shell size: 0.001 m
-Max displacement: 20.46 nm

-Element type: Brick
-Mesh type: solid, all bricks
-Max disp: 29.99 nm

-Element type: Brick
-Mesh type: solid, all tetrahedra
-Max disp: 27.7 nm

-Element type: Tetrahedral
-Mesh type: solid, all tetrahedra
-Max disp: 27.7 nm

Don't know if I'm missing anything.... thanks!

@JolileChat: yes, that is the way I did it... simply supported on all edges in the analytical method, and fixed in the FEA simulation... being the edges fixed is not the same as simply supported?

thanks!

5. Sep 6, 2010

### JolileChat

Fixed means no dispacement and no rotation.
Simply supported means rotations are allowed.
Re-run your FEA simulation using fixed edges as boundary conditions, let's see what happens.

6. Sep 6, 2010

### john.phillip

No, it is different. Clamped-Clamped will restrain the rotations also, therefore reducing the maximum deflection.

*Re-run as simply supported.

7. Sep 6, 2010

### JolileChat

Thank you for the correction.

8. Sep 7, 2010

### roy_lennon

I've run the analysis again with these settings:

Element type: Plate
I set the plate thickness to 0.005 m
Mesh type: Plate/shell with a mesh size of 0.001 m
Boundary conditions: all bottom edges with no translation
Max displacement of 22.9 nm

Still no idea what I'm missing... and it is driving me crazy...

rgm

9. Sep 7, 2010

### john.phillip

You're welcome.

For this to work, you cannot restrain more than one degree of freedom. A simply supported boundary condition will restrain only the vertical direction.

10. Sep 11, 2010

### roy_lennon

Hi, I tried something different:

I draw my plate directly in ALGOR, I draw a 2D rectangle and gave all its properties and set the element type to plate and in the element definition I set the width of 5 mm and after performing the analysis I got 53 nm of max displacement. Still dont know why my plate imported from solidworks (3D) wont give me the same result...

11. Sep 12, 2010

### nvn

roy_lennon: It sounds like your Solidworks result is different because you might be restraining the edges differently. As john.phillip mentioned, restrain edge translations only in the plate normal direction, not in the in-plane directions, also. Try it again, and let us know. If you still get a different answer for your Solidworks plate/shell finite element model (fem), then ensure your values of E, nu, and the applied load are correct for that particular fem.

12. Sep 12, 2010

### JolileChat

Hello, Roy.

Boundary conditions must be the same for the analytical model and for the finite element model.
Let us know exactly how you are setting the boundary conditions. The secret is there.

13. Sep 12, 2010

### roy_lennon

Hello nvn,

When I import the plate from solid works, in ALGOR I set the element type as plate, then set the thicknes to 5 mm, generate the mesh with a plate/shell mesh type, and I turn on the gravity and set the boundary conditions. I tried with the Tz fixed only, (gravity is acting in the -z direction) and I still got around 20 nm of maximum displacement. I have for the material properties E = 72 GPa, nu = 0.17, density 2200 kg/m^3, and 31 GPa for shear modulus. I have the same properties of the material and element type and with the 3D model from solidworks it doesnt get the 53 nm, but with the 2D model in ALGOR it does...

Roy

14. Sep 12, 2010

### roy_lennon

Hi JolileChat,

I used simply supported boundary conditions for the analytical model. I used Navier's Method and Levy's Method. In Szilard's "Theories and applications of plate analysis: classical, numerical, and engineering methods" I found the same problem solved and I read the theory and, as far as I know, I'm doing the right thing to find the analytical result of this problem.

I tried these boundary conditions in ALGOR: fixed (no rotation no translation in any axis), no translation in any axis, and no traslation in the z axis and still I can't get the same result.

When I drew the 2D plate in ALGOR, I set boundary conditions as no translation in any axis and I got the right result, but I can't get the same result with the 3D plate imported from SolidWorks...

Roy

15. Sep 12, 2010

### nvn

roy_lennon: When you mesh the Solidworks plate with plate/shell elements, is it meshing both the top and bottom surface of your 3-D plate, thereby creating something like a hollow box, with each surface of the box 5 mm thick? If not, where is it putting the mesh? Or which surface are you meshing? Only the bottom surface? I would mesh only the bottom surface; and then it should be identical to your 2-D plate fem.

16. Sep 20, 2010

### roy_lennon

I've tried that, and it gave me the same result. But the thing is... can I use the whole 3D model to make the analysis? Or can I only use the bottom surface to have the 2D plate?

17. Sep 20, 2010

### nvn

roy_lennon: In post 16, you say it gave you the same result. Which result are you referring to? What result did it give you? Do you mean meshing only the bottom surface of the Solidworks 3-D plate, with shell elements, now gave you the correct result, 53 nm?

You can alternately use your Solidworks 3-D plate, and mesh it with solid brick elements. But ensure you have, say, six layers of brick elements through the thickness of the plate. And restrain only the bottom edge, or preferably only the midsurface edge, such that the plate is simply supported, as previously discussed in this thread. With six layers of bricks through the thickness, it should give you approximately the same answer as the 2-D shell element fem. Try it, and let us know what result you get.