Axisymmetric model : Deflection discrepancy with standard formula 2

[QuasarTide]

Hey guys,

I can't seem to figure out where I'm going wrong. I analyzed an axisymmetric model subject to a uniform load along a circumference and compared the resultant deflection with the textbook closed form solution, but there's a huge difference. The modeling seems simple enough!

The disk is annular and is pinned at the outer radius (ux and uy = 0. The loading is per unit circumference along the inner radius of the disk.

Disk dimensions: (dist from axis of rotation)
Inner radius: 700 microns
Outer radius: 2000 microns
Thickness: 200 microns
Material Properties: E = 7.31E10, Poisson's ratio: 0.333

I modeled the disk section as a 2D axisymmetric shell with 8 noded quad elements. The loading is applied to the inner radius. I started off with a load of 10. (I'm guessing ABAQUS takes that as 10N per unit circumference?).

ABAQUS solution: around 130 microns
Closed form solution: 0.218 microns!!!

What's weird is, I kept playing with the load - increasing it by a considerable order of magnitude, but there seems to be no change in the deflection. I'm pretty confused at what's going wrong with my model!

 

[OnlineFEASolver]

The most common mistake with axisymmetric models is not having the model aligned correctly with the appropriate axis of revolution. Also the force should be for the entire circumfrance. If you want you can upload your input deck to my site below and I can look at it and post back here what is wrong.

Principal -

http://www.OnlineFEASolver.com

General FEA Consulting Services

 

[xerf]

The consistency of the units in FE model is solely the user's responsability.

What is the meaning of the thickness for a axis-symmetric model ? I do not follow.

 

[QuasarTide]

Hi Xerf,

Thank you for replying. I actually meant it's the height of the section, not the thickness. I'm pretty sure abt the consistency of the units.

I played around with the model a bit - I realized that I had ramped the load linearly over the step when I had to put an instantaneous force. I changed that in the step module, and turned nlgeom on - but there still is a difference from the correct value.

I uploaded the file onto ur site as you asked, thank you for that. It's named as Axisymmetric TEST. I've used different dimensions from the ones stated above for convenience.

 

[QuasarTide]

Hey,

I think turning nlgeom on has solved most of the discrepancy. However, the ABAQUS value is nearly half the calculated value (from the closed form solution). This error seems to be consistent for different variations of the model.

Any ideas why?

 

[OnlineFEASolver]

Here is what I get when I ran the model in CalculiX:

Principal -

http://www.OnlineFEASolver.com

General FEA Consulting Services

 

[QuasarTide]

Yeah, I get the same results using ABAQUS, but those are the unscaled values.

When I query the node at the inner radius, I get scaled and unscaled values of deflection. Now, do I multiply the unscaled value by the scale to get the actual displacement? Or is the unscaled value the correct answer?

 

[QuasarTide]

Sorry, ignore that question . That was dumb actually.

Yeah, but the ABAQUS deflections are different from the actual values. I can't understand the source of the error.
I input the load for the axisymmetric model as the entire Load i.e. Load per unit length multiplied by the circumference on which the load is applied.

For example in the above model, you obtained a deflection of 1.01 microns, whereas the actual answer should be 1.23 microns. This error increases as I increase the disk dimensions.

 

[OnlineFEASolver]

1.01 vs 1.23 does not sounds too far off, perhaps it is
related to mesh density. How about trying fully integrated
elements, i.e remove the 'R' from the element type.

Principal -

http://www.OnlineFEASolver.com

General FEA Consulting Services

 

[QuasarTide]

Hey, thanks a bunch. That actually worked, trying fully integrated elements. Also, changed the constraints a bit.
Thanks again