Validation of Thin Shell Cylinder Formulas

[kmlarriveeQP6BH]

Hello all,

I've been trying to calculate explosion resistance of cylindrical dust collectors and cyclones (thin cylindrical shell). For simplicity I am assuming the explosion is a static pressure, so no dynamic analysis for now. 

My journey has taken me to Roark's Formulas for Stress and Strain. I've been trying to validate the formula's found in there with FEA through Inventor Nastran and for some reason I cannot get my answers to match even with a simple cylinder. 

As a test I tried a 0.0625in thick, Ø50, 36in long (this variable does not affect theoretical calculations from my understanding) @5psi.

Hoop stress should be 2000psi (P*radius/thickness)

Longitudinal stress should be half of that. 

Any mechanical design handbook will give you those formulas, along with Roark's in Ch.13.

I am getting wildly different values from FEA. I suspect my constraints are the culprit. I must admit this is the part I understand the least along with wich stress display is which component. Solidworks simulation is a bit more intuitive for this. 

I've attached my file if someone is willing to give me a hand with this one. 

Thanks in advance,

Keven. 

[John_Holtz]

Hi @kmlarriveeQP6BH 

These are the things you need to do:

1. The constraints on the ends are wrong (TxTzRxRyRz). The cylinder is free to expand radially. The constraint on one end should by a Y symmetry constraint (TyRxRz). Remove the constraint on the other end because ...
2. ... The formulas you provided indicates the cylinder is loaded in the axial direction. Apply a force in the axial direction equal to 1/4 of the full axial load.
3. The calculations give the stress in the hoop and longitudinal directions. For shell elements, you need to define those directions so that you can look at the Shell X-Normal result and Shell Y-Normal result. You will need to create a cylindrical coordinate system and define the material axis using this article: How to define the material and stress axes in Inventor Nastran.

John

[kmlarriveeQP6BH]

Hello @John_Holtz 

Thanks for getting back to me!

1. I just tried this following your recommendation but am unsure if it applies because of 2.

2. I am not using the formulas for a radially loaded cylinder. I am using the formulas for a cylinder with uniform internal pressure. (ref. Chapter 13 in Roark's Formulas for Stress and Strain)

3. I've read this article but am still unsure on how to proceed about this.

Thanks again,

Keven. 

for info, I am using Inventor Nastran 2025.2.0.60, Nastran 2025 Version 19.1.0.27

[kmlarriveeQP6BH]

@John_Holtz 

After more experimentation, I was able to get satisfactory results!

• As the theoretical calculations mention "capped ends", I added a cap to my model and applied the pressure to it as well.
• I was also able to create a material orientation which makes my shell x-normal stress my longitudinal stress and my y-normal is my hoop stress.
• The theoretical calculation also mentions "At point away from ends" so I probe away from the stress concentration that arises at the cylinder-cap intersection and get exactly 2000psi for hoop stress and 1000psi for longitudinal stress. 
• My translation along z-axis is really close to the theoretical values for deltaR, however, translation along x-axis is slightly higher than the theoretical calculation. theoretical: 0.00142in, z-axis: 0.0014in, x-axis: 0.0016in
• As for constraints, I have a x-symmetry and z-symmetry applied to the edges of my cylinder and cap, y-symmetry to the bottom of my cylinder and the top of my cap is fixed (allowing y-translation does not seem to have an impact on values down the cylinder)

I apologize for the wall of text, I simply wanted to document my process. I've also attached my new file. I am open to constructive criticism as I am trying to learn how to usefully use this tool.

Thanks,

Keven.

[John_Holtz]

Very good. The only suggestion I have is the constraint on the cap (TxTzRxRyRz) should not be applied. There is nothing in the theory (or in a real life example) that creates those restraints, so it is better to leave them out of the analysis. (On the other hand, the symmetry constraints represent the stiffness of the vessel that is not modeled, so those a real restraints and needed in the analysis.)

It turns out that adding the cap was a big help. For comparison with the hand calculations, the cap is not needed at all. The pressure that is applied to the cap creates a force which can be added to the edge of the original model (just the side wall) to create the axial stress. If you try that, you will find out that the radial displacement is not accurate at all. The tiny variations in the automatic mesh create tiny stiffness variations. On a model of just the side wall, those small variations lead to a large difference in the radial displacement calculation with the vessel deforming into an oval instead of a uniform radial expansion. The "stability" of the cap helps to keep the side wall displacing like it should.

John