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.
These are the things you need to do:
John
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
After more experimentation, I was able to get satisfactory results!
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.
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
Can't find what you're looking for? Ask the community or share your knowledge.