Analysis Physics Question

[Burner2k]

Recently, I did a linear static (SOL 101) & linear buckling (SOL 105) analyses of an air intake using Nastran solver.

Due to proprietary nature, I won't be able to post any screen shots. However, I will try to give some generic info to help define the setup & questions.

The air intake is serpentine in nature and goes from an elliptical Cross-section at the entry to a circular cross-section at the exit. The air intake has circumferential flanges (along its length), which are then attached to bulkheads using bolts.

The analyses were carried out based on the pressure loading extracted from CFD at various V-N diagram corner points. I am just presenting here relevant details from the worst case.

Although the final air intake will be fabricated from Carbon-Epoxy composites, currently to get an initial sense, we chose Aluminum 2024-T3. The air intake wall thickness is around 0.1 in.

In the worst loading case, the pressure loading is of external type i.e. pressure inside the air intake is lesser compared to outside. So the "Delta P" causes an implosion/contraction effect (& thus the buckling analysis).

A couple of interesting observations from the results.

1. The peak displacement value is around the same as wall thickness (0.1 in) but the stress values are way less than Yield. The strains near the peak displacement are well below yield strain values. But since the displacement values are almost equal to wall thickness or shell thickness, is a non-linear analysis required to explore further?

2. The Buckling Factor as provided by Nastran which we are getting are greater than 1 but it is negative. I understand the meaning of the negative sign i.e. buckling will occur if the external loading is reversed. In the above case, the load reversal means an internal expanding pressure. But am confused as why an internal expanding pressure would create a buckling in walls especially since internal expanding pressure creates tensile hoop & longitudinal internal stresses (at least in cylinders).

I have to mention that peak displacement & buckling are happening near the entry of the intake where the cross-section is elliptical.

Just need some help in making sense of the above & increasing my understanding. I have restricted access to internet at work so I may not be able to check daily or provide immediate replies, but I will try to provide as much info as I can with-in permissible limits.

Thanks in advance,

 

[rb1957]

1 … you've given it limiting stress values and limiting strain values ??
a) usually one or the other
b) if the results are incompatible then they are not related by the Young's modulus you're provided. The FEM results should be compatible (ie FEM_stress = E*FEM_strain), but maybe stress_limit .NE. E*strain_limit ??
but to your question, composites tend not to yield in the same way metals do … if you exceed you limiting stress the thing is probably in two pieces. One thing to look at is the laminate Failure Indices, each ply should have it's own failure. If a single ply is failing then maybe you can talk to load redistribution ?

2 … I haven't used NASTRAN's buckling factor, but a -ve value implies tension stresses (easy to check). I doubt it refers to shear buckling as that's the same for +ve or -ve shear.

I'd've thought that the intake lip would be one of the strongest pieces of the duct ?? Presumably a very tight radius, hopefully not a sharp edge

another day in paradise, or is paradise one day closer ?

 

[Taz99]

I would make sure that you have looked at the mode shape of the buckling mode with the negative eigen vector that you have mentioned and see what part of the structure is buckling (it could be the circumferential flange as opposed to the walls). In your static analysis you should see whatever part is buckling having tension stress (indicating that for a load reversal it will be in compression). Another possibility is that it is dominated by shear buckling combined with either tension or compression stresses. I would also be looking at the mode shapes of the positive eigen vectors to make sure that you are seeing a buckling behavior that you expect, otherwise you might have set up your analysis incorrectly.

Regarding a non-linear analysis, as deflections are approximately wall thickness you are right at the limit of the validity of linear analysis, my expectation would be that a SOL 106 static non-linear analysis would show lower peak stress as the pressure on the walls of the intake are reacted by a combination of membrane and bending action in the non-linear analysis as opposed to bending only in a linear analysis. Another benefit of completing a SOL106 analysis of the critical condition is that if the solution converges it will give you confidence that the structure is not buckling (if it is buckling, the load step at which Nastran fails to converge will be the approximate buckling load and if you request intermediate output on the NLPARM card you will see the part of the structure that is about to buckle have large displacements for the final few converged steps).

 

[Burner2k]

Hi Taz99,
Firstly, sorry for the late reply.

Thanks for your insight. Was very helpful.

I completely missed out the shear buckling angle...

Just want to add another point. I have checked the strain values and they are much lower than strain values at yield. Considering this, does the problem still warrant a non-linear run?

But I will check for the points you have mentioned and if possible do a SOL 106 or 400 run.

 

[Stezza]

If it was me I'd do the SOL106 analysis assuming the model is not huge, i.e. the SOL101 analysis solves in a minute or so.

Changing a SOL101 to SOL106 to account for non-linear displacement is pretty easy by directly editing the .bdf add LGDISP and NLPARM cards and you are ready to run. If there is minimal non-linearity the model will run quickly with no convergence issues, if you are getting convergence issues it tells you either have lots of non-linear displacement or the model is not constrained correctly, all things that you would want to know. Once you have the SOL106 results have a look at the differences to the linear run.

Your next step of changing to a composite part is going to involve a lot of design choices so being completely confident with the behavior of the simple metallic model is important.

Looking forward make sure that you pay close attention to your composite joints, if they are bonded the bond line tensile stresses or bolted then failure in bearing bypass. Also radius bending (visualize a L angle being placed under a bending moment opening it up) is another gotcha where the radius will fail in inter-laminar tension, FEM will not predict this failure you will need to do a hand calc based on the moment at the radius.