fuselage FEM validation ideas 1

[davezil]

hi all,
I've been a long time lurker ,this is my first post.I'm glad to be joining your community.

my problem :
I try to validate an aircraft fuselage fem model(built in nastran/patran),by comparing the axial stresses derived from nastran to a cantilever beam analytic Mc/I.
in the model I applied 20000 lbs up force near the nose end and clamped the tail end.for the analytic solution I choose several stations along the body and computed the inertia(from the model),NA,and moment(20,000* distance to station) for each.
The analytic solution for axial stress varies linearly with height(obviously),but the FEM stress distribution gets asymptotic at the extremes (see attachment).
Results deviate up to 40% from the analytical solution at the upper and lower stringers.

I'm pretty confident the model is ok and the results derived are correct ,finally this leaves me with the probable possibility the model is not similar enough(it also has doors cutouts) to a cantilever beam.

if you could please explain the fem stress distribution and maybe offer a more suitable analytic approach than euler-bernolli beam. (in my case l/D~1200/200=6)

thx

 

[rb1957]

i understand where you're coming from but respectfully suggest your approach is too simplistic (given the limited definition of your model).

i'd suggest looking into other methods for validating your model. I'd suggest the MSC/MASTRAN user's guide but i'm sure you can find others (google FE model verification).

 

[SWComposites]

It makes no sense to me that the FEM strains should behave as in your plot. Are the strains from skin elements? stringer elements? P/AE from segment loads? or what? Are the plotted values at the a/p centerline (BL 0)? Where exactly did you apply the force and boundary conditions?

A fuselage is not likely to match a simple beam, particularly if there are large cutouts, wing pass-thru and/or buckled skins.

Please describe your structure and model in much more detail.

Validation of the FEM and stress analysis is typically done via correlation to an full scale test.

 

[GBor]

It appears as though your issues are at the load application point and the boundary condition location, although some additional definition would help...perhaps a graphic of the model uploaded so we can see the element types and fidelity of the mesh?

At the load application and boundary condition positions, you will get irregularities due to the point (infinitely small area) application of your load and the infinite stiffness potentially suggested by your boundary conditions (assuming pinned or fixed).

It's hard to tell the correlation suggested by the graph without magnitudes on the scale, but it looks like away from the area that is potentially affected by the loads and boundary conditions, the model correlates reasonably well.

 

[davezil]

Thank you for your replies.

I am looking for a better analytic approch(short cantilever beam under moment/transverse shear with thin circle profile) but could only find a correnction factor for shear deflection (Roark) which i dont find much useful.
Or even better maybe you can suggest a other validation test(digital), that could work.
why, from your experience ,should the axial stress distribution be different from a simple cantilever beam?

rb1957-
I choose this approach because i've seen reports using it succesfully for other model aircrafts.
SW-
full scale testing was done for a previous aircraft ,my model is a (moderately) modified version of the valid model(yes, it needs a new validation ).
The model analysis is static-linear hence no buckling/diagonal tension effects are considered.I transfer the force using mpc rbe3 from a center point to all nodes at the station diameter,done several runs using different spc's and force locations for sensitivity check all came similar,except near the boundaries (saint-venant ?)
looked at element x-stress in bars and checked it is exactly the same as element force divided by stringer area.I also compared the analytic to the panels(quads4)axial force flow (lb/inch width) by multiplying the Mc/I with panels thickness.

Gbor-
the results are far from the load application point and spc.
the graph describes schematically stress distribution for a single station over distance from na,the station is some 500 inch aft from load. I'll send pictures from the model as soon as i get to my computer at work .

 

[SAITAETGrad]

Welcome Davezil.

First, I think your approach is maybe a bit backwards as the process of validation should begin before a model starts and carry through the entire process. The problem with attempting to validate a complex model after-the-fact is that you are motivated to find a way to justify all the time you spent on that existing model. That sort of prejudice makes the validation process null.

Quick hand calculations is a very good start but you want to ramp up the sophistication as you go. Validating a constant cross-section fuselage section to classical techniques may be a missed preliminary step followed by more preliminary analysis of cut-outs, etc.

Maybe that approach sounds a bit cautious but in my mind it really isn't as almost FEA work out there is just plain garbage. To paraphrase a great Ian Taig axiom (can't remember where said),you should already know the answer before you start an FE analysis.

I would recommend Alan Morris's book "A Practical Guide to Reliable Finite Element Modeling". This book has a reasonably simple approach to model validation and verification. These are two separate processes. Validation conforms your FEM to the real world case study. Verification is the checks on mesh geometry, etc. that prove your model is mathematically sound and determines the error.

FEM requires expert level skill. Attempting to model a fuselage section is a very serious and very complex analysis that requires a very serious skill set. Find what advice exists out there in terms of published papers and OEM resources.

 

[GregLocock]

If you know the answer before you start then you may build that into the model. One of the best FEA models I ever built wouldn't correlate, because I'd made some assumptions. When I resolved the assumptions, I discovered how that structure actually worked, and was able to improve the stiffness by 30% for no increase in weight or complexity.



Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[rb1957]

"why, from your experience ,should the axial stress distribution be different from a simple cantilever beam?"

how are the skins modelled ? membranes, or shear only ?

are there cut-out and other changes in the fusealge cross-section ? (of course there are)

is the fuselage a complex structure (stringers, skins (differing thicknesses), frames, etc) ? i expect so.

is load being introduced all over the countryside ? i expect so. ok, in your test case you have a single point load ... are you really learning that much from it ?

at least you're starting from a model that has been qualified with test results, at least it isn't total fiction (no slight intended).

you can check the connectivity and assembly of your model with the methods of the MSC user guide. you can spot check the results of the FEM as a sanity check on how loadpaths are developing in the model. At the end of the day, it is the test that proves the structure, and the FEA is supporting data.

there are many real world effects that must be taken into account when actually applying the FEA results. fugge (spelling?) stresses, diagonal tenison allowables, fatgiue/damage tolerance.

good luck

 

[SAITAETGrad]

You make a great point, Greg. What I said was maybe too simplistic and incomplete. But I think what you have described is just a part of the process of starting with a simple model and improving understanding through a process of increasing complexity.