Testing boat structure with FEA

But the solution to a bar/beam of those dims with a load of 10kN is 160MPa.
Thus it is not correct .. beam theory tells you that.

 

Hi Ad Hoc thank you for pointing this to me. I just did the comparative of the testing with the two software at chosen similar resolution of finite elements mesh units. I think it may be the resolution - but I will look more closely into why it is so . The software calculates the Von Mises Stress value in a solid made of a particular material subject to a particular load; I think the value of stress you calculated is beam theory regardless of material. As well I did not mention above my thickness of my plate the thickness is 6 mm. Anybody who wants to do simulatiopns with other software of beams:/plates made of aluminium or more interesting fiberglass subjected to various loads so we can compare please y all means be my guest.

 

It is difficult to tell in the images, but is the mesh made of squares?

 

Two software two kind of mesh geometry. Scan and solve mesh surface are uniform squares . Autodesk Fusion are adaptive to the solid geometry . The more the resolution is high the less mess geometry impacts result

 

What is the thickness, I can not see any notation? Your input is "force", and the output is "pressure" alt. "displacement".

 

Lenght is 1000 mm height is 250mm thickness is 6 mm Material is Aluminium 6061 force is 10000 N applied vertically the plate is positioned vertically and held fixed at one of the short sides and the force applied to the other

It will be interesting to do the same with fiberglass panels thickness 10mm and discuss /compare

 

Firstly you should be able to control what stress direction you wish to analyse.
Secondly, why would you use a Von Mises stress limit when this is ostensibly a 2D plane stress problem?

Von Mises is all about volumetric shear strain energy, and as a volume an assumed shape is deformed under going an applied stress upon it.
Many software have Von Mises as a stress check, but this is only applicable for solids and complex structures. But this is neither, it is a simple 2D stress analsyis.

The Modulus of the 250x6mm plate = 62.5cm3.
The bending moment is wxL = 10kNm

Therefore the stress is simple 10kNm/62.5 = 160MPa.

If you wish to consider the vertical direction stress that is simple force/area = 10kN/1500 = 6.66MPa.

And since there is no z direction as this is out of plane the Von Mises, if you used this, reduces down considerably to just the 160^2 + 6.6^2 - (160x6.6) = 156.8MPa.
Thus to get a stress of, even Von Mises of 241 or 287MPa, is clearly wrong. The S&S is doing something very wrong.

A difference between 241MPa and 284MPa is not very close at all, it is 19.1% in error..that is massive in FEA terms!

Oddly the displacement is almost correct.

Using these values the displacement, vertically is 6.184mm, using beam theory.

 

So, the logical next step would be to increase the thickness enough to make it a 3d solid and check the validity of the von Mieses theory in both applications. This brings us back to the original question of definition of restrictions and how to apply.

What puzzles me in Andrei's colured images is that the stress values go from zero to max (instead of max negative to max positive), indicating tension where we expect a compressive stress. Is that just an imaging trick or does it in fact indicate that something is incorrect, f.i. in the restraining procedure?

And Ad Hoc; the combined stress of bending and shearing should not be lower than the single value for bending.....? Without leaning towards von M, but using the "old" flowhypotheses (sorry, don't know the English term), the combined stress is (sigmabend^2+n*tau^2)^0.5; where "n" is a function of L/H of the beam. In this case I'd use n=3.

Thanx guys for a good and healthy discussion, it shows the importance of validation against controllable base models. Keep it coming!

 

This is a a simple beam 2D problem, there is no z-axis component, thus the stress in this direction is always zero.

 

Yes, I am completely with you on that. My suggestion is aiming to see whether the software is introducing something that should not be there. The stress level indicated (zero to max) can not occur, unless there is a tensor in the length direction. In the classical beam theory the "holding" moment is created from the integrated stress in the span -160 to +160 Mp; a total of 320 Mp from max to min. The integrated moment from this is greater than the softwares that show between 240 and 280 Mp in total.

Now, if we use the 280 Mp value and distribute it around the neutral layer, we get stress levels from -140 to +140 Mp. If the material is plastically deformed by this stress level, we might have a non-linear stress distribution over the area. This could explain the observed differences, but nothing in the basic set of data is indicating a plastic deformation, so my conclusion is that there is something weird in the program.

My gut feeling here is that the combined stress calculation in the software is using expressions based on some "sum-of-squares" calculation, which too often gets mixed with the "square-of-sums", which is not equal.

 

And that's the whole point of this simple exercise.

The solution to the problem, any 1st year undergraduate student can calculate, it is simple beam theory of a 2D problem.
Thus if the programme is not able to provide this simple exact solution....then why not?

It is either the way the boundary conditions or the applied loads, or the programmes architecture itself, or a combo of them, that is wrong.

 

So, if we look at the principal stress, with the given bending and direct stress and the shear stress on the member:

you have 1/2(160 + 1.7) +/- sqrt[(160 - 1.7)^2 + (4.6.6^2)] = 239.7MPa

Thus it does appear that the output is giving what is the maximum principal stress.
In which case the Fusion 241MPa is very close...but it is not Von Mises, nor is it the direct bending stress!

 

Hi thank you all for the very useful and interesting feedback and greetings from the South of France where the spring has arrived

Regarding the above I want to state that I do have the highest consideration for the participants in this thread and in general for the people posting on the Boat Design forum I do consider the expertise of the authors of feedback here as very high and I do give proper thought to the postings

I did previously run two parallel simulations at the same resolution on simple aluminium plates
1000 mm height ; 250mm thickness; 6 mm the Material is Aluminium 6061 the force is 10000 N

The results are quasi similar in both Autodesk Fusion and Scan and Solve and here are the two reports in Fusion and the Scan and solve the displacement is the same 4mm and the Von Mises Stress is quasi similar.
From my perspective this validates very well the software Scan and Solve created by Michael Freytag of Wisconsin USA
The two software do not only output the Von Mises Stress values but as well the Max Principal Stress on the three axes X , Y, Z ; the shearing stress on three axes and the Reaction Force are included in their reports
As well the user can measure the values of these stresses at any chosen point on the solid structure in the 3D CAD environment
Personally I am working on and interested in the "event" meaning "collision" dynamic simulations that Autodesk Fusion does make possible wich have as well speed annd acceleration as input ; and that I try to illustrate here by an image of a simplified FEA of a hull and keel of a sail boat subjected to the force of collision in the forward of the keel

 

Hello Andrei,
On your last example (llustration just above) with the collision into the keel simulation, where have you positionned the restraints ? e.g. sheerline, rig, etc ??
Thanks, Ed

 

Hi Eddie

Restraints on the sheerstrake surface



Have a wonderful weekend

A.R