Simple cantilever beam 2

[aerohead56]

I recently came across a problem that has all of the FEM engineers at our company stumped. I generated a cantilever beam from CBARs and CQUAD4s in PATRAN (using NASTRAN 2001 for the analysis). The beam is 100mm tall, 1000mm long, has a web of starting thickness 2mm and spar caps with properties of Area=256mm^4 and I=1306666.6mm^4 (in the primary bending direction) for the caps. Bar elements run only along the top and bottom surfaces to represent the caps. The beam has 10 elements through its thickness and 100 elements down its length, making each quad perfectly square. I applied a pure up load on one end and constrained each of the 11 nodes on the other end with simple supports. This model produced results that are within 5% of beam theory. I then lowered the thickness of the web to 1mm and recalculated the model and the beam theory answers. This resulted in an error of about 9% with beam theory. A further reduction of the web thickness to .5mm was calculated and produced an error of approximately 21%. This error is on displacements. I haven't even bothered checking stress/strain yet. We have tried adding K6ROT. Epsilon for this model is less than 10^-10. The free-body balances in the model. If anyone has any advice I would appreciate it.

 

[corus]

If you're using beam elements for the flanges then you have to make sure that their centre is at the centre of the beam and not simply attached to the surface of the quads. A 5% error is too big and is probably due to not having this offset. As you reduce the thickness of the web then the flanges will tend to dominate the solution and hence increase the error.

corus

 

[aerohead56]

Yes, the beam that is used in NASTRAN exactly matches the one that was calculated using beam theory. The web makes little difference in the moment of inertia calculation.

 

[hacksaw]

please clarify the beam theory model being referenced?

 

[aerohead56]

I used the equations from "Formulas for Stress and Strain", Raymond J Roark, 4th edition, page 104, method 1. Tip vertical deflection was calculated using Max Y, and an intermediate point, at half the length, was calculated using the equation for y and an x value of 500 (which is half the length).

 

[gelu]

The tall / thickness ratio 5, 10, 20 indicate you are far from the beam theory application.
You are most in the field of shell and plate theory, and a theoretical solution is not easy to calculate, maybe impossible.
A way to validate your analysis can be mesh refinement / solution convergence.
gelu

 

[hacksaw]

There are at least a half dozen beam theories out there. The Euler-Bernoulli model is just one. It's limitations are well known when shear effects dominate. Sounds like one of the beam models that has a better accounting of shear effects might be better, but to bench mark a FEA scheme using analytical models on such a complex beam is going to be really tough.

 

[aerohead56]

Thanks for pointing out that my beam is too short. I re-ran the model within the limitations prescribed on page 96 of Roark, which states that a thin web beam needs a span to depth ratio of at least 15 to show within a 5% error. This produced results that are more consistant with theoretical. There still exists a strange phenomenon in the data though. I ran with with the same beam, except I increased the length to 2000mm (span/depth = 20, exceeding the limitation of 15 recommended by Roark). The error is nearly a linear function associated with the thickness of the web. Web thickness 4mm = 1.2% error, 2mm = 2.3% error, 1mm = 4% error, and .5mm = 8% error. Very strange.

 

[hacksaw]

Here again you have to define the beam model that you (or Roark) is basing the theoretical result on.

There are at least a half-dozen theoretical beam equations(pde) to choose from.

We found significant departures with simple beams for L/D<100.

 

[aerohead56]

Page 98 of Roark states that the vertical deflection calculation is based on solving the general differential equation for the elastic curve which is: E*I(d^2y/dx^2)=M, where E is the modulus of elasticity, I is the moment of inertia, y is the vertical displacement, and x is the position along the beam. According to page 98 this is found by the method of unit loads. The equation is re-written as: y = Indefinite Integral(M*m*dx/E*I). y, x, M, E, and I are the same, and m is the equation of the bending moment due to a unit load acting vertically at the section where the vertical displacement is being calculated. Since this equation is a direct integration of the displacement function it should be accurate. Roark mentions on page 96 that the maximum error of the calculated results should be about 5 percent.

If you don't have a copy of Roark I would highly recommend it. It is a standard in the Aircraft Industry, but would be highly useful for anyone doing strength calculations.

 

[hacksaw]

What you've described is the Euler-Bernoulli model. It's limitations are well known in the research literature. The claim of 5% error is a bit optimistic even for so called "slender" beams.

 

[aerohead56]

Can you point me to some literature on this subject? I would greatly appreciate it!! All the engineering textbooks I have just cover the Euler theory. I didn't know that there even was anything else.

 

[kujkkb]

Have you found the limitations on the Euler-Bernoulli model? I have also been looking at similar problem except I am using a couple different models, an i-beam fixed/fixed w/load applied to the center, simple/simple load at center and fixed/free w/load at free end. Like you I have found that the FEM fixed/free varies a small percentage (<5%) from the Euler-Bernoulli model. The problem is with the fixed/fixed FEM model that has ~20% more deflection than the Euler-Bernoulli model. I ran the fixed/fixed with three different models using the same dimensions but different elements (bars, bars and quads, and tet10's). Each FEM model resulted in the same deflection. I have also ran models of the same I value, fixity and loading but different cross sections (circular and square). All FEM model deflections agree within 5% of theoretical. In writing all this I would appreciate any information you have, or anyone else reading this, on corrections to or limitations of the Euler-Bernoulli model. Specifically when dealing with i-beam cross sections.

 

[aerohead56]

We have come to a solution. Be very careful with your boundary conditions. In the fixed end restraint it is important to note that the Euler equation assumes that there is full fixity (all 6 degrees of freedom) at all of the nodes at the interface. When we ran this it produced deflections in the models we are running within 1.2% of the Euler calculated deflection. The other 1.2% can be attributed to shear relief from the quad elements. We originally fixed these parts in rigid body motion only. This produced significantly higher deflections than what the Euler equations predict.

 

[kreative]

I am a beginner and the replies above have made me ask this question.

We generally dont use shell models for complicated geometry and if the geometry is simple it does not take more time to make a solid model. Besides this in using solid models we make less assumptions. So why not use a solid model and avoid all the trouble. It takes less time to run a 2D model but since we only do simple geometries in 2D, creating the same in solid should not take a lot of time and the number of DOF is not that large. Could you gurus please enlighten me on this. Thanks

YM

 

[aerohead56]

I STRONGLY disagree that solid models use less assumptions and are more accurate. We have run studies on model convergance in solid models using stress convergence as a criteria in localized locations on a complex part. Using Hex8 elements we show virtually NO convergance. The numbers are all over the place, and very GREATLY with mesh density. Tet10 models of the same structure show better convergence, but stresses are still dependant on mesh density, and vary with a +/- 5% on a model with exactly the same applied loads and boundary condition reactions. Be extremely careful with solid elements. There is no moment solution at any of the nodes due to the assumptions used to derive the solid element equations. This can greatly affect your results if you have bending through a section of interest and an inadequate number of elements to represent it. Most FEM methods are checked by running simple, closed-form solution problems. This will show you that the element appears to be accurate, when in fact, on real geometry it does not appear to be. Just because these elements fill the volume and seem to require less idealization fo the structure does not mean that they are in any way, shape, or form accurate. Whether a model is accurate or not depends greatly on the analyst's knowledge of the element formulations and limitations, his/her understanding of the proper boundary constraints for a given problem, and the ability to research the results to a degree that a high level of certainty can be achieved.

 

[corus]

In general kreative is correct. A 2D model will be made on the assumption that you have plane strain or plane stress in a stress analysis when in fact both conditions apply to a thick section, for example. 3D Shell models generally don't capture thickness effects on load distribution between two intersecting shells but can be ok if you only want to see global effects. In general it's easier just to model the whole thing in 3D solid elements though you have to bear in mind the time taken to generate the model and the run time particularly when in some cases your results may not be too different from a simpler 2D model.

corus

 

[shehzadkhan]

Hey i have a very small problem but as i am an automobile engineer and i am not at all related to structures,i have a cantilever beam 750 long and 150mm wide and i have to find a thickness which would prevent the deflection of the beam under a load of 125Kgs,the material of the beam is pure magnesium and the geometry is rectangular .......i have to find the thickness which prevents the deflection ......can u plz help me quick
khan

 

[israelkk]

shehzadkhan

You can not prevent deflection! Every material in the world will deflect under a load, this is physics!. You can only limit the deflection it to a specific deflection that you desire.

 

[DRW75]

israelkk,

you can always prevent deflection, all you need is a beam with an infinite moment of inertia. Although they can get a bit pricey

as a note, shehzadkhan, usually i treat a 'zero' deflection as less than 0.5mm... but this is quite a relative thing. I am often asked by the pipers to provide a support with no deflection, and i usually use 0.5mm as my cutoff, as you will ALWAYS have deflection.

DRW75