Hi all,
I was trying to model deflection in a rectangular cross-section beam fixed at both ends. There is a Pressure Load acting on the beam (uniformly distributed along the beam). In such system, analytical calculation of the maximum deflection is well-known (see attached). Using this formula, I found my deflection as 35.5 mm. However, in the Abaqus, the result was 41 mm (%16 error).
I tried different element types, mesh densities, 3D shell modelling, non-reduced integration; however, the results are always in the range of 39-43 mm. I couldn't converge to 35 mm in any case. I also modeled the same system in Solidworks Simulation and the results were similar to the ones that I got from Abaqus.
I also compared the results at different pressure values (see attached). Simulation results show the typical linear behavior but it looks like as if the Young Modulus was somehow lowered.
Do you have any idea where this error comes from in such a simple model?
Edit: I have checked boundary conditions, and material properties many times. I don't think there is a problem regarding to them.
Hello Utku Sönmez
As had been mentioned the difference in the two results is due to effect of shear deformation.
The approximate deflection due to shear for a uniformly loaded fix ended beam is 7wL2/(64GA)
When this is combined with bending deflection it is obtained that
Δ = (wL4/384/EI)*[1 + 7(1+ ν )h2/L2]
Using ν = 0 and h/L = 1/5.4 the coefficient can be computed to be 1.24. When this is multiplied by 35.5 it is obtained that
Δ = 44 mm an answer that is close to the numerical solution. Considering that approximate nature of shear deflection computation the agreement can be considered to be excellent.
Hi,
If you use 3D elements in your Abaqus model, the results are based on 3D elasticity. For the analytical solutions of the beam deflection, the results are based on the classical beam theory. What is the length of the beam? If the length of the beam is very large compared with the cross section dimensions, then you should get good results.
Dear Utku,
The classical beam theory is an approximation. As Xin mentioned above, you need to specify the dimensions of your beam.
If the beam is not long enough for the section, the shear deformation, which is not concidered in your calculation, is not negligible. As the result, the deformation is larger than your calculation.
Thanks everyone for your attention,
I was expecting a difference due to shear deformation. However, I wasn't expecting it to be that much.
The geometry that I am dealing with is fixed at both ends (encastre). The end-to-end length of the beam is 270 mm, and its thickness is 50 mm. Therefore the aspect ratio of it is 5.4 (I have the geometry attached).
Actually, I have an experimental data regarding to deflection. However, Young's modulus of this material is not known. Based on the deflection at the given pressure, I can calculate Young's Modulus of the material either by simulation (3D elasticity) or hand calculation (Euler-Bernoulli Beam Theory). I am not sure which one would lead to more accurate result in this specific geometry.
Hello Utku Sönmez
As had been mentioned the difference in the two results is due to effect of shear deformation.
The approximate deflection due to shear for a uniformly loaded fix ended beam is 7wL2/(64GA)
When this is combined with bending deflection it is obtained that
Δ = (wL4/384/EI)*[1 + 7(1+ ν )h2/L2]
Using ν = 0 and h/L = 1/5.4 the coefficient can be computed to be 1.24. When this is multiplied by 35.5 it is obtained that
Δ = 44 mm an answer that is close to the numerical solution. Considering that approximate nature of shear deflection computation the agreement can be considered to be excellent.
Make sure you use a refined mesh.. at least through thickness, you need to discretize it with 5 elements... more is better.
make sure the aspect ratio of the element is good
and also, make sure that you use reduced integration element to avoid locking of the element... or you can go to higher order element...
Based on the figure you attached, the beam is too short and quite wide. Hand calculations using the Euler-Bernoulli theory are not appropriate. You should expect the following: not only the transverse shear deformation to have an effect on the solution, but also 3D effects near the clamped edges that the 1D beam theory can't predict.
Also worth noting, that the encastre boundary condition in FEA is not the same as the simple hand calculations suggest. If you use encastre, you prevent the cross section from deforming due to the poisson's ratio. The hand calculations ignore the section change as their approximate the beam as a line. Depending on the dimensions of the model this can have a smaller or larger effect.
Hi,
This is simple problem and you are using FEM also. So, I think there is some small mistake you go through your program and cross check it . If you write a small program in MATLAB and using the exact solution's formula you can get the error within 2%. So my suggestion to you to go through your program and cross check it. All the best.
Hi Utku,
As I noticed, this is a effect of shear deformation in short beams. Please see Amaechi's formula carefully. The second term 7(1+v)h2/L2 is the one. The factor (1+v) actually represents "G" ("v" is Poisson's ratio). If h/L is not small enough, this term is no more negligible.
As you tried many times, your FEA calculations should be fine.
All that was said is relevant and I agree completely:
1- Beam theory is very simple and don't catch everything a 3D model will show.
2-The beam is too short, for the given dimensions, so you have shear effect wich must be considered (and was pointed out before), problems with differences from the border conditions (in 3D analysis, coupled poisson effect, etc). Everything was pointed out before. No need to repeat.
So the precedent answers focus on your numerical excessive displacement in relation to the theorical. My tip is directed about the contrary, when numerical becomes little less than theoretical.
I would like to say a word about the loading applied to the numerical model. When you apply some concentrade load, the numerical method an theoretical model match.
But, when you apply a distributed load (or a pressure), it is natural that the load is transformed in some nodal applied equivalent loads. And sometimes the discretization of the mesh makes the opposite, the numerical displacement comes lower than theory predicts.
This happened to me, when analysing a steel beam with semirigid joints at the ends. It was using 10 FE and a problem correctly especified for a Bernoulli-Euler formulation usable and still valid. The load becomes 11 concentrated loads at the nodes, but this is not the uniformly load either. As much as you increase the mesh, more your load comes to be distributed. On the other hand, the FE becomes short and the FE formulation becomes inadequate (going to Timoshenko theory). Because of this, my numerical answers were always a little lower than exact ones.
For wide beam cross-section see my paper on Topological Optimization constant beam cross section....where position and type of load perturbs the web cross section. Meaning the bending equation may not predict the beam local deflection over the cross sevtion. Of course FEM error will always be there.
Before using FE, you should study the theory. Otherwise chances are high that you will get wrong results, because they must be used with care, and having an idea of what the result should be:
1) Beam element in a FE program is exactly the beam Euler-Bernoulli
2) Euler-Bernoulli theory is accurate for length-to-thickness ratios above 10, acceptable above 6
3) FE programs also have Timoshenko theory (including shear), which extends the validity to ratios of about 3-4. In those cases, FE also gives accurate results
4) If you use solid elements in bending take into account:
4.1) Linear elements lock in bending. Do not use squares, bricks, triangles, etc. Only squares and bricks have incompatible modes to alleviate locking, but are not good enough. Plates and shells suffer similar issues
4.2) Instead use quadratic elements: 9 node and 27 noded lagrangian elements. 8 node and 20 node elements are not the best choice, but acceptable.
4.3) Loads have to be introduced consistently (i.e. look at the shear distribution in a beam)
FEA is implemented within the framework of a theory for the beam or structure. Computer implementations of structural behavior are also done within theoretical frameworks. The researcher has to clearly state the theories he used for the FEA as well as the computer programs. This will determine the appropriateness of the results for the particular beam considered. Many theories exist for beams.
FEA of beams can be implemented based on the following theories of beams: Euler-Bernoulli theory, Mindlin beam theory, Timoshenko beam theory, Refined shear deformation beam theory etc. Each beam theory is based on certain foundational, basic assumptions which would determine the applicability or scope of application of the results.
If you work in 2-dim beam analysis, I recommend you to use MDsolids Software, the results will be coincident.
- Badges
- Science topic