I am modelling a cantilever beam with a concentrated point load at its end. As a 2D wire beam I got the different response and for the 3D solid model (constrained in the width direction using symmetry Boundary condition) ,why it is so ?
Here, I am getting the almost same natural frequencies for both the models.
Here with attached image containing details.
Kindly help me.
Thanks a lot.
Hi,
What were the boundary conditions that you gave for the 3D model??
Were the frequencies and the mode shapes identical for both the models??
If u had applied a constant force, calculate the deflection of the cantilever due to this force and compare with the response. This will help you to know which model is right.
Also consider mesh refinement of the beam model. You should also be able to find a theoretical solution for this problem with which to compare.
Thanks a lot for your inputs,
3D model has modelled as a cantilever beam and sides of the beam are constrained such that it will allow 3D beam to just deform in the vertical direction.
for mesh refiniment i took 10 elements along the thickness , 100 along the length and 1 along width (As I want to apply concentrated point load at the free end of the beam of total 10N i.e. 5N load at both node ). kindly refer the figure attached.
thanks a lot for your response again.
If you do a free vibration (rather than the forced one) modal analysis then you could compare the frequencies from the two models to see if they agree. Also, how many elements did you use in your beam model?
for wire beam I took 100 elements.
And free vibration natural frequencies are matching well for the both models.
thanks again.
What is your element type in the 3D model?
If you use full integration and first order, your beam will be too stiff (shear locking, see the Getting started manual). Try second order elements
Hi every one.
As I see, the major difference is that the 1D model oscillates between -0.1 and 0.1, which means that the applied load is eliminated (applied for a short time), while the 3D model oscillates between 0 and 0.35, which means that the applied load still acting on the beam (the whole time). checked you loading in both models.
actually forcing on both of them is sinusoidal. f(t)= F * sin(omega*t )
Sorry, I should have mentioned it earlier.
I really appreciate all the responses..thanks
It is better you do the complete model (instead of symmetry), fix all the dofs at the nodes on the left vertical face and apply the forces on the nodes (more no of elements needed along the width) at the free end.
Obviously, something wrong with the loading conditions for the 3D model of the beam. If the external load is sinusoidal, f(t) = F*SIN(omega*t), then the beam must vibrate about the natural (undeformed) configuration as shown in the right figure. The solution shown in the left figure implies that a constant component (in addition to the sinusoidal component) is applied to the beam, that is f(t)=F0+F*SIN(omega*t). This effect might be due to gravity. See if the acceleration is set equal to zero.
Next point: half the beam should be loaded by a force of 10N/2=5N. I would apply 2.5N to each of the two nodes, which corresponds to a total load of 10N = 2.5(left node)+2*2.5(central node)+2.5(right node). I hope this helps.
By the way, ten elements across the thickness is too many. I think, four elements would be enough.
And finally, in order that the two solutions agree better, set Poisson ratio in the 3D model equal to zero (but I don't believe that the effect is significant).
Thanks a lot to all of you . I got my mistake.
And like to share about how we can give the point load on the 3D geometry.
To distribute the point load on the end surface we can use a Distributed coupling option in the Abaqus to avoid the local deformations.
Now it comes out to be pretty well.just little bit of shift in the frequency.
Thanks a lot again
The researcher can apply shear deformation beam theory to the analysis of the beam considering 3D geometry
- Badges
- Science topic