Modelling a Tapered Beam in ABAQUS

[Sri Harsha]

Hello Everyone,

I have been trying to create a Tapered beam in ABAQUS.
I Have followed the below steps:

1) While defining the section,I have choosen "Before analysis" option in "Section Integration"

2) Then,I have choosen "Tapered" option in "Beam Shape along length"

3) Then,it asks me to select "Beam Profile start" and "Beam Profile end".

Now,once I am done with these things, tapered beam is getting created but I am not able to understand the orientation of the tapered beam.
For e.g: If I am choosing a radius of 1 mm at one end and radius of 0.5 mm at other end,How can I understand which is the starting profile as well as ending profiles for my tapered beam.
I have even tried rendering the tapered beam profile to visualise it. But its clearly written in ABAQUS Manual that, rendering does n't work for tapered beam


Can someone please address this issue

Thanks in Advance

 

[cooken]

I suspect the taper direction will coincide with the beam tangent direction. I suggest you do a quick test to verify.

 

[Sri Harsha]

Hi cooken,

Thanks for your reply.
How can I test it? Can you please explain briefly?

 

[cooken]

Fix one end and apply a load/moment or enforced displacement/rotation at the other end and look at the result. Should be obvious which direction the taper is in.

 

[Sri Harsha]

Hi Cooken,

We basically cant visualize the beam profile even after applying the load. If we try to render the beam profile,it just seems like a normal beam,which is not tampered!

Can you explain your above comment briefly

 

[cooken]

Look at the deflection/stress distributions? You might need to use more than one element.

 

[Sri Harsha]

Hi cooken,

Thanks a lot for your reply. After properly analyzing the stress distribution,I am now able to understand the direction of Taper in the beam.
After going through the manual,my confusion has only increased.In the ABAQUS Manual, it says that if I am using tapered beam and I am meshing my beam with 3 elements, each of my beam element will be tapered.For my simulation,I need a tapered continous beam(i.e. continously the area keeps on decreasing along the length).

Can you please suggest a method to tackle this

Waiting for your reply

 

[Dave442]

This is addressed in the documentation:

Abaqus analysis users guide -> elements -> structural elements -> beam elements -> using a general beam section to define section behavior

"When you apply a tapered beam section to geometry in Abaqus/CAE, the full tapering is applied to each element along the beam’s length. For beams that include multiple elements, this modeling style can create a “sawtooth” pattern along the length of the beam. If you want to model gradual tapering along the entire length of the beam in Abaqus/CAE, you must calculate the size and shape of the beam profiles at the intermediate nodes, then apply different tapered beam sections to each beam element along the length."

 

[Sri Harsha]

Hi Dave,

Thanks for your reply. But is n't that really a difficult task? We always change the meshing of the beam right like sometimes 4 elements and sometimes 5 elements.If we keep on changing the mesh sizes,how will we automatically change the tapered sizes at each intermediate node??

 

[Dave442]

the profile size and shape is a function of the intermediate node locations along the length of the beam.

if it's a hassle to do it manually you can write a python script to do it for you.

 

[Sri Harsha]

Hi Dave,

But we are defining the Tapered section before meshing our beam right?
Even,while writing a python script , we will be following the same procedure right?

Can you please give me an algorithm for writing this kind of python script!

 

[cooken]

Glad it worked and you confirmed the direction at least.

In terms of scripting to define multiple sections, you are the one who decides the number of elements. You should know the total length, and so the section definitions will be a function of the number of divisions that YOU decide. Therefore they can be defined prior to meshing.

 

[Dave442]

section/profile definitions can also be defined/assigned after meshing. At this point:

you know the length of your beam
you know the initial and final profile shape/size
you know the total number of intermediate nodes
you know the position of each intermediate node along the beam
you know the profile shape/size varies linearly with node position

Or have I missed something?

 

[Dave442]

As an alternative, you could specify constant profile and just gradually reduce profile size-shape for each element to approximate the taper. You might not need too many elements to obtain accurate results and at least then you could clearly visualize taper etc.

 

[Sri Harsha]

Hi Dave and Cooken,

In my analysis, I am using Johnson cook hardening ...When I define a tapered beam, it is not allowing me to define material property for the section.But If I am creating a constant beam(not tapered), then there is an option to select the desired Material.
But in case of Tapered, it is asking me to enter the values of Youngs Modulus and shear MOdulus,But I cant apply Johnson cook to that particular section

Can you please let me know regarding this

 

[Dave442]

From the documentation:

"In Abaqus/Standard you can define Timoshenko beams with linearly tapered cross-sections. General beam sections with linear response and standard library sections are supported, with the exception of arbitrary sections."

 

[cooken]

To add to this - you are using a section integrated "before analysis", meaning linear. So from my understanding it doesn't make sense to use a nonlinear property with that, hence the limitation.

A possible workaround would be to use much smaller elements with non-tapered sections integrated during analysis (like a telescope) to approximate a tapered beam?

Welcome to the trials and tribulations of the FE world, where nothing is ever as easy and straightforward as it seems.