Model buckling of pipe with shell elements

[Kat_kat]

Hello, I'm having a problem modelling a straight thick pipe under compressive axial load with shell elements. I'm interested in finding the eigenvalues/eigenmodes of the pipe using a linear perturbation step (buckle).
Before that, I have tried to model the pipe with elbow31 elements and the 1st eigenvalue matched the Euler critical buckling load.
Trying the same problem with shell elements gives me an eigenvalue almost double the Euler load.
Does anyone know why? I've tried almost everything I could think of but with no success. I don't have access to it now but if needed I can attach the .inp or .cae file.
Any help would be greatly appreciated. Thank you in advance.

 

[FEA way]

What are the boundary conditions in the shell model ? Which shell elements do you use ? Are you sure that thickness is properly defined ?

 

[Kat_kat]

Sorry for taking so long to respond.
The boundary conditions are:
Left end: ux=uy-uz=0 (pinned)
Right end: ux=uy=0 (roller)
For the shell elements i used S4R elements

For the thickness: first i sketched the cross section with the internal radius and set the length of the pipe using extrusion. Then i specified the thickness through the SECTION option choosing OFFSET=BOTTOM.
I have also attached the .cae file.

Thank you for your time.

 

[FEA way]

If I’m correct, analytical result should be 249418.72 N. You will get a value close to this one if you change your BCs - disable those applied directly to the edges of the pipe (they aee redundant) and leave only those applied via kinematic coupling. Also block 2 rotations in both these BCs leaving only UR2 as free.

 

[Kat_kat]

Thank you for your reply. Yes, the analytical result is 249418.72 N. I tried what you suggested and the first eigenvalue comes to around 227162 N. Is there any way to decrease the error between the analytical and the abaqus result? Maybe increasing the elements number or changing the element type?

 

[FEA way]

With beam elements you will get a correct solution. With shells it's more tricky. Your mesh is sufficiently refined but you can try using different element type. Check the documentation example "
Buckling of a cylindrical shell under uniform axial pressure" for comparison between different types of elements in similar application.

 

[Kat_kat]

Thank you, i'll check it out. I have one last question.
I tried modeling the same exact problem but instead of the 2 coupling constraints at the ends I used 2 parts that basically act like the pipe's ends. I used the same shell elements as the pipe and a material with a much higher Young's Modulus so that there won't be any deformation. Again the BCs are:
Left end: ux=uy=uz=0, ur1=ur3=0
Right end: ux=uy=0, ur1=ur3=0
I expected the buckling load to be the same but abaqus gave me a value of 435764 N.
Is the model or my assumption wrong?

(i attached the .inp file because the .cae file was too large)

 

[FEA way]

Adding caps to this shell pipe is not a good approach. However, today I carried out some tests and finally obtained a value with high enough accuracy: 244913 kN (actually these results should be in kN not N to maintain consistency with other units in the model). What you should do to get this result (apart from what I advised before regarding BCs) is:
- model the pipe using middle surface instead of bottom offset (you have to change the diameter of the pipe’s geometry to 1.4 first)
- increase the mesh density and use S8R elements
- use rigid body constraints (with tie option) instead of kinematic couplings