Rubber cylinder to hyperboloid

[Davide Recchia]

Hi All,

I have a cylindrical rubber piece that I want to twist into a hyperboloid.
I tried fixing a circular edge, and applying a rotational displacement of 10° to the other edge but
the deformation seems quite unrealistic. I would expect the necking to happen about halfway.
Also the required rotation is 30 deg, but solution won't converge.
Any tips on how to set up this problem is greatly appreciated.

Project files:

https://files.engineering.com/getfi...e-444b-8be9-5a1b4ea046a8&file=Twist_Seal.wbpz

Thanks

 

[karachun]

Maybe you are trying to calculate problem in linear static. Linear assumption (small displacements and small rotations) give large errors when you are use rigid elements (RBE2 or RBE3 you use to apply load or fix other end) and rotation.
Try to on nonlinear solution.

 

[Davide Recchia]

I wouldn't know how to go about fixing that.
For your info, I did turn on large deflection mode in analysis settings

 

[AnPham]

If can, please share that project.
Everyone can check it.

 

[Davide Recchia]

I added link to project files to original post

Thanks

 

[rothers]

You need to also restrain the left hand circular edge in Z and radial leaving only rotational free. Does ANSYS not have cylindrical coordinate systems ? Would seem the ideal use of such.

Like this:

 

[Davide Recchia]

Hi rother,

I inserted a cylindrical coordinate system and set axial and radial displacement to 0. Rotation set to 15 mm.

It sure helped, at least now the necking is happening in the middle, as expected.
Still when I look at the deformed shape (true scale) the edge expands out in radial direction:

Any ideas why this might be happening?

Also in real life when twisting the rubber sheet overlapping folds start to appear.
I was able to reproduce this in ANSYS by tweaking dimensions of cylinder and playing with mesh settings
but it seems a bit inconsistent. I cannot get the right result every time.

Thanks

 

[rothers]

When you say "set axial and radial displacement to 0" do you mean you applied a prescribed displacement of 0 magnitude or do you mean you constrained the nodes to be fixed in axial and radial directions ?

I don't use ANSYS, we have NX Nastran & Algor. In our world 0 described displacement and fixed are different things. 0 described displacement simply means no displacement is applied, i.e the nodes are free to move.

 

[L_K]

I would check the value for the radial displacement (directional deformation in the x direction). The scaled plot can be misleading.

 

[Davide Recchia]

I checked the radial displacement and indeed it's really small at the top edge.
The plot scale was set 1.0 (True scale) so maybe just a visualization artifact of ANSYS?

 

[L_K]

Seems that the program is using the total deformation value to visualize the scaling. You can also use remote displacement boundary condition if you want to define the angle.

 

[Davide Recchia]

Here's the latest result where folds appear.
I added a step to pre-tension the membrane in axial direction before twisting.
Really hard to find convergence with a refined mesh or twist angle greater than 15°

 

[L_K]

These are hard problems. What is the error message? Distorted elements?
How much is the max plastic strain before the analysis stops?

 

[Davide Recchia]

Most of the time the errors are due to highly distorted elements.
I thought that refining the mesh would help instead it seems to make things worse.
I didn't even bother to add self contact, because solving time goes up exponentially.
Kind of stuck at the moment...

 

[L_K]

I am getting the analysis to converge to 30 degrees using linear tets and element size 1mm.
By the way, check the location of the reference node of the remote displacement boundary condition.
In this case the location does not matter though.

 

[Erik Panos Kostson]

A couple of things that will help.

-Use QUAD8 elements, since this is a thin body (higher order QUADS, to capture curvature better, ..). You can set that in mesh and element order (set to quadratic).

-Use stabilisation since the structure undergoes some form of instability (as seen in your image above).

-Move your remote point location in z top about the opposite edge (Z= ~0.0157 m).

With that and with more initial steps (100)+maximum steps (1000) for step 2, it is fine (solves for 32 degrees) just make sure that the stabilisation energy is not too high in the end (should be small compared to the elastic energy).

 

[Davide Recchia]

Thanks guys, this really helped!

 

[Erik Panos Kostson]

You are more than welcome Davide

 

[Davide Recchia]

What if I want to take this even further and go a full half rotation (180°).
Is there any chance it will converge?

 

[karachun]

Why not to try it?