Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations waross on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Rubber cylinder to hyperboloid

Status
Not open for further replies.
Davide Recchia

Davide Recchia

Mechanical
Jun 3, 2019
30
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.

Cylinder_mesh_nsqdlq.png

Cylinder_displacement_untrzh.png


Project files:

Thanks
 
Replies continue below

Recommended for you

Sort by date Sort by votes
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.
Small-Displacement-Theory_jjhqgc.png
 
Upvote 0 Downvote
I wouldn't know how to go about fixing that.
For your info, I did turn on large deflection mode in analysis settings
 
Upvote 0 Downvote
If can, please share that project.
Everyone can check it.
 
Upvote 0 Downvote
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:

Cylinder_-_hyperboloid_-_cone_hue1tr.gif
 
Upvote 0 Downvote
Hi rother,

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

Cylinder_displacement_15mm_yzfo8o.png


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:

Cylinder_displacement_hjfmr0.png

Cylinder_displacement_side_jqcata.png


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
 
Upvote 0 Downvote
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.



 
Upvote 0 Downvote
I would check the value for the radial displacement (directional deformation in the x direction). The scaled plot can be misleading.
 
Upvote 0 Downvote
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?

Radial_deformation_g7facv.png
 
Upvote 0 Downvote
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.
 
Upvote 0 Downvote
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°

Cylinder_displacement_fsdvzg.png




 
Upvote 0 Downvote
These are hard problems. What is the error message? Distorted elements?
How much is the max plastic strain before the analysis stops?
 
Upvote 0 Downvote
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...
 
Upvote 0 Downvote
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.

pic_x96pra.png
 
Upvote 0 Downvote
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).

Capture_gyd0rq.png
 
Upvote 0 Downvote
What if I want to take this even further and go a full half rotation (180°).
Is there any chance it will converge?
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

alpha000
  • Question
Bend straight beam to circular helix
Replies
1
Views
2K
Doug Hunter
Doug Hunter
M
  • Locked
  • Question
ANSYS Mechanical Scripting: how to delete an existing heatflux?
Replies
0
Views
696
MihailW
M
W
  • Question
Trying to couple a transient thermal and structural simulation but I get zero deformation and stress
Replies
0
Views
1K
weldtest12
W
Sarikahirpara
  • Locked
  • Question
Negative Temperature values due to friction between gears.
Replies
0
Views
422
Sarikahirpara
Sarikahirpara
H
  • Locked
  • Question
how to apply triangular load on an area, in ANSYS Workbench static module
Replies
1
Views
3K
karachun
karachun

Part and Inventory Search

Sponsor

Back
Top Bottom