Hyperelastic multi-layered tube buckling/compression

  • 82 Views
  • Last Post 05 October 2018
  • Topic Is Solved
zjuv9021 posted this 04 October 2018

Hi All,

I am working on a project that involves a multilayered hyperelastic tubing that I would ultimately like to be able to place displacement compressions, twist it, bend it, etc. involving nonlinear frictional contact. I am currently treating these as Isotropic, but do have uniaxial, biaxial, and shear test data available for some Mooney-Rivlin parameter fittings... but figured I'd figure out Isotropic FIRST.

 

Geometry/Materials:

  • Inner tube: Silicone Rubber; Young's Modulus: 250 psi (0.49 Poisson's Ratio)
  • Second layer: Polyethylene terephthalate (PET) monofilament (treated as a 3D surface wrapped around in contact with the silicone); Young's Modulus: 71,000 psi (0.49 Poisson's Ratio)
  • Third Layer: Polyurethane 80A; Young's Modulus: 500 psi (0.49 Poisson's Ratio)
  • Fourth outer-most layer: Polyurethane 55D; Young's Modulus: 2,500 psi (0.49 Poisson's Ratio)

The tubing below is 0.500" long.

Geometry

 

Contact:

  • Silicone Rubber->PET: Frictional Contact with a coefficient of 0.1
  • PET->PU80A: Frictional Contact with a coefficient of 0.1
  • PU80A->PU55D: Bonded Contact

Mesh:

  • I am currently utilizing hex dominant method. I'm not sure if Contact Match or Node Merge could come in handy here. Open for opinions regarding this kind of surface contact.

BCs:

  • One end is fixed, and the other end faces have constraints in the x-z plane with a displacement of 0.1" in the negative y direction to compress towards the fixed end in hopes to induce a buckling shape.
  • There is also a pressure (fluid moving through the tubing) of 1 psi inside the silicone tubing.

Issues:

  • As with most people, convergence. "Contact Status has Experienced an abrupt change". Highly distorted elements. 
  • I've even run my Eigenvalue Buckling to get my critical load factor that would induce my first buckling shape:Eigenvalue Mode 1

I took the Load Multiplier and multiplied that by my load applied to this tubing (1 lbf) to determine the critical buckling load, and then added ~20% increase to this value along with a perturbation in Nonlinear Structural to try to obtain some post-buckling behavior but had no success with this.

I'm a little lost with this, let alone how to even start including non-linear material modeling, so any help or thoughts is GREATLY appreciated!

Regards,

Zach

Attached Files

Order By: Standard | Newest | Votes
zjuv9021 posted this 04 October 2018

PS: Please see the attached .wbpz for the actual project.

Zach

SandeepMedikonda posted this 04 October 2018

Zach,

  I am unable to look at the file, but can you post a couple more snapshots of the Analysis settings and the Frictional Contact you have?

  Also, what material models are you using? Are you fitting these in Engineering Data?

Regards,
Sandeep
Best Practices to post on the Student Community

  • Liked by
  • zjuv9021
zjuv9021 posted this 04 October 2018

Hi Sandeep,

 

I am currently just treating these (for simplicity sake) as linear Isotropic materials. I have data available to fit, but figured it would be best to start with this first.

Please see the attached for Analysis Settings and Frictional Contact.

 

Analysis Settings

Contact

 Regards,

Zach

SandeepMedikonda posted this 04 October 2018

Hi Zach,

  Please see if the following suggestions help:

  • Look at the Force Convergence plot and the Newton-Raphson residuals.
    •    There are numerous posts in the forum on these 2 if you are not sure how to read them or request them.
  • Dropping mid-sized nodes helps? Just change the Mesh from quadratic to linear under Mesh.
  • See if further reducing the Normal Stiffness or aggressive update of contact stiffness help?
  • Double check your pinball radius and increase it if needed?
    •    Use the Initial Contact tool to check this. Again there are posts in the forum on this.
  • See if using the Unsymmetric solver helps? Can be changed in Analysis>Nonlinear Controls>Newton-Raphson Option
  • Introduce some Stabilization Damping Factor in contact, say 1e-02 and see if it helps.
  • If nothing helps add some Stabilization Energy to your model from Analysis Settings>Nonlinear Controls> Stabilization. Use: Constant, Energy, .05, No and 0.2 as options for the following cells. Note that you have to be careful with the amount of artificial energy you add. So, check on this while post-processing the results

Regards,
Sandeep
Best Practices to post on the Student Community

  • Liked by
  • zjuv9021
peteroznewman posted this 05 October 2018

Hi Zach,

I looked at your archive and noted that your mesh could be improved to help the solver converge.

I think putting two elements through the wall thickness is going to help.

If you split the bodies in SpaceClaim, you can get the nodes to line up exactly.

Would it be worthwhile to eliminate the frictional contact and have these different materials effectively bonded together using Shared Topology? That way, the different materials will share nodes at the common face and the likelihood of convergence would be much greater.

Regards,
Peter

  • Liked by
  • zjuv9021
zjuv9021 posted this 05 October 2018

Thank you Peter,

I am not as familiar with Shared Topology. What do I lose with utilizing this feature? Can I ever implement frictional contact in this scenario?

 

Kind Regards,

Zach

zjuv9021 posted this 05 October 2018

Sandeep,

 

Do you know why dropping midside nodes helps in this particular model?

Regards,

Zach

peteroznewman posted this 05 October 2018

Zach,

You mentioned you are using isotropic materials,  before you make the model more complicated with hyperelastic materials.

In a similar way, you can use no contact, before you make the model more complicated with frictional contact. It's just another way to take baby steps to the full model.  It would show you how the multi-layer tube behaves without sliding between the layers. However, if sliding between the layers is the behavior of interest, then there would be no point in taking this approach.

Shared Topology is found in SpaceClaim under the Workbench Tab. You should see the 3 faces and 6 edges shared. Once you have that, you don't need any contact elements. You have hidden solids that complicate sharing, so clean up your geometry before you attempt this.

Regards,

Peter

 

 

akhemka posted this 05 October 2018

Hi Zach,

 

On your query to Sandeep - midside nodes dropped (linear elements) will offer lower stiffness and help in avoiding distortion issue. Looking at the shape, do you expect a self contact? I agree with Peter on taking baby steps - you may use bonded contact between the tubes (just a suggestion - sharing the topology is a way of doing the same without contact) to see how the behavior is and then switch to frictionless or frictional. 

 

Regards,

Ashish Khemka

 

 

  • Liked by
  • SandeepMedikonda
zjuv9021 posted this 05 October 2018

Thank you Peter,

I'm interested in trying this route. Is it equivalent to bonded contact, minus having contact elements?

what recommends do you have for 'cleaning up' my geometry? For now i'll start to play around with this feature.

Regards,

Zach

peteroznewman posted this 05 October 2018

Zach,

Shared Topology allows different materials to be bonded together without Bonded Contact. One benefit is slightly smaller models that will solve in less time.

In SpaceClaim, you have 8 solids with 4 hidden.

In Mechanical, you suppressed 4 solids.

I assumed the four suppressed solids matched the four hidden solids, but I was wrong.

The better practice is to select four solids in SpaceClaim and Suppress for Physics. That is what I have done for the last four solids and I flipped the visible set.  You can see at the bottom of the image below the Share Topology setting is set to Share.  Sometimes that is all you need to do.

When I try the Share tool in Workbench, I don't get all three faces, I have to change the Coincidence Tolerance in the Options to be 0.0001 mm otherwise it tries to jump across a wall thickness and collapse one of the walls to nothing. When I try to Share, it finds 3 faces and 7 edges.  It should find 6 edges. This extra edge being shared may be a source of difficulty in meshing. If I increase the Tolerance, it goes down to 2 faces before it drops to 6 edges.

Did you import this geometry or create it in SpaceClaim?  If you imported, try creating it from scratch in SC.

Regards,
Peter

Close