bonded or no-separation getting separated

  • 3.5K Views
  • Last Post 30 October 2018
jonsys posted this 15 October 2018

Hello Community,

On modeling laminated glass (2 panes, 1 interlayer in-between), I define the contact between panes and interlayer as "Bonded" or "No separation", but I still get a separation of the geometries which is not supposed to happen with these 2 contact type definitions.

Should I change some settings from "Programme controlled"?

Order By: Standard | Newest | Votes
peteroznewman posted this 15 October 2018

Hello Jon,

No separation is not appropriate for laminated glass.  It is appropriate for two surfaces that slide on each other.  Laminated means it is bonded and should not slide.

There are several Formulations that can be used for a Bonded contact, try MPC.

Another approach is to not use contact at all and use Shared Topology (or Node Merge) to have different materials on each layer share a common plane of nodes at the interface. Then there is nothing to separate.

Regards,
Peter

  • Liked by
  • jonsys
SandeepMedikonda posted this 15 October 2018

Jon,

  Use the MPC formulation:

For the specific case of Bonded and No Separation Types of contact between two faces, a Multi-Point constraint (MPC) formulation is available. MPC internally adds constraint equations to “tie” the displacements between contacting surfaces. This approach is not penalty-based or Lagrange multiplier-based. It is a direct, efficient way of relating surfaces of contact regions which are bonded. Large-deformation effects are supported with MPC-based Bonded contact.

I often find this table from the manual very useful:

Regards,
Sandeep

  • Liked by
  • jonsys
jonsys posted this 16 October 2018

Hello Peter and Sandeep,

thank you for your support.

Please take a look at the picture;
a - two glass panes, no interlayer;
b - two glass panes with interlayer;
c - 1 glass pane with thickness equal to (2 x glass + interlayer) thickness of b.

I can see from the analysis that Bonded MPC formulation gives the same result as shared Topology. I have been using the latter so far.

But with that, I keep getting the result as in "c", even though I have a laminated one and should get results as in "b".

This made me think that probably defining some other contact would be the solution.

 

1

 

Regards,

peteroznewman posted this 16 October 2018

Jon,

Bonded MPC and Shared Topology (or Node Merge) do give very similar results, but the Bonded MPC adds equations to the solution that have to be solved and each interface has twice as many nodes which have to be solved. Since I like to reduce elapsed time, I prefer to not use Bonded Contact if I can use Shared Topology.

If you have the right material properties, you can produce the stress distribution shown for the Laminated configuration using shared topology.  In the model below, I have a 3 layer sandwich, with a top 4.4 mm layer, a middle 0.2 mm layer and a bottom 4.4 mm layer for a total 9 mm thick sandwich. The middle layer has an orthotropic material property with low shear stiffness.  I created a path through the thickness to plot the Normal X Stress. The graph looks like the Laminated configuration stress distribution you show above.

Here is the middle material:

I added a Coordinate system where Z pointed in the Global Y direction to use this material.

However, an orthotropic elastic material might not represent what is in your laminated glass. After the glass has been bent around the form and left for some time (maybe at an elevated temperature) and the glass is released from the form, does it stay curved or does is spring back to flat?  If it stays curved, you may want to model the laminate as a viscoelastic material and the two panes will, over time, slide relative to one another.

Regards,
Peter

SandeepMedikonda posted this 16 October 2018

Also, isn't the laminated configuration behavior more due to Interface Delamination or Contact Debonding?

Regards,
Sandeep

bsista posted this 16 October 2018

Jon,

Based on your second post, note that when you're using shared topology, it assumes that there is no interlayer which is why the response is similar to scenario C instead of B. Similarly, when you replace shared topology with a bonded contact, the "interlayer stiffness" is nothing but the contact stiffness calculated based on the properties of the underlying solid elements (glass in your case). So, the response is again similar to scenario C.

If you wish to simulate the scenario B, then you'll need to account for the softer interlayer. This can be done in two ways:

  • use a thin solid sandwiched between the two glass layers to represent that interlayer, you'll need to join them using a bonded contact.
  • use a penalty based bonded contact(Augmented Lagrange is preferred) and define the normal stiffness manually using command snippet( use -ve value for FKN so the solver reads it as the absolute value rather than a multiplying factor). The stiffness that you define here should be same as the stiffness of the interlayer in reality.

Finally, regarding your original question on by the bonded or no separation contact may not be holding the parts together, check these options:

use Contact Tool to see if there is any gap between the two parts, to begin with. If there is a gap, then manually define a larger pinball radius (larger than the gap).

make sure that the mesh is not too coarse.

if these are curved surfaces, then turn off the trim contact.

peteroznewman posted this 17 October 2018

bsista, I like the idea of using the stiffness of the bonded contact to provide the shear flexibility of a two-layer model. 

In my post above, I used a thin solid sandwiched between two glass layers, but I joined them with shared topology, not bonded contact. The stress profile matched the laminated scenario B.

 

  • Liked by
  • jonsys
jonsys posted this 17 October 2018

Hello Peter,

An isotropic material defined the interlayer should also give the graph shown in your picture. And to mention also your last part of the answer, I define the interlayer material as viscoelastic (in which the shear modulus will decrease with time). The Normal stress x graph, can be as "c" (my picture at previous comment) in earlier stage of loadings (since the shear mod is high), but after some time it should start to look like "b". But it doesn't in my case, even though I request the result after ~1year when Shear modulus is around 1-2 MPa.

I was doing some attempts trying Shared Topology: When I increase the thickness of the panes and interlayer [Fig 1], or when I increase the dimension in x, the behavior starts to look like "b".

 

1

Now one might think that since it works with higher thickness, the results when thickness is low is also correct. But exp results show a behavior as "b"

That made me think that I lack the necessary skills in ansys to implement something that captures the results at this position

1

I also tried to add more elements throughout the thickness and even tried to change the elements to SOLSH190 but no improvements observed.

Regards,

jonsys posted this 17 October 2018

Hello bsista,

thank you for the suggestions,

  • use a thin solid sandwiched between the two glass layers to represent that interlayer, you'll need to join them using a bonded contact.

What do you mean by a thin solid sandwiched? I guess it is the same as the one that I am using

1

I defined the bonded contact (with formulation Program controlled and later Augmented Lagrange, with trim on & off), but they still were separated from picture (is this normal?).

2

 

  • use a penalty based bonded contact(Augmented Lagrange is preferred) and define the normal stiffness manually using command snippet( use -ve value for FKN so the solver reads it as the absolute value rather than a multiplying factor). The stiffness that you define here should be same as the stiffness of the interlayer in reality.

I lack skills in Command Snippet. Can you please tell me exactly what to write there?

 

Regards,

bsista posted this 17 October 2018

Jonsys,

Yes, that's what I meant by thin solid sandwiched. Have you tried refining the mesh to see if that improves the result? The default contact formulation is Augmented Lagrange and it usually robust for these applications. Also, check the contact status using Contact Tool (under Solution), see if the contact is open or if it is closed. When the mesh is coarse, chances are that the penetration/gaps that you see are just numerical approximations. 

Regarding the command snippet, just insert this snippet under the contact object:

RMODIF,cid,3,<fkn_value>

When you define fkn_value as +ve number, it is multiplied to the contact stiffness calculated by the solver. If you define it as -ve number, it is taken as the absolute value of the contact stiffness. So, make sure that you're using consistent units.

  • Liked by
  • jonsys
bsista posted this 17 October 2018

Peter,

Shared topology is indeed the preferred method. The only drawback with that approach is that if the goal of the simulation is to assess the stresses at the interface, maybe to see if delamination occurs, then it is difficult to get the stresses on the shared surface. For such cases, replaced shared topology with a bonded contact helps. If that is not the requirement for this application, then shared topology is the preferred approach. 

  • Liked by
  • jonsys
peteroznewman posted this 17 October 2018

Thanks bsista, that confirms my understanding.

  • Liked by
  • jonsys
jonsys posted this 29 October 2018

Hello bsista,

thank you for your answer and sorry I reply this late.

I implemented the command snippet like this

1

but it does not allow to run the solver at all. It can also not run the Contact tool.
When I suppress these Command Snippets, then it ok so I guess the problem is comming fro there.

Any suggestions?

Regards,

 

SandeepMedikonda posted this 29 October 2018

Jon,

Don't use the value in the arrow brackets, Bhargava was just using that as an illustration:

RMODIF,cid,3,-220

Regards,
Sandeep

  • Liked by
  • jonsys
bsista posted this 29 October 2018

My bad! We follow that convention internally so I used it without explaining, my apologies!

As Sandeep mentioned, remove the brackets and replace with the number. But I'm glad that you have asked this question as it reminded me of another thing. Since you're intending to use a constant contact stiffness, change the Update Stiffness option under the contact object to Never so the stiffness remains constant.

  • Liked by
  • jonsys
jonsys posted this 30 October 2018

oh, alright I see now. Thank you for the answer

 

If the Update Stiffness option is set to Never, then the visco-elastic behavior of the interlayer can not be represented right?

And should the Normal Stiffness defined in the command snippet be the shear modulus of the interlayer?

Regards,

Close