default Contact

  • Last Post 2 weeks ago
  • Topic Is Solved
jonsys posted this 2 weeks ago

I am simulating in Workbench a simply supported laminated glass (2 glass panes and a PVB interlayer material in-between). It is subjected by pressure on the top face (Like the simulation of plate, subjected by a load perpendicular to its surface).
At Mechanical, I see that 3 Contact Regions are created by ANSYS by default.

  • Should there be 3 Regions?
    (In one of these Regions, the Target and Contact Bodies are the Lower and Upper Pane [Fig 1] - I find this strange because these two separate solids do not touch each other)


Secondly, compared with the analytical solution, this value is ok, because it represents the case when these panes are fully interacting with each other.

  • How can I simulate partialy bonded panes (I know the shear action value) and not full bond?



Order By: Standard | Newest | Votes
ssridhar posted this 2 weeks ago

Hi Jonsys, 

1) Workbench Mechanical uses an Auto-detection algorithm to assign contact between surfaces based on their proximity to one another.  This proximity value is decided by a tolerance that represents the separation between two surfaces. This default value set for the model can be found in the Details section of the 'Contact' field (See Image-1 attached). You can change the tolerance using the slider to tighten the contact assignment (useful for large assemblies) or you can manually assign/ suppress a contact region you find redundant. 

Also, take a look at the Contact tool functionality (

Contact Detection tolerance


2) I am not sure exactly what you mean by Partially bonded panes. In Engineering Data you can define a Cohesive zone material model and then simulate contact debonding in Mechanical. Perhaps someone on the forum with more experience in this can comment. 





  • Liked by
  • jonsys
SandeepMedikonda posted this 2 weeks ago

Hello Jonsys, 

  In addition to what Raghav mentions, you can also change the default settings in Tools>Options>Connections.

It looks like you are trying to define failure in your contact, You might have to use the EKILL commands if you know what load step you want to kill the contact but if you want to do it based on a stress in the contact elements, you might have to insert a command object with a do loop that checks for the stress in these contact elements at each equilibrium condition and kills it based on that. You can always try Explicit LS-DYNA for limits on bonded contact interfaces (TIEBREAK contact).


  • Liked by
  • jonsys
jonsys posted this 2 weeks ago


thank you.

1) If the Tolerance Type is set to Slider, what does the tolerance slider value represent?
Howerver, I changed the tolerance value and now the auto-contact detects only two regions. But when I run the simulation (there is separation between panes) [Fig 1]

2) Sorry, I was not so clear in explaining this one:
The value that I get from this simulation of laminated glass (of 2 panes with interlayer betwen) is very close to the simulation for only 1 glass pane (with the same thickness of the laminated glass). So same thickness, similiar output but one is laminated and the other only 1 pane-> I guess that is comming from contact (3 Regions instead of two - but now with 2 Regions there's an oppening).
By partially bonded, I mean that the two glass panes will not act as one; they will have some interaction which is dependent by shear modulus of the interlayer.




jonsys posted this 2 weeks ago

Hello Sandeep,

thank you for the answer.

How should that do loop that checks the stress look like?
I have never used that, but why would Explicit LS-DYNA make a better choice in this case?


peteroznewman posted this 2 weeks ago

Hello Jon,

Sandeep or Raghav may have something more to add, but I have a few comments.

Now that you have clarified that you want the PVC layer to just shear and not debond from the glass, one approach is to get rid of contact altogether and use Shared Topology to make the three layers connect to common nodes at the two coincident faces.  You do this by going into DesignModeler, picking the three solid bodies at the bottom of the outline and RMB to select Form New Part.  Now instead of 3 parts and 3 bodies you will have 1 part and 3 bodies.  Refresh the project and open Mechanical. Delete all the contacts. The mesher will connect the three bodies and you will not get any separation between the panes.

The values for the slider for contact distance tolerance is just a relative number and doesn't mean much. You can type in a distance in mm if you want, which is what I usually do.

If you were interested in debonding, Explicit Dynamics has by default a feature called Erosion, which can remove elements from a transient simulation as those elements reach a failure level defined by the material or the equivalent strain threshold that you can set.



  • Liked by
  • SandeepMedikonda
SandeepMedikonda posted this 2 weeks ago


  I think explicit is a better route to go. I would be tempted to try it with ANSYS LS-DYNA, because its much simpler and you can specify the stress criteria for breaking as your modeling requirements are:



jonsys posted this 2 weeks ago

Hello Peter,

Shared Topology resolved the issue. thank you

I will now try to implement SOLSH190 as you have suggested. After I get used to ANSYS a bit more, I might try debonding as well so thnx for letting me know.



jonsys posted this 2 weeks ago


thank you. I will try to implement that too and I will come back in case of questions