Using Modal analysis to check Static Structural contacts

  • Last Post 18 March 2020
peteroznewman posted this 28 October 2017

When bonded contact has been used to connect several parts in a structure, running a Modal analysis is a very useful diagnostic tool to verify that all the parts are connected. The ones that are not will "fly off" the model when looking at the zero frequency mode shape results.

  • Liked by
  • enors
Order By: Standard | Newest | Votes
myvue posted this 17 March 2020

Hello Peter,

I know this is an old post, and I am sorry if I should have made a new post, but I have a query related to this one.

I have a model that has bonded contacts, however when I perform the modal analysis, it shows me (in auto scale) two parts that are flying away. What should I do now to create a contact? Should I use 'zero displacement' support on those parts to limit their movement? Because when I do that, now the modal analysis shows many other parts not in contact any longer.

I have another query that might be deviating from the current problem at hand, but it is still related to this video. You used auto scale, and not true scale, to view the solution. I am confused about the use of auto scale. The internet does not help much on the issue, but what I have understood is that if displacements are very small, the results are shown in auto scale (with increased displacements) to show where the displacement would eventually occur. Is that correct? If so, then why would it do that, showing displacements that do not actually occur using the given load and boundary conditions?

Thank you.

peteroznewman posted this 17 March 2020

To answer your second question, here is a relevant discussion about Modal analysis. One of my replies in that discussion describes the two scale factors that can be chosen for the displacement results. Knowing that the displacement values are arbitrary, you can set the display scale factor to any value that makes it easy to see the motion of the body.

If you are not in Modal, but in Harmonic Response, then the displacements are real, and you can set the display scale factor to any value that makes it easy to see the motion of the body. Note that Harmonic Response is a linear analysis, so it includes the small deflection and small rotation assumption. That means if you make the load 10 times larger, the displacement will go in a straight line along the same direction it went at a 1 times load.  At some point, this produces unrealistic deformation because the small deflection assumption is no longer valid.

If edges or faces are moving apart that should be bonded together, that means the contact is not working and you need to increase the Pinball radius to get it to create the bonds.  I prefer to use Formulation MPC so I can see the Connection elements in red after the solver has run. If possible, use Shared Topology in SpaceClaim or DesignModeler to connect adjacent edges/faces, then you don't need contact.


  • Liked by
  • myvue
myvue posted this 18 March 2020

Hello Peter,

Thank you so much for the elaborate reply.

However, I am still having trouble with bonded connections. The first time around, I automatically created connections (edge to edge) and performed modal analysis. It showed me two parts flying (now I am not even sure if they are flying, they are disconnected at one end). Is this what you mean when you say 'flying':

So next time around, I created a bonded connection at that part manually (since I couldnt locate that particular connection in over a thousand connections and increase its pinball radius). I performed the modal analysis again. This time, the two parts that 'fly' in the first scenario are perfectly connected, but now there are disconnections on other parts of the geometry.

Could you please take a look at the above pictures and say that if they are actually 'flying' or if such disconnections are normal?

The actual goal is to perform static structural analysis, but I can't solve this connections problem. I tried to generate fixed joints (but cannot do that automatically for edge-to-edge joints) and then I tried shared topology/node merge (but error when meshing). So I guess, bonded connections is my only option.

peteroznewman posted this 18 March 2020

Yes, you have a "crack" in your model. It is not connected when green and red colors are adjacent to one another.

  • Liked by
  • myvue