Contact Region in Dynamic Analysis

[Yoan]

Hi,

I'm attempting to do a vibration analysis using Pro-Mechanica WF4. Essentially, I'm trying to predict the vibration response of a unit, attached to a mounting plate with 4 bolts in the corners, with this assembly attached to a shaker table with 6 bolts.

I'm looking at the unit and its mounting plate specifically. The issue I'm having is that when I assemble the unit to its mounting plate, Mechanica takes the base of the unit and the mounting plate to be bonded; basically fully welded together. Intuitively, this is not correct.

When the unit is pushing down against its mounting plate, then I suppose the bonded interface would provide a close enough approximation. However, the unit should be free to pull away from its mounting plate save for the 4 bolts. The unit should be able to rattle relative to the mounting plate.

Normally, if I were doing a static analysis I would just define a contact region between the unit and the mounting plate. However, when I go to run my modal analysis Mechanica tells me that contact regions are only for static analysis.

Likewise, if I look at the mounting plate interface to the shaker table, and I take the shaker table to be infinitely stiff and heavy, then the mounting plate can only deform "up". When it tries to deform down into the shaker table, then my theoretical shaker table should prevent this. Essentially, aside from the 6 fully constrainted mounting points, the mounting plate should be free in +Z, but constrained in -Z

Any thoughts?

 

[Twoballcane]

Hi Yoan, There should be a "bolt fastner" feature where you can bolt two parts together. The two parts will only be attached to each other at the places where you bolt. Also, ProM will know the two facing surfaces that should not be attached between the two parts. With this said, it does not matter if the box will interfear with the mounting plate when excited. Your intrest should be what resonants and mode shapes you are getting and what you can live with.

Tobalcane
"If you avoid failure, you also avoid success."

 

[PetieSmo]

Yoan,

Did some reading in Mechanica's help files - contact interfaces are not supported during dynamic analyses. ProMechanica treats all coincident surfaces as bonded. Twoballcane's suggestion of using bolt fastener elements should get you halfway there.

In the design of vibration fixtures, if your bolt pattern forms a ring, this leaves a flat plate in the center which is susceptible to "oil canning". This mode will cause ringing in your response accels when the plate contacts the mounting plate. It is common to mill out a shallow pocket in the center of your vibe fixture to prevent this. Incidentally, if you model this pocket into your vibe fixture, ProMechanica will also see this as a gap between your part and the mounting table, allowing you to see how much deflection is occurring in your fixture under the given loads (sine or PSD).

Good luck
PetieSmo

 

[Yoan]

Thanks for the replies.

I tried just doing the bolted connections, and it gave me the same results as the mated (bonded) parts. Reading thru the Help, they do mention that one may need to create a free interface between mated parts so that Mechanica doesn’t bond them together. Putting a free interface dramatically drops my natural frequencies, and unit is obviously moving around a lot more than when its bonded to the plate.

The only other thing I had tried doing was putting a small gap between the unit and its base plate, effectively separating them. To simulate the bolted connections I had simply modeled studs into the base plate that were size-on-size with the mounting holes in the unit. This gave me very similar results to the “bolted and free interface” approach I tried today.

Its starting to look like I won’t be able to fully capture what is happening here. Without being able to define a contact interface, it is my understanding that Mechanica either takes the parts as being bonded or free to interfere.

 

[seymours2571]

This limitation in not limited to Pro/Mechanica. Forced vibration simulations, which are based on modal analysis results, are inherently linear mathematical problems. The reason Mechanica (and other FEA codes) treat contacts as bonded is because it has to in order to solve the math. There are some fancy tools available in some advanced FEA codes that allow for non-linearities in a modal anlysis, but these are highly specialized.

To truly see the reponse of a structure making intermittent contact based on a forcing function I think you would have to use an explicit FEA solver like LS-Dyna or something. Other than their name...I don't have a full grasp on the mechanical simulation vodoo the explicit solvers perform.

Steve