MECHANICA: Why does displacement graph look so bad?

[Flask]

Hi all,

I've run a modal analysis and then a dynamic freq analysis.

I created a displacement measure.

When I view the results, the displacement at zero Hz (0.21 Hz to be exact) is very high (~.25"). That does not seem at all right.

I've attached a screenshot of my graph.

Does anyone know why I'm getting these erroneous results?

thanks!

http://files.engineering.com/getfil...-483e-a75a-f5921dbdfe30&file=Displacement.jpg

 

[jvian]

What are the results of your modal analysis? Do the boundary conditions seem appropriate? Are your mode shapes as expected? I would be concerned if it was me but in my experience I have never seen activity at that low of a frequency when compared to your rather large bandwidth. My guess is probably an ill constrained model. I have seen low frequency or rigid body modes contribute to such data irregularities but it was always pretty obvious that it was not what we were after. If you don't like it then it's probably not right and make sure you are verifying your inputs as to limit any GIGO.

Good luck,

-J-

 

[Flask]

Thanks Jvian.

My modes look normal. The first one is around 1000Hz.

The part has a mounting flange with bolt holes. I've constrained the bolt holes in all translational and rotational DOF.

There is no load on the part. I entered a freq vs acceleration freq input for the DynFreq analysis.

I just ran a completely different part and got a similar result, so I think I can narrow the common denominator down to being me.

I've got something wrong in my setup or perhaps freq input.

Any ideas on what would cause such an unrealistic displacement at a near zero freq ?

thanks

 

[jvian]

What version of Creo/ProE are you using (there have been several issues and fixes over various releases)? And could you describe the type of problem and parameters? Hard to tell what may be wrong without a little more information. It could be how you've set up the modal and dynamic frequency analyses as they are co-dependent. Here are some questions worth asking:

Are you requesting modes up to a frequency or a total number of modes? Also make sure to calculate Mass Participation Factors (assuming you are using base excitation since your model doesn't contain any loads) to help establish the "activity" of a given mode. Are you including all modes or just some (not recommended) and are you manually choosing the output interval or automatically? And what starting frequency and maximum frequency?

How long is your solution time and what form of convergence are you using? Are you using any mesh controls to avoid singularities? (I don't think this is the problem but always worth double checking)

Is your input log, semi-log, or linear? Make sure to double check your units, especially within your material definition.

Sorry for the onslaught of questions but I deal mostly with dynamic random and time analyses; however, I am sure some of the "quirkiness" of the inputs may be the same. My gut feel is that you are requesting your output accelerations/velocities/displacements with respect to ground instead of the supports. Stresses are not affected but the displacements will be. Just be sure whichever you select is what your after.

Good luck,

-J-

 

[GenericUser]

Displacement at zero frequency usually means rigid body motion. I thought it could be deformation caused by static load, but if I recall correctly dynamic analyses in Mechanica solve for acceleration and then integrate to get velocity and displacement.

I would check the rigid modes box in the Modal analysis and see if any are reported. Also - this dynamic frequency analysis, graph the load/base excitation in the frequency domain and see if you have non-zero load at zero frequency. If you are just using the default 'uniform' function then its probably applying the load/base excitation across the entire frequency spectrum, which may include zero frequency.

 

[bobslo]

GenericUser you are right!
Flask is using base excitation function with frequency function starting with 0Hz.
Flask you should put some load (gravity) on part, and then define frequency load starting with nonzero value.