×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Are you an
Engineering professional?
Join Eng-Tips Forums!
• Talk With Other Members
• Be Notified Of Responses
• Keyword Search
Favorite Forums
• Automated Signatures
• Best Of All, It's Free!

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

#### Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

# How to constrain an FEA model for modal analysis2

## How to constrain an FEA model for modal analysis

(OP)
Hey,

Any FEA guys out there?  I have modeled a gear in PATRAN in order to determine the natural frequencies and mode shapes.  My question is: How should I constrain the model?  I noticed that the results are very sensitive to how the model is constrained.  I simply constrained one node (completely) to fix the model in space, but is this right?

Anyone?

Anyone know of a good reference book(s) on doing modal/vibration analysis using FEA?

### RE: How to constrain an FEA model for modal analysis

If you are just performing an eigenvalue analysis to get frequencies and modeshapes then why not have no constraints at all? After all it won't move anywhere as you do not apply any forces in an eigenvalue analysis. In experimental modal analysis, small items are often suspended with "free" boundary conditions. In practice of course, there will always be some constraints but suspending the item with soft elastic is close enough. It is a lot easier to achieve nearly free boundary conditions than nearly pinned or nearly clamped conditions.

Is your gear circularly symmetric? The first two modes of a ring-like structure which is circularly symmetric occur at exactly the same frequency and modeshape, but one of the mode shapes is rotated 45 degrees around the circle with respect to the other. In the perfect case the "angle" of the modeshapes will be arbitrary (although the 45 degree separation remains). Introducing a slight asymmetry (your constraint at 1 node) will tend to force the node of one of these first two modes to occur at the constraining point and the other mode may not be exactly 45 degrees different.

However I would expect the frequencies and modeshapes to not change too much. You say your results are sensitive to a single constraint. But how sensitve? How much do the frequencies change? do the modeshapes look very different?

Michael

### RE: How to constrain an FEA model for modal analysis

I have just finished a project about the modal analysis of a simple beam structure recently. I've used I-DEAS but anyway, all FEA tools do the same and follow the same procedure for the calculations.

For your case, there is no need to apply any constraints to your model.Normally; After model preparation, boundary conditions are defined (constraints etc.), forces are applied and you pass to the solution.But in modal analysis you do not need to do all these.

After modelling you should select 'free body dynamics' option.(it should be in the boundary conditions part) Once you select it, the program will automatically disable the force buttons.Now you are ready to analyse your model.In the solution set do not forget to change the number of natural modes that you want to visualize.The first 4-5 modes will probably be static rigid body modes, with very small frequencies on the order of 10^3 or so.

As reference material:
For the basics: www.sem.org (experimental mechanics society)
Text Book:D. J. Ewins,Modal Testing

For Patran: go over the examples, workshops provided in the manuals, they would really help.

Öncü

### RE: How to constrain an FEA model for modal analysis

Hi goodvibes,
like all other have stated, actually you need no boundary counstrains for doing modal (eigenvalue) analysis.
Of course, may be you would get very little eigenvalue (near to zero) for the 1-3 first eigenvalues, these are referred to free body modes. If you want to avoid this, then simply constrained it, as you said, or take over the constrains defined for static analysis.

cheers

### RE: How to constrain an FEA model for modal analysis

I disagree. In many circumstances the constraints form a vital part of the stiffness of the system, testing the component free-free may lead you up the garden path (ie you'll optimise the mode shape correlation for a non-representative case). A non-lazy analyst would of course model the mounting structure correctly, but an adept use of constraints can results in a  good compromise between time and accuracy. eg the mounting cradle for an alternator is stiffened by being bolted to the engine block, and teh alternator itself. Its free free flexural modes bear no resemblance to the modes of interest.

Also you will always get 6 rigid body modes if the item is truly free-free, not 1-3!

Cheers

Greg Locock

### RE: How to constrain an FEA model for modal analysis

(OP)
Thanks to all for responding.  It is always good to see others opinions on a complex subject.  I spoke with the folks at MSC and they said the same thing regarding a modal analysis- no constraints.  The first six modes will be rigid body modes.  Next i will put in constraints and damping to simulate the bearings and run a frequency response analysis to see if any of the natural frequencies are being excited.

Thanks,

Goodvibes

#### Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

#### Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

#### Resources

White Paper - A Guide to 3D Printing Materials
When it comes to using an FDM 3D printer effectively and efficiently, choosing the right material at the right time is essential. This 3D Printing Materials Guide will help give you and your team a basic understanding of some FDM 3D printing polymers and composites, their strengths and weaknesses, and when to use them. Download Now

Close Box

# Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

• Talk To Other Members
• Notification Of Responses To Questions
• Favorite Forums One Click Access
• Keyword Search Of All Posts, And More...

Register now while it's still free!