## Simulation Mechanical and Multiphysics

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic to the Top
- Bookmark
- Subscribe
- Printer Friendly Page

# Natural Frequency of a Spindle - Representing Bearings with Constraints

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Hello everyone,

I'm trying to do a natural frequency analysis on a vertical milling machine spindle. Getting the right constraints to represent the ball bearings is proving to be very difficult. I want to represent each bearing as a simple support in three-dimensions (the ring of nodes "in contact" with the inner bearing race should be allowed to move along the surface of a sphere. Meaning that the spindle can still pivot in any direction at the bearing, but cannot translate)

The best I've done so far is this:

-Create spherical LCS for each bearing with the origin at the center of the bearing

-tried to constrain all bearing nodes from moving in the "R" direction, but in the constraints dialogue, only TX, TY, TZ, RX, RY, and RZ are available.

-at each bearing node, a cartesian coordinate is setup by the spherical LCS, with X in the R direction, and Y and Z in tangential directions, so I chose to constrain TX.

-when the simulation runs, the bearing nodes are each allowed move in their independent cartesian coordinate unconstrained directions, rather than remaining a specified distance from the center of the spherical LCS's.

This method is somewhat close to what I need for bending modes, but gives incorrect values for torsional modes.

I figure autodesk simulation just doesn't have a true spherical or even cylindrical LCS, but I thought I should ask if anyone has come across this or might be able to help me get the constraints I need.

Thanks!

# Re: Natural Frequency of a Spindle - Representing Bearings with Constraints

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Hi blwisema,

Working with local coordinate systems can be tricky sometimes, at least for me. I always need to stop and really thing about whether the constraints provide static stability or not. But if you are doing a "Natural Frequency (Modal)" analysis, the model does not to be statically stable. A "Natural Frequency (Modal) with Load Stiffening" does require a statically stable model. (Otherwise it is hard to calculate the pre-stress ;-)

Can you explain what's wrong with the torsional results? Maybe that will help indicate what is occurring in the model.

If it would be acceptable to use a surface to simulate the bearing, you can use the "Mesh > CAD Additions > Joint" to create a universal joint, and then pin the center of the joing. Or, you can use the "Setup > Loads > Remote Load & Constraint" to do something similar but use the nodes along the edges (the same nodes that you are using now). In either of these approaches, be sure to set the mass density of the elements to 0 so that you do not affect the results!

Note that you do have at least one rigid body mode: spinning! So the "first" mode shown in the results is meaningless. I don't think there are other rigid body modes, but I may be wrong.

Mechanical Engineer

Pittsburgh, PA

Simulation Mechanical user since Dec 1997

# Re: Natural Frequency of a Spindle - Representing Bearings with Constraints

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Thanks for the response AstroJohnPE,

When I asked those questions I was only considering the modal analysis without load stiffening. However, now I am also looking at adding a centrifugal load so I need constraints that can be somewhat consistant for both analysis environments.

Also, I'm a little bit confused as to what you mean by "statically stable". I need to have degrees of freedom for rotation in all directions at each joint, so won't that mean that I can't make my model statically stable? I guess what I'm trying to ask is whether or not it's possible for me to have the constraints I need and run a modal analysis with load stiffening.

The error in the torsional modes was caused by the bearing constraints. When the spindle strains (torsional), the bearing constraints only allow the surface nodes to move on the flat plane of the constraint... so the spindle is forced to expand and is not able to rotate any of its sections more than 90 deg. A similar effect was seen with the 3D spring bearing constraints.

I think I also failed to mention that part of the analysis I'm doing requires that I be able to vary the radial stiffness of the bearings... is that possible for the two 'constraints' you listed below?

Thanks again for the response!

# Re: Natural Frequency of a Spindle - Representing Bearings with Constraints

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Also, I tried the universal joints with zero mass. When I tried to run the simulation in the natural frequency (modal) with load stiffening analysis, it gave me an error saying that the material properties for the parts created by the joints were invalid.

Did I do this wrong somehow?

Thanks

# Re: Natural Frequency of a Spindle - Representing Bearings with Constraints

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

First, please keep in mind that I am only working from the image you provided, so there may be other things in the model that we cannot see in the image. So, some of my comments may not be relevant.

So, based on the description and image, it sounds to me that your model is free to rotate --- like a shaft !! Let's imagine that you apply a moment to one end of the shaft, and another equal but opposite moment on the other end. Theoretically, these two balance each other, so in engineering class we would say that the model is stable. But realistically, the computer will never get the moments to be perfectly balance, so there will always be a small torque. When applied over an infinite (or undetermined) amount of time, the shaft would rotate an infinite (or undetermined) angle. So this rotation is the motion of the model that causes instability problems for the solver.

Here's another way to think of it. You want to see the torsional mode. Let's imagine one end rotates +5 degrees and the other end or - 5 degrees. But because the shaft is not prevented from rotating, maybe the result is that the entire shaft rotates 100 degrees on average, with the two ends being 5+100=105 and -5+100=95 degrees. No problem, you can still see that. But if the solver decides that the entire shaft rotates 1E10 degrees on average, then the results are that the ends rotate 5+1E10~1E10 and -5+1E10~1E10. You won't be able to see the difference due to round off.

So, you need to pick one zero point for the shaft rotation, and the solver will calculate the torsion mode relative to that one point.

I do not fully understand your description of the problem with the torsion results (and I do not need to understand :-), but if it expands like what I show in the attached figure, then your results are probably correct.

For changing the stiffness of the radial constraints, I suggest that you use the local coordinate systems and the "Setup > Constraints > 1D Springs". The "General Constraints" do not have an option for stiffness, and the joint would be difficult to calculate what stiffness you need to enter to duplicate the published data. What you will need to determine is how to convert the known stiffness for the bearing into the equivalent stiffness for the dozens of nodes that are selected. In other words, if you know the stiffness of the bearing is 1000 (just making up numbers), then the stiffness for each of the 1D springs that get applied to the ring that represents the surface of 1 bearing may be 3.1415 or whatever the formula for springs calculates to.

Happy Computing.

Mechanical Engineer

Pittsburgh, PA

Simulation Mechanical user since Dec 1997

# Re: Natural Frequency of a Spindle - Representing Bearings with Constraints

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

To answer the questions "Who did something wrong?"

- If you give the truss elements a small mass density, and then the model runs, I would say that the software did something wrong.
- If you give the truss elements a small mass density and the model still does not run, then I think you must have missed something.

Mechanical Engineer

Pittsburgh, PA

Simulation Mechanical user since Dec 1997

# Re: Natural Frequency of a Spindle - Representing Bearings with Constraints

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Hmmm I gave the elements a small mass density, but now i get this error in the analysis dialogue: "Error. The truss element is not available for load stiffening."

Do I need to pick a different element type for the joints?

Thanks much

# Re: Natural Frequency of a Spindle - Representing Bearings with Constraints

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

Very interesting. You must have found a way to do the impossible! (add a truss element to a load stiffening model.)

It appears that you need to change the element type to beam. Then check the boundary condition at the center node to make sure it allows the rotations that you want.

Mechanical Engineer

Pittsburgh, PA

Simulation Mechanical user since Dec 1997