FEA of Wobble in bent crank shaft of lawn mower

[CaptainCrunch]

Hello All,

Any body have any ideas on how to analyse wobble of a mower with a bent blade and bent crankshaft USING FINITE ELEMENT ANALYSIS? I know how to do the test, and here is an example of were testing would be much easier than FEA. But say you had to do this in FEA, any ideas on the general approach?

I've done high speed nonlinear impact of a blade striking objects and I have the deformed shape but ultimately translating that into handle bar shake does not seem likely.
I am trying to capture the effects the crank imbalence and eccentricity has on the general shaking of the structure.

One idea I thought of:
1. Modal analysis or Frequency respons of the deformed shape, with a boundry condition on angular velocity. I don't think a linear implicit model would give you anything useful.

Any other ideas for setting up a finite element analysis of this?

George V.

 

[GregLocock]

If you are happy that you can describe the force input correctly (ie that imbalance is the main exciation) then a forced response of a modal FE model may get you into the same ballpark as a back of envelope calculation, or even reality.

Cheers

Greg Locock

 

[CaptainCrunch]

Greg,

I think I see where your going, a static modal with force input which represents the eccentirc loading (could be determined by a mix of fea and hand calcs.). But what I am trying to do is model this as a dynamic event (i.e. a time history) not as a modal (i.e. steady state dynamic). I may end up run this as a modal but I don't think it will yield the physics I am looking for. Specifically, I like to see the blade and crank rotating eccentrically. I think that would have to be run as a true dynamic.

I will probably have to run this in LS-Dyna as a true transient problem, and letting run for a while, say 2-3 revolutions, which probably take 4-10 days on my best workstation. I don't see any other way. But all that would yield me is transient load input into the crank bearing journal. Then step 2 would be to translate this into some kind handlebar vibration.

Again, testing would be much easier.

Thanks for the input Greg.

George V.
Any

 

[GregLocock]

For your forced repsonse use excitation
Fx=m*r*w^2*(cos(w*t))
Fy=m*r*w^2*(sin(w*t))

From the forced response resultsjust pick the frequency you wish to look at, which should have a real and imaginary component for the displacement at each point. This is the displacement relative to your time phasor and your modal package should be able to turn it into an animation.

I agree that LS Dyna, ADAMS or working model would get there quicker! Cheers

Greg Locock

 

[brad]

What other packages do you have at your disposal? I would think you could run this as a dynamic implicit analysis with the right code. If one can properly model the mechanism of the shaft rotation (without having to resort to contact), this seems like it could readily be handled with implicit dynamics. You would then not be constrained to a stable time increment, which would likely give you a much more economical solution (from a CPU standpoint).

Brad

 

[CaptainCrunch]

Brad,

I think a modal based implicit dynamic analysis may be the ticket with this problem. I have ABAQUS/Standard available to me. I have done numerous mode based steady state dynamic problems so I am familiar with the pros and cons.

In theory I could output the nodal displacements from LS-Dyna into a neutral pre-processor (i.e. Hypermesh), then output the deck in ABAQUS format.

Q: Do you think including or excuding the permanenet stress/ strains ( an effect of the high-speed impact) from the structure would alter the implicit modal dynamic solution?

Plan B would be to run this in LS-Dyna for a very long time (say 3 revolutions) on my computer, which would probably be 5-10 days for solution.

Thanks Brad and Greg for the input,

George

P.S. Testing this would be much easier than running analysis.

 

[brad]

You could within ABAQUS do an implicit dynamic analysis, treating the blade and crankshaft assembly as a superelement. Omit contact, instead modeling connections between the shaft and the rest of the structure with connectors.
I would not expect the residual stresses in the blade/shaft assembly to have any significant effect on the rest of the structure. Hence the neutral pre-processor conversion of the DYNA output to ABAQUS seems like a very reasonable approach.

Similarly, the structure could be built with flexible CMS representations with in ADAMS or another mechanism code, so long as structural nonlinearity of the FEA parts is insignificant.

Good luck.
Brad

 

[TSK1972]

I am trying to do a dynamic load calculation on a system. I have 4 cylinder/pistons connected to motor and gear box. There are 8 bearings used on the middle shaft and a crank is used to move 2 pistons on one side and then to the other. We ran the setup at 1500 psi system pressure and the bearings failed on one side. How do I analyze what's going on?