Factor of Safety and FEA for Flywheels

I have recently begun a project to optimize a flywheel design based on the ratio of mass to moment of inertia. I started with a few set dimensions and some vague limits for each variable I was going to test.

This is the sketch I revolved to create my flywheel, I chose this shape based on intuition and some not very scientific guesses. The pink dimensions are the variables I was modifying.

This is one (of many) configurations that I made in 3D, just so the shape makes sense.

I used a design table to create multiple configurations that modified each variable independently. I used an outer thickness of .25in-1in in .25in increments and I found that this dimension can be optimized, and the the best value is close to .5in. I used the same increments for the center thickness and found (unsurprisingly) that the thinner, or more importantly lighter, that section was the higher the ratio of mass:MOI. And here enters FEA, an aspect of CAD that I have some basic experience with, but I felt a little in over my head taking on this project. After all this is a 3-5lbs chunk of aluminum spinning at up to 6000rpm, breaking is not an option. So based on all of this my current goal is to reduce the mass of the center disc section as much as possible before the wheel can no longer spin to 6000RPM safely. I have run lots of simulations with different configurations of center thickness and random fillet size/location, Ill include some pictures of these simulations below. Like the title says I am looking for a factor of safety to use after my simulation to ensure that the wheel will not fail, has anybody else done simulations of you flywheel? What factor of safety did you use? Am I doing all of this completely wrong? I’m also open to any suggestions for changing the overall design to improve the mass to MOI ratio. I have considered pocketing the center disc and using “spokes” like the AndyMark performance wheel but that increases the complexity of machining considerably so I would like to avoid that.

This is the standard no fillet version, this is using a .5in outer thickness and a .5in inner disc thickness

This version has a fillet with radius .75in between the outer section and the inner disc, this is using a .5in outer thickness and a .5in inner disc thickness

This is a standard, no fillet, version that uses a .5in outer thickness and a .25in inner disc thickness

I can provide any additional information or simulations if it is necessary, including CAD files.


What a wonderful engineering exercise! Well done!

I highly doubt it.

This is a tricky question in this context. ASSUMING that you’re using aluminum, it will fatigue. That is to say it gets weaker and weaker the more times it is stressed.


This is a a fatigue curve for 6061T6. There are many types of fatigue tests and confidence intervals, so take this as an example, not ‘all aluminum fatigues like this.’ You should guess how many spin-up cycles your flywheel will experience (N in the plot) and calculate a FoS from the fatigue strength. For ‘if this fails we’ll all be really sad’ cases I suggest aiming for a FoS of 10-20.

No, but there are things you can do to make this investigation more complete.

-Material used
-Mesh used
-Mesh sensitivity study (does the answer change as you make the mesh finer? I suggest runs of 1/2 and 1/4 of your study mesh size)
-Plot all of your stress and displacement results on the same scale so the colors and effects are directly comparable. This helps readability immensely.

Keep up the good work!


Thank you for the helpful response, I am planning to use 6061 aluminum, I should have specified in the OP. I will do some work with my mesh to see if it has an effect on the results. I roughly calculated/estimated 560 spin ups in official play and then decided to double that to account for tests and practice. I changed the units of the simulation chart to MPa to fit with the graph you posted, but the numbers I’m getting still vary a lot from the graph you sent and a quick google search about the yield strength of 6061 T6. The google search showed a yield strength of 241MPa and the graph shows a strength of about 250 halfway between 1,000 and 10,000 spin ups. The numbers I’m seeing in Solidworks are like 5.515 e+01 (solidworks says this is the yield strength), I assume this is scientific notation and that I should move the decimal one place to the right to get a normal number, but this is still far below the other values you posted. Do I need to modify my simulation settings to get the correct numbers?

For the purposes of simulation you do not need to know YS, you can interpret that later.

The default SW value is 55ksi, or about 380MPa. This all seems high, and why using default SW values is extremely risky. The ‘real world’ number to get is the material cert from the material supplier. Take a look at 6in diameter stock from McMaster, which includes 6061, 2024, and 7075. Compare the FoS for each one. The real numbers would be provided for certified materials after purchase:



So how can I get accurate stress values from my simulation?

My chart currently looks like this

but this says that the max stress the wheel will experience is not even 7MPa, how can this be right? Am I misunderstanding the chart?

So, those stress values are calculated using the elastic modulus and Poisson’s ratio (and density for this analysis) and are generally valid. The actual yield stress of the material can vary widely for different aluminums and different tempers. That is to say the stress will be about the same in 6061 and 7075 (elastic modulus, p ratio, density are about the same), but 7075 is far stronger and thus will have a larger FoS. You can run the analysis for ‘aluminum’ and then present a table such as:

-cost x
-fos y

-cost a
-fos b


1 Like

So if those numbers are valid then I have a FoS of about 40 with a center disc thickness of .25. I guess I overestimated how thick that center section would need to be to be within a good FoS because I was pretty sure It would need to be thicker than .25. Thank you for all your responses, they were super helpful.

1 Like

@CarlosGJ I would be interested to see the calcs you did for your flywheels.

I would also keep in mind that the simulation assumes the rotation axis is constant. While you may go thinner and thinner, it’ll hold up to the loads imparted by spinning a perfect version of the flywheel, but any imbalance or other external disturbances, like say a robot hitting you, may prove to be too much. That being said, 0.25, or maybe slightly less will probably prove safe to that.

Another suggestion for improvement would be a small fillet on the inner edge here, since it looks like there’s a stress concentration there in your earlier post, and it’ll get you a very slightly better MOI/Mass ratio.

If you are actually approaching 1/4 of yield stress in your flywheel then you should taper the rim so its thinner at the edge than the center. The rim is effectively a cantilever beam. Optimum beam shape depends on what you parameter you are controlling. But, a simple angle will get even out the stresses quite a bit. You also want a large radius between the disc and the inner/outer tubes. A radius similar to your disc thickness would be a good starting place.

If you are high enough stress that you need to worry about fatigue, you shouldn’t be using it!!! Also, frankly, if you are getting over 1/4 to 1/3 of yield you should really be asking “should I have a potential bomb on the field?” I was about 3 feet from a high speed fan rotor that was over sped and ruptured many years ago. I was on the centerline and 5 feet off the ground, so I just rode it out; I couldn’t get to a safer place. Very scary experience with the vrrrrrRRRR BAM.

When I used to work on industrial UPS’, I saw one that used a flywheel as the energy storage system. The flywheel and motor were about the size of a washing machine and were buried under the concrete floor in case something failed. Your flywheel will not be that massive but you won’t have the containment cage either.

You might find it convenient to try out the symmetry simplifications in SolidWorks. (I’m sure the full model runs pretty quickly anyway, but this might be of interest.)

(This might not be adequate for modelling body forces like gravity, and tangential loads.)


I tried this and re-ran the simulation and my ratio calculations. The simulation showed the same amount of stress in those corners, it was (maybe) spread over a larger area, but hard to compare. It also reduced the ratio of Mass:MOI, not by any significant amount, but it was worse than without the fillets.

I am not getting anywhere close to 1/4 yield stress, but I added this taper as an experiment. I made the inner line 10 degrees further down. It reduced the Mass:MOI ratio, not by a lot but enough to make me hesitant to leave it. I re ran the simulation with the taper and it did a great job of reducing the stress on the inner corner of the outer diameter, but it also increased the stress on the center disc, especially around the hex hub.

This is a picture of the simulation results with the taper.

Yes I found this to be true in my original simulations, the OP has a simulation picture with a large fillet in that area and it shows reduced stress on the rest of the outer diameter. I currently have a fillet there that has a radius of .25. I probably wont make this fillet any larger because that larger it is the worse the Mass:MOI ratio becomes.

What would “high enough” stress be? The current max stress is around 6-7MPa. I also calculated that the number of times this wheel is expected to spin up is so low that the material will lose very little strength, I wrote about that in my first response.

The whole reason I am doing these simulations are to make sure I do not have a potential bomb on the field. I am not anywhere near 1/4 of the yield stress, the current design has a factor of safety around 40.

Nothing against the work that you’re doing. I love me a good mechanical simulation.

But keep in mind that FEA results are only as good as the information you put in and the questions you ask it. So if you’re simulations show that your design works well spinning at a constant X rpm, that’s great. But it might not handle the acceleration needed to get it there, or might not be able to take a hit from a defending robot, or it might become unstable if your tolerances aren’t perfect, or a bunch of other things. The danger of FEA isn’t usually that the results you get are wrong, it’s that you don’t ask it the right question and get lulled into a false sense of security.


Safety factor of 40 is definitely in warm fuzzy territory! Glad to hear it! I think you will find that getting anywhere near yield would result in parts so thin that they would be easy to dent.

1 Like

Wait, where’s your stainless steel wire wrap? :wink: (Search this site and you’ll find out what I am referring to, in jest.)

Seriously, you can check your FEA approach by simulating some test cases that have answers in textbooks or you can calculate by hand. These are: A thin ring, a thin disk with and without a hole in the middle, and a long solid shaft or tube. Set them up to use the same material properties and OD as your current model. You should be able to hand-calculate the hoop (circumferential, or theta-theta) stresses by hand using analogy to a thin-wall pressure vessel, where that stress is P*r/t, that it, pressure times average radius divided by wall thickness. The pressure will be that which gives the same force on an element of material as the acceleration from spinning.


This topic was automatically closed 365 days after the last reply. New replies are no longer allowed.