FEM Dropout analysis - max force ?

Get all your technical information about electric bikes here.
Post Reply
qwerkus   10 kW

10 kW
Posts: 590
Joined: Jul 22 2017 4:00am

FEM Dropout analysis - max force ?

Post by qwerkus » Sep 25 2020 5:07pm

Hello,

I'm trying to setup a simple FEM static analysis of a bike dropout to figure out metal breaking point. Model is done and software seems to work. Though I could use some help with the physics. For an instance, what's the max. force a 12mm hub motor axle edge would put on a dropout face if the motor has a torque rating of 100 n.m-2 ?
force.png
force.png (13.45 KiB) Viewed 392 times
I get that 100n.m-2 means a force of 100N perpendicular to the axle, applied at a distance of 1m. Now if I take this same force 5mm from the axle center, I get 1000/5*100 = 20 000N which seems just silly. What am I doing wrong ?

Thanks for your time,

qwerkus

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 25 2020 10:07pm

Just so we're all speaking the same language, the unit of torque is Nm (Newton metres). Not n.m-2.

So 100Nm @ 5mm is 100*1000/5=20 000N. You are correct. Since it is reacting in 2 places, each load will be 10kN.

The problem you will have is that the force is acting on a line. Since a line has no area, and stress=force/area, in a static linear analysis you end up with a thing called a singularity (effectively a point of infinite stress). So the result at the point of contact is not realistic. Sharp internal corners have the same effect. This is one limitation of static linear analyses.

In reality, materials and contacts are non-linear, and localised yielding allows for stress relief, and things don't turn into black holes...

There's a thing called St Vennant's principal, which basically says that if you ignore that localised area of unrealistic stress, the rest of the results away from that area are probably fine. Experience counts when setting up and interpreting FEA.

User avatar
E-HP   1 MW

1 MW
Posts: 1651
Joined: Nov 01 2018 9:20pm

Re: FEM Dropout analysis - max force ?

Post by E-HP » Sep 25 2020 10:14pm

Maybe I'm not reading the inputs correctly, but if it's a 12mm axle, why are you using 5mm in your calculation instead of 6mm?

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 25 2020 10:45pm

Since the area of concern is AF10mm, the distance is slightly above 5mm. But in reality, even the geometry is not so simple, because the thread is truncated which creates a serated contact line. For intents and purposes, simplifying and approximating gives ROM results.

User avatar
E-HP   1 MW

1 MW
Posts: 1651
Joined: Nov 01 2018 9:20pm

Re: FEM Dropout analysis - max force ?

Post by E-HP » Sep 26 2020 12:16am

serious_sam wrote:
Sep 25 2020 10:45pm
Since the area of concern is AF10mm, the distance is slightly above 5mm. But in reality, even the geometry is not so simple, because the thread is truncated which creates a serated contact line. For intents and purposes, simplifying and approximating gives ROM results.
I get 5.45, but doesn't make much of a difference in the calc.

qwerkus   10 kW

10 kW
Posts: 590
Joined: Jul 22 2017 4:00am

Re: FEM Dropout analysis - max force ?

Post by qwerkus » Sep 26 2020 2:54am

serious_sam wrote:
Sep 25 2020 10:07pm
Just so we're all speaking the same language, the unit of torque is Nm (Newton metres). Not n.m-2.

So 100Nm @ 5mm is 100*1000/5=20 000N. You are correct. Since it is reacting in 2 places, each load will be 10kN.

The problem you will have is that the force is acting on a line. Since a line has no area, and stress=force/area, in a static linear analysis you end up with a thing called a singularity (effectively a point of infinite stress). So the result at the point of contact is not realistic. Sharp internal corners have the same effect. This is one limitation of static linear analyses.

In reality, materials and contacts are non-linear, and localised yielding allows for stress relief, and things don't turn into black holes...

There's a thing called St Vennant's principal, which basically says that if you ignore that localised area of unrealistic stress, the rest of the results away from that area are probably fine. Experience counts when setting up and interpreting FEA.
Thanks a lot for your explanations. This proves to be less simple than expected but also a lot more fun! I ran a sim for backwards rotation (regen) on the dropouts with 8mm 304 type stainless steel, using 10kn top force (axle to dropout) on a 16mm2 surface and 5Kn bottom force (anti-turn washer) on a 32mm2 surface. Not sure how realistic this is, but it doesn't look great for now, as I get over 1035Mpa von mises stress and 0.2mm total displacement. That's 5 times more than the yield limit for that steel...
fem1.jpg
fem1.jpg (173.19 KiB) Viewed 361 times
fem2.jpg
fem2.jpg (436.4 KiB) Viewed 361 times
Still some optimizations to do...

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 26 2020 4:10am

The displacement is probably realistic. The peak stress is like I described, an area of local yielding, which can't be simulated in a linear analysis. And a sharp internal edge causes the software to miscalculate. I'm fairly certain that if you halved the mesh size, you would approx double that peak stress seen. Each refinement of the mesh in that area would produce a further increase in stress, to infinity.

To fix the stress, you can add a small fillet in that area. To fix the deflection, you might want to consider a clamping bolt.

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 26 2020 4:23am

Just another hint. Not sure what software you're using, so I'm not sure what level of control you have, but having such a fine mesh over the entire part is costing significant computational time. If you can, try running a much coarser mesh, and only refine it around the areas of interest.

If you zip your CAD geometry (step or parasolid) then rename the file extension to pdf, you can upload it here as an attachment, and I can take a quick look in Ansys if you want. Give you a point of reference to compare to anyway.

qwerkus   10 kW

10 kW
Posts: 590
Joined: Jul 22 2017 4:00am

Re: FEM Dropout analysis - max force ?

Post by qwerkus » Sep 26 2020 5:10am

serious_sam wrote:
Sep 26 2020 4:23am
Just another hint. Not sure what software you're using, so I'm not sure what level of control you have, but having such a fine mesh over the entire part is costing significant computational time. If you can, try running a much coarser mesh, and only refine it around the areas of interest.

If you zip your CAD geometry (step or parasolid) then rename the file extension to pdf, you can upload it here as an attachment, and I can take a quick look in Ansys if you want. Give you a point of reference to compare to anyway.
Thanks for the useful hints. I'm doing everything on freecad. Followed your advice and added a 0.5mm filled. Also used mesh region to speed things up. Results as you predicted: the filled produces a finer meshing which results in increase von Mises stress. See picture.
fem3.jpg
fem3.jpg (210.21 KiB) Viewed 342 times
File too big for this forum. Send me a pm to this address and I send you the step file: qwerkus at gmail com.

Yes, a clamping bolt would be the optimal solution, but I try to keep this as simple as possible. The whole point of this modular dropout would be to figure out a design/material strong enough to take 1000W hubs without annoying torque arms.

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 26 2020 7:42pm

Email sent.

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 28 2020 8:06am

Here's some preliminary results.
Setup info:
- I added the axle geometry, and applied 50Nm torque over 20 substeps. Since there are 2 dropouts, then the total load would be 100Nm combined.
- The dropout is restrained at the 3x mounting holes.
- Applied µ=0.2 friction to the contact between axle and dropout. In reality this would be slightly higher, but 0.2 is a conservative estimate.
- Mesh size is 4mm, refined to 0.5mm in the contact areas.
- The dropout material is 304SS bi-linear (YS=240MPa, UTS=580MPa, e=55%). This is a simplified way of modelling the material in a non-linear manner, which approximates the plastic deformation process in a conservative and simple manner.
- The axle material is linear steel. Since we are analysing the dropout, we simplify the analysis in a conservative manner by using a linear material for the axle. It provides the stiffness of steel, but ignores any yielding, since we don;t actually know the strength of the axle anyway.
- The analysis is run as non-linear, with the 50Nm load applied over 20 substeps.
Comments:
- The dropout material begins to yield (>240MPa = red in the image below) at around substep 14, which equates to 35Nm each dropout, or 70Nm for a pair.
- This setup has no axle nut applying friction. An axle nut would slightly increase the load capacity.
- This model doesn't have the axle threads modelled. Threads increase the stress at the loaded contact areas.
- I would seriously recommend adding a clamp. Without the clamp, there is small movement. If you run regen, then you will definitely have problems with axle nuts coming loose, and eventually wear, which may lead to failure.
If I have some time over the next couple of days, I will rerun the same analysis with a small clamping screw just to compare.
01stress.jpg
01stress.jpg (339.04 KiB) Viewed 285 times
01displacement.jpg
01displacement.jpg (342.69 KiB) Viewed 285 times

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 29 2020 5:24am

Here's the same analysis, with the following modifications:
- I added a small clamping bolt, screwed into the body of the dropout (M5, A2-70 stainless, 5.1Nm torque, 3.93kN preload)
- Analysis broken into 2 steps: 1st step=bolt preload; 2nd step=torque application.
- Increased torque to 100Nm (again over 20 substeps)
Results:
- The dropout material begins to yield (>240MPa = red in the image below) at around substep 12, which equates to 60Nm each dropout, or 120Nm for a pair.
- So just adding a small clamping bolt increases torque handling from 35Nm to 60Nm - nearly double. AND, there is minimal relative movement, so regen will not cause the same issues. Overall a much safer and stronger arrangement.
Dropout 02 stress.jpg
Dropout 02 stress.jpg (454.74 KiB) Viewed 252 times
Dropout 02 displacement.jpg
Dropout 02 displacement.jpg (418.83 KiB) Viewed 252 times

John in CR   100 GW

100 GW
Posts: 14659
Joined: May 20 2008 12:58am
Location: Paradise

Re: FEM Dropout analysis - max force ?

Post by John in CR » Sep 29 2020 6:46am

Newton meters in the dropout is crazy newtons of force at the small radius, so yes it's thousands of newtons of force in those dropouts.

User avatar
DogDipstick   10 kW

10 kW
Posts: 718
Joined: Aug 19 2018 12:39pm
Location: Fleetwood Pa

Re: FEM Dropout analysis - max force ?

Post by DogDipstick » Sep 29 2020 7:12am

wHY STAINLESS?
83.1v of Ironhorse XC.. :) :bolt: by Chevy :bolt: :D Broke 10 horsies :twisted: (..about 80% healed..).. :? Waddyamean? You cant tell me how many amperes/Ft.^2 of the plate ?!?!? WTF. :x :| (gottenymoem4115thangs?Yall?) :confused: Fabricator @ BSECo. Inc.

qwerkus   10 kW

10 kW
Posts: 590
Joined: Jul 22 2017 4:00am

Re: FEM Dropout analysis - max force ?

Post by qwerkus » Sep 29 2020 7:25am

serious_sam wrote:
Sep 29 2020 5:24am
Results:
- The dropout material begins to yield (>240MPa = red in the image below) at around substep 12, which equates to 60Nm each dropout, or 120Nm for a pair.
- So just adding a small clamping bolt increases torque handling from 35Nm to 60Nm - nearly double. AND, there is minimal relative movement, so regen will not cause the same issues. Overall a much safer and stronger arrangement.
Dropout 02 stress.jpg
Dropout 02 displacement.jpg
Wow - awesome feedback. Thanks a lot. This confirms diy tests from this forum: clamping bolt beats material strength in dropout design. Problem is manufacturing: drilling an M5 hole sideways in 8mm stainless is a pain. Only 1.5mm left on each side - a slight deviation from the drill, and you're through. Maybe M4 would be enough ?
Stainless is not a must, but it means no need for paint, which makes it cheaper for small series. CroMoly could also work.
I wouldn't worry too much about threads causing cracks: the hubs I have in mind are not threaded at the dropout holding zone.

Another option left open by the modularity of the dropout is a closed axle hole. That would mean that you'd have to remove the entire dropout when repairing a flat and the absence of clamping force will always allows for some wiggle in regen mode. But it could be manageable if we reduce the amount of bolts holding the dropout to 2 per side. What does your sim software says about this ?

Finally: send me a paypal address or equivalent - there is no way this kind of help remains unpaid.
Last edited by qwerkus on Sep 29 2020 2:08pm, edited 1 time in total.

John in CR   100 GW

100 GW
Posts: 14659
Joined: May 20 2008 12:58am
Location: Paradise

Re: FEM Dropout analysis - max force ?

Post by John in CR » Sep 29 2020 12:23pm

serious_sam wrote:
Sep 29 2020 5:24am
- So just adding a small clamping bolt increases torque handling from 35Nm to 60Nm - nearly double.
"Nearly double" is not anywhere close to the real world benefit. There is never precision machining of the dropouts to the axle size, and a press fit would be impractical anyway, so there is always play. The forces are then more focused at 2 edges of the flats instead of across the entire face of the axle flat, and with regen the only thing to prevent rocking within the play are the axle nuts, which quickly loosen due to the alternating force.

Through hole torque arms suffer from the same looseness issue.

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 29 2020 6:10pm

John in CR wrote:
Sep 29 2020 12:23pm
serious_sam wrote:
Sep 29 2020 5:24am
- So just adding a small clamping bolt increases torque handling from 35Nm to 60Nm - nearly double.
"Nearly double" is not anywhere close to the real world benefit.
Agreed on the additional benefits of the clamp. The nearly double increase is purely double of the torque to reach the yield limit of the dropout.

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Sep 29 2020 6:15pm

qwerkus wrote:
Sep 29 2020 7:25am
Wow - awesome feedback. Thanks a lot...send me a paypal address or equivalent - there is no way this kind of help remains unpaid.
No worries. It's right in my wheelhouse, so it's quick and easy to do. You don't need to pay for free advice.
qwerkus wrote:
Sep 29 2020 7:25am
Maybe M4 would be enough ?
You could go M4. A2-70 stainless is too weak though. Class 8.8 is right on the limit. It would be ok if you go to class 12.9 socket head and torque to 4Nm. Need to have minimum 8mm engagement in the dropout.

User avatar
serious_sam   1 kW

1 kW
Posts: 434
Joined: Mar 05 2017 8:07am
Location: Australia

Re: FEM Dropout analysis - max force ?

Post by serious_sam » Oct 01 2020 10:00am

Something related:
viewtopic.php?f=2&t=68843
Torque-arm-clamping-iso.jpg
Torque-arm-clamping-iso.jpg (19.16 KiB) Viewed 141 times

Post Reply