Fatigue results on Ansys Mechanical 4

[TeoAlfa]

Hello to all.
I am evaluating a project in terms of fatigue.
This is a large steel structure which is designed to take 40 tons of load.
I have done an analysis of 50ton just to be evaluate what will be the results in case the user loads the structure more than the specified maximum load.
Maximum stress occurs on a pin, which is close to 1000Mpa. Pin material is C45E steel with min yield stress of 370Mpa and maximum tensile strength of 780Mpa.
This pin obviously will fail on the first application of the load.

I then started to run a fatigue analysis of the whole structure.
Fatigue analysis input data:
Fatigue Strength Factor (Kf) = 0.8
Loading: Zero based
Analysis Type: Strain Life (the structure is designed to be low cycle loading)
Main Stress Theory: Smith-Watson-Topper (chosen because it's the most conservative option)
Stress Component: Equivalent von-Mises

The result i got was around 6.000 cycles on the pin where maximum stress occured.

My question is: How reliable this result could be? In first sight it seems impossible that a pin can withstand 6.000 cycles at a stress level close to 3 times the material yield stress!
Thanks in advance for every reply!

 

[D_UK]

I would have thought there's not much point using large displacement analysis and non-linear materials if you are incorrectly applying bonded contact at the pin/bush interface. You should be able to prevent pin rotation in your model in a realistic way (using symmetry, applying friction or adding a rotational constraint to represent the keep plate). The stress distribution will be very different.

David

 

[TeoAlfa]

Hi David,
I have tried to raise the friction coefficient when applied frictional contacts but still no convergence.
How to add a rotational constraint? An how this could be realistic either?
Thanks!

 

[D_UK]

If it's rotation of the pin that's the problem try adding a rotational constraint to one end (use a remote constraint acting over the end face but applied to a point in the centre of the face in rotation about x-axis). It's realistic as presumably the pin is (or could be considered to be) constrained against rotation to one part of the clevis. If you bond the pin to the bush you will not accurately model the contact area which will have a huge effect on the pin stresses.

Can you use symmetry to reduce model complexity - cut it in half along the push rod axis, then in half along the pin axis - your quarter model will then be much better constrained...

 

[TeoAlfa]

This is the supporting structure of a large boat trailer. In the real world, the upper structure will rotate only a small amount until it is parallel to the inclined surface of the boat.
The pads of the upper structure should follow the inclination of the boat bottom sides, that why there is the rotating pin there.
I will post a full model image later to let you understand how it works.
Since in reality the upper structure is not rotating, just supporting the load, is the bonded contact between the pin and bushes and between the pin and clevis so much off?

 

[D_UK]

The problem with the bonded contact is not really related to rotation but to the bearing pressure distribution. Rather than bearing on say half of the pin/bush, bonded contact will distribute the load path round the pin circumference. This will affect the pin stress and also the stresses in the clevis blades. If you are attempting a detailed fatigue study you really need to take these effects into account.

David

 

[TeoAlfa]

Back again, now applying frictional contacts between the pin and the bushings, also between the hydraulic cylinder end with the pin.

Constraints
I applied a remote displacement (rotation x=0 all other free) on both sides of the pin, and also to the outer sides of each bushing insert.

Results are totally different, as D_UK suggested, and deformed state looks more realistic now.
Maximum stress at the pin is only around 280MPa.
I have a doubt on the high stress on the outer side of the bushings though. Maybe this is due to the constraint i applied there?

http://oi68.tinypic.com/14jmb2g.jpg

And here is a section view of the stress plot.

http://oi65.tinypic.com/1zwm8pf.jpg

And here i uploaded a video showing the deformation on a large scale obviously.

https://www.youtube.com/watch?v=gW1useDZNrQ

Please share your thoughts, thanks!

 

[Erik Panos Kostson]

It looks strange on the edges and you are possibly right that it is due to the constraint.
(Not sure how the bushing is attached to the outer part, not the pin, but if it is pressed, perhaps a bonded contact between the outer part and the bushing might be a start there, of course, between the pin and the bushing the frictional contact is the most realistic there, and that seems from the image to work pretty OK).

Try thus to remove the constraint on the bushing, and perhaps keep the constraint on the pin because it might want to spin around before the contact is active and thus provide enough friction to prevent that. Perhaps this will reduce the edge stress.

Finally the hull provides a constraint. Of course including it might increase the model size so you might want to provide a compression only face support on the contact area between hull and the mechanism shown,

 

[Shu Jiang PEng SE]

Try manual calculate the stress of the pin ( treat it as a beam)and ignore the bushing, and check the pin fatigue life with appropriate S-N curve. This will give you a rough estimation.

 

[TeoAlfa]

@Erik
"Not sure how the bushing is attached to the outer part, not the pin, but if it is pressed, perhaps a bonded contact between the outer part and the bushing might be a start there, of course, between the pin and the bushing the frictional contact is the most realistic there, and that seems from the image to work pretty OK"

The bushing is being pressed on the outer tube, so the bonded contact is indeed a good compromise. Although i think that a rough contact would be more realistic, what would you think?

I made a change regarding the bushing constraint. Instead of constraining X rotation on the side face of the bushings, i applied it on their outer surfaces, see image below.
There is no high stress on the bushing sides now.

https://image.ibb.co/dfbgO9/bushing_contacts.jpg

Here is the stress plot on the section view.

https://image.ibb.co/g3wCwU/stress_section.jpg

And here is the stress on the pin.

https://image.ibb.co/nCEXwU/stress_pin.jpg

Pretty good results, i hope they are reliable too!
But way different in comparison with the results when bonded contacts were applied!

 

[Erik Panos Kostson]

Yes, the results look much better now.

In order to verify that the FEA model is OK, one could do as Shu Jiang recommended, approximate the pin as a beam.
(of course to validate one would need some test data to compare with)

You know the total load being applied (pad area times pressure applied perhaps, or if possible get the total force on the contact area between the pin and the other part), then you can calculate the moment, and the bending stresses (Moment/Section Modulus). This should be quite close to the bending stresses (assuming zero axial stress) at the top of the beam/pin which is in tension due to bending, thus look on the SXX (or largest positive principal stress) results component on top of the beam (this should be as we said close to the hand calcs. more or less assuming zero axial force in the pin; if there is axial force then calculate the total fibre stress on top, axial stress + bending stress, and compare with SXX or largest principal).

 

[TeoAlfa]

Hello Erik,

I made a "hand" calculation of the pin, approximated as a beam. I applied N and mm as units anywhere to conclude in MPa (N/mm2).
Pin: D=60mm / Length=305mm
Section modulus = 21168mm3
Loads: Distributed load on each side of the pin, force on each side = -85.000N, length of load acting = 90mm, -> q=945N/mm for each side of the pin

I attach an image showing the beam configuration.

Peak bending moment = -4039875Nmm
Section modulus = 21168mm3

Bending stress (hand calculation) = 191MPa
Max. Principal Stress on top of the beam/pin (Ansys) = 199MPa ( see image:

https://image.ibb.co/mvAEBU/max_principal_stress.jpg

)
Peak equivalent stress (Ansys) = 201MPa

I feel more confident about my results now.
What do you think?

 

[Erik Panos Kostson]

That is good.

Obviously you know and are the expert on how the pin behaves and the loads on it, so with the imposed loads the bending moment diagrams look reasonable.

It matches the principal stresses quite good at the tension side.

Of course I cannot tell/guarantee that this is what is happening in reality, only testing can. But as far as the verification goes, with the assumed loads and restraints on the equivalent beam it matches pretty good.
----------------------------------------------------------------------------------------------------------------------------------------------
Just my personal views, nothing to do with work.

 

[TeoAlfa]

Many thanks Erik!
BTW, do you have Greek origins?
Sorry for the OT...

 

[Erik Panos Kostson]

No mention, glad I could help as much as I can.

Part (1/2) of me yes , originally, but I grew up abroad.
(Teo are you Greek then?)
Feel free to connect:
Link