## Fatigue results on Ansys Mechanical

## Fatigue results on Ansys Mechanical

(OP)

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!

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!

## RE: Fatigue results on Ansys Mechanical

(element type, contacts, material model, meshing).

Did you make some assumptions (for example linear model)

which might affect pin stresses?

## RE: Fatigue results on Ansys Mechanical

The contact with the bushing is "no separation" as this is dictated by the available computing resources. With my current workstation capabilities, nonlinear contact options will result in days of analysis time.

My analysis is linear static. Do you think i should insert some nonlinear controls? And what would you recommend?

## RE: Fatigue results on Ansys Mechanical

a lot on the particular structure, loading etc. Could you share some pictures of the model?

You could make a smaller model of the detail to solve faster.

Regarding strain-life fatigue analysis: Did you define a new material for the steel

pin material with the correct strain-life parameters?

## RE: Fatigue results on Ansys Mechanical

Keep in mind, that strain-life is based on stresses

and strains, which are calculated by Neuber's rule or plastic calculation. In other words you cannot reach stresses higher strain tensile stress.I would also recommend a nonlinear calculation with the stress-strain diagram, which corresponds to your strain-life parameters. In this way you can check the amplitude of strains and estimate the number of cycles from your strain-life curve.

Still, check your inputs carefully.

Petr Vymlatil (www.designtec.info)

## RE: Fatigue results on Ansys Mechanical

I attach some images from the analysis. I hope it helps.

I will try to decompose the area of interest and run a nonlinear analysis.

And yes, i have defined the full strain-life parameters of the material.

Strength coefficient: 920Mpa

Strength exponent: -0.106

Ductility coefficient: 0.213

Strength exponent: -0.47

Cyclic strength coefficient: 1000Mpa

Cyclic strain hardening exponent: 0.2

## RE: Fatigue results on Ansys Mechanical

If i understand correctly, my fatigue analysis results are not correct just because the stress and strain i got from the linear static analysis are not correct either because the pin is outside the tensile strength limit.

## RE: Fatigue results on Ansys Mechanical

No I did not want to say, that your fatigue analysis results are not correct, because the pin is outside the tensile strength limit.

You should not use the tensile strength limit as strict criterion. Keep in mind that in reality have the material plastic behavior and the stresses will redistribute due to plasticity.

Your assessment procedure should look like this:

I. static assessment

- perform linear static analysis

- in your case are the stresses high above the yield strength. The basic question is, if you reached the yield strength in a critical cross-section completely. Your plots with contour 250 MPa are not very useful, use your yield strength (370 MPa). If not, there is chance for redistribution and you should perform a nonlinear calculation (with stress-strain curve). If yes, change your design.

- perform a nonlinear calculation (with stress-strain curve) and look for maximum plastic strain. If the maximum plastic strain is relatively small or acceptable for you there is chance that your design stands also cyclic load (low cycle fatigue <10e4 cycles). If not, change your design.

II. low cycle fatigue

- perform linear calculation and ANSYS will use Neuber's rule and calculate the strain amplitudes from your linear calculation. Keep in mind that Nueber's rule should be used only if the regions with stresses above yield are small (most likely not the case in your current design according the figures you shared).

However, low cycle fatigue assessment is not trivial. I would also recommend better software for low-cycle fatigue analysis (for example FEMFAT).

Petr Vymlatil (www.designtec.info)

## RE: Fatigue results on Ansys Mechanical

should be used to model the detail. One thing to consider in the subsequent strain-life analysis

is the choice of stress component.

## RE: Fatigue results on Ansys Mechanical

Many thanks for your replies.

I post again some images with corrected stress plot (370MPa).

I think the situation is quite serious as the whole circumference of the pin exceeds yield strength.

Section images also attached.

What do you think?

Would it be better to choose another steel alloy with higher yield strength or i will have more serious fatigue problems due to the brittle nature (nucleation etc) of that steel?

## RE: Fatigue results on Ansys Mechanical

Petr Vymlatil (www.designtec.info)

## RE: Fatigue results on Ansys Mechanical

I have run a nonlinear analysis (large deflections on) but i could not use nonlinear contacts between the pin and bush because the angle of the acting force causes the structure to rotate so no convergence. I will try again though.

So what we have is "large deflections on", and again bonded contacts.

As for the material model i have entered full strain-life parameters, as well as bilinear isotropic hardening data. See attached image from Engineering Data.

http://oi64.tinypic.com/fcs6qp.jpg

The loading case was 2 steps loading, zero force at the start, linear increase of the force up until 1sec, and then releasing the force up to 2sec, see attached image.

http://oi64.tinypic.com/25qchox.jpg

Finally I got some interesting results.

The maximum stress on the pin was just over yield (around 380Mpa), compared to more than 1000Mpa in the linear analysis.

Maximum total strain on the pin was 0.048.

And here is the stress-strain diagram at the node of maximum stress on the pin.

It seems that it's perfectly linear, although not returning fully to zero.

What conclusion would you come up with?

Thank you in advance!!

## RE: Fatigue results on Ansys Mechanical

## RE: Fatigue results on Ansys Mechanical

## RE: Fatigue results on Ansys Mechanical

## RE: Fatigue results on Ansys Mechanical

## RE: Fatigue results on Ansys Mechanical

Material model

http://oi65.tinypic.com/2ln9z47.jpg

Load case. Here i made a bit of a change, i added one second after the release of the force to give more time to the pin to come to its final steady state.

http://oi67.tinypic.com/2ia5x8i.jpg

Here is the maximum stress, significantly higher than the previous analysis. 382Mpa/471Mpa.

I cannot figure out why it resulted that different as what i changed were the only the bilinear isotropic hardening data.

Maximum plastic strain. Now it's significantly less than previously.

And here is the stress-strain diagram at the node of max plastic strain.

As i am new to nonlinear analysis, i would appreciate any help. Thanks!!

## RE: Fatigue results on Ansys Mechanical

Analysis Type: Strain Life

Mean Stress Theory: SWT

Stress component: Max Shear (this gives the worst result)

Fatigue life of 100.000 cycles is perfectly acceptable to my application, but something tells me that this is not a reliable result.

Could you please review this?

https://i.imgur.com/q3KbSZK.jpg

## RE: Fatigue results on Ansys Mechanical

Stress increases over yield strength because of strain hardening.

After load step 2 (unloading) only plastic strain remains.

What is interesting that max stress is achieved at 70% load, then it

decreases, and again increases to 100% load. It is hard to say what leads

to this behaviour without seeing the model fully.

In my opinion, increasing the length of load step 2 does not really make sense.

Remember this is static analysis. Equilibrium is the same at t=2 and t=3.

Results should be identical. Actually you will get all the information you need

from load step 1.

Fatigue analysis:

If you think results are not reliable, review your material parameters.

You could read the result (cycles) directly from the EN-graph, now that

you know the strain for one cycle.

## RE: Fatigue results on Ansys Mechanical

Let's take a look at the stress strain diagram of a certain node where maximum plastic strain occurs. Isn't that weird too (see image below) ?

How could you explain that stress decreases so much (29Mpa) at 1.4sec and then increases again after 1.5sec.

And why stress remains after unloading? Is it remaining internal stresses due to plastic deformation?

http://oi66.tinypic.com/16aqfdt.jpg

I also attach an image of the model. This is a small part of the whole assembly which i isolated to run the nonlinear analysis.

http://oi68.tinypic.com/r09icm.jpg

## RE: Fatigue results on Ansys Mechanical

David

## RE: Fatigue results on Ansys Mechanical

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!

## RE: Fatigue results on Ansys Mechanical

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...

## RE: Fatigue results on Ansys Mechanical

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?

## RE: Fatigue results on Ansys Mechanical

David

## RE: Fatigue results on Ansys Mechanical

ConstraintsI 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.

[img https://ibb.co/bXGkAp]

[img https://ibb.co/hXfZ39]

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!

## RE: Fatigue results on Ansys Mechanical

(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,

## RE: Fatigue results on Ansys Mechanical

## RE: Fatigue results on Ansys Mechanical

"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!

## RE: Fatigue results on Ansys Mechanical

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).

## RE: Fatigue results on Ansys Mechanical

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/mmfor each side of the pinI 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.j... )

Peak equivalent stress (Ansys) = 201MPa

I feel more confident about my results now.

What do you think?

## RE: Fatigue results on Ansys Mechanical

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.

## RE: Fatigue results on Ansys Mechanical

BTW, do you have Greek origins?

Sorry for the OT...

## RE: Fatigue results on Ansys Mechanical

Part (1/2) of me yes :), originally, but I grew up abroad.

(Teo are you Greek then?)

Feel free to connect:

Link