Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here


Fatigue results on Ansys Mechanical

Fatigue results on Ansys Mechanical

Fatigue results on Ansys Mechanical

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!

RE: Fatigue results on Ansys Mechanical

I would first think through the modelling of the pin
(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

I have used high quality and density hex mesh for the pin.
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

I think nonlinear analysis is needed if there is a risk for static failure. This depends
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

The explanation why you can obtain positive number of cycles with stress higher than tensile stress might be elastic–plastic correction method (Neuber’s rule). This method is a part of the strain-life approach in ANSYS fatigue tool. You can find more information here on slide 16 here or here.

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

@ L K
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

@ Petr Vymlatil

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

@ TheaAlfa
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

In my opinion, based on the stress results, bilinear plasticity model and frictional contacts
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

@ Petr Vymlatil + L K

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

@TeoAlfa fist I would recommend to follow advice from L_K - use nonlinear frictional contacts and nonlinear material model and check the amount of plasticity

Petr Vymlatil (www.designtec.info)

RE: Fatigue results on Ansys Mechanical

Hi again,

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.

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.

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

In first picture, yield strength is defined as 250 MPa. Should it be 380 MPa instead?

RE: Fatigue results on Ansys Mechanical

Yes, you are right.... i just copied the data from structural steel... How can i find the tangent modulus for the material?

RE: Fatigue results on Ansys Mechanical

For example in Eurocode 3, for strain hardening plasticity model tangent modulus is defined as E/100.

RE: Fatigue results on Ansys Mechanical

Thank you, i will run the analysis with the correct data and come back with the results.

RE: Fatigue results on Ansys Mechanical

So, i am back with the final results.

Material model

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.

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

Based on these results, i attach a picture of the fatigue life.
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?


RE: Fatigue results on Ansys Mechanical

Static analysis:
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

One thought about the weird stress diagram. The stress results as shown above are for the whole pin, not for a specific node. As such, i suppose that maximum stress occurred at different nodes during the loading time period. So maybe due to stress redistribution, we had let's say point X with stress A at time T, and stress A-1 at time T+1.
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?


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.


RE: Fatigue results on Ansys Mechanical

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.


RE: Fatigue results on Ansys Mechanical

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?

RE: Fatigue results on Ansys Mechanical

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...

RE: Fatigue results on Ansys Mechanical

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?

RE: Fatigue results on Ansys Mechanical

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.


RE: Fatigue results on Ansys Mechanical

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

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.
[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?


And here is a section view of the stress plot.


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

Please share your thoughts, thanks!

RE: Fatigue results on Ansys Mechanical

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,

RE: Fatigue results on Ansys Mechanical

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.

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.


Here is the stress plot on the section view.

And here is the stress on the pin.

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

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).

RE: Fatigue results on Ansys Mechanical

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.j... )
Peak equivalent stress (Ansys) = 201MPa

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

RE: Fatigue results on Ansys Mechanical

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.

RE: Fatigue results on Ansys Mechanical

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

RE: Fatigue results on Ansys Mechanical

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:

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


White Paper – Data Security and Know-How Protection
Our data is constantly exposed to the danger of being intercepted or stolen as it wends its way over global data networks. Data security measures and measures for protecting intellectual property should not, however, first be implemented when data is exchanged – companies must lay the foundation for these measures within their own organization. Download Now
White Paper – Collaboration in the PLM Context
The influence exerted by the Internet of Things (IoT) means that there is a steadily growing need for collaboration in industry. Partners from new industries and areas of application need to be integrated in cross-company business processes to ensure that the lifecycle of smart, connected products can be managed from end to end. Download Now
White Paper – The Challenges of PLM Collaboration
There is cross-company collaboration - and then there is cross-company collaboration. Large-scale corporations and joint ventures need different mechanisms to protect intellectual property from those required for communication between different company locations with heterogeneous IT landscapes. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close