FEA interpretation

[rmerlob]

Hi,

Ever since I started using inventor a couple years ago I´ve done hundreds of simulations on different parts test models etc, I feel that I´ve asked every question that needs to be asked and read every white paper/article/tutorial on FEA that I could possibly find.

The problem is: I still cant be confident when I interpret the results I get, I totally understand FEA requires training and experience to use and its not a tool that should be used blindly, but I cant seem to rely on even the simplest of results.

So this time my aproach will be different, I´m not going to direct my question to a single area or post results:

Will the part attached hold 70 kN under traction using Ductile Iron 65-45-12?

I´m sure a lot things regarding stress concentration, localized plastic strain, constrain placement are going to come up but  I really dont want to steer the topic in any direction, just want to see what other people come up with and discuss.

Thanks for your attention,

RM

[rmerlob]

Hi,

Ever since I started using inventor a couple years ago I´ve done hundreds of simulations on different parts test models etc, I feel that I´ve asked every question that needs to be asked and read every white paper/article/tutorial on FEA that I could possibly find.

The problem is: I still cant be confident when I interpret the results I get, I totally understand FEA requires training and experience to use and its not a tool that should be used blindly, but I cant seem to rely on even the simplest of results.

So this time my aproach will be different, I´m not going to direct my question to a single area or post results:

Will the part attached hold 70 kN under traction using Ductile Iron 65-45-12?

I´m sure a lot things regarding stress concentration, localized plastic strain, constrain placement are going to come up but  I really dont want to steer the topic in any direction, just want to see what other people come up with and discuss.

Thanks for your attention,

RM

[JDMather]

How will the part be manufactured? Machined from a casting?

It appears that there would be interactions with another part(s) that would apply the load and limit the displacement currently exhibited in the analysis.

More questions to follow....

[JDMather]

How will the part be manufactured? Machined from a casting?

It appears that there would be interactions with another part(s) that would apply the load and limit the displacement currently exhibited in the analysis.

More questions to follow....

[karthur1]

Here is my stab at it. You said the load was in "traction".  Not sure what you mean by that, but I assumed you meant in tension.  I set it up with the id of the end opposite the eyes being fixed. For the load, I did a bearing load of 70kN on the id of the eyes. The load direction is away from the the end that is bored out.

Inventor gives me a minimum SF of .91.  According to this analysis, it would probably start failing in the hole where the pin will be.  This is assuming that there is nothing between the two tangs that prevent them from "closing in".

If there is some element that keeps the tangs straight, then this will fail sooner.  It gives me a minimum SF=.46 under this load case.

[karthur1]

Here is my stab at it. You said the load was in "traction".  Not sure what you mean by that, but I assumed you meant in tension.  I set it up with the id of the end opposite the eyes being fixed. For the load, I did a bearing load of 70kN on the id of the eyes. The load direction is away from the the end that is bored out.

Inventor gives me a minimum SF of .91.  According to this analysis, it would probably start failing in the hole where the pin will be.  This is assuming that there is nothing between the two tangs that prevent them from "closing in".

If there is some element that keeps the tangs straight, then this will fail sooner.  It gives me a minimum SF=.46 under this load case.

[JDMather]

More information is needed.

An entry into the plastic deformation zone of the curve does not necessarily indicate "failure".  It does not necessarily mean fracture of the part.

The key is to match up a digital analysis model to physical testing of actual part, then you can have predictive confidence in (very) similar digital models.

[JDMather]

More information is needed.

An entry into the plastic deformation zone of the curve does not necessarily indicate "failure".  It does not necessarily mean fracture of the part.

The key is to match up a digital analysis model to physical testing of actual part, then you can have predictive confidence in (very) similar digital models.

[rmerlob]

Hi, thanks for answers

Yes I did mean tension, language barrier 😛

JD, the part that comes with this one goes in the middle and has about double the section, it leaves about 4 mm total clearance inside, so i dont think it will stop movement towards the inside. I'll post it when I get to work tomorrow.

We are going to cast with the two small holes and bore/drill the other one out, they are used for holding cables.

Interesting thing is, we are pretty certain this is the material that these are made of, did a spectrometric analysis for composition and even though carbon is imposible to read on cast ductile iron, all other elements suggest it is, plus they have a 70 kN stamp on them, they are also made by casting and drilling like I described.

I understand that due to strain hardening of the local high stress the part should not be asumed to fail even if a small part of it passes yield, is that right?

Did I miss some other critical info?

[rmerlob]

Hi, thanks for answers

Yes I did mean tension, language barrier 😛

JD, the part that comes with this one goes in the middle and has about double the section, it leaves about 4 mm total clearance inside, so i dont think it will stop movement towards the inside. I'll post it when I get to work tomorrow.

We are going to cast with the two small holes and bore/drill the other one out, they are used for holding cables.

Interesting thing is, we are pretty certain this is the material that these are made of, did a spectrometric analysis for composition and even though carbon is imposible to read on cast ductile iron, all other elements suggest it is, plus they have a 70 kN stamp on them, they are also made by casting and drilling like I described.

I understand that due to strain hardening of the local high stress the part should not be asumed to fail even if a small part of it passes yield, is that right?

Did I miss some other critical info?

[karthur1]

---

@Anonymous wrote:

More information is needed.

An entry into the plastic deformation zone of the curve does not necessarily indicate "failure".  It does not necessarily mean fracture of the part.

The key is to match up a digital analysis model to physical testing of actual part, then you can have predictive confidence in (very) similar digital models.

---

Testing the actual part is the best way to determine when it will fail.  Hard to argue that.

Any SF < 0.69 in this case, would indicate that its out of the plastic range and past the ultimate tensile. Its up to the OP to determine his criteria for "failure" (either facture or deformation). I would think that with a clevis, it could be deformed, but not broken, and be considered a failure.

[karthur1]

---

@Anonymous wrote:

More information is needed.

An entry into the plastic deformation zone of the curve does not necessarily indicate "failure".  It does not necessarily mean fracture of the part.

The key is to match up a digital analysis model to physical testing of actual part, then you can have predictive confidence in (very) similar digital models.

---

Testing the actual part is the best way to determine when it will fail.  Hard to argue that.

Any SF < 0.69 in this case, would indicate that its out of the plastic range and past the ultimate tensile. Its up to the OP to determine his criteria for "failure" (either facture or deformation). I would think that with a clevis, it could be deformed, but not broken, and be considered a failure.

[JDMather]

---

@karthur1 wrote:

 I would think that with a clevis, it could be deformed, but not broken, and be considered a failure.

---

Deformed by how much? 0.5% 1% 10?  any permanent deformation a failure?

[JDMather]

---

@karthur1 wrote:

 I would think that with a clevis, it could be deformed, but not broken, and be considered a failure.

---

Deformed by how much? 0.5% 1% 10?  any permanent deformation a failure?

[karthur1]

Thats totally up to the OP and how the "failure" is defined.

If the clevis is used for rigging, then normally ANY noticable deformation would deem the part unuasble. But, if it is used for something else, then it might might be reused as long as it was not "broken".

[karthur1]

Thats totally up to the OP and how the "failure" is defined.

If the clevis is used for rigging, then normally ANY noticable deformation would deem the part unuasble. But, if it is used for something else, then it might might be reused as long as it was not "broken".

[JDMather]

---

@karthur1 wrote:

...ANY noticable deformation would deem the part unuasble.

---

Is that by eyeball inspection, measuring instrument, or digital analysis?

[JDMather]

---

@karthur1 wrote:

...ANY noticable deformation would deem the part unuasble.

---

Is that by eyeball inspection, measuring instrument, or digital analysis?

[rmerlob]

karthur:

''Any SF < 0.69 in this case, would indicate that its out of the plastic range and past the ultimate tensile. Its up to the OP to determine his criteria for "failure" (either facture or deformation). I would think that with a clevis, it could be deformed, but not broken, and be considered a failure.''

Actually, I believe that since Inventor uses linear analisys whe cannont assure its actually past UTS because of strain hardening, for example attached you can find my best attempt at using Autodesk Simulation with a bi-lineal material model, and you can see SF is a lot higher. 

Material is 80-55-06 Ductile but you can see the diference from the results I get on Inventor.

Like you, I believe any permantent deformation should be avoided, thats not what im seeing and it puzzles me that I have a real part in my hands that has the 70 kN stamp on it.

Of course I'm not a finite elements expert so i would really like someone with more experience and training to comment. 

Also attached is the other part too.

thanks for replies

[rmerlob]

karthur:

''Any SF < 0.69 in this case, would indicate that its out of the plastic range and past the ultimate tensile. Its up to the OP to determine his criteria for "failure" (either facture or deformation). I would think that with a clevis, it could be deformed, but not broken, and be considered a failure.''

Actually, I believe that since Inventor uses linear analisys whe cannont assure its actually past UTS because of strain hardening, for example attached you can find my best attempt at using Autodesk Simulation with a bi-lineal material model, and you can see SF is a lot higher. 

Material is 80-55-06 Ductile but you can see the diference from the results I get on Inventor.

Like you, I believe any permantent deformation should be avoided, thats not what im seeing and it puzzles me that I have a real part in my hands that has the 70 kN stamp on it.

Of course I'm not a finite elements expert so i would really like someone with more experience and training to comment. 

Also attached is the other part too.

thanks for replies

[JDMather]

---

@rmerlob wrote:

Like you, I believe any permantent deformation should be avoided, ....

---

How much Actual (computed) displacement are you seeing in the analysis (if we ignore for a moment that results below SF might not be correct)?

[JDMather]

---

@rmerlob wrote:

Like you, I believe any permantent deformation should be avoided, ....

---

How much Actual (computed) displacement are you seeing in the analysis (if we ignore for a moment that results below SF might not be correct)?

[rmerlob]

Its the same as yours, about 0.2 mm, results on autodesk simulation is a little higher around .3 mm but stress seems lower all around.

[rmerlob]

Its the same as yours, about 0.2 mm, results on autodesk simulation is a little higher around .3 mm but stress seems lower all around.

[karthur1]

Is this with the second one "SoporteB.ipt" that was posted?  I am getting 0.101mm total displacement on the first part that was posted.

[karthur1]

Is this with the second one "SoporteB.ipt" that was posted?  I am getting 0.101mm total displacement on the first part that was posted.

[rmerlob]

No karthur, SoporteB is the part that mates with SoporteA, I will attach picture of the actual parts we are going to repoduce when I have the chance.

We dont knowand we have a lead on what the material is, thats 

Are you sure you have a fine enough mesh? I definitely get more than 0.2 mm on fully converged displacement results, actually I get 0.2749 on 289619 elements

[rmerlob]

No karthur, SoporteB is the part that mates with SoporteA, I will attach picture of the actual parts we are going to repoduce when I have the chance.

We dont knowand we have a lead on what the material is, thats 

Are you sure you have a fine enough mesh? I definitely get more than 0.2 mm on fully converged displacement results, actually I get 0.2749 on 289619 elements

[JDMather]

---

@rmerlob wrote:
Its the same as yours, about 0.2 mm,

---

My point was, is this really significant (for the usual function of this part), about the thickness of two sheets of paper - can barely see by eye.  A lot of people see the exaggerated representation take interpret it literaly.

[JDMather]

---

@rmerlob wrote:
Its the same as yours, about 0.2 mm,

---

My point was, is this really significant (for the usual function of this part), about the thickness of two sheets of paper - can barely see by eye.  A lot of people see the exaggerated representation take interpret it literaly.

[rmerlob]

I agree, what I meant about no permanent deformation being accepted didn´t quite explain itself, I tried to say that there probably shouldnt be points that are past yield.

Of course 0.2 displacement is okay on this part, what worries me is that stresses are past yield, and even though theory tells me that some localized yielding can be acceptable on ducile materials (again, keywords: strain hardening and stress redistribution) theres no guidelines on how much of it is acceptable.

This leaves no more options other that testing, even for a case that I consider could be the simplest real life application of finite element analisys.

The reason for this thread is that I DO NOT want to believe this is the case and I think there is somebody out there with more experience and training than myself that can say: this local yielding is acceptable or not because x and y reasons.

[rmerlob]

I agree, what I meant about no permanent deformation being accepted didn´t quite explain itself, I tried to say that there probably shouldnt be points that are past yield.

Of course 0.2 displacement is okay on this part, what worries me is that stresses are past yield, and even though theory tells me that some localized yielding can be acceptable on ducile materials (again, keywords: strain hardening and stress redistribution) theres no guidelines on how much of it is acceptable.

This leaves no more options other that testing, even for a case that I consider could be the simplest real life application of finite element analisys.

The reason for this thread is that I DO NOT want to believe this is the case and I think there is somebody out there with more experience and training than myself that can say: this local yielding is acceptable or not because x and y reasons.

[JDMather]

---

@rmerlob wrote:

This leaves no more options other that testing, even for a case that I consider could be the simplest real life application of finite element analisys.

---

I'm really interested in this too but I suspect the Autodesk Simulation forum might get better response.

I've always been taught that physical testing is a requirement to validate that the virtual test has been set up correctly.

In my class I wait till the last lab of the last semester with my seniors and do a similar problem that casts doubt on all FEA.  I would love to hear more on the topic from the true experts.

[JDMather]

---

@rmerlob wrote:

This leaves no more options other that testing, even for a case that I consider could be the simplest real life application of finite element analisys.

---

I'm really interested in this too but I suspect the Autodesk Simulation forum might get better response.

I've always been taught that physical testing is a requirement to validate that the virtual test has been set up correctly.

In my class I wait till the last lab of the last semester with my seniors and do a similar problem that casts doubt on all FEA.  I would love to hear more on the topic from the true experts.

[rmerlob]

Glad we are on the same page, I did enlist the help of the sim squad hopefully they will come by shortly.

On the topic of testing, its clear that it would be helpful, but what if the load were 10 times higher or maybe it wasnt simple tension, like a cantilevered beam or something.

As cases get more complex it gets exponentially more dificult to test something out on limited resources, and I always thought finite elements was supposed to fill that void and let a small engineering team test it out virtually on cases that were simple or not critical enough.

Theres just 2 possible answers, I´m not experienced/trained enough to make that call, or I have a wrong idea about the capabilities of finite elements. I dont like either lol.

Another thing to note is that doing a manual calculation for the area around the holes, I get somethig that was around 100 MPa (very roughly dont remember it exactly) without considering stress concentration, theres a page on Shigleys Mechanical Design textbook that says stress concentration factors are generally not applied to ductile materials in static loading because of the strain hardening effect I mentioned earlier, so if I were to design this manually I would believe there is like a SF of 3.

Kind of scary when you think that manual calulations had you thinking you got this and finite elements makes you doubt the entire thing.

In all fairness if we were to apply a stress concentration factor SF would drop dramatically but thats not what I should be doing from what I gather from Mr. Shigley himself.

Great now im doubting manual calculations too, great, 5 years of education down the drain lol.

[rmerlob]

Glad we are on the same page, I did enlist the help of the sim squad hopefully they will come by shortly.

On the topic of testing, its clear that it would be helpful, but what if the load were 10 times higher or maybe it wasnt simple tension, like a cantilevered beam or something.

As cases get more complex it gets exponentially more dificult to test something out on limited resources, and I always thought finite elements was supposed to fill that void and let a small engineering team test it out virtually on cases that were simple or not critical enough.

Theres just 2 possible answers, I´m not experienced/trained enough to make that call, or I have a wrong idea about the capabilities of finite elements. I dont like either lol.

Another thing to note is that doing a manual calculation for the area around the holes, I get somethig that was around 100 MPa (very roughly dont remember it exactly) without considering stress concentration, theres a page on Shigleys Mechanical Design textbook that says stress concentration factors are generally not applied to ductile materials in static loading because of the strain hardening effect I mentioned earlier, so if I were to design this manually I would believe there is like a SF of 3.

Kind of scary when you think that manual calulations had you thinking you got this and finite elements makes you doubt the entire thing.

In all fairness if we were to apply a stress concentration factor SF would drop dramatically but thats not what I should be doing from what I gather from Mr. Shigley himself.

Great now im doubting manual calculations too, great, 5 years of education down the drain lol.

[Anonymous]

I didn't read through every entry in this post but I would just like to toss in a few things I was taught years ago in grad school and employ when performing FEA.  When performing FEA it is always good practice to perform some type of hand calculation to validate the model.  The results won't be identical but within 4% or 5% is pretty good.  This will help verify the model, loads, and constraints are correct.  Without that, the accuracy of the FEA model is uncertain.  Often, inaccurate FEA results are related to a poor quality mesh which sometimes stem from a model that is too complex.  One source for various hand calculations with different load and geometry configurations is Roark's Formula for Stress and Strain.  Also, to the best of my knowledge, stress concentration factors are only considered in Fatigue Analysis and not applied to Linear Static Analysis.  Lastly, it is not uncommon to see local yielding at discontinuities, etc. with FEA.  That doesn't always mean the part will fail.

Regards,

Mike  

[Anonymous]

I didn't read through every entry in this post but I would just like to toss in a few things I was taught years ago in grad school and employ when performing FEA.  When performing FEA it is always good practice to perform some type of hand calculation to validate the model.  The results won't be identical but within 4% or 5% is pretty good.  This will help verify the model, loads, and constraints are correct.  Without that, the accuracy of the FEA model is uncertain.  Often, inaccurate FEA results are related to a poor quality mesh which sometimes stem from a model that is too complex.  One source for various hand calculations with different load and geometry configurations is Roark's Formula for Stress and Strain.  Also, to the best of my knowledge, stress concentration factors are only considered in Fatigue Analysis and not applied to Linear Static Analysis.  Lastly, it is not uncommon to see local yielding at discontinuities, etc. with FEA.  That doesn't always mean the part will fail.

Regards,

Mike  

[karthur1]

The displacement that I am seeing is a little different than yours. Since you have the male part that keeps the ears on the clevis from bending in, I added a frictionless constraint on the inside so they cant move in.  The surfaces I added it to is highlighted in the image.  I get a displacement of around .10mm.  I am using an element size of 0.01.

I can get the same displacement as you if I dont have this frictionless constraint.

[karthur1]

The displacement that I am seeing is a little different than yours. Since you have the male part that keeps the ears on the clevis from bending in, I added a frictionless constraint on the inside so they cant move in.  The surfaces I added it to is highlighted in the image.  I get a displacement of around .10mm.  I am using an element size of 0.01.

I can get the same displacement as you if I dont have this frictionless constraint.