Inventor General Discussion

Inventor General Discussion

Reply
Distinguished Contributor
138 Posts
29 Kudos
Registered: ‎10-21-2011
Post 1 of 30
Accepted Solution

FEA interpretation

970 Views, 29 Replies
10-08-2012 01:49 PM

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 wrote:

... 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. 

 


Firstly numerical analysis is always and approximation of the real world and is only as accurate as the simplifications and assumptions made creating the 'model'. It is never intended to be used as replacement for load testing, rather to reduce the number of tests required when developing prototypes. Obviously in many industries conditions are well known and FEA is used as a calculation method only where physical testing is not required. I believe the latter would apply in your case too since a clevis would usually always have been used in similar successful circumstances.

 

Regarding local yielding, the structural codes don't cover this well but is well documented in the pressure equipment industry. It is all just basic stress analysis and failure theories so can be applied to structural too. First it helps if you understand stress classification so I will only give the short version. Basically stresses can be classified a primary and secondary, whereby secondary stresses are self limiting by nature i.e. displacement limited where local yielding will redistribute the load. Primary stresses are not self limiting and will cause failure or gross distortion if the load is applied past yield.

 

Primary stress can be sub-divided into general and local membrane, and bending. General membrane, i.e. direct stress that has not been affected by stress concentrations at discontinuities should be limited to your allowable stress per your design code, you don't want this near yield. If you have pure bending or combined stress such as membrane and bending, like in most FEA then you can go up to about yield (I try to use 90% for structural work, 1.5*0.6=0.9). If your stress result also includes secondary stresses (self-limiting) then you can exceed yield because the stress will 'shake down' on repeated reapplication of the load. What the PV codes use as the check for protection against ratcheting (low cycle fatigue), in linear analysis is an allowable of twice yield in local areas. Obviously twice yield is not attainable in real life but in linear analysis any stress beyond yield is fictitious anyway and only indicates a lower bound for shake-down. This can be checked in more detail with non-linear analysis if required.

 

There are also lots of cases where the stress at the surface show excess of yield but the through thickness stress distribution drops off rapidly, in these cases local yielding is not always likely to occur. Also, when using stress classification, how you judge whether stress is considered local for complex geometry is not clear cut (for vessels it is based on thin shell theory). So it comes down to engineering judgement and experience when deciding if the stress above yield on a case by case basis is acceptable.

 

In some cases it might not be a strength limit state but a serviceability limit state where deformation would prevent it performing as intended, just as the clevis becoming out of round to the extend where it is deemed unacceptable (which JD has already discussed).

 

If you are interested Google 'stress classification' for more information.

 

Hope it helps.

*Expert Elite*
28,589 Posts
2,120 Kudos
Registered: ‎04-20-2006
Post 2 of 30

Re: FEA interpretation

10-09-2012 08:47 AM in reply to: rmerlob

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....

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2015 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015-SP1 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
*Expert Elite*
4,353 Posts
504 Kudos
Registered: ‎04-27-2005
Post 3 of 30

Re: FEA interpretation

10-09-2012 02:12 PM in reply to: rmerlob

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".

 

Load Case 1.jpg

 

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.

 

Load Case 2.jpg

 

*Expert Elite*
28,589 Posts
2,120 Kudos
Registered: ‎04-20-2006
Post 4 of 30

Re: FEA interpretation

10-09-2012 02:41 PM in reply to: karthur1

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.

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2015 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015-SP1 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
Distinguished Contributor
138 Posts
29 Kudos
Registered: ‎10-21-2011
Post 5 of 30

Re: FEA interpretation

10-09-2012 10:25 PM in reply to: rmerlob

Hi, thanks for answers

 

Yes I did mean tension, language barrier :smileytongue:

 

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?

*Expert Elite*
4,353 Posts
504 Kudos
Registered: ‎04-27-2005
Post 6 of 30

Re: FEA interpretation

10-10-2012 06:29 AM in reply to: JDMather

JDMather 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.:smileyhappy:
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.
*Expert Elite*
28,589 Posts
2,120 Kudos
Registered: ‎04-20-2006
Post 7 of 30

Re: FEA interpretation

10-10-2012 06:55 AM in reply to: karthur1

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?

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2015 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015-SP1 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
*Expert Elite*
4,353 Posts
504 Kudos
Registered: ‎04-27-2005
Post 8 of 30

Re: FEA interpretation

10-10-2012 07:16 AM in reply to: JDMather

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".

*Expert Elite*
28,589 Posts
2,120 Kudos
Registered: ‎04-20-2006
Post 9 of 30

Re: FEA interpretation

10-10-2012 07:23 AM in reply to: karthur1

karthur1 wrote:

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


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

Please mark this response as "Accept as Solution" if it answers your question.
-----------------------------------------------------------------------------------------
Autodesk Inventor 2015 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional
Inventor Professional 2015-SP1 64-bit
http://www.autodesk.com/edcommunity
http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm
Distinguished Contributor
138 Posts
29 Kudos
Registered: ‎10-21-2011
Post 10 of 30

Re: FEA interpretation

10-10-2012 09:51 AM in reply to: JDMather

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

 

Post to the Community

Have questions about Autodesk products? Ask the community.

New Post