Inventor General Discussion

Reply
Active Contributor
rhinterhoeller
Posts: 43
Registered: ‎08-07-2002
Message 21 of 30 (642 Views)

Re: FEA interpretation

10-11-2012 07:02 AM in reply to: rmerlob

I simulated all of this a bit differently.

 

Firstly I took advantage of symmetry and removed 3/4 of the fork.  Frictionless constraints were used on the 'cut' faces.  This produces the same results but with 1/4 of the elements plus I get to easily see what happens internally.

 

Secondly I added a toggle and a pin so that we could model the loading on the fork more accurately.  See (Assembly.jpg).  The toggle is 1mm thinner than the gap in the fork, leaving a 0.5 mm gap.  The load (70 kN/4) was applied to the top end of the toggle.

 

In the first simulation I applied a separation contact between the pin and each of the other components.  The minimum safety factor occurs in the hole (not visible).  This is to be expected.

 

A safety factor of 0.93 occurs where the legs of the fork meed the shank.  This simulation suggests some work hardening but I would guess not an outright failure. (see Separation.jpg)

 

But, is the assumption of a free-sliding pin accurate?  In my 2nd simulation the contact between the pin and the fork was changed to "separation / no sliding".

 

I made the pin and toggle invisible (See Separation-no-Sliding Isolated.jpg).  Again, the highest stress occurs in the hole but we have to consider the loading here is not representative of real life.  However, the friction from the pin dials out much of the X Displacement at the hole and the safety factor at the root of the fork is now a bit greater than 1.

 

The Y displacements that I see are 0.15 and 0.13mm respectively.

 

My $0.02.

 

Richard

IV 2013 Product Design Suite 64 Bit
Win 7 64 bit
Distinguished Contributor
rmerlob
Posts: 135
Registered: ‎10-21-2011
Message 22 of 30 (576 Views)

Re: FEA interpretation

10-15-2012 04:59 AM in reply to: rhinterhoeller

Hi, thanks for answer, why isnt the loading in the hole representative of real life, what do you mean ?

Active Contributor
rhinterhoeller
Posts: 43
Registered: ‎08-07-2002
Message 23 of 30 (555 Views)

Re: FEA interpretation

10-15-2012 06:06 AM in reply to: rmerlob
<...why isnt the loading in the hole representative of real life, what do you mean ?> One has to consider that the bracket and the pin are interacting. Consider: 1/ model the bracket with an evenly distributed pressure 2/ the only way a pin could exert that pressure is if it doesn't bend 3/ the pressure on the pin is equal and opposite to the pressure on the bracket 4/ if you analyze the pin under this loading you will see that it bends, thus violating 2 above, therefore applying an evenly distributed bearing stress does not represent real life. In real life, the pin will bend a little and the contact stress will follow some distribution where the stress is higher on the inside of the bracket and lower (or 0) on the outside. There will also be friction which will restrict the "fork's" movement in the x direction. All combined these provide a kinder loading at the root of the fork and keep the factor of safety above 1. Richard
IV 2013 Product Design Suite 64 Bit
Win 7 64 bit
Distinguished Contributor
rmerlob
Posts: 135
Registered: ‎10-21-2011
Message 24 of 30 (540 Views)

Re: FEA interpretation

10-15-2012 09:51 AM in reply to: rhinterhoeller

I agree with your statements and agree it would make it kinder on the base of the fork, then why are you ignoring the hole part, I think real life loading would be kinder on the base and harsher on the hole, shouldnt that be your area of focus?

 

Thanks again, RM

Active Contributor
rhinterhoeller
Posts: 43
Registered: ‎08-07-2002
Message 25 of 30 (510 Views)

Re: FEA interpretation

10-15-2012 03:21 PM in reply to: rmerlob

I wish I could give you that answer. Rods on holes or flat bar are a horse of a different colour and I'm not sure FEA can handle that. The classical analysis was Hertzian contact stress and that was out by as fator of 3.

 

Richard

IV 2013 Product Design Suite 64 Bit
Win 7 64 bit
Distinguished Contributor
rmerlob
Posts: 135
Registered: ‎10-21-2011
Message 26 of 30 (506 Views)

Re: FEA interpretation

10-15-2012 05:05 PM in reply to: rhinterhoeller

I´m not talking about contact stresses, I mean the tensile stress that gets developed on the side of the hole due to stress concentration, as far as I know Hertz was for the part where the rod actually compresses the material.

Active Contributor
rhinterhoeller
Posts: 43
Registered: ‎08-07-2002
Message 27 of 30 (497 Views)

Re: FEA interpretation

10-15-2012 07:09 PM in reply to: rmerlob
Ah! I had split the pin and applied a separation/no sliding contact on the top half. The intention was to prevent the fork from slipping in or out from the toggle due to friction. The unintended consequence was that as one looks at the portion of the pin where the contact surface approaches vertical no sliding is permitted. This causes an unrealistic loading in that region. I expect that by moving the split up toward the top of the pin and applied the aforementioned contact to the top portion and a separation contact below the split one could achieve a more realistic simulation. Richard
IV 2013 Product Design Suite 64 Bit
Win 7 64 bit
*Expert Elite*
Inv_kaos
Posts: 728
Registered: ‎07-26-2007
Message 28 of 30 (487 Views)

Re: FEA interpretation

10-15-2012 11:59 PM in reply to: rmerlob

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.

Please mark as "Accept as Solution" if it answers your question or "Kudos" if you found it useful.
---------------------------------------------------------------------------------------------------------------------
Stew, AICP
Inventor Professional 2013, Autodesk Simulation Multiphysics 2013
Windows 7 x64 Core i7 32GB Ram FX2000
Distinguished Contributor
rmerlob
Posts: 135
Registered: ‎10-21-2011
Message 29 of 30 (432 Views)

Re: FEA interpretation

11-04-2012 05:15 PM in reply to: Inv_kaos

Thanks Inv_kaos, very insightful, I'll be sure to google stress clasification, sorry if I took to long to reply.

 

As far as the problem goes, foundry tooling is being made, physical prototype testing planned afterwards, if someone's still interested I'll be sure to post back with results.

 

Thanks all, marked as solution.

 

RM

*Expert Elite*
Inv_kaos
Posts: 728
Registered: ‎07-26-2007
Message 30 of 30 (422 Views)

Re: FEA interpretation

11-04-2012 09:12 PM in reply to: rmerlob

Glad you found it useful.

 

I would be interested to see the results of the physical testing comparison.

Please mark as "Accept as Solution" if it answers your question or "Kudos" if you found it useful.
---------------------------------------------------------------------------------------------------------------------
Stew, AICP
Inventor Professional 2013, Autodesk Simulation Multiphysics 2013
Windows 7 x64 Core i7 32GB Ram FX2000
Post to the Community

Have questions about Autodesk products? Ask the community.

New Post
Announcements
Are You Going To Be @ AU 2014? Feel free to drop by our AU topic post and share your plans, plug a class that you're teaching, or simply check out who else from the community might be in attendance. Ohh and don't forgot to stop by the Autodesk Help | Learn | Collaborate booths in the Exhibit Hall and meet our community team if you get a chance!