How far from a singularity is far enough... 2

[321GO]

Hello Guys,

basically i have a flange which is restrained by another part. This restraint is stiff enough to cause a local stress singularity right on the intersection between the two parts.

Error Energy Norm is high on this intersection but quickly goes low few elements away.

Now my question:
how far is far enough from this singularity for the stress to be uneffected?

Could one say if the Energy Error Norm is low<5 the stresses are real? So only a few elements away is enough?(where i probed the results)

I would think so but not sure.


Thanks to you all in advance!

 

[rb1957]

1st off, yuor model doesn't have a singularity ... no support will, in reality, create a singularly ... what you have is a high stress concentration.

this is a linear FEA, right ? the peak stress is ficticious because i the real world plasticity takes over ... your part will locally yield and redistribute load away from the stress peak. not a serious problem unless this is a fatigue load.

 

[321GO]

rb1957,

thank you, and point taken.


1) what is then the most sensible way to interpret the stress? Simply probe stresses some distance away, say 1/3 up the fillet and use as guidance?

2) stresses on the intersection do go up with mesh refinment, although the "restraint" is a line, not a point. Why does this then happen?

p.s. the stresses are highly fringed on the intersection


Again, thank you so much highly appreciated.

 

[321GO]

To clearify some more,

the material is grey cast iron, so basically no plastic yield would be present.

There is some plastic yield, but very small<0.6% and when this happens the material itself would have failed, since yield and ultimate are almost identical

 

[rb1957]

what exactly do you mean when you say "both parts", like in the balloon in your pic "high error on intersection of both parts, ..." is the FEM two pieces that are linked together ??

cast iron uh, based on what you've shown us, i'd undercut the intersection, removing the high stressed material.

any repeated loading ?, shock or impact ??

 

[321GO]

Yes, it is an asmbly, one part is restrained(in a certain way) and the part shown is bonded to this on the inner flange section.

The strange thing is that it is an actual part years in service, so that's why i know the stresses are ficticious.

 

[rb1957]

"is bonded" so there is an elastic interface between the shaft and the flange ?

i'm assuming (yeah, i know ...) that your FEm is one piece, and that the real thing is a two piece assumbly, glued or shrink fitted together. if glued than there is an elasticity that you need to account for.

 

[321GO]

Normally it is bolted together, which i simulated with the "bonded" condition(i know not 100% exact but the model would simply be unsolvable due to the size).

I made a simple test one part model with roughly the same loading and restraint.

I restrained the surface as to simulate the other part. The same high stresses occurs, which i gues is somehow due to the siff transition.

Those high ficticious stresses do not surprise me, i was wondering how far away from the "problem" area stresses can be taken for real?


Thank you again!

 

[rb1957]

ok, bolted means a discrete connection, bonded a distributed elastic connection.

if you rigidly restrain the surface you're applying an infinitiely rigid bond. if you model the two parts as one homogeneous whole, you're applying a rigid connection, completely distributed connection. both don't properly represent the elasticity of the assembly.

model the two parts as two parts; have coincident nodes or offset them 0.005" (or something small). join the two parts where you have bolts with contraint equations, RBEs, stiff beams, whatever. a discrete attachment should help the stress peak.

 

[321GO]

Yes, i agree 100% that both cases are not fully watertight so to speak.

But..

i have modelled the two parts with a no penetration contact condition(incl. friction) between them and used the actual bolts for clamping.

The results where basically the same, high stress on the intersection.


Results do seem ok some distance away, don't you agree?
Is this not a common problem?

 

[rob768]

There is obvisously a flaw in the boundary description. If this was a desing and for a gray cast iron material, the calculated stress would be unacceptable (and, based on the fact that it is a tensile stress, i'd recommend nodular cast iron).
Perosnally, I don't like tensile stress in grey cast iron at all.

 

[PriamEngineering]

I am finding it a bit hard to visualise what the complete setup looks like. Maybe you could post a picture showing the complete assembly?
As I’m sure that you are aware the Youngs modulus of grey cast iron is highly non linear. Most published data uses the secant modulus. You may have to perform a Neuber correction to get accurate stress.
Your stress level may be ok (if it’s a static load) any cycling at that assembly load will likely lead to failure (depending on load level and class of iron)
Plenty of Diesel engine blocks live happily with tensile stresses everyday.

http://www.priamengineering.co.uk

 

[rob768]

yep, but higly stressed areas are carefully avoided or carried by steel components.

 

[321GO]

The material is grey cast iron grade 250

Tensile strength 250N/mm^2 / 36kpsi.

I used an uniform E value of 110KN/mm^2 / 15.9Mpsi, which is about the half compaired to steel.

Normally i would handcalc as a check, but in this case i'm nor sure how to calculate the stress, e.a. what SCF to use for the fillet radius transition(for the simple case of tensile, see the arrow in the attachment).





p.s. what do you Guys normally use for a material model for gey cast iron? A uniform value, or a non-linear material model?

 

[rb1957]

uh ?

if this is what you input, no wonder that an N-L run didn't help ...
you need to model the elastic-plastic behaviour of the cast iron (and not use an average value) ...
E = 30E6psi up to yield (36ksi) and then you could try a zero slope but i think the math will get unhappy pretty quick ... i'd use a plastic slope of something like 1psi.

 

[321GO]

Hello rb1957,

i meant a NL-run for the non-linear E modulus of GCI.

Plasticity is not present so why would i want to model this?


In a similar post someone stated that even the stresses some distance away where not viable, do you agree wih this?

http://www.eng-tips.com/viewthread.cfm?qid=237265&page=13

Thanks to all again, highly appreciated!

 

[PriamEngineering]

I am finding it a bit hard to visualise what the complete setup looks like. Maybe you could post a picture showing the complete assembly?

http://www.priamengineering.co.uk

 

[rb1957]

plasticity is not particularly present, 'cause it's cast iron (not very ductile, hence a very shallow slope in the plastic range).

however yielding is ... the FEA will aloow everything to strain linearly whilst all is less than yield stress. once a point yields it doesn't attract more load 'cause it's now on the plastic side of the stress-strain curve. so the peak stress should limit itself to yield, removing the peak stresses you've gotten so far.

sorry, but using an average E, the way i think you have in order to come up with a vlaue of 16E6psi is just wrong, IMHO.

 

[321GO]

PriamEngineering,

no problem, hope this clarifies.

1) internal dia. of the internal hub is restrained in that only rotation is possible
2) contact condition (no penetration)between hub and disc, tried both with/without friction


I'm basically interested in wether or not the stresses some distance away from the problem zone are viable(some distance in the fillet radius).


I don't see how i can improve the setup without wondering of from the original assembly.

 

[PriamEngineering]

Thanks for that. it helps a lot. Looking at the setup. If I interpret it right, the high stress region has low error norm? If so, I believe that the stresses are real. This of course is assuming that the rest of the assembly is correctly constrained. Sure you have some high error numbers at the edge of the contact region but it looks for enough away from the high stress area to be believable. I have analyzed a few cast iron flywheels and we perform two types of analysis.

A burst speed analysis, where the flywheel must be capable to 2.5x the max engine speed.
A fatigue analysis going from 0-max RPM.

Your setup looks almost the same.

http://www.priamengineering.co.uk