×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

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

Jobs

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

How far from a singularity is far enough...

How far from a singularity is far enough...

(OP)
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!


 

RE: How far from a singularity is far enough...

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.

RE: How far from a singularity is far enough...

(OP)
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.

RE: How far from a singularity is far enough...

(OP)
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

 

RE: How far from a singularity is far enough...

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 ??

RE: How far from a singularity is far enough...

(OP)
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.
 

RE: How far from a singularity is far enough...

"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.

RE: How far from a singularity is far enough...

(OP)
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!

RE: How far from a singularity is far enough...

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.

 

RE: How far from a singularity is far enough...

(OP)
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?


 

RE: How far from a singularity is far enough...

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.

RE: How far from a singularity is far enough...

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.
 

www.priamengineering.co.uk

RE: How far from a singularity is far enough...

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

RE: How far from a singularity is far enough...

(OP)
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?



 

RE: How far from a singularity is far enough...

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.

RE: How far from a singularity is far enough...

(OP)
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&amp;page=13


Thanks to all again, highly appreciated!




 

RE: How far from a singularity is far enough...

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?  

www.priamengineering.co.uk

RE: How far from a singularity is far enough...

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.

RE: How far from a singularity is far enough...

(OP)
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.

 

RE: How far from a singularity is far enough...

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.
 

www.priamengineering.co.uk

RE: How far from a singularity is far enough...

(OP)
Hello guys,
to get better results i modelled the inner hub as an elastic wall condition(in SW CosmosWorks).

The results seem much better, no ficticious high value's, this seems to be the solution.

problem is that i'm not familiar with these elastic supports at all and what value's to use?!

Initially i used a value 0f 1e12 N/m^3, somewhat based on the equation:
E/t, where t is the thickness of the wall.

To be honest this value is nothing more than a guess, as i said i'm not familiar with these supports.

I needed to make several re-runs(with lower wall stiffness value's) to get results without the ficticious value's, basically had to massage/soften the restraint...

Does this practice of re-running with lowered siffness make sense to you guys?

p.s. first image in the attachment shows the small displacement in the x-direction, which is apparantly enough to prevent the singularity





  
 








  

RE: How far from a singularity is far enough...

(OP)
priamengineering,

great to hear that you are doing some familiar setups.

Yes, the uper part of the fillet is error free, but
the transition is right on the tangent part of the fillet, basically the intersection ends a the start of the radius.

So, as a result the stress on the bottom part of the radius are obviously wrong. So then i'm basically forced to make a judgement call as to from where in the fillet the results are valid again.

On the second setup i don't need to mak ethis judgement call, since the sress looks ok along the whole fillet.
the second setup however does make some simplifications regarding the contact though, so it is also not 100%.

On this second setup the stresses are roughly half up the fillet as opposed to the initial setup where the highest stress occurs in  the start(low end) of the fillet.

When disregarding the abnormal stress region in the initial setup, both setups do somewhat correlate.  

RE: How far from a singularity is far enough...

With rb1957 here.

You seem to be reporting a "stress level" of 113MPa for grey iron, UTS 250MPa using a linear run. What you've actually got is a stress level for an elastic material for whatever E you've typed in. Stress-strain curve for grey iron isn't linear, and there is a massive difference between its behaviour in tension and compression. You need to account for this if you are seeing stresses above where (a) the stress-strain curve is linear and (b) the tension and compression curves diverge. The attachment gives an example of the type of modelling approach required.

I think you need to step back and get the material properties into the model correctly as a first step. Also, once you've got your constraints correct, remember that grey iron has a low fatigue stress concentration factor!

 

RE: How far from a singularity is far enough...

RE:how far is far enough from this singularity for the stress to be uneffected?

I deal with models that have high stresses at constraints,attachment points, and load points all the time. If I see stresses that exceed yield in one of these locations, the first thing I do is look at the mesh in that region and see how many elements away from the singularity does the high stress region extend(as a quick rule of thumb, I don't get concerned unless the high stresses extend more than one element beyond the point of load application or constraint). I also look at how quickly the stress drops at adjacent nodes.  If the stress falls off very quickly that is a good indication that what you are seeing is not exactly real.  As a further test of realness, I will refine the mesh in the area in question and rerun the model.  If you truly have a singularity, the high stress region will shrink and your peak stress will increase.  Theoretically as your elements become infinitely small, the peak stress will grow to infinity.  On the other hand, if the size of your high stress region is mesh invariant, the stresses are probably real. However, this is not exactly the end of the world.  If you can determine that the high stress is localized yielding, and you can live with it, there is probably no need to refine the design.  As an example, I was analyzing a bracket that holds some electrical switches.   The FEA model (shell elements) showed that the stress due to a shock event exceeded yeid in the region near where the bracket bolted to the foundation. I refined the mesh and determined that the stresses were indeed real.  Next, I calculated the bending stresses through the thickness of the shell.  This showed that yield was only exceeded at the outer fibers of the shell, and that the bulk of the material thickness was below yield.  I took it one step further and calculated the shear stress.  I did this and made the claim that since the shear stress was below yield, the screw heads that hold the bracket will not tear through the material under load.   I explained it away as possible "localized yielding" that would not effect the function of the bracket. This may not apply to your case, but maybe it will give you something to think about in dealing with these types of high stress regions in your models.
 

RE: How far from a singularity is far enough...

Check this out:
http://machinedesign.com/print/75312
Talks about singularity and how to get around them...

Tobalcane
"If you avoid failure, you also avoid success."  

RE: How far from a singularity is far enough...

(OP)
rb1957,

thank you for the cast iron material document, great stuff.


Generally the transit between linear/non-linear is about half way up the curve to my knowledge at least.

APart from the (fairly)high stress fillet area, overall stresses are low.
To my understanding the only location where my linear assumption could go faul would be in the high stress fillet area.

But even then, isn't the linear assumption conservative because it overstiffens the fillet area(and thus overstress the results)?


rb1957, i'm not trying to fight your point as i fully agree with it, it is just that my software cannot run non-linear stuff so i'm bound to the linear model.


Furthermore i'm doing a compare study on different concepts of this part, with slight modification(but not in the fillet area) and thus exact stresses are not the main objective.





   

RE: How far from a singularity is far enough...

if your software does linear analysis ... do a linear elastic analysis, E = 30E6psi.  thinking about this, it might not change the results at all, since you're looking at stress ... it'll change the strains for sure.  but fudging E to "account" for plasticity is just 'rong, IMHO.

you seem to have found other modelling solutions for the localised stress peak.  if the part's in-service and has seen (regularly ?) this type of load then you know the part is reasonably ok.  if it is a seldom occurrence then possibly the few specimens that experienced the load were over spec.  possibly the load is not experienced in service (like airplane ultimate loads), then you should look at a typical service load.  

RE: How far from a singularity is far enough...

(OP)
Thumbs up to you all! The feedback is priceless.



 

RE: How far from a singularity is far enough...

321GO

In response to your post... 15 Apr 10 13:26.

I think you can work upto about 25% rather than 50% before the curves diverge, so upto around 25% of UTS you should be fine with your linear model.

If you end up having to do some fatigue analysis, remember my earlier point about grey iron having a low fatigue stress concentration factor (otherwise you could worry yourself unnecessarily).

Furthermore, grey iron casting tensile strength varies with thickness. EN1561 says that a separately cast sample of grade 250 iron must (and this is mandatory) have a UTS between 250 and 350MPa. It then gives anticipated (ie expected, and not mandatory at all) values in "real castings" based on section thickness as below:-

Thickness, upto (mm)      UTS (MPa)
       10                    250
       20                    225
       40                    195
       80                    170
      150                    155

Working with grey iron is a lot more complicated than people think you know!

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!


Resources