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!

 

[321GO]

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

 

[321GO]

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.

 

[sdra2]

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!

 

[spongebob007]

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.

 

[Twoballcane]

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."

 

[321GO]

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.

 

[rb1957]

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.

 

[321GO]

Thumbs up to you all! The feedback is priceless.

 

[sdra2]

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!