Analysis approach 3

[Hurricanes]

I have a bit of a personal interest problem I am hoping some of you guys can help me out with. I am mainly a piping guy, my pressure vessel knowledge is distinctly lacking (so forgive me if any of the following is stupid).

I was reading an old report (~3 years old) produced by my company on the analysis of a cyclone which had some excessive localised deformation. The report raised a few questions in my mind with regards to the analysis approach taken. Unfortunatly the engineer who did the analysis has since moved on, so I thought I might see if I can get some comments from people in the know on here.

Some brief background, a set of cyclones in an industrial plant all displayed the same localised inward deformation on one side. This side of the cyclone was below where the outlet chute connected into the cyclone resulting in unsymetric gravity loads acting on the cyclone. The cyclone contained hot gases at ~900 degrees C and was under a slight vacuum -1kPa or so.

Basically the engineer was asked to analyse the cyclone and determine the cause of the localised deformation with an eye to rectifying it.

Working through his analysis, first he did a thermal analysis (the cyclone was lined) to see what the temperature at the cyclone shell might be. He then used this to determine the thermal expansion.

In the stress analysis he simply 'summed' the expansion, gravity and pressure loads as the operating load case and looked the the von Mises stresses comparing them to yield. This was all done in a FE package.

The question I have, leaving aside the more complicated matter of cycles and what not for now, is this;

Technically the cyclone is not a pressure vessel (at least according to AS 1210 it is outside of the range of pressures within which you must analyse it as a pressure vessel), but is it smart or correct to just look at equivalent stresses and compare them to yield?

Would a better approch not be to go off BPV VIII Part 2 and look at the membrane and membrane+bending stresses and compare that way?

Sorry for the long winded post, I guess I am really just asking, how would you approach a problem like this?

 

[EngAddict]

Comparing to yield is a pretty standard comparison for structural work. AS1210 is not really that different but has an allowable stress of UTS/3.5 or Yield/1.5, which ever is lesser.
It depends where the stress is located and how it should be classified.

There is nothing wrong with using a vessel code to design a cyclone even if it is not required to do so. There is no need to use VIII-2, AS1210 has a similar section.

Sounds like it has buckled in the shell, in this region I would limit the membrane stress to 'f'. It doesn't matter whether you use AS1210, ASME VIII-1 or VIII-2, this requirement is the same.

Was his yield comparison based on yield at temperature? I would calculate my allowable stress based on yield at temperature / 1.5 for this analysis.

 

[TGS4]

In my opinion, the originating engineer, Hurricanes, and EngAddict all have the wrong approach (although EngAddict started to point you in the right direction).

So, you have a component that "failed", right? You want to figure out what happened, so that you can modify the design so that it doesn't happen again, right?

So, you have a plethora of failure modes that you can examine. as a first pass, I would start with the failure modes in ASME FFS-1 / API RP-579: Plastic Collapse, Local Failure, Buckling, Ratcheting, and Fatigue. We really can't start talking about classifying stresses or comparing against limits until we actually understand that failure modes, and how there would act to cause the damage that was observed.

So, was there cracking in the metal? Was there any cracking in the refractory? Other signs of degradation in the refractory? Was the "local deformation" sufficient to cause a noticeable change in performance (or was this an aesthetics issue)? Were there any external loads applied at or near the deformation (or was there the potential for external loads if there was sufficient displacement during operation)?

Once you've answered these (and hopefully a whole lot more similar) questions, then you can start to pick up your pencil and start examining the various failure modes. Once you have outlined a plan on how to evaluate the cyclone for the various failure modes, then, and only then, should you start your FE program. By this time, you will know what you are looking for in the post-processing, and can tailor your analysis in the pre-processor to work towards finding that.

Remember, to start with you're trying to figure out what happened, so concepts such as allowable stresses are essentially meaningless. Actual, at temperature, material properties are useful.

 

[EngAddict]

To clarify I was assuming a particular method failure based on what he had described. Therefore, as a starting point I would check the previous design against the allowable stress to see if there is a gross miscalculation that caused the failure. If it occurred because he undersized the shell then there is no point in investing days doing a detailed fitness for service audit of the cyclone.

If that is not the case then you will need to start working through the other failure modes. Most of these can be ruled out purely by observation anyway.

 

[corus]

It would be wrong to simply combine all the mechanical and thermal loads and compare the stresses against yield as each stress categroy has different limits. Mechanical plus thermal stresses, for example, have a limit of twice yield on the stress range.

You must also consdier the thermal expansion of the lining and the pressure load that that imposes on the outer shell. in some cases you may have to consider the axial expansion as well as radial. These stresses can be considered as secondary as they are self limiting, but some codes define them as primary, with the appropriate stress limits.

If it's at high temperatures then you'd have to consider a transient thermal analysis as the differential thermal expansion stresses between the shell and lining can be initially high before reducing to a steady state condition as the mechanical properties of the lining material change with temperature.

Local distortion could have occurred due to a failure of the lining causing localised high temperatures. These could cause localised buckling of the shell. Do a google for 'hot spots' as there are methods for assessing these.

 

[Hurricanes]

Thanks for the replies.

TGS4,
The cyclone hadn't 'failed' but it 'looked bad' and the client was worried the localised deformation would worsen leading to failure. The engineer seems to have started off along the same track as you have suggested. He initally thought it was a buckling failure and ran a linear buckling analysis. This analysis indicated that the cyclone shouldn't have buckled.

So he moved on, looking at thermal cycles. Long story short, the area in question yielded slightly over a single thermal cycle. He then assumed that cracks etc in the refractory may have lead to higher temperatures in this area and greater yielding. That was pretty much where the report ends with regards to how the localised deformation happened.

The second part of the report deals with some possible migation methods, mainly using ring beams to stiffen up that area. This is where he just compared von Mises stresses resulting form expansion + gravity to yield, and where like Corus suggests, I think he may be incorrect.

So, if you guys were to do this, would some thing like this be your methodology?

- investigate possible failure modes
- check for any cracks, abnormalities etc in the shell and refractory
- check loading conditions, possiblity of material build up inside the cyclone etc
- determine which loads/combinations drive which failure modes
- analyse for each failure mode

Should a non-linear geometry analysis have been done? From my understanding, any deformation greater than half the thickness of the plate elements used indicates that a nonlinear analysis is required, for any decent level of accuracy.

 

[corus]

It could be possible that the deformation of the shell would cause the refractory to open up and allow heat through to the shell. In that case you'd need to a large deformation/plastic analysis. What is common with refractory linings is that if the hot face is cooled too rapidly then the hot face opens up, which can again cause local hot spots. As I said before though, the critical period for stresses is in the initial stages where the hot face causes a large radial deformation whilst the stiffness of the refractory is high. This causes large stresses in the outer shell. Later the mean temperature of the refractory increases and its stiffness reduces, and hence the stresses in the shell also reduce to a steady state condition. You can reduce these initial stresses by inserting a thin layer of soft material which will take up the initial thermal expansion of the refractory.

 

[Hurricanes]

Thanks Corus. So if you were doing this, would you try and model the refractory as well?

The refractory was modeled in a seperate analysis to determine the mean temperature at the shell, but the model used to determine the deformations and stresses only incorperated the shell using plate elements.

Large deformation was not included as the FE package he used (Strand7) would not converge in this case. We now have Ansys and I am considering re-doing his analysis in my own time using it.

 

[corus]

A way of including the effects of the refractory is to first run a 2D plane strain axisymmetric analysis of the refractory and shell from which you can calculate the pressure load from the refractory, as well as the shell temperatures. For this you'd need to know the temperature dependent material properties of the refractory, which isn't that easy to get.

A better way is to run a 2D axisymmetric analysis of the shell and refractory but treat the refractory as a homogenous material with no joints. Any opening of the joints could be seen by looking for tensile stresses in the refractory material. It'd be virtually impossible to model joints opening and heat penetrating into the shell so any such 2D analysis would be merely indicative of where a problem might occur.

I've not used Strand7 but Ansys might be better at getting a converged solution. Problems with convergence are often due to some localised problem in the model which may be overcome by improving the mesh or convergence parameters.