PL+Pb Limits, Linearization, and FEA 3

[cab1990]

Help,

I have been explaining to my colleagues that the primary membrane + bending stress calculation found in APPX 4, section VII, is designed to prevent collapse due to plastic hinge and that it is the highest value found at the reference section (see para 4-133). I have finished a linear FEA and rather that take the liearized membrane + bending from the reference line, I am suggesting that we use the maximum SI as viewed from the SI stress distribution. There are no peak stresses in way of the reference line. My rationale is that since they are combined and reference the same allowable, no separation is required. And really the only reason the separation is required is to compare the primary membrane to its lower allowable. I'm looking for arguments for and against.

Thanks,

CAB

 

[prex]

The linearization procedure may result in a membrane + bending stress that is higher than your highest local stress: though this might seem an odd condition, it is a possibility and is a reason for making the linearization.
Of course if you don't need to check the membrane component alone (possibly because you know it is negligible), you don't need either to separate the two components. Personally I wouldn't do that, however: it is neater and simpler to present the calculations in a standard way, rather than having to explain why some checks were not necessary...

prex

http://www.xcalcs.com

Online tools for structural design

 

[MarkCopland]

main question..????..
There is not way to change a 100% radiographic examination in asme div2 for a steel casting?....that mean... for any casting a 100% Radiographic apply?....

 

[Bobfromoh]

I think you need to evaluate membrane stress and membrane+bending separately. The membrane stress component should be compared against the Code allowable stress. The allowable stress can be increased for the combined membrane+bending. Depending on the loading condition, the allowable stress can be increased by a factor of 1.5 to 3.
For instance, the 3 factor would be used to evaluate local stresses from nozzle loads.

That's how I would evaluate the stresses!

 

[daveb9]

Bob

Where does the 1.5 to 3. stress factors come from?

Dave

 

[bvi]

Those limits come from Section VIII, Div 2, Appendix 4 which provides rules for evaluation of results of detailed stress analysis. The 1.5 limit is for local primary membrane plus primary bending. About the only location where you have primary bending in a pressure vessel is in flat plats (e.g. blind flanges). The 3x limit is for local primary membrane plus primary bending plus secondary. The ilnearized bending stress in the shell at a nozzle is secondary.

 

[cab1990]

Dave, the 1.5 factor comes from the plastic hinge (see Z factor in steel manual for rectangular beam) calculation for a rectangular beam in bending. The intent is to insure that a primary load does not cause a plastic collapse failure. The 3.0 factor is an entirely different failure mode. In this case, the codes' intent is to prevent a plastic strain which will accumulate (or ratchet). When we limit the max stress to twice yield (2/3*3) then the load will follow an unloading (stress-strain) curve parallel to the original modulus without moving to the right of zero permanent strain. There is a residual compressive stress in the part and subsequent loading will have to overcome this compressive stress to reach yield again, but as long as it never exceeds twice yield it remains linear and stable.

 

[Celebur]

I have inadvertantly discovered that our valve-design calcs, based on VIII-2-App4, are done improperly, so it has been put on me to figure out how they should be done. So wading through the code for the first time, I am having similar questions.

For PL + Pb, 4-133 does say "highest value across the thickness of a section", but membrane stress is explicitly defined in 4-112f as the "average value of stress across the section". So does this mean that (average) membrane stress is to be combined with maximum bending stress?

This seems strange to me--the theorist in me wants to find worst-case stresses throughout the section instead (but I see the validity of using average stresses from a burst point-of-view)--it doesn't make sense to me that one should combine some average stresses and some worst-case stresses.

I checked to see how our sister company does their calcs, and they use bending stress at mid thickness (i.e. average bending stress) combined with membrane stress.

The same ambiguity exists in 4-134. But not in 4-135, which circumvents the problem by not mentioning membrane stress at all; rather, it states "all primary, secondary, and peak stresses", so now the "highest value" would presumeably refer to non-averaged stresses.

Comments?

Thanks!

 

[bvi]

Some day, there may actually be an ASME Code appendix that guides you on this issue, but in the mean time, there are papers, WRC bulletins, etc to guide you. Without going into some of the rather complex issues, such as what is a valid stress classification line, the basics are these.

You draw a line through the wall thickness, normally normal to the sufaces. You linearize each stress component (there are six, three normal and three shear). The average value of each stress component through the thickness (same as the mid thickness linearized value) are combined to get the membrane stress intensity.

The linearized stresses will give you a maximum on one of the surfaces (that in which the membrane and bending add). At that surface, you combine the linearized components to get the (membrane plus bending) stress intensity.

Having said all that, primary bending is rarely present in a pressure vessel (or valve) except in flat plates. Most bending in pressure components (other than flat plates) is secondary. In this case, the combination of linearized stresses on the surface gives you local membrane plus bending plus secondary stress.

If you want to up the level of sophistication a notch, you should consider that linearization typically gives some fictitious values of stress components on the surfaces, and that you should consider the real values. On the free surfaces, two values of shear (if the line is perpendicular to the surface) must be zero, and the stress normal to the surface must equal the surface traction of the pressure acting on it.

 

[prex]

Celebur,
cb4 is correct (though the first part of their last sentence is not clear to me), but trying to answer more directly to your questions:
-no ambiguity in sentences 'highest value across the thickness of a section' of 4-133 to 135: in 4-133 and 4-134 the highest value is necessarily at either wall surface, whilst in 4-135 it may be everywhere
-it is difficult to use the concepts of App.4 without a basic understanding of the underlying theory, as also suggested by cb4: if you want to go on alone, you should get some book on the subject, or at least put your hands on a (supposedly correct) stress report of the same kind as yours

prex

http://www.xcalcs.com

Online tools for structural design

 

[bvi]

Clarifying that last sentence of my last response.

On the inside surface of a pressured cylinder, from equilibrium, we know that shear (radial-tangential) and shear (radial-meridional) must both be zero. Shear (tangential-meridional) may be non zero. Further, the radial stress at the inside surface must equal the internal pressure, also based on equilibrium.

 

[Celebur]

Thanks both for the input. I do understand the theory, but ASME dispenses with theory to some degree in order to apply tried-and-proved methods as industrial codes are want to do.

A couple of more questions. I had originally assumed that "linearization" meant "averaging", but that doesn't follow. Bending stress, for example, varies linearly across the section whereas radial and hoop pressure stresses do not.

So by "linearization", do you mean that the radial pressure stress will be assumed to vary linearly from -P at inside to 0 at outside, from which -P/2 is the actual average of this linearized stress rather than just an approximation of the average of the true stress distribution?

But assuming this belies the equation for average hoop stress, which is given as PR/t; this is the equation for thin-walled pressure vessels, which is derived by assuming that the stress is uniformly distributed. Hence, it should be the average of the true stress distribution (not the linearized stress distribution). Or was App 4 done on the assumption that all pressure vessels are (or may be considered) thin walled?

What's throwing me as well is that I can find no mention of linearizing the stresses in the code (though I haven't read the whole thing).

Next, regarding bending, if I'm reading the replies correctly, you combine (average) membrane stresses with the actual bending stresses rather than actual pressure stresses with actual bending stresses anywhere across the section (this is supported by the description of bending stress on fig 4-130.1).

I do have some more questions, but maybe I should sketch out our specific problem. Our valve body may be thought of as a thick-walled cylinder with a reduction at the outlet and a nozzle at the inlet (all integrally forged).

Up to now, we used to idealize this as simply a cylinder (i.e. we ignored the discontinuity caused by the inlet). To compound matters, we simply calculated the pressure stresses, and then used the maximum normal stress (dangerous considering that we have a negative sigma 3) to compare to material yield. We did this for both design pressure (Sa=2/3*Sy) and hydrotest (Sa=.83*Sy). Fortunately, we also did distortion-energy theory at hydrotest (Sa=Sy). Note that we ignored external loadings from our calcs.

Obviously, the above method doesn't follow ASME VIII-2 App 4 at all. How would you recommend setting this up?

I have a copy of some stress calcs done by our sister company, and I'm not convinced they do theirs right either. They idealize their bodies as thick-walled clinders too. And they do the hydrotest conditions correctly (using membrane stress intensity). But for operating conditions, they assume an external axial load plus external moment. They include the stress from axial load in the membrane stress (fair enough), but they also include the bending stress at the mid-point of the section. In other words, it appears as though they are treating this like a nozzle (4-138). But no allowance is made for the discontinuity caused by the inlet (this should result in an increased PL).

Comments? I really do appreciate the help on this. I can read the code over and over, but there's danger in interpreting things incorrectly. I am also looking to take a course put on by the local ASME organization in order to gain a better understanding of how to apply this code, but in the meantime, your feedback will very useful.

 

[bvi]

Well, this will be my last respnse on this thread. You really should engage an appropriate consultant to help you on this issue.

Having said that, here is a couple more items of advice. When liniarizing, your determine what linear bending stress distribution gives the same bending moment about any abritrary point in space, as those in the section you choose.

When doing the bending moment calculations, don't forget that you have to weight average the node point stresses based on element size (e.g. if the elements are equal width across the thickness, the end nodes only count for half [because they are are attributed to halft of of the width] as the mid nodes).

When y1ou are doing membrane stress caclulations, it is a straight forward weighted average.

When you are doing membrane plus bending, you use the combined, linearized values, but should consider the actual values of the two shear and one normal stress value, previously mentioned, on the free surface.

Thats the deal. Get a consultant or WRC bulletin if you need more detail.

 

[prex]

Celebur,
as far as I can remember, the term linearization is not used in the code. The correct concepts to be used are membrane stress (the average constant through thickness portion of a stress component) and bending stress (the component of stress proportional to distance from centroid of solid section). Hence a bending stress is combined with membrane stress only at the wall surfaces, as only there the maximum stress intensity may occur.
So -p/2 is in fact a first order approximation of the membrane radial stress due to pressure in a cylinder, but you could get a better approximation by integrating the actual stress distribution(4-221). However, as this stress component is normally of minor importance, this is really not necessary (see also 4-222(c)).
Another important concept to be understood is that general primary stresses are normally easily obtained by the laws of equilibrium: the exact value for the membrane hoop stress is indeed pR/t for all (thick or thin) cylinders.
Concerning your valve body you should be able to analyse the single parts alone (cylinder, inlet, outlet), but you should also decide whether you want (or need) to do a detailed analysis (FEM). The assumptions done by your sister company are not surprising: if an external moment is present, it must be accounted for, and it will contribute to the membrane component of axial stress. Of course the discontinuity represented by the inlet opening must also be analysed: how to do that is really a matter of design analysis and I cannot go farther on that here. Note however that if the inlet opening is properly reinforced (as of course it is), this is a first positive (though not necessarily conclusive) answer to that issue.

prex

http://www.xcalcs.com

Online tools for structural design

 

[Celebur]

Thanks for the responses.

This company has been in business for 25+ years designing valves to ASME VIII-2 App 4 and API 6A (which references the former). But I've only been here a short while, and already I find that I cannot rely on learning how to apply these standards by examining what was done before.

I agree that the membrane hoop stress is exactly pR/t, but this is because of the definition of membrane stress (i.e. average stress, or resultant stress assuming uniform distribution). Actual hoop stress varies across the section according to equation in 4-221.

It seems that I am being confused by ASME's use of the term "bending". If I understand the responses correctly, bending due to external applied moments is not considered a bending stress but rather a membrane stress, which jives with the description for nozzle stresses on table 4-120.1. Therefore, the average bending stress should be used, which corresponds to the stress at half thickness, which is what our sister company does (this instills enough confidence in their procedures that I'll consult with their designers).

As I've been writing this, I've been having some "ahhs" as more things click into place. Of course, I may just be misleading myself!

I appreciate the help.

 

[cab1990]

Hello folks,

Seems this thread is catching fire, so I thought I would throw some kindling on it. First, I'd like to tip my engineering hat to everyone for asking and answering good questions(not that I haven't been anymore confused than others). Secondly, I would like to boldy predict that the global engineering community is tired of wrestling with these same issues anymore in light of the fact that we have advanced technology far past the roots of our beloved code. To support this statement, I will point you to a URL where these issues are debated and overcome by a new European proposal, Design By Analysis. You can find the whole shooting match at

http://ped.eurodyn.com/jrc/jrc_design.html

To give you at taste of the proposal here is an excerpt from the discusiion on linearization:


A technique for linearising stress was first suggested by Kroenke, W. C. Kroenke, (Classification of finite element stresses according to ASME Section III stress
categories,” Proc 94th ASME Winter Annual Meeting, 1973., and W. C. Kroenke et al, “Interpretation of finite element stresses according to ASME III,” ASME Tech. Paper 75-PVP-63, 1975)....

The ASME code is not particularly helpful on the problem of linearisation. ASME III & VIII admit a non-linear bending stress, but also contains some ambiguities: bending stress is described as a normal stress - and it is bending stress that may need linearisation. In Paragraph NB-3215 a note is provided to the effect that “.. membrane stress intensity is derived from the stress components averaged across the thickness of the section. The averaging shall be performed at the component level ...”. This implies that only stress components may be linearised (by definition this could include shear stress), and not derived principal values. However, through omission from the code, it may be argued that shear stress should not be linearised. Inclusion of shear stress linearisation will mostly affect the surface stress: in practice linearisation of the normal stress only is adopted to modify the surface stress in application of the design criteria.

Finally, I'll throw my 2 cents in on linearization. Linearization is a decomposition of the stress distribution we see in FEA of pressure vessels. It decomposes a basically parabolic distribution into a uniform value ( membrane stress), a linearly chnaging value (bending stress), and possibly an extra component (peak stress). By doing this, we can take a finite element distribution and pick one or more stress classification lines to decompose the stresses such that we can apply the code.

prex, I agree with you completly when you say that the primary stresses should be calculated by basic equilibrium calculations. We should not forget that basic fact. It's a good check on the FEA work. However, when fatigue and ratcheting are a possibility, we have the technology and should distinguish between primary, secondary and peak stresses.

 

[MarkCopland]

HI..

Somebody can explain me why the code allow value of 3 in the evaluation of stress levels.. (2/3 Sy is the definition of S ) so..if any part of the material reach this allowable stress of 3 (2 x 2/3 x S) that mean we are 2 time more than the yield point (2Sy)..so we have got a plastic deformation in the material… can someone give me a point of view about this issue, because for me,, if I reach more than the yield point this design should be rejected.

 

[prex]

MarkCopland,
this is a fairly complex matter, if you want to understand this in depth, and it is impossible to treat it in detail here.
These are some points for your consideration:
- yes, the limit of 3S[sub]m[/sub] allows for some plastic deformation: this is not necessarily dangerous for the so called self-limiting loads (e.g. thermal expansion, mutual constraint between adjacent structures) and of course this limit is only applicable to such type of loadings
- the limit of 3S[sub]m[/sub] holds for an elastic analysis; the calculated stresses may be of course quite unrealistic, but this doesn't impair the results, if the method is correctly applied
- such a limit is based onto the existence of a plastic range, the method is hence applicable only to ductile materials (metals, plastics)
- the limit of 3S[sub]m[/sub] insures that there is no increment of plastic deformation between successive loading cycles: at the first load application there is a plastic deformation, but afterwards the elastic range doubles its amplitude (to understand this you should look at the treatment of hysteretic deformation) and successive cycles will behave in a pure elastic manner.

prex

http://www.xcalcs.com

Online tools for structural design

 

[cab1990]

Mark,

The reason for the 3X limit is not to protect against yielding. The yield limits are for primary (global) membrane and bending stresses. The code allows for localized plastic straining and applies this 3X limit to these areas. What the limit actually does is guarentee that shakedown of the plastic straining occurs. Shakedown means that the plastic strains and deformations do not accumulate (ratchet) upon repeated cycling. All of this has a very solid foundation in Melan's shakedown theorem.

The practical application of this theorem goes something like this:

For pressure vessel materials, this theorem can be satisfied if the strains do not exceed ~5% true strain. Since strain is not amenable to everyday calculation, this strain limit was recast into a linear stress limit. If we look at a stress-strain curve and draw a vertical line upwards from 5% strain and intersect it with the elastic modulus line for steels, it is less than twice yield. In other words, if the linear stress at a local stress concentration does not exceed 2 times yield, then the actual true strain will be less than `5% and shakedown is assured.

Having writtten this, we must remember that this limit is only applied to peak stresses and never used for global or primary stresses. Also, we should perform a fatigue analysis whenever this limit is employed (assuming cyclic loading).

For a nice set of figures which describe the various material responses we can find in loaded structures see:

http://www.iam.rwth-aachen.de/Research/hachemi2/me1.htm

Notice figure six. This is the material response the 3X limit guarentees. The red portion of the curve is the steady state stress strain response for repeated cycling.

Hope that helps

cab

 

[HolaPronto]

To tips-eng.com

Mr. Copland

First. I am working with a FEA model of a pressure vessel with the same software than you (pro/wilfire and pro/mechanical as FEA processor). Pro/mechanical has got the linearization process, please find in the following paper How pro/mechanical perform the linearization.

If you are using 3D elements (brick-tetra etc..) you should perform the calculation of the membrane and bending stress using this methodology (witch is the more used nowadays but it is not the only one.)

If you are using another kind of elements, you need to check what output the element give to you. (stress, displacements etc..), for instance if you uses shell elements the concept of “membrane” and “bending stress” are in they “shape formulation.”

Please follow the advise from prex and cab1990, I greed with their criteria applied in ASME Div 2 “design by stress analysis”.

The following information come from the PTC web page:

““Component for Linearized Stress Results”
Use the Component option menu to select the specific type of linearized stress quantity results you want Pro/MECHANICA to display on the Linearized Stress Report dialog box. You can then view linearized stress values for different locations in your model, using the same component option.
These stress quantities apply to 2D shells, 2D solids, 2D plates, and 3D solids.
You can select from these options:
· Max Principal — the most positive principal stress
· Min Principal — the least positive principal stress
· Max Prin – Min Prin — the difference between the most positive and least positive principal stress
· Von Mises — a combination of all stress components
· Local XX — normal stress along the local X axis
· Local YY — normal stress along the local Y axis
· Local ZZ — normal stress along the local Z axis
· Local XY — shear stress in the local XY plane
· Local XZ — shear stress in the local XZ plane
· Local YZ — shear stress in the local YZ plane
· ZZ — normal stress along the local Z axis for 2D shells and 2D solids. This stress component is always 0 for 2D plates.
And
Use Info>Linearized Stress Query to display linearized stress values for integrated mode. In independent mode, the equivalent command is Query.
After you select Linearized Stress Query or Query, Pro/MECHANICA prompts you to select two locations. For each location, select a point, an edge, or the intersection of two plotting grid lines. Pro/MECHANICA labels them points 1 and 2.
The line connecting the two locations defines the X axis. For 3D models, you enter a location to define the positive Y axis.
Pro/MECHANICA displays a Cartesian UCS with the origin at the midpoint of the line between point 1 and point 2.
The Linearized Stress Report dialog box then appears, displaying the results.
“Linearized Stress Value Calculation”
Pro/MECHANICA calculates the linearized stress values with respect to a local coordinate system with the X axis aligned with the line from location 1 to location 2 and the origin at the midpoint of the line from location 1 to location 2.
Pro/MECHANICA first calculates the total local coordinate stress components at each point. It then calculates membrane, bending stress, peak stress, and total stress as follows:
· Membrane and bending stress values are obtained from numerical integration along the line between location 1 and location 2 as follows:
where:
is any local stress component
L is the distance from location 1 to location 2
· Total stress is the value calculated by Pro/MECHANICA, and the peak stress is defined by:
Peak = Total – (Membrane + Bending)
Peak, Total, and Bending Stresses vary along the line from location 1 to location 2; however, membrane stress remains constant; Pro/MECHANICA then processes the component values of these stresses at each point to obtain principal and von Mises stresses, using the standard formula for principal and von Mises stress.
Note: The formula for peak and total stress applies for each component of stress, but not for the principal or von Mises stress.
For axisymmetric models, similar formulas are used, with correction terms to account for the offset of the neutral bending axis from the midpoint.
Have a lock in the following elements library for more information about what input and what output each elements needs.

http://sc.tamu.edu/softwareDocs/ansys61/Hlp_E_SHELL63.html