## Correct Interpretation of Stress Linearization Ansys/Sec VIII

## Correct Interpretation of Stress Linearization Ansys/Sec VIII

(OP)

When interpreting solid models in Ansys in relation to allowable stesses of Sec. VIII Div. I, is the following methodology reasonable for primary stresses?

1. Excluding discontinuiies in the structure, locate the section that appears to have the highest stress by a Stress Intensity or von Mises plot.

2. Locate the two surface nodes which most accurately "draw" a stress classification line normal to each surface (if possible). These nodes define the path that the stresses are linearized.

3. This is where I get hazy. Find the linearized membrane stress for each of the three normal and three shear and add them together algabraeically. Do the same for the linearized membrane+bending stress at each surface and take the larger of the absolute value of the two.(someone suggested in a previous post that it might be accurate to exclude one or more linearized results from the shear components at the surface?)

4. Repeat 3 for a few locations in the vicinity to ensure the max. value was captured (is this essential as this process is quite laborious in Ansys?)

5. Structure is OK if B+M <= 1.5Sa and M <=Sa . However 1.1M<=Sa is OK over small areas, so step 4 would be necessary if Sa<M<=1.1Sa.

Finding the linearized stresses in Ansys is a pain, particularly picking 2 nodes in a sea of nodes. Would like to know if anyone has any time-saving ideas there.

I would like to know if anyone has any conservative rules of thumb, as a quick check, that would ensure I'm in compliance with the membrane and bending stress criteria. Would averaging the values of von Mises or Stress Intensity at the 2 surfaces at the section in question and comparing this value to the allowable stress, Sa, be appropriate?.

Thanks,

Chris

1. Excluding discontinuiies in the structure, locate the section that appears to have the highest stress by a Stress Intensity or von Mises plot.

2. Locate the two surface nodes which most accurately "draw" a stress classification line normal to each surface (if possible). These nodes define the path that the stresses are linearized.

3. This is where I get hazy. Find the linearized membrane stress for each of the three normal and three shear and add them together algabraeically. Do the same for the linearized membrane+bending stress at each surface and take the larger of the absolute value of the two.(someone suggested in a previous post that it might be accurate to exclude one or more linearized results from the shear components at the surface?)

4. Repeat 3 for a few locations in the vicinity to ensure the max. value was captured (is this essential as this process is quite laborious in Ansys?)

5. Structure is OK if B+M <= 1.5Sa and M <=Sa . However 1.1M<=Sa is OK over small areas, so step 4 would be necessary if Sa<M<=1.1Sa.

Finding the linearized stresses in Ansys is a pain, particularly picking 2 nodes in a sea of nodes. Would like to know if anyone has any time-saving ideas there.

I would like to know if anyone has any conservative rules of thumb, as a quick check, that would ensure I'm in compliance with the membrane and bending stress criteria. Would averaging the values of von Mises or Stress Intensity at the 2 surfaces at the section in question and comparing this value to the allowable stress, Sa, be appropriate?.

Thanks,

Chris

## RE: Correct Interpretation of Stress Linearization Ansys/Sec VIII

Also in your procedure you don't mention the most difficult (IMHO) point in this type of analysis: the distinction and separation of primary stresses from secondary ones. In a complex 3D structure (why use a solid model for a simple structure?) there will always be some mutual constraints between the adjacent parts of the structure and so non negligible secondaries superposed to the primaries. Once again primary stresses (M+B) should always be determined by a simpler analysis and the solid model used only for primary+secondary stresses.

About your points:

1)Can't see how you can determine the highest stress excluding discontinuities, as the stress will normally steadily increase from 'calm' zones (where a simpler model would possibly be used) to the discontinuities, without any separation indicating where the discontinuity begins. Also the point with the highest local stress will not necessarily indicate the section with highest averaged stresses.

2)The line trough the thickness is not required to be normal to the surfaces (this is not possible, by the way, when the two surfaces are not parallel)

3)Correct. Personally can't see how some of the stress components could be withdrawn. One can note that general primary stress distributions are normally composed of direct stresses only or of shear stress only: when a mixup of stresses arises, this is often due to the fact that a more complex stress distribution is under examination, that contains secondaries too: however the procedure of excluding some of the stress components is certainly not correct to separate the secondaries from the primaries.

4)Ansys has a builtin feature for calculating linearized stress components (however when I used it far in the past, I found it giving incorrect results). Of course you must look for the maximum of stress indicators, so some kind of trial and error is inevitable.

5)Can't see where the limit 1.1S

_{a}comes from. This limit is only used for determining whether a primary stress is local or not, but the limits are 1.5S_{a}for a local primary membrane stress intensity and S_{a}for a general one.My position on your concluding remarks is that a complex solid model should be never used alone for a pressure vessel part: some simple rules of thumb would normally permit the calculation of general stresses, an axisymmetric or thin shell model would allow for determining areas of local stresses and primary+secondary stresses, and a solid model should be reserved to the analysis of peak stresses and of complex interactions (e.g. thermal stresses).

prex

http://www.xcalcs.com

Online tools for structural design

## RE: Correct Interpretation of Stress Linearization Ansys/Sec VIII

Wouldn't implementation of "Step 4" result in a sort of stress classification plane rather than "line" and permit you to get some sort of average M, M+B for the structure in this area? With certain loading and structures I think it's pretty hard to equilibrate external loads (e.g., the single anchor ring I brought up in another post) without making a lot of assumptions and having to err on the very conservative side.

By my statement "excluding discontinuities" I meant secondary stresses, which is pretty hard to do without a bit of judgement, isn't it?

1. Isn't this where a bit of that judgement comes into play? At what distance from a weld or other abrupt change in geometery does one consider the secondary stresses to have been attenuated sufficiently such that you're looking at just primary stresses? Would it be appropriate to have an initially quite coarse mesh to identify areas of high primary stresses and then further refine this area rather than that of a weld or abrupt geometrical change(for instance) to help avoid inclusion of secondary stresses?

2. Correct. I was thinking about cylindrical shells which I normally deal with.

4. By "looking at maximum of stress indicators" do you mean indentifying sections of interest by stress intensity or von Mises surface plots?

5. Right.

The problem is that for many of the structures I'm looking at a shell model is inappropriate due to large thicknesses and small diameters. Also, axisymmetric models are not possible because of how the structure is loaded.

Often times I have to determine thicknesses, weld sizes, etc. when a project is in the quotation stage. It is obviously not practical to do a detailed analysis for each quotation that comes my way. That's why I was asking for a rule of thumb that would err on the conservative side and if the project was won, a detailed analysis could be performed. For example, if I ran a model with a 5% convergence criterion and all von Mises (or SI) on a surface plot were below Sa (not even approximating a quasi-average by looking at the surface plots on both sides of a section) would the structure be OK for quotation purposes.

It is sometimes more economical to err on the conservative side. Is it worth tying up an analyst for a few hours or days in order to shave an 1/8" or 3/16" off of a pipe thickness, not to mention delaying production while drawings are finalized? Time constraints and staff shortages are another roadblock to a thorough, detailed analysis.

BTW, all of the structures that would be analyzed in this manner are subjected to a shop hydrotest. Although this is no substitute for proper analysis, it can help validate the analysis by strain gage measurment or identification of gross structural deformations.

Thanks for your input.

## RE: Correct Interpretation of Stress Linearization Ansys/Sec VIII

Where I agree less is on the difficulty of applying the equilibrium laws: in your example of the support ring the general primary membrane component is simply the weight divided by shell section area (assuming the weight transmitted above the support as negligible), and the local primary membrane may be conservatively estimated with the procedure I suggested in another post. That's all for primary stresses: all the rest is secondary and may be calculated either by formula or by FEA.

Also do not agree very much on the judgement required to separate the secondaries: there is no space for judgement there, primary is primary and secondary is secondary. If you can't separate sharply the two contributions, then you should classify the total stress as primary (but of course this can be very uneconomic!).

Concerning the quotation stage, I would never try to estimate the mass of the equipment by a FEA model (unless it is a standard type of vessel, where only some dimensions change from one equipment to the other): calculations based on formulae would normally suffice, the detailed analysis being reserved, in case of order, to critical localized areae.

And of course I agree with you that very often it costs much less to make simple conservative calculations than to refine the design with costly analyses.

prex

http://www.xcalcs.com

Online tools for structural design

## RE: Correct Interpretation of Stress Linearization Ansys/Sec VIII

Chris

## RE: Correct Interpretation of Stress Linearization Ansys/Sec VIII

The procedure for getting the membrane SI at a section is:

1)You have the six stress components specified at every point along the segment representing the section

2)Take the average of each stress component. In formula:

σ

_{im}=(∫σ_{i}dx)/twhere t is the length of the segment and x is the abscissa along the segment (Note:that formula is not exact for axisymmetric models).

Now you have a single set of six (membrane) stress components

3)Determine the principal stresses of that set

4)SI is the absolute value of the largest algebraic difference of the principal stresses taken 2 by 2

For membrane+bending the procedure is:

1)as above

2)Take the average static moment of each stress component. In formula:

σ

_{ib}=(∫σ_{i}(x-t/2)dx)/(t^{2}/6)Now you have a single set of six (bending) stress components

3)Calculate two sets of m+b stress components at each segment end as:

σ

_{i(m+b)1}=σ_{im}+σ_{ib}σ

_{i(m+b)2}=σ_{im}-σ_{ib}4)Determine the principal stresses for each of the two sets

5)Calculate SI for each of the two sets of principal stresses and take the larger value as the M+B stress intensity

prex

http://www.xcalcs.com

Online tools for structural design

## RE: Correct Interpretation of Stress Linearization Ansys/Sec VIII

Chris

## RE: Correct Interpretation of Stress Linearization Ansys/Sec VIII

Leonard

## RE: Correct Interpretation of Stress Linearization Ansys/Sec VIII

prex

http://www.xcalcs.com

Online tools for structural design