pipe Junction

Hi all!

here is a pipe junction to be analysed for stresses due to 1)internal pressure
2)My,Mx and Mz.,each of them acting independently at "A"and "B". (linear static analysis).suggest me proper boundary conditions for each load case.


| A |
| |
---------- -----------
C | |
| B |
-------------------------

^Y
|
|
|--------->X

Thanks in advance.
BestRegards

 

[flamby]

Based on what I have understood from your question, I want to add that boundary conditions are definitions of the relations between the structure and its support conditions/ freedoms. It has nothing to do with loading. A fixed point remains so whether or not there are any loads acting on it.

Similarly in your case too, how these pipes are actually supported is important before you can model a boundary condition.

 

[prex]

Is this a tee?
If so:
1)for pressure calculation connect a pipe at each outlet and cap it with a flat plate (if the pipe is sufficiently long, 2 or 3 D max, there will be no influence of bending stresses at cap to pipe junction). Then support the center node of one cap (or any other node) in all 6 dof's and that's it.
1)for external moments I don't understand what you mean by acting independently and you should be more precise about this. Anyway the only restraint you can apply to a tee is at the end of a pipe connected to one main outlet, as no real tee is supported on its body. Then the moments will be applied at the other main outlet, but don't know if this corresponds to what you mean as independent
prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

flame..this is a pipe tee junction and it is not supported.Straight pipes are attached at 'c' 'B' and an elbow is attached at 'A'.I want to find stresses at the tee junctioan and I am using a solid model for it.As I can not model the entire lengths of pipes attached to this tee,I wanted to know what conditions I should consider at the boundaries.
************************************************************

Prex..thank you very much for your suggestions.

I am using a solid model of 20 noded isoperametric solid elements.

I by "independently acting " meant each of the moments Mx,My and Mz acting one at a time .Since it is a linear analysis,I feel,I can use the principle of superposition to add the stress components at the tee junction due to all the 3 moments and the internal pressure and from them find out the von Mises stress.

To apply torque on the Header what is the easiest method?

one can apply the twisting coulpe by attaching a rigid rod in +/- Z direction at 'B' and then applying on its equal and opposite forces at equal distance from the center of the header.Is there any other easier method?

I would also like to know if there is any formula to find stresses at a tee junction.

BestRegards

 

[prex]

Your model is quite heavy: it will be difficult to extract from it only the stresses that are relevant to failure analysis. Anyway it's up to you...
The torque is easily applied as a couple in the center node of the cap at B (you should cap it!).
Stresses at a tee junction are normally analized by means of stress concentration factors or with a method of opening compensation, depending on the piping code used. However the results obtained will be hardly comparable to what you get from a solid model!
prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

Prex,Thanks for your suggestions.
Could you explain what do you mean by my model being quite heavy?What other type of model can one use for this analysis?Obviously shell model is not suitable for finding local stresses.I have also modeled fillet at the junction.

Your are right...piping code gives very conservative stress values.Apart from the code equations,I want to know if there is any closd form solution for tee junction.

Thanks in advance.

 

[prex]

Well a shell model would be perfect for your problem: in modeling too much details of a structure one obtains stresses that are very complex, if not impossible, to analyse. In fact this analysis requires to separate various categories of stresses, as not all the stresses have the same importance: as an example, the stresses close to your fillet (weld?), besides being probably unrealistic, as a very fine mesh would be necessary, are relevant only to high cycle fatigue failure.
What is not clear to many people using FEM is that structural calculations based on FEM are not merely a matter of modeling a real thing: after the analysis comes the synthesis, that requires to divide the stresses into categories based on their origin and localization.
I don't know any closed form for a tee junction: if the branch is much smaller than the run, one could also use the Bijlaard solution (WRC107 and WRC297) for a nozzle on a cylindrical vessel, but anyway it is in table form, not really closed (see the site below for WRC297).
By the way I don't intend to say that piping codes give very conservative results. On the contrary they generally give something which is very close to the required thicknesses, based only on primary stresses, the only ones relevant to failure under pressure. In your model you'll find much higher stresses, as also secondary and peak stresses will contribute.
(Please excuse the sermon...)
prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

Well,Why do you think the stresses near the weld become unrealistc? All that one has to do is to model the fillet weld carefully.Yes ,very fine mesh is required if one uses linear solid elements but if one uses 20 noded solid element,the mesh need not be superfine.And then whatever stresse appear there for a give set of loads,one has to take them in good spirit.

The very purpose of doing a 3D stress analysis is to find out the accurate stress distributin near the discontinuities(whether they are gross structural discontinuities like the case in point ,or other local discontinuities).Here I must mention that my analysis results go into fatigue life analysis.Also my tee joint(!)is not an ordinary tee joint.It is a class one component as per ASME SecIII classification.And I have to design it according to ASME secIII,Divison -I,subsection NB.Thats why I need to tak einto account all primary membrane,primary bending,and secondary stresses into consideration.


The point I would like to mention is that a shell model can never represent stress distribution at discontinuties like a pipe tee joint correctly,unless the mesh is superfine...even then I doubt its credibility.

If one is interested in only primary stresses ,one can simply use a piping analysis package to satisfy codal equations.Like I said,the very purpose of doing 3D analysis is to find all the local stresses correctly.

Thanks for your info.

 

[prex]

OK, if you need the peak stresses for a fatigue analysis, of course you need a very detailed 3D model, but there are many comments that come to mind:
-the fillet weld is a local discontinuity, not a gross one; the tee junction, instead, is a gross one of course
-the distribution of stresses near a weld, with all the inevitable shape imperfections of a real weld, cannot be realistically analyzed for high cycle fatigue purposes: it is preferable not to include the local effects in the model (that's why shell elements may be better suited) and to account for them with engineering intensification factors
-if you don't believe me, try a second calculation with a finer mesh: you should see sharp changes in local stresses that will make your analysis a bit unstable...
-if your weld is neatly ground off, then it's different, but your local stresses will still critically depend on the local fillet radius.
Just out of curiosity: how do you intend to classify the stresses generated by the tee junction into primaries and secondaries, and how are you going to distinguish them in your model?
prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

Prex,

your first comment:its true.

second comment:The purpose is not high cycle fatigue life calculations(the tee is not like a rotating shaft in a high speed machine..its never used like that).It is a low cycle fatigue life calculations,say only for 30 to 40 cycles in its life time,primarily coming from thermal stress cycles due to plant shut downs and start ups.and ofcorse ,earthquake cycles if it occurs.

If the fillet(whether its a weld or simply a pull out from run pipe)IS NOT modeled,then I agree..that shell elements CAN be used.My comments regarding unsuitability of shell elements in my earlier post stem from THEIR UNSUITABILITY TO MODEL A FILLET (weld/pull out) where the fillet thickness itself is changing.

Third comment: I modeled the fillet with very fine mesh and did convergence studies.and found no sharp changes in local stresses(the very meaning of convergence )

4th comment:who doent agree that local stresses depend onfillet radius?Once fillet radius is fixed as per design,it is no more a variable in analysis.

last one:well,for fatigue life analysis(he primary purpose of this 3D study) I need only the peak stresses(whatever may be its causes) araising from MX,MY,MZ(they can come from for eg. DEAD weight load in which case they are grouped as primary,or they can from for eg.thermal expansion and seismic anchor mation etc in which casethey are secondary)

These terms Primary and Secondary are relevant for general piping layout codal qualification according to,for eg, Eqs 9,10,11,12 and 13 of ASME SecIII,DIV I-NB.

For finding peak stresses I apply Mx,MY,MZ(whatever may be their category-primary or secondary)and also internal pressure and then,as I said earlier I wud calculate stress components first,sum up each component for different loads,and from these summed up comonents I wud calculate von Mises stress.(since von Mises stress cant be superposed from different loads)

So everything is crystal clear.and ther eis no confusion at all.

BEST REGARDS.

 

[prex]

I have some further comments on what you're planning, but, of course, if you don't need any advice just tell that.
1)The term peak stress is used in ASME III-1-NB as a separate item with respect to primary and secondary stresses. Peak stresses are due to local discontinuities only and are not relevant to low cycle fatigue (ratcheting) analysis: so you should keep them off from your model, unless you want probably unrealistic and for sure very conservative results
2)The equations you reference are meant to be used on the results of a flexibility analysis, where the piping system is represented with 1D pipe elements.
3)What I understand you are doing is in fact a detailed analysis per NB-3200: if you go there and study it in depth, you will see that the classification of stresses into primaries and secondaries is not a matter as easy as you seem to consider
4)In my opinion, to do that classification, you should consider the run of your tee as a shell, the branch as a nozzle, then go with the typical classifications of table NB...(don't remember the reference) and try to find those that apply to your model. prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

(smiles)

Prex,

Thank you very much for your comments,concern and for taking so much interest in my postings. Your valuable comments are always welcome.

At the moment I am concerned with NB-3600(more specifically NB-3650) which deals with piping design.

I would like to Idraw your kind attention to NB-3630 ,paras(b)and (c) which say" ..within a given piping system,the stress and fatigue analysis shall be performed in accordance with one of the methods given in NB-3650,NB-3200 or appendix-II....When a design doesnt satisfy the requirements of NB-3640 and NB-3650,the more detailed alternative analysis given in NB-3200 or the experimental stress analysis of Appendix-II may be used to obtain stress values for comparison with the criteria of NB-3200".

So I am at the beginning .If necessary I will have to go to NB-3200,which is a much more detailed analysis.

I want to check NB-3653.2(satisfaction of peak stress intensity range--EQ (11) and from there to go to NB-3653.3 to NB-3653.5.Eq(11) can be checked from the results of flexibility analysis.I am going a bit further and doing detailed 3D analysis of this tee for use within NB-3600 and not in NB-3200.If fillet is not modeled,one can go for shell model and apply a stress indice.I will also check that.I have curiosity to see the results from 3d analysis ,shell model and results from EQ11.I hope you understand where I am presently standing.This is only beginning of the beginning of al ong journey.

And I always consider any kind of advice given to me.

with est regards,
BestRegards

 

[prex]

Good luck and keep us informed! prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

Sure!
Thanks!