Safety factor for point stress in pipe with holes

[chocolatebelt]

Hi,

We have a 6 5/8" OD pipe with 23x 1" holes drilled in a spiral. We are trying to determine that max tension limit. As expected, we see a 3x higher stress (VM) in the holes in the ANSYS simulations (according to Kirsch's Solution, 1898). However, I have been told that the max tension is not necessarily limited by this point stress, and that I should be looking at shear stress instead.

How do we set a max tension for this part and what SF should we use?

 

[dhengr]

Chocolatebelt:
Show us some sketches, with dimensions, hole dimensions, locations, spacing (longitudinal and angular), loadings, etc., so we can see what you actually have and are dealing with. Show us some of your FEA output. A 3 times higher stress concentration does not particularly surprise me, but I can’t see what you are looking at. At one extreme, if you spaced the holes 1.5" apart lengthwise, and 20̊ apart, round the pipe, you would almost cut the pipe, girthwise in a short distance. Alternatively, if the holes are spaced 6-8+" lengthwise, and at 45̊ around the pipe, I think you could work with that.

FEA programs really have trouble dealing with stress concentrations like holes or reentrant corners, etc. You don’t know how to model them (mesh them) finely enough, and the software blows up as it tries to pull the tension stress field around that tight direction change in the field direction. There is plenty of literature out there on tension fields around holes in a plate, and the like. Look at some good Advanced Strength of Materials, Theory of Elasticity, Machine Design text books. There are a couple good books specifically about these kinds of stress concentrations, one being “Stress Concentration Factors,” by R.E. Peterson. If the hole size and spacing is not too tight, you should be able to look at this, initially as a single hole in a fairly narrow plate.

One of the things that happens in a structure like this is that, while you see a high stress concentration at the hole edge; you get a little localizes yielding in that immediate area, and it sloughs off some of its stress (load) to immediate surrounding material, which is at less than yield stress, and in fact protects, absorbs, or confines the high stressed area. A more important consideration than just the red color at that point in the print out is how you drill and finish the holes. They should be smooth and clean on their i.d., and you should put a nice radius of the edges (corners) of the holes, at the surfaces on the pipe. You don’t want to leave any crack starters, stress raisers, at these high stress locations. Corrasion or erosion could end up being a problem.

 

[rb1957]

since you're doing FEA, apply a load that produces failure (how ever you define that to be) and that's your allowable load, SF = Allowable/applied ... simple ?

you could define failure as max von Mises stress = ftu ... this is IMO very conservative (if you're using a linear FEA).

you could define failure as net section yield (handcalc, (pi*d-1)*t*fty) ... probably not too far wrong.

you could define failure as max von Mises stress = ftu using a nonlinear FEA.

another day in paradise, or is paradise one day closer ?

 

[chocolatebelt]

Hi,

Thank you very much for your replies.

I do not have access to ANSYS myself, so I have to communicate with an engineer in another department (in another city) to get them done as I do not have access.

The 23x holes are 1" OD, spacing along the length of the pipe is 60mm and around the diameter 50mm. Pipe itself is 6,63"OD and 5,92"ID. Material is 13Cr80 and yield is 552MPa.

The simulations I had made were with the yield tension (kN) that applies to this size pipe. Then I could calculate what the yield based on what the max stress was manually, as it is linear.

https://www.dropbox.com/sh/eydpchirmw3v3hh/AABR2WhWKySWHwchE46JTPNJa?dl=0

I have made this link above which has VM stress, XZ stress (along diameter and length, Y axis would be into the page which is not included), and S1 and S3 stresses. Unsure about the mesh size but based on results it looks quite coarse. Lastly, finely finishing the holes was instructed in order to prevent additional stress concentrations and subsequent potential fatigue issues. Corrosion will not be an issue due to material and lifetime this pipe is under loading. It is used for about 7 hours, mostly in compression actually, but briefly in tension with at the most 40mT. However, I have to set a max tension on this for contingency reasons.

Just briefly, my background is Mech Eng, but it has been 7 years since last looking at design engineering as I am now in the petroleum sector, and I never looked at evaluating safety factors for point stresses like this.

 

[ESPcomposites]

Actually, FEA does an excellent job of evaluating stress concentrations. That is one of the best uses of FEA and some Kt values from Peterson were developed with the help of FEA. Provided the geometry is not "sharp" or there is a crack, a refined mesh will converge to the correct solution. If the geometry is "sharp", such as an internal corner without a radius, then you need to model the radius. If there is no radius in the actual design, then it may not be robust and may exhibit fatigue failure (not the fault of the FEM). In any case, true situations with a crack or non-convergent stress are fracture mechanics problems (not stress concentration problems).

So now that we identify that FEM is not the culprit, the question becomes how to evaluate the effect of the stress concentration. If you want to know the ultimate load capability (2 piece fracture) via FEM, then you would need to run a nonlinear material model. If the material is relatively ductile, then the effect of stress concentration is not very significant. The part will be about as strong as its net section. *Note - Not the case for composite laminates because they are quasi-brittle (pseudo-plastic).

Typically stress concentrations (for metals) are of practical importance when the fatigue load levels (and associated number of cycles) are significant. The difference between the fatigue strength of a part (with and without a stress concentration) is very significant. Fatigue analysis is usually performed via classical methods, but the FEM can determine the stress concentration (necessary input to the fatigue analysis) if you have geometry/loading that is unique. Otherwise, it would more convenient to get the Kt from Peterson or another source.

Brian

http://www.espcomposites.com