Fracture mechanics analysis with residual stresses using FEA 2

[julian89]

Hi guys & girls,

I'm trying to enter the world of fracture mechanics of pressure vessels using FEAs. The first challenge I've encountered now is how to include residual stresses at weld beads?

An example of what a residual stress may look like (from API 579, Annex 9D):

I've also attached a simple ANSYS file with a shell and simple elliptical crack.

So, how does one go about applying residual stresses in a finite element model before doing a crack analysis? Is it possible to insert the residual stresses as an initial condition? To start of simple, I'd like to first have a uniform tensile stress of 10 MPa in the vertical and circumferential direction at t0 (before fracture mechanics assessment).

Julian

 

[Jay_]

Okay so lets put some ground rules.
You are saying to received your pressure vessel with no cracks originally and with PWHT if required.
And with time, probably due to cycling loading a crack appeared in the weld bead, i’m assuming you are referring to a nozzle to shell weld.
So you have two choices to make, either fixing the crack, or stopping the entire plant to do your FEA analysis and make your decision.
But why would that crack have a residual stress after years of operation?
Are you doing a research or you have a real life problem?
FYI most cracks appear at the shell to nozzles attachments.

Detailing is a hobby,

 

[r6155]

Jay_
"But why would that crack have a residual stress after years of operation?"

Do you mean that long time in service acts a stress relieving?. Why?

Regards

 

[Jay_]

No,
I’m only saying that if the vessel residual stresses were relieved during manufacturing, why would the residual stress just reappear after years of operation.
Unless he means by it, stress relaxation cracking.

Detailing is a hobby,

 

[julian89]

Guys, thanks for pitching in. Since API 579 does not allow NOT taking residual stresses into account, I think that ends the debate (for my part). Assume, for the sake of argument, that some idiot machined in a crack in the vessel during manufacture.

The intention of this post was to ask how to implement a residual stress in an FEA fracture assessment (in general terms). You may make any assumptions or simplifications if you wish, but there has to be residual stresses.

Julian

 

[mskds545]

I don't do these sorts of calculations so please do your own reading and research to confirm, but I will offer a few ideas on how you might approach this. I did not look at your model, and I am answering more generally.

1) If you want to calculate the residual stress distribution, you need to do a welding simulation. This is typically done by people that primarily do this, and I would not recommend it for a layman.

2) You cannot have a uniform residual tensile stress. Residual stresses need to be self-balancing. A uniform stress would require a net force. If you want a self-balancing residual stress, use thermal expansion. You can give a volume of material a different expansion coefficient, a different temperature, or both. Select a temperature field and set of properties that will match the canned residual stress solutions in the code. Do a lot of sensitivity studies. If the crack is in or near a sharp stress gradient, your answer will be very sensitive. If it is near a change in material properties or an instantaneous change in temperature, your result will likely not converge. If you do this, perhaps you could capture the effects of stress relief in an elastic-plastic model, but I would again recommend leaving this to an expert.

3) If you want to conservatively apply a uniform tensile stress to capture the upper-bound effect of residual stress, just apply it as a force. In the case of a cylinder, apply a pressure. When evaluating the FAD, you could just lump this in with KIP or you could run two load cases to get KIP and phi*KISR. The latter is exactly what you're doing when you use analytical stress intensity solutions. The former would be a bit more conservative. If you're planning to do an elastic-plastic model, you can't do two separate load cases, of course.

In general I would make sure you have a very strong understanding of fracture mechanics fundamentals before trying to model cracks in finite element analysis software. The software makes it so easy to create and run a model with a crack in it, especially with the advent of unstructured mesh methods. As with everything else, though, the art is in knowing how to set up the problem and interpret the results to draw a physically meaningful and safe conclusion.

And, for Jay, not all vessels require stress relief and even stress relieved vessels have some residual stress. If fitness-for-service calculations were always more expensive than finding and repairing every defect, companies would not do them.

-mskds545