i want to do detailed 3- d analysis of pipe bend since stresses were not met in beam model analysis using caesar. Can any one suggest guidelines on transforming boundary conditions from global piping model to the local pipe bend model(force & moments or displacements & rotations-whihc one will be better) to ensure accuracy of detailed analysis.Any reference literature or case studies will be useful available,kindly suggest the required steps to be followed for proper simulation to capture detailed stress distribution

Hi, Dont think its possible to carry out the detailed 3D analysis is possible in CAESAR, You need to use detail FEA software similar to ABAQUS or ANsysis

Uday,

Exact workflow will depend partially on which software packages you intend to use and how much budget you have to consider it.

Ideally, you would model the system in its entirety in FEA to get an accurate answer.

Instead, you could put CNODE anchors on either end of your elbow in CAESAR and merely model the elbow in FEA. You're subject to the accuracy of beam analysis of the piping delivering accurate loads to your elbow.

Another option you could use is FE/Pipe, which offers canned FEA for piping.

Normally you're concerned about 3 different allowable stresses with associated loads - sustained, operating, and occasional, but you're free to run as many sustained, operating, and occasional cases as you'd like, the expectation is you ought to use the most severe of each case.

Thanks for the replies,

i have planned detailed bend analysis in ansys. suppose my bend is modeled in caesar with node number 90-100 -110 (with 98 ,99 intermediate nodes).From the results, i will get Force and moments (displacements & rotations) as output in caesar at nodes 90,100,110. From these results, i want to know which kind of boundary condition will give better results (whether fixing one end & applying absolute force and moments at other end,or applying relative displacement & rotations ).

apply displacements and rotations form CAESAR II analysis at the end of bend.
In ansys define all input parameters like wall thickness, pressure temprature etc

I think that you shall use CII results which depend on the Code calculated flexibility factors.

I suggest you include about 2ODs of straight pipe (if it is straight pipe on either end of your bend). If you end your FE model at the elbow ends and apply your displacements or loads there (at the centerline with radial components to transfer your load out to the elbow wall), you will introduce, essentially, a ring stiffener. The straight runs will remove this artificial constraint from your model.
You could anchor one end and apply the relative load or displacement at the other end.
Your FE model may (will?) produce different stiffness for your elbow. To make things more complicated, if this adjusted stiffness was inserted back into your CAESAR II model, you may get a different set of displacements/loads for your FE model.

Like Dave said, you should add some straight pipe, if any. You need to allow the bend to ovalize as much as it's supposed to.

The first thing you should do is run the FEA to calculate the K factors. you'll end up with two: in-plane and out-plane K factors.

go back to Caesar and try each K factor developed from FEA. You can only define one K factor at a time. So maybe try two runs, one with each K factor. If your stresses are okay, I think that's the end of it. If not, then you'll proceed with evaluating the stresses in FEA using the forces from Caesar analysis (forces calculated using K factors from FEA).

Calculating the K factor using general-purpose FEA (as opposed to PRG's FEBend) will take some post-processing of your FE analysis. But I don't think you should skip that step.

I tend to fix one end and apply the forces and moments at the other.

And follow the guidelines from ASME Section VIII Div 2 Part 5 in your finite element analysis. That will take you some time to learn if you haven't done it before.