Burst Pressure estimation in Ansys. Solver does not stop when failure happens

[Anatoly_k]

Dear all,

I am learning Ansys and trying to estimate pipe burst pressure with FEA. I use nonlinear material as per ASME VII-2 part 5, however my solution does not stop when failure has happened. On the picture it is seen that thee pipe wall is open but I had to interrupt the solver due to endless process.

Also somehow the opening happens on one side only, despite I would expect some symmetry, what is the possible the reason?

I would also want to know how to "replace "nodes distortion with their disintegration to obtain more realistic result?

 

[TGS4]

Details?

 

[Anatoly_k]

Dear TGS4,

I have put some information together in the attached pdf.

edit:
In the solution output I also noticed the below messages which seam to be related. My understanding was that solution would stop if beyond material's max strain but it keeps going on and I even suggested to define more points. Not sure if I need to slow down the load or modify CUTCONTROL.

1)
*** NOTE *** CP = 26760.781 TIME= 06:07:16
The incremental plastic strain 16.3974692% computed in this iteration
is larger than the criterion of 15% leading to bisection. You may try
incrementing the load more slowly by increasing the number of substeps
or use the CUTCONTROL command to re-specify this criterion.

also

2)
*** WARNING *** CP = 13657.094 TIME= 02:25:38
Accumulated equivalent plastic strain value outside of bounds of
defined multilinear hardening table(s) for 618622 element integration
points at load step 1, substep 80, equilibrium iteration 4. Consider
defining more table points to cover range of behavior.
FORCE CONVERGENCE VALUE = 0.4957E+05 CRITERION= 2903.
ARCLEN NEW TIME = 0.38491 ARC-LENGTH = 87.746
EQUIL ITER 4 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= -0.5676E-01

 

[TGS4]

Three comments/questions:
1) What are your boundary conditions on the ends of the piece of pipe? if they are fully fixed, then that would tend to give some erroneous answers.
2) Have you included the pressure thrust?
3) What have you done to initiate the failure in the middle like that?

 

[Anatoly_k]

Three comments/questions:
1) What are your boundary conditions on the ends of the piece of pipe? if they are fully fixed, then that would tend to give some erroneous answers.
2) Have you included the pressure thrust?
3) What have you done to initiate the failure in the middle like that?

1) The boundary conditions are simple: just fixed support and pressure.
2) I have not included pressure trust as I just wanted to experiment with the analysis
3) I have not done anything special, even in the attached file I demonstrated that the geometry is correct, meaning there is no eccentricity of pipe walls

 

[TGS4]

By fixing both ends, you may be inadvertently causing some axial compression, leading to an actual fixed-fixed columnar buckling problem, combined with hoop tension.

Correct your boundary conditions.

 

[Anatoly_k]

I have applied the same BCs to a shell model and it is working as expected. So it is something to do with solid... I also do not get why the solution continues when deformation is beyond material properties or it is not?

 

[Anatoly_k]

I also have done calculations of a piece of pipe (corroded portion only) in frictionless supports and it ends up in similar way: solution did not interrupt somehow.

 

[Anatoly_k]

Just for information, I have activated week springs and reduced mesh density and the result is similar but not the same

 

[TGS4]

You have hoop tension, but axial compression. Fix your boundary conditions, and your buckling behaviour will disappear.

Note that typical true stress-strain behaviour is that the curve will be perfectly-plastic after the true ultimate stress. Therefore, there will be deformation after. But unless you implement an actual failure criteria (see the local failure criteria), you will see behaviour similar to what you are showing.

 

[Anatoly_k]

Thank you for your advice!

 

[FacEngrPE]

Your model is not too far from reality. Overpressurization often results in fishmouth failures. The comments above about end connection constraints while valid can be ignored if your purpose is to experiment with the software to see what kind of failures occur with different constraints.
This method is more useful for understanding the situations that lead to a failure, than for a design case where the goal is to never have a failure.