Convergence problem

highpressuretube

Hello,

I am trying to see beforehand how a 41mmx55mm square profile will behave close to bursting. Roughly estimated burst pressure was set to 40Mpa, however my model starts diverging already at around 2,85MPa inner pressure. Please don't mind the mesh. Meshing is too fine - I have just been experimenting in refining it a couple times with the same result, i.e. early divergence.

I am sure there is some simple mistake in units, bc's or code employment which I just don't see. Could someone have a look? I am already blind from looking too many times.

MED, COMM and MESS attached.

Thanks a lot in advance,

Katrin

Attached file:
SquareProfile.zip, 156843kb

VincentMagnenet

Dear Katrin,

I've had a quick look at your comm file, what happens if you increase the parameter D_SIGM_EPSI ?

Try for instance D_SIGM_EPSI=0.2 * E, with E the Young's modulus.

(For now, your hardening modulus is only 0.00529 times your Young modulus).

highpressuretube

Dear Vincent,

thanks for the reply. That got me thinking that I plugged engineering stress vs. eng. strain into the material model instead of true stress vs. true strain. Is there a general rule of thumb up to which degree of deformation and which behaviour models one may still use with eng. strain? Problem is that mostly true strain data is not available. I will try to get those values for my material anyway. Should just be a question of time.

Until then, I used your suggestion of D_SIGM_EPSI=0.2 * E. This postpones my divergence problem to a later stage. I reach about 9.9 MPa. Since this is still far away from rule of thumb burst pressure I fear there is a different problem still - not only material curves.

What really bugs me is that I am not only not converging (i.e. algorithm parameters), but really diverging quickly:

Instant de calcul: 7.423443603977e-01

---------------------------------------------------------------------

---------------------------------------------------------------------

| 0 X | 2.42741E-06 X | 3.18654E-01 |TANGENTE |

| 1 X | 2.42753E-06 X | 3.18672E-01 | |

| 2 X | 6.31498E-06 X | 8.28983E-01 | |

| 3 X | 6.32372E-06 X | 8.30142E-01 | |

| 4 X | 2.03235E-05 X | 2.66787E+00 | |

| 5 X | 2.08268E-05 X | 2.73406E+00 | |

| 6 X | 6.56080E-05 X | 8.61184E+00 | |

| 7 X | 6.91393E-05 X | 9.07677E+00 | |

| 8 X | 2.11829E-04 X | 2.77997E+01 | |

| 9 X | 2.24357E-04 X | 2.94585E+01 | |

| 10 X | 6.83919E-04 X | 8.96986E+01 | |

| 11 X | 7.15681E-04 X | 9.40158E+01 | |

| 12 X | 2.21045E-03 X | 2.89320E+02 | |

| 13 X | 2.20491E-03 X | 2.90104E+02 | |

| 14 X | 7.20656E-03 X | 9.36989E+02 | |

| 15 X | 7.07785E-03 X | 9.36037E+02 | |

| 16 X | 2.53971E-02 X | 3.22353E+03 | |

| 17 X | 5.23005E-02 X | 7.04359E+03 | |

| 18 X | 2.14799E-01 X | 2.24818E+04 | |

| 19 X | 2.35662E+00 X | 3.72966E+05 | |

| 20 X | 1.84583E+01 X | 1.47495E+08 | |

| 21 X | 1.45109E+01 X | 7.81110E+11 | |

| 22 X | 1.40113E+01 X | 4.17713E+15 | |

| 23 X | 1.40010E+01 X | 2.25469E+19 | |

| 24 E | 1.40071E+01 X | 1.21878E+23 | |

---------------------------------------------------------------------

COMM and MESS with changed D_SIGM_EPSI attached.

Any other hints?

Best regards,

Katrin

PS: How do I "professionally" include code pieces into the posts?

Attached file:
burstpress_2nd.zip, 90991kb

RichardS

Hello,

from the convergence table it seems that the stiffness matrix is not being updated.

You should try it with REAC_ITER=1 in the CONVERGENCE setting, this would update the stiffness matrix EVERY iteration.

Best regards,

Richard

highpressuretube

Hello,

I plugged in what RichardS said and it seemed to really help: This time I went into an "ArretCPUError" at approximately 11.9MPa. Convergence was extremely fast in the last steps though (always second Newton iteration). Thus I am wondering: What do I have to do with the comm file to not only reduce step size while not converging, but to increase step size when converging fastly?

I will try to restart via POURSUITE over the weekend and tell about success/failure afterwards. Hoping to get the POURSUITE-comm file to work - it will be my first try :-)

Thanks,

Katrin

ThomasDESOZA

Hi,

Are you familiar with limit analysis ?

This is a systematic type of analysis to determine the limit load of a structure which is well suited for steel structure such as pipes or tanks.

This training material (available in the training section) will provide the basics and the must-read manuals related to this type of analysis : http://www.code-aster.org/V2/spip.php?action=dw2_out&id=1915

Applying this to your problem should get you nearer to your estimated load.

Also note that the way you apply the pressure should change the limit load in the same way it may change the buckling load of a structure (following pressure that is always normal to the wall or not).

TdS