ASME PTB-3 Validation – Limit Load Analysis

Limit Load analysis are non linear in nature and may require significantly more computation time and resource than a linear elastic analysis. As such a linear elastic analysis is always a recommended first step. It helps to ensure the FEA problem is correctly setup i.e. there are no rigid body motions, deformations and far field stresses are of expected order and reactions match closely to hand calculations. However though computationally expensive, limit load analyses are fairly easy to set up and require very less post processing work for ASME Sec VIII Div 2 code compliance. It shall be only ensured that the analysis converges for the applied factored load as per table 5.4 of ASME Sec VIII Div 2.

Here an ASME PTB-3 Validation for “Example E5.2.2 – Limit Load Analysis” to check for protection against plastic collapse is carried out using ANSYS.

Problem Statement:

Evaluate the vessel top head and shell region for the vessel for compliance with respect to the limit load analysis criteria for plastic collapse provided in paragraph 5.2.3 of ASME Sec VIII Div 2.

For Vessel Data, Geometry, Mesh Details refer the post – ASME PTB-3 Validation – Elastic Stress Analysis

ANALYSIS SETUP

A static structural analysis was carried out with large deformation effects switched off as limit load analysis is done with the assumption that the strain-displacement relations are those of small displacement theory (Refer para 5.2.3.1(c)(2) of ASME Sec VIII Div 2)

MATERIAL PROPERTIES

  • An elastic-perfectly plastic material model was used for the analysis. This can be done by selecting bi-linear isotropic hardening model and entering the tangent modulus as zero. Note that since strain hardening is not being considered here both isotropic and kinematic hardening models are fine.
  • Yield strength defining the plastic limit shall equal 1.5S as per para 5.2.3.5 step 3 of ASME Sec VIII Div 2.

Yield Strength for SA-105 = 34950 psi

Yield Strength for SA-516-70N = 36825 psi

Young’s Modulus was taken from table TM-1, ASME II D at design temperature while poisson’s ratio was taken from table PRD, ASME II D. Yield Stress was computed as 1.5S, where S was taken from table 1A, ASME II D.

Stress Strain Curve for SA-105

Stress Strain Curve for SA-516-70N

 

LOADS & BOUNDARY CONDITIONS

  • Factored Internal Pressure of 1.5P = 630 psi was applied on the inner surfaces of the model as per table 5.4, ASME Sec VIII Div 2.

  • Pressure Thrust of 1473.45 psi was applied on the flange face as negative pressure.

  • Axial displacement was arrested at the shell base

ANALYSIS RESULTS

The analysis converged for the given load and thereby satisfy the global acceptance criteria for limit load analysis as per para 5.2.3.4 of ASME Sec VIII Div 2. No service criteria was provided in this problem hence they are not checked here.

Von-Mises Stress

Von-Mises Stress from PTB-3 example

The result plot compares pretty well with those provided in PTB-3 (ASME Sec VIII Div 2 – Example Problem Manual)

Note that deformations and strains computed in a limit load analysis have no physical meaning and are therefore not been plotted here.

Though convergence is achieved its always a good idea to find the actual limiting load for which plastic collapse occurs. This kind of gives a feel of additional margin above the applied factored load. This can be done by taking a large factor on the load say 10P and subsequently checking the load step upto which convergence is achieved. Say convergence upto a max time of 0.7 will imply 0.7*10P is the limit load.

A load (Internal Pressure in this example) vs max deformation is plotted here to get an idea of the limit load.

Load vs Deformation curve from PTB-3 example

Again the plots compare fairly well and gives an estimate of the limit collapse pressure load of 818 psi vs applied factored pressure load of 630 psi.

Find PTB-3 Validation Elastic Stress Analysis here

Find PTB-3 Validation Elastic Plastic Analysis here

2 thoughts on “ASME PTB-3 Validation – Limit Load Analysis

Leave a Reply

Your email address will not be published. Required fields are marked *