Pressure vessel analysis according to an ASME standard#

This example demonstrates how you can use PyDPF to postprocess a Mechanical model according to the ASME Section VIII Division 2 standard for pressure vessel designs.

This example is taken from Workshop 02.1 from Ansys Mechanical Advanced Topics. Instead of using several user defined results as it is done in the workshop, DPF is able to calculate the triaxial strain limit and compare it with the equivalent plastic strain, as specified in Equation 5.7 assuming 0 forming strain.

Please be aware that this is just an example, so it is the user’s duty to verify that calculation is made according to latest ASME standard.

# Import the result file from Workshop 02.1.
# Because it is a elastic-plastic analysis, there are several substeps. The focus
# here is on the latest substep (number 4)

import ansys.dpf.core as dpf
from ansys.dpf.core import examples

path = examples.download_example_asme_result()
model = dpf.Model(path)
data_source = model.metadata.data_sources

time_scoping = dpf.Scoping()
time_scoping.location = dpf.locations.time_freq
time_scoping.ids = [4]

Parameters input#

You must go to ASME Section III Division 2 to get values for the parameters alfasl and m2. This is the code for introducing these parameters manually:

  • alfasl = input(“Introduce alfasl parameter from ASMEn”)

  • alfasl = float(alfasl)

  • m2 = input(“Introduce m2 parameter from ASMEn”)

  • m2 = float(m2)

For this exercise, alfasl = 2.2 and m2 = .288, which is the same as the original.

alfasl = 2.2
m2 = 0.288

Stresses and strains#

Stresses and strains are read. To get the same results as Mechanical, read elemental nodal strains and apply von Mises invariant. This operator does not have an option for defining the effective Poisson’s ratio. Consequently, a correction factor is applied.

seqv_op = dpf.operators.result.stress_von_mises(
    time_scoping=time_scoping, data_sources=data_source, requested_location=dpf.locations.nodal
seqv = seqv_op.outputs.fields_container()

s1_op = dpf.operators.result.stress_principal_1(
    time_scoping=time_scoping, data_sources=data_source, requested_location=dpf.locations.nodal
s1 = s1_op.outputs.fields_container()

s2_op = dpf.operators.result.stress_principal_2(
    time_scoping=time_scoping, data_sources=data_source, requested_location=dpf.locations.nodal
s2 = s2_op.outputs.fields_container()

s3_op = dpf.operators.result.stress_principal_3(
    time_scoping=time_scoping, data_sources=data_source, requested_location=dpf.locations.nodal
s3 = s3_op.outputs.fields_container()

strain_op = dpf.operators.result.plastic_strain(
pstrain = strain_op.outputs.fields_container()

eppleqv_op = dpf.operators.invariant.von_mises_eqv_fc(fields_container=pstrain)
eppleqv = eppleqv_op.outputs.fields_container()

poisson_ratio_correction = 1.3 / 1.5
eppleqvmech_op = dpf.operators.math.scale_fc(
    fields_container=eppleqv, ponderation=poisson_ratio_correction
eppleqvmech = eppleqvmech_op.outputs.fields_container()

eppleqvave_op = dpf.operators.averaging.to_nodal_fc(fields_container=eppleqvmech)
eppleqvave = eppleqvave_op.outputs.fields_container()

Triaxial strain limit calculation#

# S12=S1+S2
s12_op = dpf.operators.math.add_fc(fields_container1=s1, fields_container2=s2)
s12 = s12_op.outputs.fields_container()
# S123=S12+S3
s123_op = dpf.operators.math.add_fc(fields_container1=s12, fields_container2=s3)
s123 = s123_op.outputs.fields_container()
# SVM_scale=SVM*3
ratio = 3.0
seqvs_op = dpf.operators.math.scale_fc(fields_container=seqv, ponderation=ratio)
seqvs = seqvs_op.outputs.fields_container()
# S123/SVM*3
sratio_op = dpf.operators.math.component_wise_divide(fieldA=s123, fieldB=seqvs)
sratio = sratio_op.outputs.field()
# S123/SVM*3-0.33
sterm_op = dpf.operators.math.add_constant(field=sratio, ponderation=-1 / 3)
sterm = sterm_op.outputs.field()
# -alfasl/(1+m2)*stressterm
ratio2 = -alfasl / (1 + m2)
expt_op = dpf.operators.math.scale(field=sterm, ponderation=ratio2)
expt = expt_op.outputs.field()
# exp(-alfasl/(1+m2)*stressterm)
exp_op = dpf.operators.math.exponential(field=expt)
exp = exp_op.outputs.field()
# elu*exp(-alfasl/(1+m2)*stressterm)
strainlimit_op = dpf.operators.math.scale(field=exp, ponderation=m2)
strainlimit = strainlimit_op.outputs.field()

Strain limit condition (less than 1 pass the criteria)#

strainratio = dpf.operators.math.component_wise_divide(fieldA=eppleqvave, fieldB=strainlimit)
strainratio = strainratio.outputs.field()

Strain limit condition is plot#

10 asme secviii divtwo

Total running time of the script: ( 0 minutes 1.907 seconds)

Gallery generated by Sphinx-Gallery