Extrapolation Method for strain result of 2D-element#

This example shows how to compute the nodal component elastic strain from Gaussian points (integration points) for 2D-element by using the method of extrapolation.

Extrapolating results available at Gauss or quadrature points to nodal points for a field or fields container. The available elements are:

  • Linear quadrangle

  • Parabolic quadrangle

  • Linear hexagonal

  • Quadratic hexagonal

  • Linear tetrahedral

  • Quadratic tetrahedral

1st step : Get the values at the data source’s of integration points (this result file was generated from MAPDL with EREXS, NO).

2nd step: using operator of extrapolation to compute the nodal elastic strain.

3rd step: Get the nodal elastic strain result from the data source. The analysis was computed by Ansys Mechanical APDL.

4th step: Compare the results between nodal elastic strain from the data source and nodal strain computed by extrapolation method.

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

Get the data source’s analyse of integration points and data source’s analyse reference

datafile = examples.download_extrapolation_2d_result()

# integration points (Gaussian points)
data_integration_points = datafile["file_integrated"]
data_sources_integration_points = dpf.DataSources(data_integration_points)

# reference
dataSourceref = datafile["file_ref"]
data_sources_ref = dpf.DataSources(dataSourceref)

# get the mesh
model = dpf.Model(data_integration_points)
mesh = model.metadata.meshed_region

Extrapolation from integration points for elastic strain result#

In this example we compute nodal component elastic strain results from the elastic strain at the integration points by using the gauss_to_node_fc operator.

# Create elastic strain operator to get strain result of integration points
strainop = dpf.operators.result.elastic_strain()
strain = strainop.outputs.fields_container()

Nodal elastic strain result of integration points:#

The command ERESX,NO in Mechanical APDL is used to copy directly the gaussian (integration) points results to the nodes, instead of the results at nodes or elements (which are interpolation of results at a few gauss points). The following plot shows the nodal values which are the averaged values of elastic strain at each node. The value shown at the node is the average of the elastic strains from the gaussian points of each element that it belongs to.

# plot
strain_nodal_op = dpf.operators.averaging.elemental_nodal_to_nodal_fc()
05 extrapolation strain 2d

Create the gauss_to_node_fc operator and compute nodal component elastic strain by applying the extrapolation method.

ex_strain = dpf.operators.averaging.gauss_to_node_fc()
# connect mesh
# connect fields container elastic strain
# get output
fex = ex_strain.outputs.fields_container()

Elastic strain result of reference ANSYS Workbench#

# Strain from file dataSourceref
strainop_ref = dpf.operators.result.elastic_strain()
strain_ref = strainop_ref.outputs.fields_container()


Showing plots of Extrapolation’s elastic strain result and reference’s elastic strain result

# extrapolation
fex_nodal_op = dpf.operators.averaging.elemental_nodal_to_nodal_fc()
# reference
strain_ref_nodal_op = dpf.operators.averaging.elemental_nodal_to_nodal_fc()
  • 05 extrapolation strain 2d
  • 05 extrapolation strain 2d


Compare the elastic strain result computed by extrapolation and reference’s result. Check if two fields container are identical. Maximum tolerance gap between to compared values: 1e-3. Smallest value which will be considered during the comparison step : all the abs(values) in the field less than 1e-14 are considered null

# operator AreFieldsIdentical_fc
op = dpf.operators.logic.identical_fc()



Total running time of the script: ( 0 minutes 4.883 seconds)

Gallery generated by Sphinx-Gallery