How to extract force reactions using DPF inside mechanical ?

Vishnu

Vishnu

Below is a simple code to extract the Y Reaction using DPF inside mechanical

import mech_dpf
import Ans.DataProcessing as dpf

#Result Data
analysis1 = ExtAPI.DataModel.Project.Model.Analyses[0]
dataSource = dpf.DataSources(analysis1.Solution.ResultFilePath)

#model
my_model = dpf.Model(analysis1.Solution.ResultFilePath)

#my mesh
my_mesh = my_model.Mesh

#Time list
timelist = dpf.operators.metadata.time_freq_provider(data_sources=dataSource).outputs.gettime_freq_support().TimeFreqs.Data

reaction = dpf.operators.result.reaction_force(time_scoping=timelist,data_sources=dataSource)
Y_reaction = dpf.operators.logic.component_selector_fc(fields_container=reaction,component_number=1).outputs.fields_container.GetData()[0]

print(sum(Y_reaction.Data))

#Release Locked RST
my_model.ReleaseStreams()

prasadmsonar_123

Hello Vishnu,
Thanks for this.
Can we extract the results for total deformation at particular location for all the steps in the analysis and export it as csv??

Vishnu

@prasadmsonar_123
You can

Look at below code the dispfield_container is a field container which is a list of multiple fields (field for each time point)

and the fields in turn contains the data of displacement(x,y,z) for each node

now all you need to do is push the data to a CSV file:

import mech_dpf,csv
import Ans.DataProcessing as dpf

#Result Data
analysis1 = ExtAPI.DataModel.Project.Model.Analyses[0]
dataSource = dpf.DataSources(analysis1.Solution.ResultFilePath)

#model
my_model = dpf.Model(analysis1.Solution.ResultFilePath)

#my mesh
my_mesh = my_model.Mesh


#Time list
timelist = dpf.operators.metadata.time_freq_provider(data_sources=dataSource).outputs.gettime_freq_support().TimeFreqs.Data


dispfield_container = dpf.operators.result.displacement(time_scoping=timelist,data_sources=dataSource).outputs.fields_container