How do I calculate Joint constraint moments for a General Joint (MPC184)?

Find more posts tagged with

Comments

All joint / MPC184 results can be extracted using NMISC and SMISC operators of DPF. Please note this is supported only from Ansys DPF server version 2025R1 onwards (you need to have Ansys Mechanical 2025R1 installed or a DPF standalone server).

Below is an example to extract JMX - NMISC22, refer to MPC184 General Joint help documentation in Ansys Help:

Adjust the `item_index` and the operator name `smisc` or `nmisc` based on the result you want to extract.

import ansys.dpf.core as dpf

server = dpf.start_local_server(ansys_path=r"C:\Program Files\ANSYS Inc\v251")
print(server.info)

rst_path = r"D:\…\file.rst"
ds = dpf.DataSources(rst_path)

model = dpf.Model(rst_path)

mesh = model.metadata.meshed_region
mesh.available_property_fields
field = mesh.property_field("apdl_element_type")

# Elements supported by DPF
print(set(field.data))

prop = dpf.operators.scoping.on_property(
    property_name="mapdl_element_type", data_sources=ds, property_id=184)
prop_scoping = prop.outputs.mesh_scoping.get_data()
print(prop_scoping)

moment = dpf.operators.result.nmisc(data_sources=ds)
moment.inputs.item_index.connect(22)
moment.inputs.mesh_scoping.connect(prop_scoping)
my_fields_container = moment.outputs.fields_container()
print(my_fields_container[0])