Several joint element output quantities are available for review purposes. You can use either POST1 or POST26, or both, to review those results.
The solution output associated with the element is in two forms:
Nodal displacements included in the overall nodal solution
Additional element output to the results file listed below
The following output is available for joint elements as SMISC quantities:
Constraint forces and moments
Constraint forces (moments) if stop is specified
Constraint forces (moments) if lock is specified
Stop status
Lock status
Relative position
Constitutive displacements and rotations
Joint elastic forces (moments)
Joint damping forces (moments)
Joint friction forces (moments)
Relative displacement and rotations (cumulative)
Relative velocities
Relative accelerations
Average temperature in the element
The following output is available for joint elements as NMISC quantities:
The components of the bases vectors at the two nodes in the deformed configuration.
The bases vectors are specified as the local coordinate systems via the SECJOINT command and evolve with the rotation of the underlying nodes.
The constraint forces and moments in the evolved basis at the first node of the joint element.
The Ansys Workbench Products generally use NMISC output for postprocessing.
See the MPC184 element documentation and the individual joint element descriptions for details about the SMISC component specification and the use of the ETABLE command.
In POST1, you can print joint element output (such as relative reaction forces, relative displacements, relative rotations, etc.) at the free or unconstrained relative degree of freedom via the PRJSOL command. To obtain the nodal forces at the joint element nodes, issue the PRESOL,FORC command.
In POST26, you can use the JSOL command to specify result items (such as relative displacements, velocities, accelerations, etc.) that must be stored for a joint element. Then, you can plot or print the stored items via the PLVAR or PRVAR command, respectively.