Static stress analysis setup for rigid body motion

[AH_AK]

I am trying to analyze the stress in a simple link (straight link, pins at both ends) that is part of a mechanism (planar analysis).
I have solved the planar kinematics/kinetics equations (rigid body motion), so I know the reactions at the pins and accelerations (linear and angular) at the center of mass of the link in question.

I am trying to manually set up the loads for an equivalent static stress analysis. I know that some programs will let you import RBM loads, but I want to establish the general procedure for manual setup to avoid erroneous results when using the import.

Right now my procedure for the generalized link AB is:
Apply a cylindrical fixture to A that constrains radial and axial displacement (body can still rotate about A).
Apply roller constraint to back face to avoid out-of-plane twisting.
Apply centrifugal load (in SOLIDWORKS) at the center of mass, enter the angular velocity and angular acceleration of the link from the RBM solution.
Apply gravity using the accelerations of the center of mass from the assembly, but in the opposite directions.
Apply the reactions from the solution for pin hole (cylindrical face) at B
Apply a remote displacement control at pin hole B (cylindrical face) restricting translation in the tangential direction (w.r.t. the axis AB). The resultant force of this constraint should be near zero as it only provides resistance to instability (rotation) due to rounding errors in the analytical solution.

When I solve, the reactions at the pin A fixture match the analytical solution. The stresses look as one would expect when one isolates the individual stress sources. I am looking at this from a superposition standpoint in the sense that every link will be composed of (1) centrifugal stresses from angular velocity (tensile stress for a straight link), (2) bending stresses from the angular acceleration of the link, (3)stress from additional axial (transmitted) loads (tensile or compressive) based on the rest of the model. The reason I am comfortable that the above procedure represents reality well is because when I isolate each of the aforementioned stresses, I get stress distributions and deflections that make sense (at least to me).

My question is this: is there an easier manual procedure for converting a rigid body solution to a static stress analysis? I tried messing around with inertia relief, but that seems to be a tool for translation (linear acceleration).

 

[rb1957]

yes, you need to apply body forces that are the inertial reaction to the applied loads.

It is much easier to use a code intended for mechanisms, like Adams.

There's another path for you ... go see how Adams set up their analysis.

"Hoffen wir mal, dass alles gut geht !"
General Paulus, Nov 1942, outside Stalingrad after the launch of Operation Uranus.

 

[FEA way]

Depending on the software there are various ways of handling MBD + FEA problems. Some codes allow for co-simulation (data is exchanged in both ways, during the whole analysis) and can include dynamic substructures (superelements) in MBD runs. But the traditional approach would be to export the loads on attachment points as load cases for FEA and use inertia relief to stabilize the model without boundary conditions. From what I've noticed, the procedure of importing motion loads in SolidWorks consists of applying linear (gravity load type) and angular (centrifugal load type) accelerations to the part together with remote forces and moments applied to faces participating in connections. Inertia relief is also activated by default in such studies.

Your manual approach requires a bit of work but seems to make sense. It would be best to test it by comparing it with the automatic procedure described above.