Simulation Constraints Issue

[tgperret]

Shaft Assembly (Modeled in Inventor)

    To replicate the bearing used on our shaft ends, I modeled a shaft assembly where the shaft ends are supported through a race so the race has the freedom to rotate at will when a force is applied to shaft for simulation.  The DE (drive end) support is grounded and the NDE (non-drive end) is a given distance from the shaft end.

Simulation Results:

   The simulation is not allowing the race to rotate within the supports resulting in both the shaft and the support realizing stresses (see bookmarks SIMULATION Shaft Assembly NDE and SIMULATION Shaft Assembly DE in the attached file).  All the assembly constraints are reacting as I expect within Inventor. Bookmarks MODEL Shaft Assembly NDE and MODEL Shaft Assembly DE show how I expected the ends to appear after Simulation.

Simulation Constraints:

    DE bottom is fixed.

    NDE bottom is frictionless

One force is applied to the shaft.

I have tried many different approaches all having the same bending of the support along with stresses on the shaft at the support.  If anyone sees where I'm going astray please help.

Tommy Perret

Komline-Sanderson

12 Holland Ave.

Peapack, NJ  07977

[John_Holtz · Accepted solution]

Hi Tommy,

The Inventor assembly constraints are not carried through to the Inventor Simulation. Thus, the bearings are welded to the supports, leading to the effect that you saw.

You need to define the type of contact between the parts in the Stress environment. (My Inventor is on a computer that is currently in the repair shop, so these steps are from my faulty memory and may be inaccurate. ) Use the "Manual Contact" command on the "Contact" panel to define a "Separation" contact type between the race and support.

There is a slim chance that Inventor Simulation will have a problem solving because the above steps leave the shaft free to rotate about its axis. In Simulation, there is no unigue mathematical solution when this occurs. You end up with an equation such as rotation angle = torque/0 which is  undefined. In your situation, the answer is theoretically the same regardless of whether the shaft rotates 0 degrees about its axis (probably what you want) or any other angle. If this problem occurs, apply a constraint in the X direction only anywhere to a node along the very top (+Y) of the shaft.

If this doesn't fix the problem, I can contact one of the experts from the Inventor Simulation team; they normally monitor the Autodesk Inventor discussion group. The Autodesk Simulation group is normally used to discuss the product formally known as "Algor", now known as Autodesk Simulation Mechanical or Autodesk Simulation Multiphysics. (Yes, confusing I'm sure.)

[tgperret]

Thanks John,

   Your faulty memory was accurate enough to set me on the right track.  Automatic Contacts are first required and then simply edit any particular Bonded Contact as needed.  A whole new set of light bulbs are now lit in my mind (how dangerous)!  The simulation is now reacting exactly how I want it.  Thanks.

New Question:

    The Simulation visually shows the shaft "sucking in" what appears the same thickness of the shaft.  The "sucking in" occurs where the shaft goes from solid (12" on both ends) to hollow (see attached file).

   If the "Adjusted Display" is Undeformed, Actual, or all the way to Adjustedx5 the "sucking in" still displays the same.  I don't understand why this does not change with different Displays?  Is this a valid concern?

Tommy Perret

Komline-Sanderson

12 Holland Ave.

Peapack, NJ  07977

[John_Holtz]

Hi Tommy,

Think of it like this. When the CAD model is converted to a FEA mesh, the perfectly round cylinder is represented by a polygon. If a coarse mesh resulted in a hexagon cross section, then viewing the shaft "across the corners" would appear to show the shaft with the correct diameter. If you rotated the shaft about its axis and viewed the shaft "across the flats", it would appear to be a smaller diameter. (see my crude sketch attached).

If you turn on the "Mesh View" and/or rotate the shaft about its axis, you can see this effect better.

Now, does it affect the results? If you could slice the shaft in the XY plane (I think you cannot slice the results in Inventor Sim), you might see a situation where the inside diameter across corners aligns with the outside diameter across flats, as shown in the attached. This would result in underestimating the wall thickness at that area which could affect the results.

The only way to know for sure is to do a simplified hand calculation to compare the displacements, or create a finer mesh. Inventor Sim also has the "Convergence Settings" where you can specify the desired "accuracy", and it will adjust the mesh until that goal is acheived.

[tgperret]

Revised the mesh and the shaft is now round again.  Another light bulb has been turned on.

Now getting into "Convergence Settings" to put the higher mesh only where needed with accuracy.

You have been a big help!  Thanks!