Torque on rotating shaft

[BEC_Kevin]

Hello everyone,

I am currently doing FEA on a rotting shaft and I need some help.  There is a steel disk in the center of the shaft with an aluminum shaft running through it.  I have attached an image below.  This shaft is being rotated by a motor at 3,000 RPM to produce electricity.  The shaft is supported by bearings on each side of the disk. For the bearing constraints i though that i would use a pinned constraint to still allow rotation.  Please let me know if this is correct.  I also don't know how to apply the torque to the shaft and incorporate the 3,000 RPM into the model.  Any help would greatly be appreciated.  The analysis I am looking for is stress and maybe some frequency analysis.  Thanks alot.

[dharhay]

I cant tell from the photo if  you have the shaft surface in the area of the constraints separate from the rest of the shaft.  This way you can select the shaft portion in the bearing area and via the mesh window create a pin joint or a universal joint to match your style of bearing.

This should help in some manner, others will chime in on other aspects of your question.

[BEC_Kevin]

I dont have the shaft area separate from the rest of the shaft.  I just used the rectangle select and selected nodes and then did the pinned boundary condition.  

[John_Holtz]

The method that you used to restrain the shaft will not produce the effect that you want. It may be easier to understand by looking at the cross-section (see "BC wrong.png"). Since the four nodes that are restrained in translation cannot move, then the shaft will not "rotate". It may be helpful to review this page in the documentation: Help > Contents > Autodesk Algor Simulation > Getting Started > Introduction to Autodesk Algor Simulation FEA > Nodes and Elements.

What Dave was suggesting is to split the surfaces of the shaft in the area of the bearings. This would be done in your CAD application. Then in Algor Simulation, you would use the "Mesh > Create Joint" command twice -- once for each bearing. This will create a space truss to represent the bearing connection to the surface of the shaft. Then one boundary condition (for a "Universal Joint") or two boundary conditions (for a "Pin Joint") will hold the model but allow the shaft to rotate. (See "BC correct.png")

For the rotation, I suggest using centrifugal loading ("Analysis > Parameters > Centrifugal").

Finally, keep in mind that for a static analysis, the model needs to be statically stable. So if you apply two torque loads that "counteract" each other, you still need a boundary condition somewhere that takes the numerical inaccuracies in the torque. This is usually done by applying one of the torques as a load and using a boundary condition at the other location to represent the other torque (either the input or output). For example, imagine a gear driven by a motor. A pin joint could be used on the end of the shaft, define the lines as beam elements, and apply a torque produced by the motor. Then a boundary condition could be applied to a gear tooth to represent the force that gets transmitted to the mating gear. (In other words, the force created at the boundary condition on the gear is identical to the force needed to resist the applied torque, but the boundary condition also produces a statically stable model.)

[sure0007sh]

hai ,

 i want to how to give a torque in fusion 360 sumulation...

[John_Holtz]

Hi @sure0007sh

You should ask your question in the Fusion 360 forum. But the answer is easy enough: apply a load and change the load Type to "Moment". You will probably need to change the Direction Type to Vectors -- that makes it easier to enter the proper directions.

[danies.mechanic]

Could you tell me it more clear, iam still not undesrstand, is Algor in Autodesk inventor?  The shaft was broken on the neck

[John_Holtz]

Hi @danies.mechanic

Simulation Mechanical (which was Algor before 2009) is a stand alone program; it is not "in" Inventor. But if you have a model open in Inventor, there is a command to transfer the model to Simulation Mechanical. You can also open Inventor files directly from within Simulation Mechanical.

Inventor has two different stress analysis capabilities:

1. "Environments > Stress Analysis". This capability exists if you are using Inventor Professional.
2. "Environments > Autodesk Nastran In-CAD". This is an add-on which requires a separate purchase and a license.

[imalleab]

Hi,

I know this should be posted on Inventor forum, but I guess it is a basic thing, so you could help me.

I'm following the same procedure that the post creator (analyzing shaft stresses), and I'm trying to split the body (Inventor tool) on the bearings. My shaft has two central bearings, so I will have five bodies after I split the bearings parts. The problem is that I can't split more than one of them, when I try to split the second bearing, it gives me an error about the split lines. (I'm not sure how to translate the error from spanish).

Any ideas?

Thanks

[John_Holtz]

Hi @imalleab

You should post your message to the Inventor forum, along with the error message and any images of the model (or a screencast video) that demonstrates what you are trying to do.

Note that it is usually not necessary to split the body in order to have a region for the bearings. You usually only need to split the face. Maybe that will help.

[imalleab]

Finally I was able to do the split thing.

Now I'm trying to use the centrifugal analysis. As you said, I created the pin joints (one for each bearing). Now I need to define the rotation center point and rotation axis. What should I put there?

Another thing. The shaft transmit a torque from one end to the other, and in one of them it has a radial and a tangential force (absorbed by the bearings). How should those forces be added since the shaft is supposed to be rotating, so if I apply a force, after a moment it will rotate along with the shaft (or not?). Hope you understand what I tried to say.

Thanks!

[John_Holtz]

Hi @imalleab

You are settings up a static analysis, so the shaft is not going to rotate. The centrifugal load simulates what happens if the shaft were to rotate. So you will apply the torque that you mentioned and some counter-acting torque or constraint to balance it. In other words, because you are doing a static analysis, the model must be statically stable: it cannot be free to translate or rotate about X, Y, Z. (Even if you were doing a transient analysis like an MES, it would be a waste of time to rotate the shaft unless there is a very, very good reason to do so.)

In the centrifugal load dialog, you want to enter the information to simulate what your shaft is doing. I assume that it is rotating at some RPM about an axis parallel to X (so the rotation axis would be 1,0,0) passing through the point X, Y, Z. You need to determine some point on the axis of rotation and enter the Y and Z coordinates. (The X coordinate does not matter since all X coordinates are on the centerline of the shaft.)