Simulation of a rotor rotating to find vibration

[Anonymous]

Good day 

I am very new to Nastran, I am trying to simulate a rotor for an electrical motor to rotate at a certain speed and to be constraint to where it will be running on the bearings, im trying to see what type of vibration the rotor will be subject to at a certain rotational speed an frequency 

If anyone has any info or delt with the same type of simulation I would appreciate any help

[John_Holtz]

Hi @Anonymous 

In 99.9% of the cases, you do not need to physically rotate the model. You apply loads that simulate the rotation.

One method is a modal frequency response analysis, where you assume that a rotating, unbalance mass causes a sinusoidal force to act in one direction (up-and-down, left-to-right, and so on). See this article: Analyze a rotating component with an imbalance load. 

The other aspect of your analysis is simulating the bearings. Depending on whether the bearing prevent out-of-plane rotation or not, the two most comment methods are as follows:

1. Use a pin constraint and fix the radial displacement (leaving the hoop direction free).
2. Create a rigid body connector to attach the surface of the shaft (where the bearing makes contact) to a point on the centerline of the shaft, and then put a constraint at the center point. (This is often referred to as creating "spokes" that connect the nodes on the shaft's surface to a common point on the centerline, and the point on the centerline is constrainted in the appropriate directions to simulate the bearing.)

Let us know if you have any follow-up questions.

[Anonymous]

Hi John

Thanks for responding to my post, its really great help, so basically iv tried a few ways already with my rotor but only two were successful in giving me any results, so below is what iv done and then I don't know how to simulate modal frequency analysis so if you could assist in someway with that i would really appreciate it.

My one other questions is, my rotor consists of an assembly where there are 3 fans and then a core with copper bars and rings on it, I'm having problems meshing that assembly but is it possible to do the actual simulation with the shaft alone and apply the forces (weights) of the other parts to run the simulation and get the same results with regards to modal frequency analysis, as i have only managed to do displacement and a somewhat rotational force on the shaft alone, i have attached the two screen shots below of what i managed to do but not really the result i need, this is with the shaft alone, any other advice will be much appreciated.

1st Screen shot

I applied bearing loads in both directions on the below simulation I'm not sure if that was the correct way or not but the other three forces are added as you can see.

2nd Screen shot

I attempted to do a rotational force on the shaft to simulate a running speed of 3000rpm (50rev/s) and i added a pinned constraint to the 2 shaft journals where my rotational vector on the z axis is 1 but i had no loads/forces acting on the shaft so its not simulating to give me and vibration

Displacement3000rpm rotational force

[John_Holtz]

Hi @Anonymous 

A modal frequency analysis can be performed like in this tutorial: Modal Frequency Response of a Bracket.

Any type of modal or vibration analysis needs the mass of the fans, so applying a force to represent those is not the correct procedure. If you cannot get the fans to mesh, or if you do not want to include them in the analysis, then you should create a rigid body connector and apply a concentrated mass (at the center point of the rigid body) to represent the mass of the fans.

In the first image, I do not understand what the various forces are representing or what direction they are applied in. Can you clarify what the known loads are that you are trying to simulate?

In the second image, the "rotational force" load creates forces at each node that are pointed in the radial direction. The force magnitude is calculated from F=m*a, where m is the mass of each element, and the radial acceleration a = (radius from centerline)*(angular speed)^2, where the radius from the centerline is calculated for each element. So the results are as follows:

• It looks like you are performing a linear static analysis, so all of the loads and results are static. There will be no vibration in a static analysis.
• If the shaft and mass are perfectly symmetric about the axis of rotation, then all of the loads are balanced. The shaft will expand in the radial direction, but that is all that will happen. (It is hard to tell from the image whether the radial expansion is visible or not.)

I think what you want to simulate is the following:

1. The shaft or each fan is balanced to within some tolerance, such as a mass at a given radius.
2. As that mass located at a distance R rotates at some RPM, it creates a radial force that rotates around. This is what causes the vibration.
3. Because of symmetry, the rotation is not that important in the analysis. What is important is that at an angle of 0 degrees, the force is pointed in the +Y direction, and 180 degrees later the force is pointed in the -Y direction. Therefore, the shaft can be analyzed as vibrating in the Y direction with a time varying force in the Y direction.
4. The magnitude of the Y force versus time = mass*r*RPM^2*sine(RPM*time), and this is what creates the vibration in the Y direction. (That equation also needs the appropriate conversions from RPM to radians/second and so on. 😀) This type of analysis is performed using the modal frequency response and the article I referenced in an older post. You will model the shaft and fans (or use the concentrated mass for the fans), and apply a force in the Y direction to represent the unbalance mass. The analysis "multiplies the force" by sine(RPM*t) and gives the maximum result.
5. If you have 3 fans, you will have 3 forces applied to the shaft. In one scenario, you can assume that all 3 offset masses are in the same direction, so the 3 forces are in the same direction (+Y). In another scenario, you can assume that the offset masses at the two ends are 180 degrees apart, so one force is in +Y and one force is in -Y. I do not know if it is necessary to analyze it with forces in the +Y and +X to simulate the offset mass being 90 degrees apart, but that could be another scenario.

Cheers!

[Anonymous]

Hi,

I`m new on that, I did a 3D electric motor, I would like to simulate the vibrations of the rotor  and so one, but I can`t understand how the SW works. I tried to learn from your comments but I did not understand. Can you please generate a tutorial? It is possible to analize the shaft or another components in assembly not individually?.

Thanks for your response.

[fan.jiang2S3G9]

Can you do a shaft frequency calculation example for, say a generator shaft ?

Thanks

Fan