Modal Analysis of Electric Machine

  • 159 Views
  • Last Post 04 April 2019
shuvajit_1462 posted this 20 December 2018

Hello,

I'm trying to do modal analysis of an electric machine. the results that I'm getting are way off compared to experimental results that I've. I'll try and narrate the stuff that I'm doing. Let me know if I'm doing anything wrong or should I be doing it differently .

  • stator, winding, rotor assembly including shaft, bearing and housing assembly all have been modeled in the simulation.
  • I'm trying to simulate with the exact weight as in the prototype by tweaking the mass densities a bit.
  • all the parts have proper material assigned to them.
  • Considering isotropic elasticity. 
  • Fixed support at the location of the bolts.
  • the outer surface of the bearings have been given a friction less support. (Is this the right thing to do ?)   

I don't get any errors or warning while running the model. It's just that the results are off. I'm very concerned about the way I'm giving a friction less support to the bearings. I'm not sure if that's the correct way to do it. 

Any suggestions or reference or reasoning what might be going wrong here would be highly appreciated. 

And thank you for reading this far. Let me know what you think.

Best

Shuvajit  

Order By: Standard | Newest | Votes
peteroznewman posted this 21 December 2018

Hello Shuvajit,

A Modal Analysis creates information that can be useful for other analyses, like Harmonic Response. Data from a Harmonic Response Analysis can be directly compared with data from an experiment. The only thing you might compare from an experiment is a resonant frequency with a modal natural frequency. Please describe the results that you got from the experiment and the results from the modal analysis. Show me how far off the results are.

Please describe the experimental setup and the data that was gathered. What sensors were used to gather data? Where were those sensors located? What data sampling rate was used to digitize data from those sensors? How was the structure excited to create the vibrations? What speed was the machine running at?

You ask about frictionless support at the bearings. There is a support called a Bearing and you have to put in the bearing stiffness. That might be a more accurate way to model the bearings.

If you can show some images of the electric machine, or screen snapshots of the model, that would be great. You can even attach a Workbench Project Archive .wbpz file to your reply so I can open your model.

Regards,
Peter

shuvajit_1462 posted this 21 December 2018

Peter,

Thank you so much for your reply. So the experimental setup goes as follows:

  • the natural frequencies were determined from an impact hammer testing.
  • accelerometers were used to obtain the response of the structure upon impact with the hammer. 
  • accelerometers were located on the machine housing at different locations. 
  • Sampling frequency was around 8 kHz. Frequency resolution was 1 Hz. 
  • It was not a powered on test. the machine wasn't spinning. 
  • we were specifically looking at the mode order 2 frequency. the simulation is off almost by a 15%.

I thought a modal analysis in ANSYS would be the best way to obtain the resonant frequencies and compare them with the ones from experiment. Is there any other way to replicate the impact hammer testing in ANSYS ? if there is can you please help me with a reference ?

And I'm using workbench 19.1. The type of support that I see here are as follows. 

 I'm afraid I won't be able to share the archived project at this moment. 

Thanks for your time again ! 

Best

peteroznewman posted this 21 December 2018

Shuvajit,

Actually, a Bearing is created under the Connections folder, like Joints and Springs. I misspoke when I said it was a support.

I see you have good data on the natural frequency of the machine.

You didn't specify if the simulation predicted a natural frequency that was 15% higher or lower than the experiment.

One reason the model can predict a higher frequency is if the mesh is too coarse, the model becomes stiffer than the true stiffness. You can perform a mesh refinement study and use a series of mesh element sizes that are smaller by a factor of 1.5 and observe how the natural frequency changes.

Another reason the model can predict a higher frequency is if the boundary conditions are too stiff. For example, the Fixed Support on the bolt holes.  You can add the base that the machine sits on to the model and connect it at the bolt holes using a Beam connection.

One reason the model could predict a lower frequency is if the base is supporting the frame over a large area, and the bolt holes that are fixed are at the corners and the lack of support under the machine frame adds flexibility to the model that is not present in the machine.

Regards,
Peter

  • Liked by
  • shuvajit_1462
sk_cheah posted this 21 December 2018

Shuvajit,

Trying to correlate an electric machine is not easy. There are many unknown variables with a lot of assumptions. 15% doesn't sound too bad on the first correlation attempt. If your goal is to help troubleshoot, that may be good enough for the model to give relative results. If your goal is to have a good model to make absolute predictions, a lot of work needs to be done to verify different mass and stiffness of individual parts.

From an academic's perspective... take a look at the test mode shape and compare that to the analytical mode shape. It may provide hints as to where stiffness needs to be tweaked. I'm guessing the stator is generally very stiff and acts almost like a rigid body. The housing sheet metal may have a lot of modes. If you're not interested in those, remove them from both test and analysis as they are relatively light and shouldn't affect the global modes. As Peter pointed out, the boundary condition is critical. If your purpose allows for it, testing it free-free would be the simplest for correlation. 

Some speculation on my part:

  • You mentioned rotor winding was included in the model. Does it contribute too much stiffness in your model? Can you correlate a free-free modal test of the rotor alone? 
  • Bearing stiffness has both torsional and linear stiffness in real life. How would you like to approximate that in your model? This may be difficult. 

Correlation is a difficult challenge. Similar to optimization, you may find many local minimums by tweaking variables but it may not be the global minimum (reflect reality).  

 

Good luck,
Jason

  • Liked by
  • peteroznewman
  • shuvajit_1462
shuvajit_1462 posted this 21 December 2018

Peter,

Thanks to both of you for your suggestions. I'm sorry I didn't mention whether the prediction from simulation was higher or lower. The simulations right now are predicting higher than experimentation. So, judging from your suggestions, I guess that implies higher stiffness in the model considering that I've tried to model exact mass as the experimental setup. 

I've tried putting in quite a controlled dense mesh. Can you guide me to any link/reference which tells me how to determine if I've a good enough mesh ? 

And I'll try modeling the base plate of the machine as you suggested. 

 

Jason,

The winding on stator has been modeled and it has around 160 g of mass. And It makes the stator quite stiff. I'm not familiar with any techniques for stiffness measurement. So, same goes for the bearings as well. I guess I'll try to find some general value of bearing stiffness and use it in the model if possible. 

And the main modes of concern are on the stator. We aren't that much interested in the housing mode shapes. But removing it would impact the natural frequencies. Right ? and moreover, if I remove the housing I don't have a way to provide fixed support for the stator. You mentioned about a free-free boundary condition. Is there any reference on that one on how to do the simulation setup ? 

I really appreciate both of your time. This is great help for me.

Best 

sk_cheah posted this 21 December 2018

Shuvajit,

How did you model the windings of the stator? Would that introduce more stiffness than reality? Sorry, you mention it is 160 grams but it doesn't help my understanding given I don't know the mass of your stator. 

Removing the sheet metal around it would affect the modes but depending on the contributing effective mass, the error should be small. What is the mass of the housing and stator? I would suggest first testing only the stator with it's windings free-free and compare it to your model. Please see this paper on discussion on experimental supports. In simulation, free-free means no fixed boundary condition yielding six rigid body modes with natural frequencies close to 0Hz.

 

Kind regards,
Jason 

  • Liked by
  • peteroznewman
shuvajit_1462 posted this 21 December 2018

Jason,

This is how the winding (Green part) is modeled. the stator is around 600 g. Housing is about 650 g.

Thanks for the paper. I'll start going through it right away. and will do the free-free simulation as well. Once I've the results I'll reply to the same discussion thread and will let you know. 

Best

shuvajit_1462 posted this 22 December 2018

Jason, 

So I kind of did the free-free simulation with just the stator and the winding. Now I'm getting an almost 38% lower mode 2 frequency compared to the test. 

Let me know what you think. 

 

Best

sk_cheah posted this 23 December 2018

Shuvajit,

The housing is much heavier than I expected. You are right it has to be included later. 

Are you comparing the free-free analytical model frequency to fixed test frequency? If so, that would not tell us much. Comparing apples to apples is the best way. 

I found this paper which may interest you: https://www.researchgate.net/publication/243365175_Vibration_analysis_of_an_induction_motor

 

Kind regards,
Jason

  • Liked by
  • peteroznewman
Bharathi123 posted this 04 April 2019

Dear Sir,

How I download this student version. I need to design an electrical machine. Can you provide the link to download the electromagnetic simulation...????

Close