Torsional Vibrations of a shaft and a rotor 2

[Bharathsf]

Hi,

I want to find out the torsional frequency of a shaft attached to a rotor. the shaft is massless and with a torsional stiffness 5000Nmm/rad and the rotor is of a diameter of 200 mm and a thickness of 1.5 mm.. I am using the young's modulus of aluminum for the shaft and the rotor..Since I have considered the shaft as massless I have given very low density for the shaft material and the mass of the rotor is about 80 grams because I have considered the exact density of aluminum. The problem i am facing is that the the natural frequency should come about 17.79 hz if I use the torsional vibrations formula which is f =(sqrt(K/Izz))/2pi but in the FE analysis I am getting 0.000545 hz in the first mode.I am using 1 d cbar element for the shaft and 2d cquad element for the rotor
The Izz for rotor is 400kgmm^2. Please help

Thanks in advance

Bharat

 

[almpunk]

Hi Bharat

Any SPC in your model?? it sounds like you have free body movement. If you have not any constraint that prevent the solid rigid movement in your model the first 6 modes that you will obtain are the six rigid body modes.These modes should have frequencies less than or equal to 1.0E-04 Hz. After these 6 modes you will obtain the vibration modes of your structure.
Hope this will help you.
Have a nice day!!

 

[Bharathsf]

Thanks a lot almpunk I forgot to mention.I have used a Spc to constrain all 6 DOF's on end of the shaft and connected the other to the rotor.Is there any other way to model torsional vibration of rotor and a shaft with shaft fixed at one end i.e a single mass cantilever rotor system. Please help

Bharat

 

[almpunk]

Could you pass me the .bdf??

 

[almpunk]

Hi again!!
I know what is the problem, the problem are the CQUAD that you are using to modelate the rotor. For CQUAD element there is no stiffness associated to the rotation about the normal to the plate. The CQUAD can only represent in-plane, bending, and transverse shear behavior. That´s the problem!! you have a stiffness singularity in the connection of the cbar with the CQUAD, the rotation about the cbar axis is not constrained for the CQUAD.
Try to model your rotor with a mass element, CMASSi or CONMi, have a look to the "quick reference guide" to check what mass element fit better to your rotor, other solution will be to model your shaft with 2D elements...........another alternative could be to connect your cbar to the rotor by means of a RBE2, as independent node choose the bar extreme and as dependent nodes choose some symetric nodes on the CQUADS, I think that this can works.........
Hope that this will help!!

 

[Bharathsf]

Thank you so much..I will give it a try

 

[Bharathsf]

I tried with a concentrated mass and the answer was exact this was easy because I knew the Mass moment of inertia of the rotor was known. Next I have to model a Micro air vehicle mounted on the rotor which in turn is attached to the shaft. I have no idea how to carry out this model and I do not know the mass moment of Inertia for the MAV. Can you please help..Is there any element which has stiffness associated to the rotation about the normal to the plate.Thanks a lot...I hope I am not troubling you. I have attached the dat file too with this link

 

[almpunk]

I have connected the shaft with the rotor by means of a RBE2, I think it should works, have a look to the attached file, and let me know if it works ok??
Have a nice day ;-)

 

[almpunk]

Hi again!!! I have just run the model and I have found that your SPC was not well defined, the rotation about Z was not constrained, I have fixed it and also fixed the 123456 DOF of the RBE2 element and the freq. obtained is 14.79Hz. the error comes because of the moment that the RBE2 (element with infinite stiffness) is adding, the error will decrease as you attach the RBE2 to nodes closer to the shaft, you can refine your mesh around the connection to the shaft so you will have nodes closer to reattach your RBE2. Hope I have explain myself well (I am not english native speaker) ;-).
I have attached the new model.
Have a nice day!!

 

[Bharathsf]

Thanks a lot but the 1st torsion mode of vibration is still 0.0005hz. I think as you said the reason is the lack of rotational stiffness of cquad element about its normal.Is there any other way I can model the same? Is there any element which can be used to model rotational stiffness??Thanks again I am a bit new to FEM so I have a lot of doubts

 

[almpunk]

In the second model I have sent you the first mode is 14.79 Hz and is the torsion mode. The firs model that I have sent you was not right, the SPC was not constrained in the rotation about Z and the RBE2 was not constrained also in rotation, in the last model that I have sent you all was corrected and working. If you don't want to use RBE2, you can model the Rotor with solid elements, they have Rx,Ry and Rz stiffness........don't worry about being new, everyone has been once new!! just practice makes the master!!

 

[Bharathsf]

Thanks a lot Thanks a lot I did refine, and the answer is accurate Thanks a lot for your time just one last doubt what is the reason why we should use rbe 2 element to connect the cbar and the rotor?

 

[almpunk]

The RBE2 is a rigid element that can transmit your torsion moment to the CBAR. If you attach the RBE2 with just one node of the CQUAD it will not works, connecting to more than one node is transmitting your torsion moment through the shear stiffness of the CQUADS. Hope this help you! ;-)
I highly recommend you to read the MSC documentation for NASTRAN, you will learn a lot about FEM and the philosophy behind NASTRAN, you can find for free the docs in

http://simcompanion.mscsoftware.com...D_NASTRAN_DOCUMENTATION&channel=DOCUMENTATION

You should start by the "Getting started User's Guide" and after reading it go to the "Linear Static User's Guide". Also you can find the "MSC Nastran Demonstration Problems" that will help teach you a lot.
Good luck with your way in the FEM and do not hesitate in contact me for further questions.
Have a nice day!!!

 

[Bharathsf]

Thanks a lot I will surely go through the documentation and I will contact you if I require any help