I have done a modal analysis of Jeffcott rotor in ANSYS Workbench for the extraction of natural frequencies but the data (Natural frequencies) obtained from the simulation and theoretical calculation are quite different. I am pretty sure that the theoretical values are quite accurate and being a newbie to the ANSYS software I need help in resolving this problem.
- Topic Is Locked
- 2K Views
- Last Post 14 January 2020
Did you do a mesh refinement study to know that the ANSYS solution has converged on results that don't change as the elements get smaller?
Are the theoretical values of natural frequency for a stationary rotor or a rotor at operating speed? If the later, did you perform a Static Structural model to apply the rotor angular velocity to the model and feed that solution into the setup cell of the Modal analysis? That is called a Pre-stress input to the Modal and results in a shift of the frequencies to account for the stress stiffeneing that the rotor exhibits at its operating RPM.
Do the theoretical values include damping? If so, you can add damping to the Modal model.
If these suggestions don't get you closer to agreement, you will need to provide a lot more information about your model and the theoretical values.
Well, thank you for your quick response.
I am doing the analysis for a Jeffcott rotor having shaft length 1m, diameter 20mm carrying disc at the middle having the mass of 3kg. The value of E = 2.1E11 and density 7850 kg/m3. The model is rotating at the speed 3000rpm and I am analysing the model for undamped vibration.
I have supplied the rotational velocity from the 'Inertial' option where I provide the direction and magnitude of the rotational velocity. From the simulation, I got the fundamental natural frequency around 47 Hz but from the theoretical calculation, the frequency is obtained in order of 81 Hz.
I have not performed the mesh refinement study until now but I will look into it.
this is a model I made on ANSYS and for this model, I did mesh refinement 2 times but still obtained the result in order of 48 Hz.
What are the supports at each end of the shaft in the ANSYS model?
What are the supports at each end of the shaft in the theoretical calculation?
Fixed supports will give different natural frequencies than pinned end supports.
The shaft is simply supported in the theoretical calculation but in ANSYS I don't know how to simulate the simply supported condition so I made two small rings around the periphery to simulate inner race of the bearings and fixed those rings.
I'd be more than happy if you could help me with supplying the simply supported end conditions.
Delete the two small rings. Make sure the shaft length is equal to the theoretical length.
Supports > Simply Supported, pick one end face of the shaft.
Supports > Simply Supported, pick the other end face of the shaft.
Now the shaft is free to spin on the axis, which gives one natural frequency.
Supports > Fixed Rotation, pick one end face of the shaft and keep X Fixed but set Y and Z Free (if the shaft is on the X-axis).
This gives another natural frequency.
Supports > Fixed Rotation, pick the other end face of the shaft and keep X Fixed but set Y and Z Free.
This gives a third natural frequency.
If you Fix the Y and Z rotations at both ends, that turns the BCs into the equivalent of Fixed Supports and you will get a fourth natural frequency.
Does the theoretical result use an actual disk or a point mass of 3 kg?
There is a different natural frequency for an actual disk with a mass of 3 kg and a point mass of 3 kg.
To make a point mass at the center of the shaft, you have to split the shaft at the center to create a face in the middle. Use shared topology to reconnect the two pieces. Then insert a Point Mass on that face at the center. This will shift the natural frequencies of all the above results.
If the theoretical result uses an actual disk, specifying that the disk has a 3 kg mass is an incomplete specification. You need to know its diameter also. Without that, I can make a large diameter, thin disk or a small diameter thick disk that both have a 3 kg mass, but they will each give different natural frequencies.
Well I have deleted the two rings and tried to give the simply supported end conditions but the options showed like this
So, I could not give the simply supported end conditions. Is there any solution to fixing this problem?
Also, I could not split the shaft at middle using face split tool for providing point mass in the middle so I used the slice option. Is it valid to use the slice option?
Yes, you can slice the shaft in the middle. Put the two bodies into a multibody part to reconnect them, while keeping the face in the center.
You can use Remote Displacement instead of Simply Supported. Just leave the Rotations Free at one end, except for the rotation about the axle centerline, where you can set both, one or no ends fixed in rotation.
Instead of a solid model for the shaft, you can also model that with beam elements, which means you draw two lines in DM create line bodies and create a cross-section to assign to those line bodies. The line has a vertex at the end instead of a face, and that will allow Simply Supported while a face will not.
Still, the results are not matching.
I gave remote displacement as a support condition and confines the motion in all direction except the rotation about X. I got 21 Hz as a natural frequency value.
for theoretical calculation, I have used [12EI/(L^3)] to calculate the stiffness and natural frequency is obtained by sqrt[K/M] and for my case, I obtained the natural frequency value as 81.22 Hz. (I have used K = [12EI/(L^3)] for the case of bending frequency).
Here is a reference on Jeffcott rotors.
Where did you get the formula for K? This reference says K = 48EI/L^3
It says the shaft is massless, your shaft has mass.
It says the rotor point mass is eccentric from the shaft with a distance of e, where is your eccentricity?
It says the prevalent vibration is synchronous whirl, which means it is equal to the rotor angular frequency of 50 Hz from the 3000 rpm you stated above.
Hello, i had modeled a steel beam of dimensions as Length = 4000 mm, Cross section = 250 x 150 mm, E=2E+11 N/m^2, Density = 7850 kg/m^3. Boundary conditions: Left support is applied using Remote Displacement option with X=Y=Z= 0 & RX=RY = 0 and RZ = Free Right support is applied using Displacement option with X=Z= Free & Y=0 Please note, beam is along X-Axis. There is a difference of theoretical and FEM results. First two bending natural frequencies are almost comparable as you can see below while in higher modes like 3rd and 4th there is significant difference in results. I am confused, how it would be done, so that i can get all FE results according to theoretical values? I guess there is something wrong with the boundary condition. With same boundary conditions, if a more slender beam is considered like 1044 mm length and 23x5 mm cross section then all theoretical and FEM results comes almost equal for each natural frequency. Looking forward for the solution if someone could help in this matter. Thanks
- All Categories
- Community Rules, Guidelines, and Tips
- News & Announcements
- Student Products
- Pre and Post Processing
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Physics Simulation
- Student Competition Teams
- eMasters Degree from UPM
- Site Feedback