Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

To find the critical speed of a vertical shaft

  1. Mar 31, 2009 #1
    i am in great need of help.........
    i need to determine the critical speed of a vertical shaft using ansys software .......my questions are:

    1. which kind of element type should i choose?
    2. wiil it be ok if i carry out the analysis without giving any constraints as it is not supported by bearings...it just has a line contact so what kind of boundary constraints am i supposed to give..

    plzzzzzzz help me as soon as possible
    Last edited: Mar 31, 2009
  2. jcsd
  3. Mar 31, 2009 #2
    The question is rather vague, your talk of elements leads me to the conclusion that you are trying to use some sort of FE software.

    The natural frequency depends havily on the boundary conditions.
  4. Mar 31, 2009 #3
    ya i m using ansys software.......i mean that the shaft is not supported by bearings......it just has line contact.........so what kind of boundary constraints am i supposed to give
  5. Mar 31, 2009 #4
    How is the shaft supported then? Line contact? to what?
  6. Mar 31, 2009 #5


    User Avatar
    Science Advisor

    You're in luck, I happened to catch an ANSYS modal analysis webinar a couple of weeks ago.

    1. It depends on what version of ANSYS you have. If you have the new version 12, then you can use almost anything, solid elements included (e.g. 183, etc). With the slightly older (what I'm using) version 11.x, you are restricted to using BEAM elements I believe.

    2. Yes, you can carry out the modal analysis with no constraints. In this case, your critical speeds will coincide with the natural frequencies. Sometimes we call this the "free-free" case with no supports.

    3. I can't remember exactly the steps, but it's a modal analysis with an incremental omega defined (IIRC). In v12, you can define both rotating and non-rotating geometries, so defining structures and supports can get complex. With v11 I believe that you are restricted to using COMBIN element types for bearing and supports.

    The documentation for any type of modal/vibrational analysis is very poor, so I understand your frustration. If all else fails, the ANSYS tech support is pretty helpful though. Try giving them a call.

    A simpler approach would be to try and calculate it by hand if the shaft is simple enough, or try a rotordynamics program such as Dyrobes (which we use) which is quite a bit simpler. You can probably ask for a trial version.
  7. Mar 31, 2009 #6
    the shaft i am talkin about is called a declamp shaft that is used in a cnc machine to clamp and declamp the tool after an operation. the declamp shaft is loacted inside a spindle cartridge which is driven by a servo motor..the shaft is just supported by a part called sleeve which is connected to the spindle cartridge (here there is a line contact)..............
  8. Mar 31, 2009 #7
    Interesting stuff minger, I tried a harmonic analysis with a crankshaft for a project but couldnt get it to work. Im on ansys 11 and found the documentation to be poor for more complicated analysis, which is odd as the rest of it is really good.

    I get what you mean now vikkispike, that makes some sense :D.
  9. Mar 31, 2009 #8


    User Avatar
    Science Advisor

    In your case you'll need to make some assumptions when finding the critical speeds. Your constrains will be the sleeve. Chances are, its constrained in all directions, so you can typically do something like this.

    Select the area of the shaft that is attached to the sleeve, then in a cylindrical CS set UX, and UZ to zero. This will restrain the part in the radial and axial directions respectively. Ideally this would be enough to get you started.

    For more advanced representation, you could use the COMBIN elements that I mentioned before to represent the stiffness of the sleeve, then attach it to the spindle.

    Either way, yes its a PITA right now, but they say that v12 will be much better performing and much better documented.

    Also, after a quick Google, I found some more information on calculating the numbere analytically. If the shaft is constant area, then one needs to find the eigenvalues of:
    [tex] \frac{d^4 y}{dx^4} - B^4 y = 0 [/tex]
    [tex] B^4 = \rho \frac{A}{EI}\omega [/tex]
    You would use your "constrains" as the constants of integration (i.e. y(0) = 0) so on and so forth to try and obtain the eigenvalues.

    edit: Here is a website that lists some solutions including cantilevered beam
  10. Mar 31, 2009 #9
    I've been reading some papers and most people seem to use matlab and do it analytically, with a similar method to the link you gave. COMBIN elemnts are a good idea I never thought of that. I've only ever done static structural analysis, so im kind of flying blind atm.

    This would be for interest only at this point, as I decided that it wasnt strictly necessary for me to complete the work so i've just lumped in the future study section.

    ZING! that response probably wasnt for me. but could help anyway :D
    Last edited: Mar 31, 2009
  11. Mar 31, 2009 #10

    Attached Files:

    Last edited: Mar 31, 2009
  12. Apr 1, 2009 #11


    User Avatar
    Science Advisor

    Well the shaft needs to rotate, so don't fix it in that direction, fix it in the other two: axially and radially. Fix in particular the part that slides into the sleeve. Assume the sleeve to be rigid.

    I would highly recommend using the link provided and do an analytical solution. Your shaft is essentially pretty "ideal" so the analytically predicted answer should be pretty damn close to the actual one. If your numerical results are not close, then you know that you messed something up.
  13. Apr 1, 2009 #12
  14. Apr 1, 2009 #13


    User Avatar
    Science Advisor


    Apparently I need at least 4 characters to post a message. Please ignore this part of this message.
  15. Apr 1, 2009 #14
    The full stop counts as a character :P
  16. Apr 1, 2009 #15
    actually my main aim is to determine the failure of the shaft.....it fails when it is rotating at 8000rpm....So i think there may be two reasons for the failure of the shaft 1} It may be such that the shaft is rotating near it is natural frequency......and the shaft is subjected to 800kgf load itz an impulse load may be due to that the failure may be occuring.....
    Last edited: Apr 1, 2009
  17. Apr 1, 2009 #16


    User Avatar
    Science Advisor

    How wide is the range of failures? i.e. is it occuring at 8k and 10k? If so, that's a pretty large range to be critical speed failure. Typically for an undamped system, you're either at the critical speed, which is apparent, or your not.

    What do you mean subjected to an 800 kgf (what is kgf?) impulse load? Have you done simple static analysis on this?
  18. Apr 1, 2009 #17
    the shaft's operating speed in normal condition is 8000rpm......
    1)first i need to check whether the reason of failure is whether the shaft is operating within the critical speed range.........
    2)MY second part of analysis wil be this one....... a impulse load acts on the top of the shaft in order to declamp the tool so the force applied onto the shaft is by a pnuematic cylinder i.e around 800N..
  19. Apr 1, 2009 #18
    What do you mean subjected to an 800 kgf (what is kgf?) impulse load? Have you done simple static analysis on this?[/QUOTE]
    I wil be carrying out the static analysis after determining the critical speed
    Last edited: Apr 1, 2009
  20. Apr 1, 2009 #19


    User Avatar
    Science Advisor

    Well you should be able to pound some hand calcs out pretty quick. Get the critical speed, then do a buckling analysis to make sure you don't have a problem there. The normal compressive stress should be easy enough.
  21. Apr 1, 2009 #20
    Does the shaft slide through the adaptor, or is it fixed in the adaptor?

    You say it fails when rotating at 8000 rpm. Does it operate at a steady 8000 rpm, or does it operate over a speed range?

    Do you have a drawing showing these two parts in position together?
  22. Apr 2, 2009 #21

    ya i have the assembled drawing of the shaft.Actually i need to determine the critical speed of it because the shaft is failing and i need to determine the cause of it's failure.So my 1st step is whether the shaft is operating within it's critical speed range.I am facing problems when i select the element as beam element 2node 188 i am not able to mesh an error comes.I am able to mesh only if select the element as Solid 45.So can i select the element as solid brick 45.........and i need the procedure of determining the critical speed.............I am uploadin the photo of how the shaft assembly looks.the adaptor comes at the top and the shaft has only line contact at the middle and is not connected by any other means.

    Attached Files:

  23. Apr 2, 2009 #22
    there s a other part called sleeve. the shaft slides inside the sleeve.
  24. Apr 2, 2009 #23
    The problem is you are importing a solid model and tring to mesh a beam. A beam mesh is a line, with the CSA and radius of gyration/ 2nd moment area and other stuff inputted as a real constant. To do it as a beam mesh, just draw several horizontal lines (each corresponding to a certain cross section). Mesh then with different real constants.

    Where was the shaft failing?
  25. Apr 2, 2009 #24
    You say that the shaft slides inside the sleeve. Is it in contact with the sleeve, so that the sleeve constrains the motion, or is the sleeve simply around it but not touching?

    What about the matter of steady speed versus operation over a range of speeds?
  26. Apr 2, 2009 #25


    User Avatar
    Science Advisor

    To elaborate on what Chris said, you will generate the lines, each representing a cross section. When the cross section changes, start a new line. You will then LMESH to mesh the lines, which will just be more lines basically.

    You should be able to LMESH on beam elements. After that, you will define a cross-section. There are pre-defined cross sections such as rectangles and tubes and such. From those, you simply enter length, heights.

    If you are doing this in batch, you will says omething like,
    Code (Text):

    For circular solid or arbitrary section respectively. You then use SECDATA to describe the geometry of the section. For CSOLID you define:
    Code (Text):

    For ASEC, you need to define a bunch of stuff, see the SECDATA command reference for more information.
Share this great discussion with others via Reddit, Google+, Twitter, or Facebook