Harmonic Analysis - no rotordynamics content

Hi All,

 I have an issue with harmonic response analysis. I'm analysis student project of shaft with gear assembly. I have no rotordynamics content in Analysis Settings of harmonic response. For modal analyse  everything is ok.

What could be the reason? Should it be performed via APDL?

Comments

  • jj77jj77 Member
    edited January 2019

    Make sure you have coupled the two (see image below), That is in order to do a harmonic analysis one needs to calculate the modes first (for mode superp. option) which can be then used by the harmonic analysis. If that is done in the harmonic analysis settings there should be a section for Rotordynamic controls (see yellow marking below). I think though to use the Coriolis effect (Rotrod. Controls), one needs to use the full solving method (thus modal and harmonic needs not to be linked like shown below, only a harmonic analysis is enough, one would still see the Rotrod. Controls though).

     

    If this does not help feel free to upload your model or some screenshots of what you are missing in the harmonic settings.

  • raffikkoraffikko Member
    edited January 2019

    Hi,

    thank you very much for response.

    Please look on attachments.

    In my opinion it goes ok. Maybe it is Ansys bug? Connection Map, Harmonic analysis settings, Modal analysis settings and model.

  • jj77jj77 Member
    edited January 2019

     

    Which version of ansys are you using (perhaps 13 or 14, where this option is not possible as far as I can see)?

     

    Also one would need to use the full method to include Coriolis effect, thus try to use only a harmonic analysis with no links to modal.

  • raffikkoraffikko Member
    edited January 2019

    It is 15th.

    I tried to do standalone harmonic but no rotordynamic again. Please look on photos:

    So similar results we can achieve in rigid dynamics analysis right?

  • peteroznewmanpeteroznewman Member
    edited January 2019

    raffikko,

    I expected to see a load in your harmonic analysis but I don't see one, so the Harmonic Response branch shows a ?

    What is the harmonic load to which you want to calculate the response?

    Regards,
    Peter

  • raffikkoraffikko Member
    edited January 2019

    Thank you for your support.

    I based on youtube movie:

    My goal was to find harmonic response from rotating force which is calculated from unbalanced mass.

  • peteroznewmanpeteroznewman Member
    edited January 2019

    Thanks for the video. Did you see him Insert > Rotating Force on the Harmonic Response branch?  That is the load your model is missing.

    Regards,
    Peter

  • raffikkoraffikko Member
    edited January 2019

    Ye, but I don't have this rotating force in my loads tree. Please look on photo:

  • peteroznewmanpeteroznewman Member
    edited January 2019

    Rotating Force was added after Release 15. You will have to use APDL commands such as CORIOLIS and OMEGA to define angular velocity input to the rotating structure. Here is the section in the ANSYS 15.0 help

    Here is a command object inserted with these commands

    Here is the Freq. Response in Y with the command snippet. It is the same magnitude in Z.

    Here is the Freq Response in Y without the Command Snippet. It is 1000 times smaller in Z.

    You can create Force in the Y direction (assuming your shaft is along the X axis). It is sufficient to have a single unbalanced force since it is rotating.

    Attached is the Release 15.0 model of an unbalanced shaft.

    Alternatively, you could download ANSYS Student 19.2 and use Rotating Force.

    Regards,
    Peter

  • Hadi96Hadi96 Member
    edited March 2019

    Dear sir, i had insert the rotating force, but after generate it show that no hit point

Sign In or Register to comment.