prestressed harmonic analysis

dardhruvdardhruv Member Posts: 23
edited November 2020 in Structural Mechanics

hello,

@peteroznewman

I am trying to do prestressed harmonic analysis.

for that, first I have used static analysis and solution of static analysis used in harmonic analysis

One silicon cylinder membrane clamped on edge and using trans126 I haver applied 400v (ramped). Static analysis works fine but in harmonic analysis I didn't get any plot.

Could anyone please help me?

I have attached workbench file.



Thanks in advance

Regards,

Dhruv

Comments

  • peteroznewmanpeteroznewman Member Posts: 11,073

    @dardhruv

    I haven't opened your model, but looking at the images, I don't see any load applied in the Harmonic Analysis. I don't know what is in the Command object.

    The loads applied in the static analysis are only for computing the pre-tension stress and are not harmonic.

  • dardhruvdardhruv Member Posts: 23

    Hello Sir,

    @peteroznewman

    I have used large signal analysis in static and want to use small signal for harmonic.

    I have applied load using apdl command

    apdl command which I have used.


    If its possible then please check my file.


    Thanks in advance sir


    Regards,

    Dhruv


  • BenjaminStarlingBenjaminStarling AustraliaMember Posts: 88

    Hi Dhruv,

    You do not need to create the TRANS elements again using the EMTGEN command, in fact this is not possible as it is a linear perturbation analysis of the static structural. In your solver files directory of the static structural, find the ds.dat file. In this file you will see where the EMTGEN command is input.

    I have highlighted all you need for your harmonic response. I took those highlighted commands, and placed them in a command snippet, changing 400 to 10. the result I got is shown below at 2.5e6 MHz. I supressed your original command snippet.


  • dardhruvdardhruv Member Posts: 23

    Hello Mr. BenjaminStarling,


    I got same result using your code. But I don't why it is showing distortion in geometry.

    anything wrong?

    I am planning to understand one research paper

    https://ieeexplore.ieee.org/stamp/stamp.jsp?arnumber=6813847.


    Could you please suggest me? Am I going in right direction according to this paper?

    First I have to apply large signal (DC) in static then small signal (AC) in harmonic. for that, should I delete degree-of-freedom constraints suing DDELE command??


    Thanks and Regards,

    Dhruvin

  • BenjaminStarlingBenjaminStarling AustraliaMember Posts: 88

    Hi Dhruvin,

    I do not have access to that article so I am unable to understand their modelling methods.

    Your question is not clear regarding distortion. Are you referring to the non uniform displacement field? This is due to the very small displacements of this model and the parabolic elements being used. If you swith to linear elements and mesh much finer this displacement field will appear much smoother.

    The reason the parabolic elements are doing this is the corner nodes of a parabolic element actually have negative stiffness. This along with uniform reduced integration, and a non uniform mesh, results in this random-esque appearance of the displacement field.

    Also to remember is that the displacement field is being applied to the undeformed geometry in the Mechanical application. This is not what is actually happening, the harmonic response is using the deformed shape from the static structural analysis. You can confirm this by viewing the result file in MAPDL.

  • dardhruvdardhruv Member Posts: 23

    Thank you so much Benjamin. I will simulate using fine mesh size.

  • sharveysharvey San Diego, CAMember Posts: 75

    Hello @dardhruv,

    We noticed your questions in the Ansys Learning channel on YouTube. You asked a few questions. Let's see if this helps.

    To perform a pre-stressed harmonic analysis you can do a pre-stressed modal followed by harmonic. This video details the pre-stress modal method.

    https://www.youtube.com/watch?v=XyCZVHl8QKg

    If you are going to use the full method, you can connect static structural to harmonic as shown below and this will be a pre-stress harmonic using the full method.


    Now you also asked about MSUP (Mode Superposition Harmonic) vs Full. It is discussed in this course.

    There are advantages to both methods, but in general, here are some key points;

    -Solve for the modes once, then the solution of the harmonic equations is quick and you can experiment with different loads without having to rerun the modal analysis. In full you will have to resolve all the equations and this can take increased time

    -You can use modal damping where the damping ratio is a function of frequency, and this can help in correlating simulation with test

    -MSUP harmonic solves fewer uncoupled equations

    -If you extract too few modes, you will get inaccurate results, so take care that sufficient modes are extracted


    Finally, you had asked about damping and you will also find a newly release damping course on the platform, and in that course we discuss some general guidlines on damping values, but also, how to experimentally compute damping ratios.

    I hope this helps. Please let us know. Thank you.

    Regards,

    Sean Harvey

Sign In or Register to comment.