Learning Forum

[dardhruv]

hello,

test2.rar

[peteroznewman]

Array
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.

[dardhruv]

.

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

.

[BenjaminStarling]

.

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.

.

[dardhruv]

.

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

.

[BenjaminStarling]

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.

[dardhruv]

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

[Sean Harvey]

.

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

.

[hhusker]

.

Hi sharvey

I noticed how you coupled static to harmonic. I am trying to run a harmonic analysis to retrieve frequency response while the structure is prestressed. But I am unable to apply any load in Harmonic analysis when I couple the static structural for pre-stressing. What am I missing?

Regards,

Haafiz Husker

.

[Sean Harvey]

.

Hello hhusker,

So, if you right mouse button on harmonic response, do you see such a menu? There are different available options whether using this full method versus using the MSUP method. Thank you.

Regards,

Sean

.

[hhusker]

.

Hello sharvey

I was pointing to the fact that I cant apply a unit force in harmonic analysis to the prestressed structure. I was able to do so when using MSUP, but full method is returning much more accurate when not prestressed. So i would prefer to use full method to get the results AM I going fundamentally wrong somewhere in my approach?

Regards,

Haafiz Husker

.

[Sean Harvey]

.

Hello hhusker,

Thanks, just so I understand, you are not able to use a nodal force scoped to a named selection of nodes which can be any region of your model? Maybe I am missing something, and if so, my apologies. Regarding Full and MSUP not matching, have you extracted sufficient modes, and If your unit force is concentrated, you may wish to turn on residual vectors. There is a good video on that topic here /courses/index.php/courses/topics-in-harmonic-response-analysis/lessons/how-to-utilize-the-residual-vector-method-lesson-2/

Thank you

Sean

.