Learning Forum

[Carlos Pérez de Lema]

Hello, first post here. Usually I am able to find the responses to my questions in older posts, but I have not been able.

 

Currently I'm studying the vibrations of a water turbine. I have perfomed a modal acoustic analysis to veify that the mode shape and frecuency coincides with the one meassured experimentally. My model is the turbine with a simplified 1D element axis with an acoustic body in the place of the water. The acoustic body is very important because it has a huge added mass effect due to it being confined to a small space. Rotor is no spinning in the simulation, so the natura frecuencies are calculated for the machine stopped.

 

 

Modal Acousics is behaving as expected and the desired mode is found at the expected frecuency.

 

 

What I am really interested in, is calculating the stresses on the structure. I have meassurements on the amplitude of the vibrations and was hoping to extrapolate those amplitudes into the model and obtaining a harmonic response calculation. Harmonic Acoustics shows the expected vibrations at the right excitation frecuency.

 

The main problem is I am not able to get ANSYS to output the stress values on the structure like I'd be able to in an Harmonic Response. Clicking on the option in the output Controls Window does not work.

 

 

 

Am I doing something wrong? Should I use some other kind of module? 

 

Thank you in advance.

 

ANSYS version is 2020 R2

[Erik Kostson]

 

Hi

Not sure why it is locked (perhaps you are sharing the modal acoustic model with harmonic acoustic, then set this in modal acoustic).

Otherwise, use an apdl command snippet with the below in harmonic acoustic (put in the tree, where you apply loads and boundary conditions):

OUTRES,ALL,ALL

All the best

Erik

 

[Carlos Pérez de Lema]

I'll try that and report back. You are right, I am sharing the model, since I'm not able to import the results of the modal acoustic as the setup of the harmonic acoustics.

Also, sorry for the duplicate posts, won't happen again. :)

[Carlos Pérez de Lema]

Tried both options. Modal Acoustics allows me to check yes to all of the output controls, but harmonic acoustics still does not allow it. Using the commands does not work either.

[Erik Kostson]

Hi

So do a separate harmonic acoustic  - so without sharing the modal acoustic system with it and set all outputs to yes. 

All the best

Erik

 

[Carlos Pérez de Lema]

I found the culprit. I used ANSYS bearings to define the stiffnes of the bearings attached to the axis. For some reason they are not compatible with outputting stresses in an harmonic response. I will find a way around modelling them this way and everything should work. 

[Erik Kostson]

 

Hi

Thanks for letting us know.

I should say that in 2022  and 2023 R2 having a bearing in fully coupled vibroacoustic harmonic analysis (so harmonic acoustic system) is fine and we can post process stress results on the structure without any problems. 

All the best

Erik

 

[Erik Kostson]

SO the issue is that you have beam elements (1D line bodies) - only 3D elements / geometries are supported in harmonic acoustic.

All the best

Erik