natural frequencies milling machine

[JeroenDevos]

Hello everybody,

I am a first time ansys user, charged with the job to find the natural frequencies and modes of a milling machine. However, I've got a few problems with the results I get.

first problem:
1. I do a modal analysis in the domain 20-200Hz with Power dynamics or Block Lanzcos method
2. I get millions of natural frequencies (understandable, a complicated system has infinit natural frequencies). However, I am interested in the most important ones. What do I have to change in my model? I allready use the biggest mesh size possible to reduce the details in the model.

second problem:
I considered using the reduced method. Hereby however, you have to define master degrees of freedom. I don't really understand how to define them. When I let the computer define them, ansys gives me no solutions (no results file available). Can anyone explain me how to define the MDOF?

Can anybody help me out please,
I'd appreciate it!!

Jeroen

 

[cbrn]

Hi,
to find which are the "most important" modes, I'd suggest looking at the participation factors for each DOF. Ansys outputs the participation factors in the Output Window, so in order to save them you have to redirect the output to file prior to launch the solution:
/OUTPUT,<filename>,<extension>
and then restore the original setting when you're finished:
/OUTPUT,

Regards

 

[JeroenDevos]

Hi,
thx for the reaction cbrn. Now, I thaught about adding damping to the system to suppress the less important natural frequencies.
I use the damped method with SOLID 187 elements. However I don't manage to find a way to define how much damping I want to add. When I change the value of the constant damping ratio under "solution>load step options>Time/freq>damping" it doesn't affect my results.
Do I have to change the elemnt type, solution method (QR damping) or change another setting to influence the damping?

I'm very sorry if these are simple questions for most of you, but I use ANSYS for the first time!

Thanks in advance,
Jeroen

 

[JeroenDevos]

And a few other things,
1. what's the physical meaning of a negative participation factor?
2. what's the effective mass (outputted next to part.factor)?
3. I hope you have to give frequencies in Hz (cycles/s) in Ansys and not in rad/s?

Thank you!!!!
Jeroen

 

[cbrn]

Hi,
damping is a very complex topic in Ansys (as in all the other top-of-the-class FE systems). You have several possible inputs to create damping:
- DMPRAT: damping ratio, for use only in harmonic response, mode superposition transient, and spectrum analyses
- ALPHAD, BETAD: Rayleigh damping constants, can be used also for modal analyses in combination with Damped or QR-Damped solvers
- DAMP or DMPR in MP command: intrinsic damping of the material, can be used for modal analyses with Damped or QR-Damped solvers
- TB commands: used to specify non-linear tabular data for the material (a bit complicated...)

The key for modal analysis is to choose a solver which handles the damping matrix [C]; see the Help system (Chapter 3: Modal Analysis) for more details, it's very well explained.
Then, another point will be finding the correct values for alpha and beta or for the material damping...

However, you DON'T need damping to filter-out insignificant modes: you'd better use the SIGNIF setting in the MXPAND command: in this way, the mode expansion will be done only on those modes where the mode coefficient divided by the maximum modal coefficient is greater than the threshold you specify.

Hope this helps...

Regards

 

[JeroenDevos]

Hi,

thanx again cbrn! I'm trying to figure it out. One more thing though,
- what's the physical meaning of a negative participation factor?
- what are the residual masses?

thanks in advance,
Jeroen

 

[JeroenDevos]

Oh yeah,

what does a participation factor represents in fact? I thaught it was the participation of the mode in the total vibration of the system. This implies however that the sum of all the participation factors has to be one and that a participation factor has to be greater than 0. However, I obtain values greater than 1 (2000 and more) and even negative values.
What does this represent?

thank you for help!
Jeroen

 

[cbrn]

Hi,
all depends upon how you choose to normalize the eigenvectors. In fact, by definition any arbitrary linear combination of the base of the eigenspace is a solution of the eigenproblem; in other terms, the amplitudes of the eigenvectors are arbitrary.
If you normalize them to unity, then the vectors norms vary from 0 to 1; if you normalize them to mass (the default in Ansys), the norms range from 0 to [M].
In addition, the participation factors are calculated based upon an arbitrary unit spectrum amplitude along each global cartesian axis, so when you see a negative value it means that the eigenvector is in antiphase. The residual mass is the fraction of "mass" (eigenvecors factorization unit...) which is not covered by the processed vectors: this value tends to 0 by increasing the number of extracted modes.

Regards

 

[JeroenDevos]

Hi,
thank you very much cbrn!!!! I'm on the roll now I manage to find natural frequencies of the system. I use the SIGNIF command like you proposed before. One thing I still don't understand though is the 'Spectral value versus frequency curve'. I don't get what it represents. I just use the values that are given in an example in the help file. By using these values I get solutions, but I don't know if they are correct because I don't understand the nature of these values.
I read every file that mentions this curve, but I still don't get it!
Is it the spectrum of the force that's applied?
And what about the spectral values?

I sincerely hope that this is the last question about this topic!!

Jeroen

 

[cbrn]

Hi,

oops, you are mixing up things a little bit, I fear... If you come across the "spectral values vs frequency", it means that you are doing a spectrum response analysis, not an eigenmode extraction.
In a spectrum response analysis, you have to input an excitation as spectrum (can be displacement spectrum, velocity or acceleration). Ansys can't manage a continuous law curve, however it will discretize your spectrum in a sequence of linear segments connecting the points "frequency - spectral value" which you input separately with two tables: the frequency table and the spectral values table.

All this is perfectly useless in a modal analysis. Perhaps it's the SIGNIF command that directs you to that. I personally never used it in a modal analysis because I've got a series of Excel files in order to do some post-processing. If this is the case, then I believe that you can input a constant displacement spectrum (=constant excitation -> the response will be uniformly affected by all the excitation frequencies, without emphasis of some modes despite of others). But I would really check if you aren't in a spectral analysis "by error"...

Hope this helps!

Regards