Learning Forum

[d.g.]

Hi everybody,

I'm Domenico and I'm new in the forum.

I need to solve a trouble with Ansys WB 18.0. I have to do a damped modal analysis, and so I need to set the damping values somewhere. I read in an official Ansys guide referred to 15.0 version, that it is possible to set alpha and beta damping values in the material editor (in this case different values can be assigned to different materials), or in the analysis setting options (in this case is a global damping value). However, if I try with the first option, an error message is generated:

"Material alpha and/or material beta damping coefficient defined in Engineering data are not contributing to modal damping calculation" 

How can I solve the problem? 

Moreover, how can I introduce directly the Damping coefficient ratio (that is funcion of alpha and beta coefficients)?

Thank you 

 

p.s. screenshorts are desirables.

[peteroznewman]

Hi Domenico,

I have the R17 Dynamics lectures, so I used some of that at the top and added R18 snapshots at the bottom.

The Rayleigh damping constants α and β can be saved either in the Material definition for each material individually...

or globally for all materials in Damping Controls.

Note that under Solver Controls, you have to set Yes for Damped.

If you know the value of the damping ratio ξ, you can calculate α and β from that value.
In many practical structural problems, mass damping may be ignored so α is set to zero.

        

Note that the coefficients are a function of frequency. It is commonly assumed that the sum of the α and β terms is nearly constant over a range of frequencies. Therefore, given ξ and a frequency range ω₁ and ω₂, two simultaneous equations can be solved for α and β.

 

Element Damping allows you to apply viscous damping directly to spring or bearing elements.

The above is all viscous damping and hence the dependence on frequency.

There is also Constant material damping that is independent of frequency. One model can have both types of damping. 

Release 18.2 Notes

The Analysis Settings provide the same ability to define damping as R17 when using materials that have not had damping added.

When I left these values at zero, and added damping to the material, the solver gave me the same results.

If you want to use Damping Ratio instead, click on the pull down on Stiffness Coefficient Define By and select Damping vs Frequency.

Then you can input the frequency and the damping ratio and the program will calculate β for you.

The attached file is an R18.2 archive (Domenico, you have to upgrade to Restore Archive).

I am curious how you obtained your Damping Ratio value, if you are willing to write about that..

Regards,

Peter

 

[MemoriseXuxu]

Hello,here I have another problem. Now have the value of modal damping ratio, which is 0.05 provided by a paper. However, in the ANSYS, it required me to input just one Frequency instead of two values and it doesn’t match the equation above. So , firstly, the value of frequency how I should input. Secondly,in the option “frequency vs damping ratio “ ,how the software calculate the stiffness.

I will appreciate it a lot if you can rely me. 

[peteroznewman]

In the dialog above, repeated here,

you put in one frequency in Hz and a Damping Ratio, then Mechanical calculates the Rayleigh Damping β coefficient for stiffness using this formula:

Note that ω does not equal 30 Hz, but is equal to 30*2*π. Did you forget to convert to rad/s?

You can type in your own Rayleigh Damping Mass coefficient, α.

ANSYS will then form a Damping Matrix using this formula:

The equation for the Damping Ratio given the two Rayleigh damping coefficients is:

The Damping Ratio is not a constant, but a function of frequency. If you want a relatively constant damping ratio between two frequencies, then you select the coefficients according to the formula shown in my last post. Say in addition to 30 Hz, you also want 10 Hz to be at 0.05 Damping Ratio, then the coefficients need to be:

Note: it is better for you if you start a New Discussion, rather than tack on to the bottom of an old discussion. The reason is you will be notified of replies if you start the discussion. In this situation, you have to remember to check back to see if there is a reply.

[Autonewbie]

Hi Peter,

May I know how to choose the two frequency if Modal analysis has been performed?

[saifali]

*

[peteroznewman]

@Autonewbie, you add damping to the model for harmonic response or transient structural using data acquired from experiments on the structure.  If you know the first natural frequency of the structure, you can excite that with a hammer strike, and using the log-decrement method, calculate a damping ratio for that frequency. Then you can make a hammer strike at a different location, in a different direction to excite the second natural frequency and record with an accelerometer the acceleration-time history and compute the damping ratio of the second natural frequency.

[Yuying]

Hello everyone, I'm yuying and I'm curious about the structural damping and hope someone can give me advice.

I'm using the student version of ANSYS WORKBENCH R18.0. And I'm trying to use the modal and transient dynamic analysis to do the same material in different shape of structure to see whether the quality factor will be affected by different structure, I have read some information from the internet and I know how to input the damping value and calculate the value, but I still have some questions from the formula(see the picture below). 

 

1. what's the physical meaning of alpha damping and beta damping

2. Are the alpha damping and beta damping related to frequency or independently

3. The first term of the formula is the material damping, how to define this term and what's meaning of this term

4. I would like to realize how does the damping work in the ANSYS transient dynamic analysis, will the program setting a model to calculate 

Thank you 

[Yuying]

ζ_i=α⁄(2ω_i )+(βω_i)⁄2+ζ+ζ_mi

ζ_i : integrated damping ratio

α⁄(2ω_i ) : relates to the component structure and mass matrix

(βω_i)⁄2 : represents mode internal friction which is derived from material stiffness matrix

ζ : material damping ratio which is derived from the material loss angle

ζ_mi : the individual modal damping that can be prescribed for each mode separately

 

β=2ζ/ω_i      α=2ζω_i       ζ=?/2, ? : loss angle

 

[tombowers]

Hi Peter,

Any chance of a link to a source for the equations for the damping coefficients?

Thanks, Tom

[Paolo]

Dear all

I'm  facing issue with beta coefficient. When I apply it as a global option in analysis settings, it works as I expect. But if I assign it to a specific material, it is ignored in the analysis, i.e. I always get the same (undamped) result regardless the beta value that I set in the material property. On the other hand, if I assign to the specific material the constant damping ratio, it works just fine. I'm performing harmonic response analysis with MSUP solver, to speed up the computation. Any suggestion?

[Erik Kostson]

 

 

 

 

Hi

 

In the help manual you will see that only damping ratio (MP,DMPR) is available on the material definition for MSUP.

Not beta damping, this is only available for the Global solver level for MSUP (analysis settings):
1.2. Damping (ansys.com)

See this video also for more details on MSUP and damping – also the help manual linear dynamics section has a lot of information.

https://www.youtube.com/watch?v=_1BASk_VyCQ

 

MSUP damping:

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

 

All the best

Erik

 

 

 

 

[Paolo]

Thanks, this clarifies my doubt. So, if I have a damper in my system (e.g. a viscous damper in a specific location, with a known "c" in N*s/m), what is the best way to simulate its damping behaviour in a MSUP analysis? I'm using the bushing element, and I'm assigning a constant damping with MP,dmpr, and I'm computing the value as c/(2*sqrt(k*m)), thus setting the damping ratio with respect to the first mode even if the component is involved in many other modes of the assembly. Is it reasonable?

Additionally, is there an easy way to plot the distance between two points in frequency domain? The only way I can think about is to export to matlab ux, uy and uz of both points and do some computation outside ansys,  but I would really appreciate if I could define this result (in frequency domain) inside the ansys workbench simulation.

Thanks!