material damping and modal analysis

  • Last Post 17 December 2017
d.giaccone posted this 12 December 2017

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 posted this 17 December 2017

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..




Attached Files