You can define MATERIAL DAMPING as material property. 

Thank you Anshul for your reply but:

Unfortunately Abaqus itself considers some kind of numerical damping in implicit analysis that differs to material damping, so even by considering a material damping, some additional damping would be taken into account with ABAQUS. consider that you want to model a simple structure with out damping under impuls load and determine the free vibration. The question is how can we control the exact damping that is considered by Abaqus in implicit analysis.

This is from ABAQUS analysis user's manual:

Marching through a simulation with a finite time increment size generally introduces some degree of numerical damping. This damping differs from the material damping discussed in “Material damping,” Section 23.1.1 (and in many cases these two forms of damping will work well together). The amount of damping associated with the time integration varies among the operator types (for example, the backward Euler operator tends to be more dissipative than the Hilber-Hughes-Taylor operator) and in many cases (such as with the Hilber-Hughes-Taylor operator) depends on settings of numerical parameters associated with the operator. The ability of the operator to effectively treat contact conditions is often of considerable importance with respect to their usefulness. For example, some changes in contact conditions can result in “negative damping” (nonphysical energy source) for many time integrators, which can be very undesirable.

Attached you can find the ABAQUS manual about the considered unknown numerical damping.

http://www.ilsb.tuwien.ac.at/v6.10/books/usb/default.htm?startat=pt03ch06s03at07.html

Manual says that for Hilber-Hughes-Taylor operator you can modify these parameters. Using following command. 

*DYNAMIC, ALPHA=, BETA=, GAMMA=

There parameters controls numerical damping. Default values of these parameters are given in Table 6.3.2–1 of attached manual. 

First, consider the fact that you have to deal with damping waves of different nature: One, the damping physical wave(s) that you really are trying to simulate: This type of damping you should deal with by using material damping.  Two, the undesired but nonetheless existing numerical waves that appear because of the discretization of both space and time: This waves have no direct relationship with the actual physical problem and are very much dependent on the mesh density and the time increment; this type of damping is the one dealt with the parameters used in the *DYNAMIC keyword; the values provided by default resulted after extensive numerical testing done by the developer but may need to be adjusted for specific problems like yours.  What I suggest you can do is to check the sensitivity of your model to at least three mesh densities and three time increments, as well as a to three changes on the alpha, beta, and gamma parameters about the defaults.  Hopefully you have either measurements, or a theoretical solution, or a particular behavior you are trying to match; throw in sensitivity to the two parameters in material damping about the values that result from the first eigenvalue on linear vibration, and you have quite a collection of simulations to run and deal with, so it can be quite cumbersome, sorry.

Thank you for your valuable comments. So the question could be changed to:

How can we control the EXACT amount of damping ratio (for example 1%) during analysis by changing the ALPHA,BETA and GAMMA in ABAQUS?

Hi Hamid,

Please go through Chopra's Structural Dynamics to find equations to estimate alpha and beta.

Xiangxiong

Hi,

For Rayleigh's Damping (ie.Alpha-Mass propotional  and Beta-Stiffness propotional) you can go through this article.

https://wiki.csiamerica.com/display/kb/Damping+coefficients

cheers.

Hamid, from your earlier and your updated question that I take refers to my previous answer, and the fact that you include gamma in your questions it seems that you are asking about the damping of the high-frequency numerical waves.  If this is a case, here goes a brief advise.  Otherwise remit to the answers of the other fellows which obviously believe you are asking about damping of the physical (material, Rayleigh) waves.  Hence, for the parameters in the *DYNAMIC keyword, you could simplify the work of studying the damping of numerical waves by taking advantage of the following.   If you only change alpha, Abaqus will compute beta and gamma automatically.  If you chose a fixed time increment equal to 40% of the period of oscillation of the mode of your interest then a (negative!) value alpha = -0.3333 produces the maximum damping approximately equal to 6%.  With the same fixed time increment and alpha = -0.05555 you will get about a 1% of damping of the numerical waves.  Please realize this is independent of the damping of the physical waves! 

Dear Leonard,

You point out exactly what I mean. The problem which I am dealing with is so sensitive to the exact considered damping in the analysis so I shall control the damping during the computer simulations accurately.

I know how Abaqus considered the damping in its procedure but as the numerical damping also would taken into account, I shall determine the amount of it exactly so one possible solution could be trying to get the results in zero damping conditions and comparing with the main simulation.

I am working on it and in this regard, any idea would be appreciated.