Warning: The use of stiffness proportional material damping in Abaqus/Explicit may reduce the stable time increment dramatically and can lead to longer analysis times. See “Material damping,” Section 25.1.1 of the Abaqus Analysis User's Manual.
This option is used to provide material damping for mode-based analyses and for direct-integration dynamic analysis in Abaqus/Standard and for explicit dynamic analysis in Abaqus/Explicit.
Damping is defined in a material data block except in the case of elements defined with the *BEAM GENERAL SECTION option, the *SHELL GENERAL SECTION option, the *ROTARY INERTIA option, the *MASS option, or the *SUBSTRUCTURE PROPERTY option. For the *BEAM GENERAL SECTION, the *SHELL GENERAL SECTION, and the *SUBSTRUCTURE PROPERTY options the *DAMPING option must be used in conjunction with the property references. For the *MASS and the *ROTARY INERTIA options damping must be specified using either the ALPHA or the COMPOSITE parameter associated with these options. Damping may also be defined as step data using the *GLOBAL DAMPING option and may come from damper elements like connectors and dashpots.
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
Type: Model data
Level: Part, Part instance
Abaqus/CAE: Property module
“Material damping,” Section 25.1.1 of the Abaqus Analysis User's Manual
“Dynamic analysis procedures: overview,” Section 6.3.1 of the Abaqus Analysis User's Manual
“Explicit dynamic analysis,” Section 6.3.3 of the Abaqus Analysis User's Manual
Set this parameter equal to the 
factor to create Rayleigh mass proportional damping in the following procedures:
*DYNAMIC (Abaqus/Standard or Abaqus/Explicit)
*STEADY STATE DYNAMICS, DIRECT
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
*STEADY STATE DYNAMICS that allows nondiagonal damping
*MODAL DYNAMIC that allows nondiagonal damping
This parameter is ignored in mode-based procedures that follow Lanczos or subspace iteration eigenvalue extraction.
The default is ALPHA=0. (Units of T–1.)
Set this parameter equal to the 
factor to create Rayleigh stiffness proportional damping in the following procedures:
*DYNAMIC (Abaqus/Standard or Abaqus/Explicit)
*STEADY STATE DYNAMICS, DIRECT
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
*STEADY STATE DYNAMICS that allows nondiagonal damping
*MODAL DYNAMIC that allows nondiagonal damping
This parameter is ignored in mode-based procedures that follow Lanczos or subspace iteration eigenvalue extraction.
The default is BETA=0. (Units of T.)
This parameter applies only to Abaqus/Standard analyses.
Set this parameter equal to the fraction of critical damping to be used with this material in calculating composite damping factors for the modes. Composite damping is used in modal based procedures that follow Lanczos or subspace iteration eigenvalue extraction, except for *STEADY STATE DYNAMICS, SUBSPACE PROJECTION. Use the *MODAL DAMPING, MODAL=COMPOSITE option to activate it.
The default is COMPOSITE=0.
Set this parameter equal to the 
factor to create imaginary stiffness proportional damping in the following procedures:
*FREQUENCY, DAMPING PROJECTION=ON
*STEADY STATE DYNAMICS, DIRECT
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
*STEADY STATE DYNAMICS that allows nondiagonal damping
*MODAL DYNAMIC that allows nondiagonal damping
This parameter is ignored in mode-based procedures that follow a Lanczos or subspace iteration eigenvalue extraction.
The default is STRUCTURAL=0.