Abaqus 해석에서 댐핑(damping)의 적용

Abaqus 해석 프로시져 별로 damping source(material damping, element damping, global damping, modal damping, friction damping) 및 type(viscous, structural, friction-induced)에 따른 적용법을 설명한 문서입니다.

2013년 경에 정리했던 글인데, 오늘 보니 업데이트된 내용이 있어서 다시 공유합니다.

Applying damping in an Abaqus analysis

 

Q. How are the different types of damping used in Abaqus analysis procedures?

A. (The following applies to Abaqus 2016 and higher)

Damping is a phenomenon by which mechanical energy is dissipated in dynamic systems. Because it is impractical to incorporate a detailed representation of actual damping mechanisms in the computational analysis of mechanical systems, simplified models of damping are used in practice. These models are typically of the following types:

댐핑은 동적 시스템에서 에너지가 소산되는 현상임. 기계 시스템의 전산해석에서 실제 댐핑 메커니즘을 상세하게 표현하여 포함시키는 것은 실용적이지 못하기 때문에 실제 사용을 할 때는 댐핑의 간략화된 모델들이 사용됨. 이 모델들은 전형적으로 아래와 같은 타입으로 나누어짐

• Viscous
• Modeled as a force that is proportional to, but out of phase with, the velocity of the object; i.e., it acts in a direction opposite the velocity 물체의 속도에 크기가 비례하지만, 위상은 반대인 힘으로 모사됨. 즉, Viscous의 방향은 속도에 반대임
• Widely used, but only a small number of real engineering structures have damping elements where viscous dynamic properties can be readily assessed 널리 사용되고 있지만, 실제 엔지니어링 구조물에서 viscous dynamic property를 쉽게 측정(assess; 평가)할 수 있는 댐핑 요소를 포함하고 있는 경우는 많지 않음
• In most cases modal damping ratios are used in the computer model to approximate the complicated nonlinear energy dissipation mechanism within the structure 대부분의 경우 modal damping ratio는 구조물내에서 발생하는 복잡한 비선형 에너지 소산을 근사적으로 모사하기 위한 컴퓨터 시뮬레이션 모델에서 사용됨
• Structural
• Modeled as a force that is proportional to the displacement of the object, acting in phase with the velocity 물체의 변위에 크기가 비례하며, 속도와 동일 위상을 같는(in-phase) 힘으로 모사됨
• For many dynamic systems this model better reproduces the real life behavior than the viscous model 많은 동적 시스템에서 viscous 모델보다 실세계의 거동을 더 잘 재현함
• Damping mechanisms that originate in viscoelastic materials contribute to structural damping 점탄성 재질에서 기인한 댐핑 메커니즘이 structural damping 메커니즘을 만드는데 기여함
• Friction-induced
• Energy is dissipated at the interface of two sliding surfaces because of friction 두 미끄럼 표면의 계면에서의 마찰에 의한 에너지 소산
• Exists at points of contact, joints, supports, bearings, gears, etc. joint, support, bearing, gear 등의 접촉점에서 발생

 

The damping types described previously are introduced in an Abaqus model through: 상기 기술된 3가지 타입의 댐핑이 아래 5가지 방식으로 Abaqus 모델에 반영됨

• material and element damping
• global damping
• modal damping, and
• friction damping 

 

Using each source, both viscous and structural damping types can be introduced, and different damping sources can be combined in a single model: 각각의 댐핑 소스(materal, element, global, modal, friction)를 사용하여 viscous와 structural damping을 반영시킬 수 있음

• Material damping is included as part of a material definition
• Element damping may be included in mass, beam, and shell elements with general section properties. Also, the damping properties of dashpots, springs, and connectors are defined using this source of damping
• Global damping is used to apply abstract damping factors to an entire model. This source of damping is strictly a property of the computational model; therefore, sound engineering judgment should be exercised when using it in an analysis global damping은 전체 모델에 추상적인(abstract) 댐핑 효과를 부가하는데 사용됨. 이 댐핑 소스는 엄격하게는 전산모델에만 있는 속성임. 그러므로 이것을 사용할 때는 충분한 공학적 판단이 수행되어야만 함
• Modal damping provides a means to apply damping directly to the modes of the system and, therefore, is applicable only to mode-based linear dynamic analyses modal damping은 시스템의 모드에 직접적으로 댐핑을 적용하는 방법을 제공해줌. 그러므로, mode-based linear dynamic analysis에만 적용 가능함
• Friction damping can be included in some linear dynamics procedures and accounts for damping caused by a velocity differential at nodes in contact and/or a velocity-dependent friction coefficient friction damping은 일부 linear dynamics procedure들에 포함될 수 있음. 접촉하고 있는 노드들의 속도 차, 속도에 의존하는 마찰계수 등에 의해 유발되는 댐핑을 설명함

 

There is another source of damping in Abaqus that is called artificial damping. This source is purely numerical and therefore different from those discussed previously. For implicit dynamic analysis, it is used to allow the automatic time stepping procedure to work smoothly. You can control artificial damping by specifying the APPLICATION parameter or directly specifying the numerical damping control parameters α, β, and γ for the HHT-TF and HHT-MD time integration schemes. Abaqus에 artificial damping이라는 또다른 댐핑 소스가 있음. 이 소스는 순수하게 수치적이며, 이전에 논의했던 댐핑 소스들과는 다름

For explicit dynamic analysis, artificial damping is applied to the whole model using bulk viscosity, which is associated with volumetric straining. Linear bulk viscosity is included by default in the explicit dynamic analysis. Quadratic bulk viscosity is introduced to prevent elements from collapsing under extremely high velocity gradients and is applied only to solid continuum elements. You can control bulk viscosity using specific parameters that can be redefined and changed from step to step.

 

Treatment of viscous and structural damping in Abaqus dynamic procedures is summarized in Table 1.

 

Table 1 Treatment of viscous and structural damping in Abaqus dynamic procedures

Abaqus analysis type	Damping type	Sources of  damping in Abaqus
		Material damping	Global damping	Modal damping
Implicit dynamic	Viscous	*DAMPING, ALPHA=αR BETA=βR
	Structural
Subspace-based dynamic	Viscous		*GLOBAL DAMPING, ALPHA=αglobal, BETA=βglobal
	Structural		*GLOBAL DAMPING, STRUCTURAL=sglobal
Explicit dynamic	Viscous	*DAMPING, ALPHA=αR BETA=βR NOTE: Alpha damping acts on scaled mass if using mass scaling
	Structural
Direct-solution steady-state harmonic response	Viscous	*DAMPING, ALPHA=αR BETA=βR	*GLOBAL DAMPING, ALPHA=αglobal, BETA=βglobal
	Structural	*DAMPING, STRUCTURAL=s	*GLOBAL DAMPING, STRUCTURAL=sglobal
Complex eigenvalue extraction using SIM architecture	Viscous	*DAMPING, ALPHA=αR BETA=βR	*GLOBAL DAMPING, ALPHA=αglobal, BETA=βglobal	*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING *MODAL DAMPING, VISCOUS=RAYLEIGH
	Structural	*DAMPING, STRUCTURAL=s	*GLOBAL DAMPING, STRUCTURAL=sglobal	*MODAL DAMPING, STRUCTURAL
SIM architecture-based modal superposition procedures:  · Mode-based steady-state harmonic response · Subspace-based steady-state harmonic response · Mode-based transient response	Viscous	*DAMPING, ALPHA=αR BETA=βR	*GLOBAL DAMPING, ALPHA=αglobal, BETA=βglobal	*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING *MODAL DAMPING, VISCOUS=RAYLEIGH *MODAL DAMPING, VISCOUS=COMPOSITE
	Structural	*DAMPING, STRUCTURAL=s	*GLOBAL DAMPING, STRUCTURAL=sglobal	*MODAL DAMPING, STRUCTURAL
Response spectrum	Viscous		*GLOBAL DAMPING, ALPHA=αglobal, BETA=βglobal	*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING *MODAL DAMPING, VISCOUS=RAYLEIGH *MODAL DAMPING, VISCOUS=COMPOSITE *DAMPING, COMPOSITE=ξm
	Structural		*GLOBAL DAMPING, STRUCTURAL=sglobal
Random response	Viscous		*GLOBAL DAMPING, ALPHA=αglobal, BETA=βglobal	*MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING *MODAL DAMPING, VISCOUS=RAYLEIGH *MODAL DAMPING, VISCOUS=COMPOSITE *DAMPING, COMPOSITE=ξm
	Structural		*GLOBAL DAMPING, STRUCTURAL=sglobal	*MODAL DAMPING, STRUCTURAL

 

Abaqus/CAE Usage
*DAMPING, [ALPHA=αR | BETA=βR | STRUCTURAL=s | COMPOSITE=ξm]	Property module: material editor: Mechanical → Damping → [Alpha | Beta | Structural | Composite ]
*GLOBAL DAMPING, [ALPHA=αglobal | BETA=βglobal | STRUCTURAL=s]	Not supported in Abaqus/CAE
*MODAL DAMPING, [MODAL=[DIRECT | COMPOSITE ], RAYLEIGH | STRUCTURAL]	Step module: Create Step → Linear perturbation → any valid step type → Damping [Direct modal | Composite modal | Rayleigh | Structural]

 

Notes

• Table 1 does not include damping effects created by dashpots, connectors, acoustic elements, mass, rotary, and spring elements, added inertia, and viscoelastic material definitions.
• Please see Abaqus > Prescribed Conditions > Loads > Distributed loads to learn about the use of *DLOAD to specify mass-proportional damping in Abaqus/Explicit.

Treatment of contact interface damping in Abaqus linear dynamics is summarized in Table 2.

Table 2 Treatment of contact interface damping types in Abaqus linear dynamic procedures

Analysis type	Abaqus keyword
Direct-solution steady-state harmonic response analysis	*STEADY STATE DYNAMICS, DIRECT, FRICTION DAMPING=YES
Complex eigenvalue extraction	*COMPLEX FREQUENCY, FRICTION DAMPING=YES
Subspace-based steady-state harmonic response analysis	*STEADY STATE DYNAMICS, SUBSPACE PROJECTION, FRICTION DAMPING=YES

 

Abaqus/CAE Usage
*STEADY STATE DYNAMICS, DIRECT, FRICTION DAMPING=YES *COMPLEX FREQUENCY, FRICTION DAMPING=YES *STEADY STATE DYNAMICS, SUBSPACE PROJECTION, FRICTION DAMPING=YES	Step module: Create Step → Linear perturbation → any valid step type → Include friction-induced damping effects

 

Other uses of damping in Abaqus include:

1. Automatic stabilization of unstable static problems

If the instability is localized, there will be a local transfer of strain energy from one part of the model to neighboring parts, and global solution methods may not work. This class of problems has to be solved either with the aid of dynamic analysis or (artificial) damping; for example, by using dashpots.

Abaqus/Standard provides an automatic mechanism for stabilizing unstable quasi-static problems through the automatic addition of volume-proportional damping to the model. The applied damping factors can be constant over the duration of a step or can vary with time to account for changes over the course of a step (typically preferred).

For more information please see Abaqus > Analysis > Analysis Solution and Control > Solving nonlinear problems > Automatic stabilization of unstable problems

2. Viscous regularization for VCCT

*DEBOND, SLAVE=slave, MASTER=master, VISCOSITY=a

For more information please see Abaqus > Analysis > Analysis Techniques > Special-Purpose Techniques > Fracture mechanics > Crack propagation analysis > Defining initially bonded crack surfaces in Abaqus/Standard

3. Unconstrained rigid body motions

For more information please see Abaqus > Interactions > Defining Contact Interactions > Defining contact pairs in Abaqus/Standard > Adjusting contact controls in Abaqus/Standard

 

<출처>

https://onesearch.3ds.com/mashup-ui/page/resultqa?from=search%3fq%3ddamping&id=QA00000008411e&q=damping