##### Modeling rigid bodies

LS-DYNA allows the modeling of rigid-bodies by assigning any part with the MAT_RIGID material law (MAT_020). This is by far the most easiest method available when compared with all finite element codes. When using MAT_RIGID, there are three distinct ways to model a rigid part and they are briefly explaine below.

#### 1. Finite Element based rigid bodies

In this method, we first discretize the geometry using nodes and elements and use this information in LS-DYNA. The mass, inertia tensor and the center-of-gravity is then computed based on the density in MAT_RIGID keyword and the finite elements description.

#### 2. Coupling based rigid bodies

In this method, the rigid body is coupled to a third party sortware such as CAL3D or MADYMO. The parameter N allows the coupling between LS-DYNA and the third part software. When N = 0 (default), normal LS-DYNA rigid body updates are used. Using N>0, abs(N) refers to an ellipsoid while N < 0 , abs(N) refers to a plane. Further to this input, the parameter COUPLE , can be used to specify the reference coordinate system the nodal positions refer to. The parameter M is the actual number that links this LS-DYNA part to the part in the third-party software. When M > 0, all rigid body updates are assumed to be done by the third part software such as Madymo or CAL3D.

#### 3. VDA Surfaces based rigid bodies

This last method allows the direct input of VDA originally defined by the German automotive industry, to describe surface information. The VDA file describes the surface or a collection of surfaces by a alias name that refer to that surface. The first step would be to use the parameter COUPLE = -1 to inform LS-DYNA that the rigid body is represented by a VDA surface. The second step is to use the parameter ALIAS to specify the alias name as defined inside the VDA file. The third step is to provide the VDA surface to LS-DYNA which is accomplished by using ` vda = vda_file_name.vda ` at the execution command line when launching LS-DYNA.

#### Mass, Inertia Tensor and Center-of-Gravity (MIC)

In finite element based rigid bodies, the MIC is computed based on the density and discretization information. In Coupling based rigid bodies, the MIC is governed by the third-party software. In VDA rigid bodies, the MIC is computed based on the internal discretization of the surfaces.
All three methods allow overriding the MIC values by using the _INERTIA option in PART and specifiying user defined MIC values.

#### Contact

All general purpose contacts handle rigid bodies using penalty contact treatment. The Young’s modulus, E specified in the MAT_RIGID keyword and the thickness offsets (if the rigid body is discretized using shells) are used in contact treatment and must be chosen so they closely represent the physical part. When using Coupling or VDA based rigid bodies, instead of using nodes and elements in contact, the user can also use surface based contact such as CONTACT_ENTITY where the rigid bodies are defined as master and the impacting parts are defined as slave.

• Len says:

Thanks Suri.

A ‘trick’ I often use with rigid bodies is to specify the modulus of the deformable material to be contacted by the rigid body, rather than the modulus of the rigid body material.

Since a rigid body is rigid (obvious) the provided modulus is required to form the penalty stiffness for the contact. A well balanced penalty stiffness is obtained when both contacting bodies have the same material properties, i.e. the modulus in this case.