Control cards are often handy to overwrite local values. A good example would be if we need all parts to use a certain element formulation THEORY which is specified in *CONTROL_SHELL.
As with any global control cards that manipulate local values, the global values specified in *CONTROL keywords are used ONLY if the local values are either zero or blank. If any of
the parts that uses a SECTION_SHELL keyword whose ELFORM parameter is non-zero, then THEORY is ignored and the value from ELFORM will be used.

An exception that I recently found is in the values ISOLID, IBEAM, ISHELL and ISOLID found in *CONTROL_IMPLICIT_EIGENVALUES keyword. These element formulation
parameters were originally implemented for handling NASTRAN input files read using *INCLUDE_NASTRAN but it applies for now for any model. Unlike other global
value setting, these values overwrite all local values irrespective of them being ZERO or blank.

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.

Happy New Year !

Wishing everyone a very happy new year.

Significance of IGAP Parameter in *CONTACT in Implicit Analyses

In traditional explicit analysis, there is no convergence criteria that is checked for each time step. However, in Implicit calculations, incremental displacements are evaluated such that a displacement norm and the energy norm are within a pre-defined tolerance before convergence is assumed to be obtained. This is the so-called iterative scheme in Implicit Non-Linear Analyses (Static and Dynamic).
Any non-linear problem will eventually involve contact between surfaces for large deformation problems. LS-DYNA handles these contact much the same as in Explicit analysis where a penalty-force is imposed if a node is found to be inside a volume of another part. In the case of the Implicit a penalty is imposed by adding a stiffness matrix when the contact is detected and the penalty force is added to the right hand side.
In certain cases, the sudden detection of contact penetration and subsequent addition of the stiffness causes some difficulty in convergence for Implicit analyses. To overcome this, LS-DYNA introduced a parameter called IGAP where the stiffness is not added instantaneously but rather ramped up to 100% over a certain number of iterations. Also, no force vector is added to the right hand side. This has a tendency to cause a ’sticky’ condition which seems to help overcome convergence issues. IGAP is now set to ON by default. Care must be taken to ensure no excessive penetration is present in the model even with IGNORE=1.

Marsha Victory, Thank You For Your Blog Hosting Sponshorship !

I am pleased to inform that Marsha Victory has continued the sponsorship of D3VIEW blog hosting. If this blog has been of help to you, please take a moment to thank Marsha. She can be contacted at marsha at lstc dot com.

Thanks very much, Marsha, for your support.

Boundary prescribed motion and Contact

When nodes are involved in both contact (penalty) and prescribed motion, contact failure is expected to occur. This is because the boundary conditions are always processed after all the contacts are handled that results in nodal accelerations being updated to enforce the boundary conditions. I will soon publish some examples to illustrate this phenomenon.