Mesh Refinement Studies Involving Shell Elements

In many situations, we tend to change the mesh density to study its effect on simulation responses. Two issues things that are seldom addressed are the contact thickness and the mass-scaling which blend in with the true effects of the mesh refinement. As stated in some of the earlier posts, LS-DYNA computes the contact thickness that is some fraction of the element edge length if SSTHK=0. For any mesh studies involving shells, one must always use SSTHK=1 such that the contact thickness is independent of the element dimensions. The second issue is the use of mass-scaling which can be minimized by choosing a DT that results in identical mass-scaling in all the comparitive runs. This can cause additional difficulties when several parameters such as contact stiffness in SOFT=1,2 are based on global DT which if changed will change stiffness. To avoid this, it is recommended to choose the minimum DT of all mesh variations as global DT for all simulations involving mesh refinements.

DKT Triangular Shell for Crash

Default element sorting for 3-noded shell elements uses the collapsed BT formulation which is not recommended but is maintained for backward compatibility. The first option that LS-DYNA offers is to sort these elements to use a C0 triangular shell formulation which may provide better answers than the default formulation. LS-DYNA 971 (R3 and later) now offers the sorting to use a DKT formulation that shows encouraging results for crash analysis. You can read the original paper (PDF) for more information. You can invoke the DKT sorting by setting the ESORT=2 in *CONTROL_SHELL keyword.

Contact Surface Generation for Solid Elements

By default, when a solid part ID is included in a contact slave or master part set, LS-DYNA generates a segment list for only the outer skin of the solid element volume. This is truly only if the slave or master set type is a segment list since for a node slave or master list, all nodes of the solid part ID will be included.
In certain situations, such as in foams or rubbers or honeycombs, it may be necessary to include the segment list of the interior elements of the solid PART ID. In such cases, the use of *SET_SEGMENT_GENERAL can be used along with PART_IO which causes LS-DYNA to not only generate the list of segments for the outer skin but it also generates the segments for ALL interior elements as well. This allows the automatic inclusion of interior segments in contact even for non-EROSION type contacts when the outer solids erode.

Consolidating Multiple Contact Definitions to a Single Contact

Over the last few years, the simplicity of defining a global AUTOMATIC_SINGLE_SURFACE contact to treat the interactions between multiple parts of varying stiffnesses and element types has changed the way we model contact interfaces. They are not only simple to define but also promote better modeling since they hugely eliminate the need to manually identify contact surfaces which may be prone to errors. Legacy models which could have several hundred contact definitions (one-way and two-way types) can be extremely difficult to convert to a single contact definition since it requires a thorough review of manually defined segments. Here are some approaches that could be followed to migrate the legacy models to use a single consolidated contacts.

Approach 1
The simplest approach is to identify all the segments and use the parent parts to define a single surface definition. The main disadvantage is that segments which may not have been included in original contact definitions will now be included which may introduce new errrors especially if the newer segements are inter-penetrating.

Approach 2
The second approach, which is the recommended approach, is to take advantage of the output from D3HSP file. For every contact defintion (one-way or two-way) in the legacy models, LS-DYNA outputs the list of slave-segements (two-way) and a list of master-segments into the D3HSP file. We can consolidate all the slave and the master segments from the D3HSP file into one global segment list and use this segment list in a single surface definition. This avoids the addition of new segments. If we need the forces of interface as in the original legacy model, we can simple change the old contact defintions to a FORCE_TRANSDUCER contact which will provide a way to extract crucial interaction forces.
In some situations, the frictional constants can be different between various older contact interfaces. To model this, we can use the DEFINE_PART_FRICTION along with FS<0 to model part-pair based frictional coefficients.

Principal Stress Calculator for Shell Elements in DYNAIN File

Recently, there was a request to ouput the principal stresses for each element at lower and upper surfaces of each shell element in DYNAIN file to use in some failure theories. I beleive this feature is a routine output in PamStamp simulations. To enable this, the attached ‘C’ code can be used that reads in a DYNAIN file (valid output from LS-DYNA) to use the stress-tensor and output the principal stresses for each element at lower and upper surfaces.

Principal Stress Calculator (Version 12)