Skip to main content

Analysis in LS-DYNA

GSA provides most of the analysis capabilities for structural models, however for advanced analysis there is an option to create an LS-DYNA analysis task.

This feature is provided to make it simpler to maintain a single reference model and analyse in the appropriate tool.

Mapping between GSA and LS-DYNA​

Some features available in GSA are not available in LS-DYNA and other features have been added to GSA, to facilitate LS-DYNA analysis, but which are not available for analysis in GSA. Analysis stages provide a way of coordinating between the GSA and LS-DYNA models. Using the analysis stages nonlinear (LS-DYNA) materials can be assigned to the model while retaining the linear materials used by GSA.

Analysis Parameters​

The Analysis Wizard allows an LS-DYNA keyword file to be created, generally for a selected analysis stage. The analysis parameters for specification of timings, excitation and elements formulations. Termination and output times (whole model and time history) can be set. Excitation can be selected as a force excitation or base excitation. Assemblies can be specified – these are exported as cross sections.

In addition to the mass of the structure additional mass can be added for the LS-DYNA analysis. This is selected as a loading which is converted to a mass elements when creating the LS-DYNA model.

The final stage in the analysis task selects a keyword file for output and the environment to launch. A default environment can be set in the Preferences.

Materials​

GSA is used primarily for materially linear problems, while LS-DYNA generally uses nonlinear materials. To accommodate this a number of LS-DYNA material models can be defined in GSA. The following models are available for LS-DYNA:

  • Concrete EC2
  • General Nonlinear Beam
  • Hysteretic Beam
  • Hysteretic Reinforcement
  • Park Ang Beam
  • Plastic Kinematic
  • Seismic Isolator

Some of these material models refer to Load Curves in LS-DYNA. These are defined as Material Curves in GSA, and transferred as load curves.

Spring/damper elements​

LS-DYNA considers some spring elements as variants of beam elements and in general regards springs as single degree of freedom entities. These simple springs are written as ELEMENT_DISCRETE. For simple springs the orientation option (VID) is set to 0 so the spring acts along the axis between the nodes. For more general springs the GSA element is written as a DYNA element for each stiff direction. In this case the orientation option is set to the number of an DEFINESD_ORIENTATION record with option (IOP) set to 1 and a vector defining the direction of action (XT,YT,ZT). Springs and dampers are differentiated by using different material definitions. For a spring the element relates to a *MAT_SPRING definition and a damper refers to a *MAT_DAMPER_VISCOUS definition.

The properties for a linear elastic spring are written as MAT_SPRING_ELASTIC defining the stiffness (K). A nonlinear spring is written as MT_SPRING_NONLINEAR_ELASTIC with the spring curve written as a load curve referred to by LCD. Tension and compression only springs are written as *MAT_SPRING_INELASTIC and a load curve is generated for the stiffness (LCFD) and the compression tension flag is set (CTF) as required

GSA springs

Linear spring in x - This is written as a ELEMENT_DISCRETE with a MAT_SPRING_ELASTIC for the stiffness

Linear spring in all 6 dof - This is written as a ELEMENT_BEAM with ELFORM set to 6 with a MAT_LINEAR_ELASTIC_DISCRETE_BEAM defining the stiffness in all 6 dof

Nonlinear spring in all 6 dof - This is written as a ELEMENT_BEAM with ELFORM set to 6 with a MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM defining the material curves of stiffness in all 6 dof. If some of the dof are linear these must be converted to (nonlinear) material curves

Tension-only and compression only springs - These must be converted to a nonlinear spring and can then be written as ELEMENT_DISCRETE with material MAT_SPRING_INELASTIC

Lockup elements - These must be converted to a nonlinear spring and can then be written as ELEMENT_DISCRETE with material MAT_SPRING_INELASTIC

Connector elements - These are exported as ELEMENT_BEAM with ELFORM set to 6 with a MAT_LINEAR_ELASTIC_DISCRETE_BEAM defining a stiffness in all 6 dof of 1e10.

Gap elements - These are not exported at present

Friction elements - These are not exported at present

GSA Damper

Linear damper in x - This is written as a ELEMENT_DISCRETE with a MAT_DAMPER_VISCOUS for the damping

Linear damper in all 6 dof - This is written as a ELEMENT_BEAM with ELFORM set to 6 with a MAT_LINEAR_ELASTIC_DISCRETE_BEAM defining the stiffness in all 6 dof.

Rayleigh damping

In addition to damper elements , Rayleigh damping can be specified. Rayleigh damping is written as α and β in the DAMPER_GLOBAL record and DAMPING_PART_STIFFNESS respectively.

Composite shells​

GSA does not provide options to analyse composite shells. To allow for this in LS-DYNA there is an option in the 2D element properties wizard to define a composite shell. This allow a series of layers to be specified in terms of a material, a thickness and an angle. If these are specified the element thickness is the sum of the thicknesses of the layers.