Media transport analysis using import from Abaqus/Standard to Abaqus/Explicit
Elements tested
- C3D8R
- M3D4R
Problem description
The verification test in this section is a media transport analysis of a periodic media consisting of nine blocks modeled using M3D4R and C3D8R elements. The membrane elements are used to model the conveyor belt, and the brick elements are used to model the packages on top of the belt. The packages are tied to the belt with a tie constraint. The model is pre-stretched using Abaqus/Standard and imported to Abaqus/Explicit, where the periodic media is defined and activated. The belt is set in motion at the beginning of the Abaqus/Explicit analysis by specifying a uniform initial velocity. The model is illustrated in Figure 1.
Because the periodic media analysis technique is not available in Abaqus/Standard, the ties between blocks must be defined explicitly using a tie constraint and the boundary conditions at the inlet and outlet must be defined directly at the nodes. In addition, the front end nodes of the inlet block must be constrained to have identical displacements as their corresponding nodes in the back end of the inlet. This is accomplished by defining an equation constraint between corresponding nodes that forces the y-direction displacements to be equal. The belt is stretched by fixing the inlet nodes and displacing the outlet nodes in the x-direction.
In the Abaqus/Explicit analysis the periodic media is defined using element sets and node sets. Two rollers are added with general contact defined between the belt and the rollers. Both the inlet and outlet control nodes are fixed in the y- and z-directions and given a velocity of 1000 in the x-direction. All of the belt and package nodes are given an initial velocity of 1000 in the x-direction. Block shuffling takes place when the back end of the inlet passes the trigger plane. The trigger plane is located at an x-coordinate of –200 and is normal to the x-direction.
Results and discussion
The belt is stretched in the Abaqus/Standard analysis, and the stress state and deformed configuration are imported properly to Abaqus/Explicit. In the Abaqus/Explicit analysis the belt moves through the process zone in a steady-state manner while maintaining the stretched stress state. The stress state remains nearly constant even as blocks are shuffled when the inlet blocks pass through the trigger plane.
Input files
Abaqus/Standard analysis file
- belt_standard.inp
-
First Abaqus/Standard analysis.
Abaqus/Explicit analysis file
- belt_explicit.inp
-
Second Abaqus/Explicit import analysis.