This article demonstrates a high fidelity approach for the prediction of the static structural response of bulk solids handling systems that combines Discrete Element Method (DEM) modelling in Altair EDEM with Finite Element Method (FEM) modelling in Altair OptiStruct and Altair SimSolid.
All requisite model files can be downloaded from here:
The bunker shown below is used as an example and the focus of the analysis is on the static case at full capacity which is often the critical design load case for this type of structure.
The complexity of the loading in this case is a result of the non-uniform spatial distribution of the stored bulk solid. The filling stage is simulated in Altair EDEM to predict the final state at full capacity and the resulting loads.
The loads are then transferred either into an OptiStruct or SimSolid FEM model of the structure and the structural response is predicted using linear static analysis.
The key steps in the DEM modelling with EDEM are detailed first. The FEM modelling workflows in OptiStruct and SimSoid are then outlined and their comparative advantages are discussed.
1. Modelling the filling stage in Altair EDEM and exporting the forces on the structure
The complex behaviour of bulk solids and their interaction with equipment parts can be simulated in Altair EDEM, which is a market leading DEM software. In EDEM, bulk solids are modelled using discrete numerical particles, which is the highest fidelity modelling approach for these materials available today. Setting-up an EDEM model is relatively simple and the key steps in the workflow are outlined next.
1.1 Import and mesh the CAD geometry of the bunker
Right click on geometries and import the Bunker_Shell.stp file which contains the 2D surface geometry of the bunker. The mesh density in EDEM will not affect the results and the default mesh settings can be used but make sure the merge sections option is enabled to reduce the number of parts in the model.
1.2 Select a bulk solids material model from the GEMM database
Right click on bulk material and open the GEMM wizard:
Use the following properties:
|
System size |
Large |
|
Bulk density (kg/m3) |
> 2000 |
|
Angle of repose (deg) |
40 |
|
JKR (J/m2) |
40 |
|
Wall friction |
High |
The below bulk solid and equipment materials should now have been automatically defined by EDEM.
1.3 Define a particle factory to introduce the bulk material into the bunker
Create and position box geometry in EDEM for the particle inlet.
Right click on the geometry to create a factory.
Define the mass flow rate, total mass to be created and the initial particle velocity as shown below. The initial velocity dialog is triggered by clicking on the cog wheel.
1.4 Solve the simulation from the EDEM simulator
1.5 Export the geometry contact forces from the EDEM analyst
From the EDEM Analyst navigate to File->Export and select HyperMesh data if using OptiStruct or SimSolid Data if using SimSolid. Use the below settings in both cases to export the contact forces on the bunker walls at the end of filling.
2. Modelling the bunker in Altair OptiStruct
OptiStruct is Altair’s high-fidelity FEM solver, which is capable of both linear and non-linear analysis, has a wide range of constitutive models and extensive topology optimization functionality. It is a classical mesh-based FEM solver which uses Altair HyperMesh and Altair HyperWorks as pre-processors. The modelling in this example is performed in Altair HyperWorks with the OptiStruct solver interface.
The bunker is modeled as a thin shell which has the advantages of geometric simplicity and numerical efficiency.
2.1 Import and mesh the CAD geometry of the bunker
Navigate to FIle->Import-> Geometry Model and import the Bunker_Shell.stp file, which contains the 2D surface geometry of the bunker, and mesh it using a general 2D mesh with the settings below.
2.2 Define and assign material and shell section properties
The structure is modelled as a 2D shell made of a linear-elastic isotropic material with the elastic constants for structural steel. Thes should be defined as shown below.
2.3 Define boundary conditions and geometry loads
All nodes at the base of the stiffeners and the outlet of the bunker should be fully constrained.
The force field from EDEM is imported using the linear interpolation option where OptiStruct automatically maps the forces within a search radius of an element centroid to the element nodes. It is good practice to keep the search radius similar to the element size to avoid distributing forces too widely. The fill gap option should be disabled as we only want to apply forces to nodes that are within the force vector field. The force field is shown below and corresponds to the particle material distribution in EDEM.
2.4 Define a static linear load step and solve the model
Define a static linear load step as below. In this case the EDEM and BCs forces are load collectors containing the force field from EDEM and the boundary conditions respectively. The model is now ready to be solved.
The results can be visualised by opening the .h3d file in Altair HyperView and reveal the complex stress state in the structure as shown below.
3. Modelling the bunker in Altair SimSolid
SimSolid is Altair’s state-of-the art meshless FEM analysis suite. Its highly automated workflow and mesh independent solver enable the structural analysis of fully featured CAD assemblies in a fraction of the engineering time required by traditional FEM modelling methods. While not as extensive in terms of solver features as OptiStruct, is it capable of both linear and non-linear analysis but is limited to three-dimensional solid CAD geometries only.
3.1 Import the CAD geometry of the bunker and auto-generate component connections
Got to Project -> Impot from file and import the Bunker_Solid.stp file, which contains the three-dimensional solid geometry of the bunker. No meshing is required with SimSolid as it uses a meshless FEM solver.
The connections between geometry components can be auto-generated by SimSolid and a sufficiently low tolerance should be defined to ensure that the model is not over-stiffened by connecting distant components. Use the settings shown below when prompted.
3.2 Define and assign materials
Under Assembly click on the Apply materials button, load Steel from the material model database and click on the Apply to all parts button.
3.3 Define boundary condition and import EDEM loads
From the top ribbon create a structural linear load step and add immovable support to the bases of all stiffeners and the bunker outlet. The selection is made by surface and not by node as there is no mesh in the model.
To import EDEM loads select Apply forces -> Imported Forces -> Import from csv and load the .csv file exported from EDEM.
3.4 Run the analysis and post-process the results
The model can now be solved, and the results can be visualised under the results tab. The results are very similar to the ones obtained by the classical mesh-based FEM solution in OptiStruct, demonstrating the validity of the SimSolid meshless FEM solver.
4. Further resources
To get started with Altair EDEM please see: 4 steps to accelerate your EDEM learning curve!
To get started with Altair OptiStruct for linear analysis please see: OptiStruct for Linear Analysis E-learning
To get started with Altair SimSolid please see: SimSolid Quick Start v2022 eLearning