EDEM-Abaqus Coupling User Guide April 2018 Revision
Copyrights and Trademarks Copyright 2018 DEM Solutions Ltd. All rights reserved. Information in this document is subject to change without notice. The software described in this document is furnished under a license agreement or nondisclosure agreement. The software may be used or copied only in accordance with the terms of those agreements. No part of this publication may be reproduced, stored in a retrieval system, or transmitted in any form or any means electronic or mechanical, including photocopying and recording for any purpose other than the purchaser s personal use without the written permission of DEM Solutions Ltd. DEM Solutions Ltd. 1 Rutland Court Edinburgh EH3 8FL UK www.edemsimulation.com EDEM incorporates CADfix translation technology. CADfix is owned, supplied by and Copyright TranscenData Europe Limited, 2007. All Rights Reserved. This software is based in part on the work of the Independent JPEG Group. EDEM uses the Mersenne Twister random number generator, Copyright 1997-2002, Makoto Matsumoto and Takuji Nishimura, All rights reserved. EDEM includes CGNS (CFD General Notation System) software. See the Online Help for full copyright notice. EDEM, EDEM Creator, EDEM Simulator, EDEM Analyst and Particle Factory are registered trademarks of DEM Solutions Ltd.. EDEM Field Data CouplingTM, EDEM CFD Coupling InterfaceTM and EDEM Multibody Dynamics Coupling InterfaceTM are Trademarks of DEM Solutions Ltd.. All other brands or product names are the property of the respective owners. Page 2 of 10
Introduction The EDEM-Abaqus Coupling works with Abaqus 6.16 and newer and is an included feature in EDEM 2018 and newer. The coupling has been confirmed as working with Abaqus 6.16 and 6.17. Please note that you need to elect to install Abaqus cosimulation services when installing Abaqus. Setup - You can access the Abaqus coupling tools in the analyst under Tools > Abaqus Co-Simulation. - Before using the EDEM-Abaqus Coupling you must define the Abaqus Launcher Path. For Abaqus 6.16 this defaults to C:\SIMULIA\CAE\2016\win_b64\code\bin\ABQLauncher.exe. - If the Auto-Invoke Local Abaqus Solver option is selected, Abaqus solvers will automatically launch on the local machine in the background. If this is unchecked you can nominate a non-local machine on the same network to run the Abaqus solvers. You must invoke the co-simulation director and Abaqus solvers manually on the non-local machine. Page 3 of 10
- To run the coupling a complete EDEM simulation and Abaqus input file (.inp) are required. The rest of this document outlines the work flow for setting up and running an EDEM-Abaqus coupled case. Example Case To describe the workflow of the EDEM-Abaqus Coupling an example case has been included in this guide. The example case can be downloaded on our user forum. EDEM: - It is assumed users have a basic understanding and experience of setting up and running EDEM simulations. - The EDEM part of the example case is called DumpTruckBody.dem. This is a simple case involving a single factory and a dump truck body unloading material. - Run DumpTruckBody.dem to solve the DEM side of the coupling. Abaqus: Separately an Abaqus.inp file must be created in order to solve the FEA side of the coupling. Complete DumpTruckBody.cae, DumpTruckBody.inp and DumpTruckBody.odb files are included with the example case. The steps taken to setup the Abaqus side of the coupling file are outlined below. 1) Start Abaqus CAE and create a Standard/Explicit Model save this under the name DumpTruckBody.cae. Page 4 of 10
2) Right click on Parts and select Import. Import Body.igs and scale by multiplying all lengths by 0.001 (the.igs file is in mm and we want to work in m). Note that the geometry is loaded into Abaqus in the same position as it is at t=0 in the EDEM deck. 3) Mesh the component that you have just loaded into Abaqus by applying a global seed to the of 0.1 and using Assign Mesh Controls set the element shape to Tet and technique to Free. Click on Mesh Part you should now have a meshed dump truck body in Abaqus. 4) Double click on Materials and add an elastic isotropic material. For this set a Young s Modulus of 200 GPa and Poisson s Ratio of 0.27 (Structural Steel). For dynamic cases you must set a material density at this stage. Page 5 of 10
5) Right click on Sections and select Create. Create a Solid, Homogeneous section and assign it with the material you have just created. Click on Assign Section and assign the section you have just created to the part called Body. 6) Under Assembly double click on Instances and create a new instance using the part called Body. Under Assembly double click on Surfaces and create a new surface and call it EdemCoSimInterface (this must be the exact name of the co-simulation surface and it is case sensitive!) using Type: Geometry and select all of the surfaces that you expect the have contacts with material in EDEM pressing and holding Shift to select multiple surfaces (make sure you do not accidently select edges). Page 6 of 10
7) Right click on Steps and select Create. Create a Static, General step for Static and Averaged cases and leave all settings as default. For a Dynamic case, create a Dynamic, Implicit and set the application type to Moderate dissipation and setup field and history output requests as required. 8) Under the newly created step double click BC and add a boundary condition to the dump truck body i.e. Encastre on the side edges of the dump truck body. 9) Right click on Jobs and select Create. Name the job DumpTruckBody and leave all settings as default. Right click on the job DumpTruckBody and select Write Input this will create the.inp file required to run the coupling. It is also advised to run Data Check on the job to identify any issues with the setup before running the coupling. Co-Simulation: - With the completed EDEM deck and Abaqus.inp file you can now run the coupling. Open the Abaqus Co-Simulation dialogue as described above. Select the units you want to use options include EDEM specified units or SI units. Select the mode you want to use for example Static. Select the geometries to include in EDEM (in this case Body ). Specify the Abaqus Launcher Path as described above and point to the Abaqus.inp file and the name of the.odb file which you want the results to be saved under. Click solve to run the coupling (Abaqus solvers run in the background). - For example, these settings run a Static case at 1.9 seconds looking at contacts on the geometry called Body and saves the results to output.odb. Page 7 of 10
- Open output.odb and analyze the FEA results in the normal way. Page 8 of 10
Known Issues The EDEM Abaqus coupling contains the following known issues: Small length scale contact force mapping Mapping of forces from contact location to FEA mesh is handled by the Abaqus Co- Simulation Director and it has been found that below a certain absolute length scale (~ 1e-5) contacts do not get mapped. A solution to overcome this is to work in a different unit system in Abaqus i.e. from N/m 2 to N/mm 2. Small EDEM save intervals.odb output In some cases where small save intervals are used in EDEM (< 1e-3s) the.odb file which Abaqus outputs after running the coupling contains many copies of the same static results. This is understood to be an issue between save intervals in EDEM and output requests in Abaqus. EDEM Coupling Interface The current version of the EDEM Abaqus coupling does not support contact force mapping for geometries whose movement are driven via the EDEM Coupling Interface. This includes EDEM + MBD simulations. Final time step There is a known issue where if mapping contact forces from the final time step no forces will be mapped. Current work around is to simulate for one more save interval. Troubleshooting Issues can arise when setting up and running the coupling. This troubleshooting guide highlights some of the common issues that can arise when running the coupling: Test Abaqus Co-Simulation Director is working The EDEM-Abaqus coupling relies on the Abaqus Co-Simulation Director for transferring data from EDEM into Abaqus. To test the Co-Simulation Director users can run these commands from a command prompt: abaqus fetch job beam_2d_dyntodyn_subcycle_std abaqus fetch job beam_2d_dyntodyn_subcycle_xpl abaqus -cosimulation cosimlog -job beam_2d_dyntodyn_subcycle_std,beam_2d_dyntodyn_subcycle_xpl -int This tests the Co-Simulation director in isolation of EDEM. If successful the command prompt will output: JOB beam_2d_dyntodyn_subcycle_std SUCCEEDED JOB beam_2d_dyntodyn_subcycle_xpl SUCCEEDED Page 9 of 10
If unsuccessful, please contact EDEM support (support@edemsimulation.com) and your local Abaqus supplier for support. Admin privileges The EDEM-Abaqus coupling requires read/write privileges to C:\Program Files\DEM Solutions\EDEM 2018\bin\config folder. If you do not have privileges to read/write to this location youwill get a Failed to amend configuration file error in the EDEM- Abaqus coupling dialogue window. If you do not have privileges open EDEM as admin or alternatively contact your IT support to grant full access to this folder location. Abaqus setup These are the steps you should be aware of when setting up the Abaqus side of the coupling that can cause issues. Note: this list is limited and assumes users have a good working knowledge of Abaqus CAE. Make sure that materials have been set up correctly in Abaqus and assigned to the correct sections/geometries (Note: for dynamic cases material density must be set). Ensure that you have properly specified the surface EdemCoSimInterface. This is the surface which interacts with contact data in EDEM and must be called EdemCoSimInterface. Make sure that the kind of Step used is correct for the kind of analysis you are doing (Static, General for Static and Averaged cases and Dynamic, Implicit typically using Moderate dissipation for Dynamic cases). Log files In the directory of the coupled job there is a folder called abqworkingdir created when you run the coupling. This folder contains information about the coupling job. The.dat,.log,.msg and.listener files should be sent to EDEM support if you encounter any issues when running the EDEM-Abaqus coupling. An additional edem.listener file can also be created by creating a new environment variable ABAQUS_MPF_DIAGNOSTIC_LEVEL and set its value to 1023 and then running the coupling. Please contact support@edemsimulation.com for any support queries you may have about using the EDEM-Abaqus coupling. Page 10 of 10