October 19, 2020 at 5:39 pmJohn DoyleAnsys EmployeeIs there any guidance for using commands to define materials in Workbench Mechanical?n
October 20, 2020 at 6:09 pmBill BulatAnsys EmployeenANSYS Mechanical by default assigns a unique material id number (MAT attribute) to each part automatically and a unique number is also used for contacts/targets, springs, beam connections, surface elements, and other entities. The user cannot control the numbering that Mechanical does. A command object can be inserted under a part in the geometry branch that can make use of the material id number which the program makes available as ANSYS parameter named matid and then that parameter name can be used in a command object. Any part without a command object will use the material as set by Mechanical. So if you have many parts with different material for each, then you can put a command object under each part such as: nmpdel,all,matid ! this deletes all Mechanical material data for material id of matid nmp,ex,matid,3e7 nmp,dens,matid,0.283 nthen for another part: nmpdel,all,matid ! Mechanical knows that matid is different for each part nmp,ex,matid,2e7 nmp,dens,matid,0.25 nIf the material is nonlinear then add the desired TB commands for each part. nnIf you have many parts but only few materials, then you could use command objects like this: nmpdel,all,matid nmp,ex,matid,3e7 nmp,dens,matid,0.283 npart1_matid=matid ! needed to be used later - change part1_mat to a different name for a different material then any other part that uses this same material can just use this command object nesel,s,mat,,matid nemod,all,mat,part1_matid nesel,all nThere are many alternative methods to changing materials using commands but I believe these are the most common. As Mechanical does many operations internally you should definitely test all command objects carefully. Add a command object such as this under the environment (such as Static Structural) to check the material data: nMPLIST,ALL ! list all linear material data for all material idsn
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.