September 19, 2023 at 2:51 pmhelen.durandSubscriber
In a transient thermal and transient structural simulation, I am using APDL command objects to change material types (using the MPCHG command). I want to display the element material assignments during the solution by creating a user defined result.
I tried to do this using the expression PNUMMAT (which displays element material numbers); however, the displayed results seem to only show the material assignments from the prep phase, and any changes to the material assignments that I am making during the solution phase are not displayed.
Is this a limitation of the PNUMMAT expression, or could this be a sign that material types are not getting changed during the solution phase?
September 20, 2023 at 2:13 pmGovindan NagappanAnsys Employee
This is probably a limitation of PNUMMAT that it only shows material assignment done under /prep7
Can you use /PREP7, change the material and go back to /SOLU?
Another way to check material assignmnt is by selecting the "solution" branch, go to "Worksheet" and show "Material and Element Type information"
September 20, 2023 at 2:14 pmGovindan NagappanAnsys Employee
You can also check the "solution information" for the feedback from the MPCHG command
For example, I used these commands
I got the following feedback in solution information:
SELECT COMPONENT BODY1
SET MATERIAL OF SELECTED ELEMENTS TO 3
SELECT ALL ENTITIES OF TYPE= ALL AND BELOW
September 20, 2023 at 4:36 pmhelen.durandSubscriber
Thank you for the reply!
Looking at the worksheet in my simulation, I still only see the element assignments from the prep phase.
I used the ELIST,ALL command to verify that some elements are being changed at every loadstep (I put the command at the beginning of the APDL command object that is set to run at the start of every loadstep in the solution phase).
For example, at the start of loadstep 1, the printout is this (all elements are assigned material type 50 during the prep phase):
At the start of loadstep 2 (elements 1 and 2 were assignd material type 30):
At the start of loadstep 3 (elements 3 and 4 were assigned material type 30):
However, when I look at the worksheet I do not see any mention of materialtype 30:
The issue has been that calling ELIST,ALL at every loadstep for a reasonably large geometry makes the solution file extremely long, and it is difficut to assess whether the element numbers are being assigned correctly.
September 20, 2023 at 9:23 pmGovindan NagappanAnsys Employee
Consider using prep7 if possible
Or if the ETLIST is sufficient, select 1 element or few elements and write the output instead of writing it for full model
Or you can redirect the feedback from MPCHG command to a separate text file using /output
Material number is not a result. So the historical change in mat number is probably not saved in the rst file.
September 20, 2023 at 11:11 pmhelen.durandSubscriber
Those sound like good options. Thank you for your help!
- The topic ‘User defined result with the PNUMMAT expression’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- User manual
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Defining rigid body and contact
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.