TAGGED: ansys-mapdl, apdl, composite-laminates, graph-plot, material-damage
May 7, 2023 at 12:50 ammpirkleSubscriber
When graphing stress-strain results in POST26 for a composite laminate, are the results (see graph below) for the laminate, or for a particular lamina?
Is there a way to plot stress-strain results for a specific node within a particular lamina (0, +/-45, 90, etc.)?
Here is the /POST26 code:/POST26SHELL,MIDANSOL,3,14944,S,X,SXNODE14944ANSOL,2,14944,EPEL,X,EPSXNODE14944/AXLAB,Y,STRESS [MPa]/AXLAB,X,STRAINPLVAR,3XVAR,2
Also, I receive the following warning:
Is this warning cause for concern? If so, how can I avoid it? Should I be using NSOL instead?
Any help is greatly appreciated!
May 8, 2023 at 12:48 pmChandra SekaranAnsys Employee
To get results for a particular layer, you will need to use "Layerp26" command in Post26. Then you can use ESOL (and ANSOL) to get results for a particular layer.
Yes, the warning is important. Post26 does not do coordinate transformations. The ANSOL documentaiton gives the below note: Shell elements: The default shell element coordinate system is based on node ordering. For shell elements the adjacent elements could have a different RSYS,SOLU, making the resultant averaged data inconsistent. A message to this effect is issued when ANSOL is used in models containing shell elements. Ensure that consistent coordinate systems are active for all associated elements used by the ANSOL command.
May 15, 2023 at 11:09 pmmpirkleSubscriber
Great! So If I want the results from the middle layer of the shell281 element for node 14944 in the first lamina (0 degree fiber orientation for this lamina), my code should look like this:/POST26LAYERP26,1SHELL,MIDANSOL,3,14944,S,X,SXNODE14944ANSOL,2,14944,EPEL,X,EPSXNODE14944/AXLAB,Y,STRESS [MPa]/AXLAB,X,STRAINPLVAR,3XVAR,2Do I need to activate the coordinate system using RSYS,11 in POST1, or does it automatically use the coordinate system for the fiber orientation (0 degrees in this case) based upon the LAYERP26 choice?Also, do you know if the ANSOL averaged nodal results are typically preferred for a tensile test stress study?Thank you!
May 17, 2023 at 1:30 pmChandra SekaranAnsys Employee
The solver writes element results such as stress/strain in element coordinate system for each element, and nodal results such as displacements in nodal coordinate system. By default the results will be in layer coordinate system. Layer results are written in layer coordinate system. So Post26 will display results in layer coordinate system. RSYS is not valid in Post26.
ESOL is the more accurate number to use because there is no averaging. ANSOL is a convenience tool to get average values at a node.You may want to compare ANSOL results against individual element ESOL and see if it makes sense.
- You must be logged in to reply to this topic.
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
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- 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
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.