July 20, 2023 at 3:21 pmBrian KeatsSubscriber
I'm using the relative dispacement extension (https://catalog.ansys.com/product/5b3bc6857a2f9a5c90d32eaf/relative-displacement).
I would like to define the coordinate system with respect to the pilot node of a remote point. I can't seem to find a way to select that node. If I can get it into a names selection, that would work but I couldn't figure that out either. I see the option in remote point to assign a pilot node APDL name, but I'm not sure if I can take that and turn it into a selction somehow.
TL;DR, how do I either slect a remote point pilot node, or get it into a named selection?
July 21, 2023 at 7:38 ammjmiddleAnsys Employee
I haven't used the relative displacement extension, and you should know that all the unpaid extensions are not supported. Each one should have a page near the beginning of the documentation that states:
Please pay attention to paragraph 9 of the CLICKWRAP SOFTWARE
LICENSE AGREEMENT FOR ACS EXTENSIONS regarding TECHNICAL
ENHANCEMENTS AND CUSTOMER SUPPORT (TECS): “TECS is not
included with the Program(s)”
But I can tell you that pilot nodes of remote points aren't defined until the input file is written to the APDL solver, so you can't access them in Mechanical. So I doubt you could get the extension to report a displacement relative to a remote point node, since it can't be accessed in Mechanical. But possibly the extension can do some things through APDL insertion.
You would need to use an APDL command snippet. That is what the "Pilot Node APDL Name" is for:
This is meant for APDL scripts that you would place under the analysis branch or solution branch. You enter a variable name, and this variable will contain the ID of the node. I named it "My_pnt1" above.
If you want to measure the distance to some other point after solution, you would insert a command snippet under the solution branch, and probably use *GET commands to get the location of the pilot node and a different node (placed in a named selection, and use CMSEL to get the contents). Then you can compute the difference and store in a variable. If the variable begins with "my_" it will be printed in the Details of the command snippet:
Or you could write to a file using APDL commands CFOPEN, *VWRITE, CFCLOS. Or maybe you can just see the value in the Solution Information.
You can compose APDL commands by working with the documentation, which are listed in alphabetical order here:
To quickly learn APDL you can look at the ds.dat written in the solver directory to see how each section was written to the solver from your Mechanical model in workbench. Set up something in Mechanical that is similar to what you want to do, and look at what it wrote. For example, insert a spring and see what APDL code it wrote.
By the way you can make a spring with negligible stiffness to measure a direct-line distance after solution since you can insert a spring probe that reports elongation.
July 21, 2023 at 12:33 pmBrian KeatsSubscriber
Thanks mjmiddle, that's very helpful. For future readers of this thread, the relative displacement app appears to be outputting garbage data and I'm not inclined to spend any time debugging. I'm going to use some combination of nodeal extraction/manual math and the negligible-stiffness spring approach described above.
- 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
- 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.