January 11, 2022 at 10:35 pmnds88Subscriber
Are there any new techniques that are being used to separate out rigid body motion from strain based deformation to create a relative displacement? There is an app in the ANSYS App store but that is no longer supported for current versions. I tested it and it did not produce a correct result for a cantilever beam with a known translation at the base. I have read some of the PADT blogs about it but I am not very skilled in APDL, so they were not very clear to me.January 17, 2022 at 1:42 pmAniketAnsys Employeeare you referring to Extracting Relative Displacements in ANSYS Mechanical ÔÇô PADT, Inc. ÔÇô The Blog (padtinc.com)? I believe there are examples as well.
How to access Ansys help links
Guidelines for Posting on Ansys Learning Forum
January 18, 2022 at 5:37 pmnds88SubscriberYes, thats the blog. I looked this over and re-worked their examples. One thing I don't understand about this is that for rotations, they are using remote points to get RBE3 constraints, then they are pulling the rotation data from that. This approach doesn't seem to produce a different result from using a remote point and a flexible rotation probe (a native ANSYS probe). Both methods still require the user to either know the area of interest ahead of time, or, resolve the analysis. So, the script they have doesn't seem to add value there.
The script worked for my translational DOF discrepancy on a cantilever model with a moving base. I assume there is no other native ANSYS way to recreate this. I was able to separate out the strain based deflection as predicted by FL^3/3EI . One outstanding issue is that I this result is only in the Global CS. If my component is not aligned to global, then I would have to find a way to rotate my results to match the local CS. Would I take those values and have to manually create a rotation matrix and multiply results by that?
This is the best way, currently, to extract a relative displacement?
January 19, 2022 at 6:31 pmGary StofanAnsys EmployeeThe core functionality that was used in the Relative Displacement ACT extension is being replaced by Ansys DPF or Data Processing Framework.
January 20, 2022 at 12:03 amnds88Subscriber
Thanks Gary. I'm not familiar with that tool. How is it related to finding Relative Displacement? The link describes that it processes user defined data, but it sounds like that still leaves me to have to create a process to get that data somehow.
January 25, 2022 at 8:54 pmnds88Subscriber
I know this is a common question, but I really am not seeing a lot of information on this topic other than the PADT solution, of which I have some conflicts with using. Is there anything else to add about this?
January 26, 2022 at 6:05 pmGary StofanAnsys EmployeeThe applications in the Ansys App store (such as the Relative Displacement) made use of ACT extensions, which are essentially JScript / Python wrappers around APDL code.
I placed the link to the Ansys DPF so that those who have developed the classic ACTs will begin to migrate their applications to this newer technology.
I am not aware of any similar "Relative Displacement" apps using this new DPF technology.
February 11, 2022 at 8:02 pmnds88SubscriberI don't know if anyone else is interested in this topic, but as PADT mentions, its a common inquiry.
So, I found a method that works to extract the 6 degrees of freedom as relative displacements (3 rotations, 3 translations). In the test case of a cantilever beam in bending with a translating base, the user can insert a General Joint with all degrees of freedom set to free. Define contacts as usual (for example, a bonded connection between base and beam). Create remote points; one at the connection between bodies and one at the free end (or location of choice). Set the joint to be defined by these remote points. You will need to choose a newly defined coordinate system for these remote points that have 0,0,0 coordinates at the chosen locations. Make sure Joint Behavior is set to deformable. When solve is complete, use Joint Probe for any chosen degree of freedom by the Relative options.
Unfortunately, this does require some pre-planning or resolving but it does allow the user to define the coordinates in which they want their relative results, which PADT's solution does not allow.
Heres the setup:
Time Step 1: Apply end load, F = 1000N (beam geometry: 70mm Length, 10x10mm cross section; structural steel default)
Time Step 2: Apply end load + base displacement of -0.2mm in X and -0.125mm in Y (arbitrary amounts).
As expected, ANSYS combines those translations of TS2 into the directional deformation. TS1 shows only the strain based deflection (plus some small elastic interaction at the base im assuming since the analytical solution is 0.686mm).
When using the Joint Probe method as proposed, the analytical solution is constant through all time steps regardless of the base translations that I prescribed from the displacment loading.
Ideally this method should be able to be used for any geometry, but I would be careful to check a test case. Any degree of freedom should be able to be probed for relative results now.
Any reason this might not be a good solution for Relative Displacements?
Viewing 7 reply threads
Ansys Innovation Space
- 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.Trending discussions
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- 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.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.