September 12, 2018 at 11:22 pm
September 13, 2018 at 12:23 amSandeep MedikondaAnsys Employee
There is a very good article on this in the PADT Inc blog. Search for:
Donny Don’t – Remote Objects
If you haven't already, Can you take a look at it and come back with any specific questions you might have?
September 13, 2018 at 12:14 pmpeteroznewmanSubscriber
That was a great blog about Remote objects that Sandeep mentioned in his post.
You ask about the pros and cons of Displacement vs. Remote Displacement.
Displacement doesn't add any extra equations to the model, it actually removes some equations from the model, so that might have some small effect on solution time compared with Remote Displacement. Maybe Displacement allows the model to converge more reliably than a Remote Displacement. If you are doing just displacement, then a Displacement Support is generally going to be better than a Remote Displacement.
Joint - Displacement requires a joint, while Remote Displacement doesn't. A joint can define a relationship between two bodies (face or edge) or between a body and ground, while a Remote Displacement is only to ground.
September 18, 2018 at 9:28 pmjonsysSubscriber
Hello Peter and Sandeep,
thank you for your answers.
- By the definition, "A enables you to apply both displacements and rotations at an arbitrary remote location in space". What I don't understand properly is what example can there be, in which we apply displacement at a remote location?
- So, when the relationship is between a body and ground, using Remote Displacement will give same results as using Joint-Displacement?
September 18, 2018 at 11:57 pmpeteroznewmanSubscriber
An example of when I would use a remote displacement is where I have an 800 mm long cantilevered structure (bracket) that carries a load at the tip and has a base bolted to a wall. I define plasticity for the metal of the structure and I want to plot the force-displacement curve to determine the ultimate load capacity of the bracket for a load at the tip. It is generally best to apply displacements to generate a force-displacement plot when you want the force to reach a maximum and then continue plotting lower forces as the bracket fails.
The bracket design is such that no high stress occurs along the most of the length of the 800 mm, all the high stress is less than 100 mm away from the wall. I could mesh the whole structure and apply a 300 mm displacement to the tip and that would give me a result. Maybe the mesh has 80,000 nodes and takes 80 minutes to pull the tip down 300 mm.
Or, I could go into geometry and cut 600 mm off the structure and just leave 200 mm from the wall on out. Now I still want to pull the tip down 300 mm, but the tip is gone. That is where a remote displacement comes in. I can put the coordinates of the remote point 800 mm off the wall, and scope it to the cut face that is 200 mm off the wall. The mesh on this model may only have 20,000 nodes and take 20 minutes to pull the remote point down 300 mm. Since all the plastic deformation is happening in the first 100 mm from the wall, the ultimate load calculated from the maximum value of the force-deflection plot is the same as above, but I saved 60 minutes compared with the full model solution.
A remote displacement and a joint to ground may create the same code, under-the-hood. They seem to be equivalent to me.
September 20, 2018 at 12:04 pmjonsysSubscriber
this is the best explanation I ever read regarding remote displacement. thank you very much
November 5, 2018 at 1:32 pm
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- 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.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.