June 29, 2018 at 3:12 amFabricio.UrquhartSubscriber
I would like to know, if somebody could help me with the load application. The model is composed for solids and cross-section, connected for a rigid joint. Now I am applying the load. It is distributed load along the cross-section and solid.
But when I apply a line pressure in the solid and the cross-section the model does not converge. If I apply only in the cross-section it is ok. The objective is to analyse the connection, so I have to apply load along all the beam of the portic.
The picture below, shows the model with the line pressure applied only on the cross-section.
Attention, that I have a plane of symmetry. With concentrate load, it is ok, but distributed load I have problems with convergence.
July 1, 2018 at 2:09 amSandeep MedikondaAnsys Employee
Can you explain a little about the type of error you are seeing? What kind of material and contact's are you using?
I see plasticity in the model, do you have large deformation effects ON? If not, can you try turning those on?
Have you looked at the Newton-Raphson residuals and tried the tips and tricks suggested in this article?
July 1, 2018 at 11:38 amFabricio.UrquhartSubscriber
It was an unknown error. The materials are:
- Bolt: ASTM A325
- Beam and column: ASTM A572
- Plates: ASTM A36.
Yes, I have large deformation effects ON. Oh! I have not looked at the Newton-Raphson residuals, I will read the article, thank you.
But the problem was that I was applying the load in a edge of the solid parts, so I applyed a pressure on the beam flange with the same value of the crosssection (line pressure) and it converged. The results are OK, now I posted another topic: Symmetry.
Thank you, very much!!!
July 1, 2018 at 11:47 amFabricio.UrquhartSubscriber
The materials are:
- Bolts: ASTM A325
- Beam and columns: ASTM A572
- Plates: ASTM A36
Yes I have large deformation effects ON. I have not looked at the Newton-Raphson residual, I will look and read the article!
Now I have wrote another post: Symmetry. I am trying to model the half portic, because the other side is impacting in the connection results that I am studying.
Thank you ver much!!
July 2, 2018 at 1:57 ampeteroznewmanSubscriber
I have changed your model that was posted in the Symmetry post and have results.
July 2, 2018 at 11:36 amFabricio.UrquhartSubscriber
July 2, 2018 at 11:48 ampeteroznewmanSubscriber
But Fabricio, that is a real effect of applying a pressure load. The more flexible outer flange deforms more than the center of the flange that has the vertical face of the I-beam under it. If you look at the magnitude of the flange flexing down below the center of the beam, it is only 0.068 mm or 68 microns. Can you even measure that? Why do you care?
In a real structure, there might be a reinforced concrete slab resting on the I beam. You could model that and it would press with much more pressure on the part of the face above the vertical face of the I beam under it and the pressure would ramp off to nearly zero at the outer part of the top flange. If the concrete slab was flexible, it would make contact along the full length of the I-beam. But if that slab was stiffer than the I-beam, it would only touch out near the joint and the center of the beam would have no contact.
I expect you don't want to add a slab. What you can do instead is split the top face of the I-beam at the plane of the vertical face, and apply the pressure to the newly created narrow face. That should avoid the convergence problems of applying a force to an edge of solid elements (which is never good), and avoid local flexing of the flange.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- 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.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.