

May 27, 2021 at 7:10 pmLilloSubscriber
Hi,
I have a problem with the solution of the statical analysis of a onedimensional framed structure (only beam elements). As you can see from the attached figures I created a structure in Design Modeler using line bodies in three different modes: 1) share topology to connect the line bodies, 2) joining all the line bodies in one part, 3) leaving the line bodies "free". After that, for all three cases, I applied the boundary conditions you see in the figure: 1) gravity, 2) two concentrated loads, 3) a fixed support for the four node at the base of the structure.Then, going to solve the structure, in all three cases, I get a pivoting error (as you can see in the figure). What could be the problem?
Thank you so much in advance for the answers!

May 27, 2021 at 9:13 pm

May 28, 2021 at 2:26 amMike RifeAnsys EmployeeThat shorter beam with node 118 at its middle  the end nodes do not appear to line up and be shared with the vertical beams. I expect you mean nodes 60 and 116 should not be separate nodes. You already know the assembly is not fully connected. But one way to find out all the ways it is not connected is to add a Modal analysis to the WB Project, sharing the same model. Then constrain the model just against rigid body motion. Solve and post process the mode shapes. There will be zero or near zero modes with the unconnected parts rigidly translating.
Mike

May 28, 2021 at 6:13 amErik KostsonAnsys Employeemake sure all the beams share a vertex, and are thus all connected  then you can use multibody parts in DM to merge all the common vertices and hence obtain a compatible connected mesh between beams (but first they need to share vertices).
multi body parts  so select all parts in the tree right mouse button lick and select form a new part
All the best
Erik

May 29, 2021 at 8:30 pmLilloSubscriberThank you so much for the advice. I fixed it using the "merge node" command.
But now I have another problem. Going to run a buckling analysis I get weird results. I explain myself better. I run the buckling analysis in two different modes: 1) assigning two loads of total value equal to 1 N, 2) going to assign the actual values of the two symmetrical loads (12250 N). In the first case I get a load multiplier of 384,14 (which corresponds to a critical load of 384 N) and in the second a load multiplier of 32 (which corresponds to 784000 N). Why this large discrepancy?

May 29, 2021 at 11:17 pmpeteroznewmanSubscriberI see three loads, not two. The third load is Standard Earth Gravity. The load multiplier applies to gravity as well as the two forces.
Increase the applied force loads and rerun the buckling analysis. Find the force that delivers a load multiplier of 1.0 then you have found the critical buckling load with standard earth gravity.

 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 lifesaving 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.
Ansys Blog
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

2032

1730

957

738

415
© 2022 Copyright ANSYS, Inc. All rights reserved.