

September 7, 2020 at 6:53 ambusraekinciSubscriber
Hello! I need an urgent answer for my loader arm mechanism. I modeled an basic arm structure with its bucket. I am trying to make a simple static analysis to obtain the joint forces on the structure. Normally, I have 2 pistons in this system but I modeled those as beams for simplicity. The only input is the bucket force.
I connected the arm mechanism by three revolute joint ( body to ground). All the other joints are revolute joints ( bodytobody) in the structure. When I do a static analysis on my model, I am getting the warnings:
1) Not enough constraints appear to applied to prevent rigid body motion. 2) The warning related to large deflection
Also,
Joints forces do not make any sense because there are huge forces on the rotation axis of revolute joints.
I could not find the mistakes in my analysis. Could you please help me? Is there anyone who has an idea?
Thanks very much!
please see the figures related to my model and analysis.

September 7, 2020 at 1:09 pmAshish KhemkaAnsys EmployeennI cannot look into the model but can you turn on the large deflection on? On Rigidi Body motion  do you see excessive deformation in any of the part than expected? If yes then try to apply a joint load like rotation.nnRegards,nAshish Khemkann

September 7, 2020 at 1:22 pmbusraekinciSubscribernHow much rotation and on which joint do you think? nBy the way, when I use bushing joints instead of revolute joints, results make sense and match my hand calculations.ps: In the model, every components are rigid, not flexible. nThanks for your help! n

September 7, 2020 at 2:09 pmpeteroznewmanSubscriberBushing joints are good because they provide the needed flexibility in the model.nWhen all the components are rigid and all the connections are joints, that is a mechanism and the Rigid Dynamics solver is better at solving that model than the Static Structural solver, even though there is no motion.nIf you analyze this model like a rigid body mechanism, each part has 6 DOF, and you want the number of constraints to equal six times the number of parts. It looks like there are six parts, or 36 DOF. You have way more constraints than that. Each revolute joint is 5 constraints, and I count 10 revolutes. That is 50 constraints, so there are 14 redundant constraints. The Rigid Dynamics solver has logic to analyze the constraints and eliminate the redundant constraints. For example, you have three Revolutes to ground. There should only be one, the main link in the center. The other two links to ground should only provide 1 DOF, a constraint in the axial direction of the link. nThe Static Structural solver doesn't have logic to eliminate redundant constraints because it doesn't assume the parts are rigid since that is the exception, it assumes all bodies are flexible. If you change the bodies to be flexible, you might get a better result from the Static Structural solver, but first, try the Rigid Dynamics solver.n

September 7, 2020 at 3:02 pmbusraekinciSubscribernFirstly, thanks for your detail answer. I got it but I have no access to Rigid Dynamics Solver. I have only static and modal analysis packages. nTo understand your constraining method, I want to make a simple analysis only on bucket. According to the method, I need 6 constraints. What kind of a constraint do you suggest for this bucket? Still using the same input force at the far edge. nI will define a single joint instead of two bottom joints for the simplicity. I have 2 joints totally. Please see the pictures. nThanks so much for your help! n

September 7, 2020 at 3:14 pmpeteroznewmanSubscriberThe first General joint is exactly like a Revolute. All Fixed except for Rotation about local Z. The second General joint should have All Free except for Translation along local Y. That is exactly 6 constraints, but it is not quite right.nInstead, make the second General joint a Revolute, All Fixed except for Rotation about local Z.nThe first General Joint represents the force going through the tancolored link that is suppressed.nEdit the Joint coordinate system to make the local Y axis point to the hole at the other end of the tancolored link. nMake the first General joint have All Free except for Translation along local Y. That force represents the compression in the tancolored link.nAs the line of action of that tancolored link comes closer to the Z axis of the other joint, the compression force will increase.n

September 8, 2020 at 6:56 ambusraekinciSubscriberDear thanks very much for your great and helpful answers. I applied it and see the logic. It will be so helpful for my future tasks as well. nThanks a lot! Have a good day! n

November 11, 2022 at 9:11 amEashwar RaajSubscriber
I'm Getting This error In Structural Analysis after Composite Modelling in ACP , Where I have no connections related analysis its just like Cantilever type Analysis so Why this Error Come to me . Anybody Help In solving this error ASAP please

 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?
 Saving & sharing of Working project files in .wbpz format
 An Unknown error occurred during solution. Check the Solver Output…..
 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

2092

1748

981

762

423
© 2022 Copyright ANSYS, Inc. All rights reserved.