3 Point Bending in Ansys

- December 19, 2019 at 10:30 am
  1234mamanunu
  Subscriber
  Hello to all,
  
  I would like to simulate a 3point bending case with ansys. In this case, a plastic bar is loaded by a cylinder. I would like to see the stress in the bar after a 7.5 mm displacement in the y direction of the loading cylinder
  
  I am using the static structural model with the following setup:
  
  Geometry [has a symmetryPlane]:
  
  Boundaries:
  
  Fixed support
  - Remote displacement
  Analysis settings
  
  I am getting the following error "Solver pivot warnings or errors have been encountered during the solution. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully " , however the solver still works but it does not move the loading in the y direction. It has a strange behavior.
  
  Result:
  
  https://gfycat.com/sillyleanaustralianfreshwatercrocodile
  
  Does anyone know how to solve this?
  
  Is the static module adequate for this problem?
  
  Best Regards!
- December 19, 2019 at 12:54 pm
  
  peteroznewman
  Subscriber
  
  Yes, Static Structural is the right analysis to use.
  
  1) Check that the direction of the Normal in the Symmetry Region is the X-axis.
  
  2) Add a second Symmetry Region for the Z-axis to reduce the degrees of freedom of the beam. Since you are using frictionless contact, there is nothing to stop the beam sliding along the Z-axis. You should slice the geometry in half, or just say your beam is twice as wide.
  
  3) Does the top roller begin tangent to the beam? That is what you want. You don't want to start with a gap.
- December 19, 2019 at 2:55 pm
  
  1234mamanunu
  Subscriber
  
  Hello Mr Peter,
  
  Thank you very much for your valuable help
  
  I added both symmetry planes and reduced the model in half
  
  Plane1:
  
  Plane2:
  
  Contact1:
  
  Contact2:
  
  Solver:
  
  Error:
  
  partial Result:
  
  https://gfycat.com/vapidwidekillifish
  
  Its almost there, but it seams to have convencenge issues
  
  Best Regards!
- December 20, 2019 at 1:40 am
  
  peteroznewman
  Subscriber
  
  Do not begin the analysis with a gap between the roller and the beam. In CAD, move the roller to be tangent to the beam.
  
  In the Details window of the Symmetry Region, is the Normal correct? You showed the faces, what is in the Details window? The reason I ask is because the default value in the Detail is NOT to automatically be normal to the faces picked. You have to set it to the correct normal yourself.
- December 20, 2019 at 2:48 pm
  
  1234mamanunu
  Subscriber
  
  The normals are Ok.
  
  I moved the roler to be tanget to be beam.
  
  Symmetry regions:
  
  I am still getting the same error:
- December 20, 2019 at 6:54 pm
  
  peteroznewman
  Subscriber
  
  1) Under the Solution Information folder set the Newton-Raphson Residual plots to 5.
  
  2) Solve.
  
  3) Reply with an image of the Maximum value of the Newton-Raphson Force Residual. This is often where a smaller element can help convergence.
  
  4) Under Solution Information, reply with the Newton-Raphson Force Convergence Plot. In some models, it is helpful to insert a command to tell the solver to use more than the default 26 iterations before starting a bisection.
  
  5) There are changes to the element formulation that can help such as Reduced Integration if the above does not help.
- December 26, 2019 at 5:12 pm
  
  1234mamanunu
  Subscriber
  
  Here are the results:
  
  To topic 3:
  
  1st :
  
  2nd:
  
  3rd:
  
  4th:
  
  5th:
  
  worksheet:
  
  Are these type of cases hard to solve?
  
  Is it possible to upload the case?
  
  Best Regards!
- December 26, 2019 at 6:14 pm
  
  peteroznewman
  Subscriber
  
  Here is how to create a file that can be uploaded using the Attach button that appears after you post.
  
  This post has a video showing how to track down convergence issues. There are other posts in that Disucssion you might find interesting.
- December 26, 2019 at 7:14 pm
  
  1234mamanunu
  Subscriber
  
  I will update the case here if anyone wants to help.
  
  If I am able to solve it, I will upload the solution.
- December 26, 2019 at 8:31 pm
  
  peteroznewman
  Subscriber
  
  The biggest problem is that the contacts are not closed. Insert a Contact Tool under the Connections folder to learn this information.
  
  The corrective action is to Adjust to Touch on the two contacts since the gap is small.
  
  I flipped the Contact and Target sides of the contact.
  
  I made smaller elements. I changed the Step controls.
  
  It now solves.

Viewing 9 reply threads

You must be logged in to reply to this topic.

Ansys Innovation Space

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.

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.

Trending discussions