October 7, 2018 at 8:22 amMohankumarSubscriber
I ran a static structural simulation by applying 100 MPa pressure to measure the models Total Deformation and Strain. It gave me the following error and 2 warning messages. Whereas, when I ran the simulation on same model with 10 MPa, I didnt get any errors.
Hence, with these messages, can I consider that the model is incapable of bearing 100 MPa? or does this mean any other? How to solve?
October 7, 2018 at 3:19 pmpeteroznewmanSubscriber
This error does not mean the structure that solved with 10 MPa cannot support 100 MPa. It just means the solver failed to apply the full load without incurring an error.
Please provide more details about your model, the geometry, the supports, the loads, the materials, the contacts, and we can help get the solution up to 100 MPa of pressure. Show us the Solution Information Force Convergence plot.
Is there nonlinear contact in your model? The error you show is sometimes seen when a contact fails to be established and one part passes through another part. Is this error on the first substep of your model? If there is contact, did you use the Contact Tool to check initial contact status?
What other nonlinear behaviors are in your model, do you have plasticity in your material model? Did you turn on Large Deflection? Are you using more than one Step?
If you create a Workbench Project Archive .wbpz file, you can attach that to your reply. I can open your model and see what you need to do to fix it.
October 8, 2018 at 12:34 amSandeep MedikondaAnsys Employee
Please take a moment to look at the manual on this error if you haven't already?
October 8, 2018 at 12:27 pmAshish KhemkaAnsys Employee
Just a suggestion - you can also create a named selection (via worksheet) of the node in error message. This will help to identify the location.
October 9, 2018 at 8:54 amMohankumarSubscriber
Hello Mr. Peter,
I am running a Static Linear analysis in Ansys 17.2 (Academic Research). The model was created using Materialise software with Tet4 elements and mesh size of 2mm. I want to apply pressure at one end of the bone and check how much pressure is received by the disc. Material properties are mentioned in the wbpz file. The initial contact tool showed no gap in the model. Whereas, after adding a manual contact point between 2 bones, it showed a gap. Actually, it is not supposed to be in contact but may happen while applying moment (rotation).
I haven't turned on Large Deflection and no sub steps.
*Note: I am a medical student running simulations for my research. Hence I request you to give me your feedback or suggestions in simple terms so that I can understand!!
October 9, 2018 at 8:58 amMohankumarSubscriber
Thank you Mr. Sandeep.
The error suggests that same as my belief. Their might be some problem in the boundary condition or the model couldn't withstand the applied load.
October 9, 2018 at 11:34 ampeteroznewmanSubscriber
Here is a view of what happened in your solution that failed to converge:
The solver tried to apply the full load (Time = 1) and did some iterations to find force balance and failed, cut the load in half (Bisection Occurred) and tried again, failed, cut the load in half again, failed, cut the load in half again to 1/8 the full load and failed then gave up.
For the next try, you need to tell the solver to start with 1/100 of the full load and see if it can converge at least once. You do that by setting Auto Time Stepping On and setting the Initial Substeps to 100. (See next image).
To see where it failed, you have to type a non zero integer into the Newton-Raphson Residual Plot. The maximum value in that plot is the location in the model where the largest force imbalance exists. The corrective action is usually to apply Mesh controls to reduce the element size.
You should turn on Large Deflection for models where the displacement is going to involve significant changes in shape of the elements.
After those changes, I ran the model and it failed again.
But now I know where it had problems. Five of the six requested plots show the problem is on the disk.
Here is a zoomed in view of a slice through that point of the elements.
Here is the residual force plot
I wanted to change the Mesh to put more elements there, but you have an External Model, so I can't remesh with smaller elements. Was that done in Materialise?
Try cutting the element size in half and solving with the 100 substeps and report back.
October 10, 2018 at 2:31 amMohankumarSubscriber
Hello Mr. Peter,
I tried as you mentioned. Auto Time Stepping - On, Initial Substeps - 100, Large Deflection - On and Mesh Size of the Disk from 2mm to 1mm (meshed the model in Materialise). Still got errors. Since the wbpj file is large, I have uploaded the cdb files.
October 10, 2018 at 3:26 ampeteroznewmanSubscriber
I'm not going to look at your mesh. You can try to reach out to Mauyra, who built models of bones of the spine. You can find several discussions I had with him.
You should create a Named Selection using the Worksheet to highlight the location of that Element. You may need smaller element size but you don't have to reduce the global element size if you can apply local mesh control. I don't know what is possible in Materialise. In Mechanical you can create a Sphere or Influence to make the element size smaller over a local radius about a coordinate system origin.
You should also plot the N-R Force Residual to see where it had the largest force imbalance.
October 10, 2018 at 9:04 amMohankumarSubscriber
Thank you Mr. Peter. Much appreciated.
November 14, 2019 at 2:40 amskpbSubscriber
November 15, 2019 at 7:20 pmpeteroznewmanSubscriber
Change Identify Element Violations from 0 to 1, 2, or more and you will get Named Selections automatically created with the elements that have unacceptable distortion.
- You must be logged in to reply to this topic.
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.
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
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- How to calculate the residual stress on a coating by Vickers indentation?
- 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.