October 16, 2018 at 5:26 pmGoddySubscriber
I am having problem doing analysis on this hip implant. I get the error of a highly distorted element. I have done many things turning off pilot solver, using the ncnv command changing the magnitude of my force, checking my contacts, refining the mesh, checking to make sure my fixed constraint on the cylinder is right but i still get the highly distorted element problem and failure of solution to converge.
Can you help me please.
October 16, 2018 at 5:50 pmSandeep MedikondaAnsys Employee
What materials are you using? Can post snapshots of your force convergence plot, analysis settings etc?
October 16, 2018 at 6:07 pmGoddySubscriber
I am using titanium (E=114 GPa) for the implant and epoxy resin (E=3.7 GPa) for the cylinder. I also use poisson ratio of 0.3 for both. I thought you could see all the information in the file of my project i attached above. I'll post the snapshots you requested.
October 16, 2018 at 6:19 pmSandeep MedikondaAnsys Employee
We are not allowed to open those files. Your initial force is extremely high and you don't have even one substep convergence. How are you loading this and what do you have in the command snippets?
October 16, 2018 at 6:29 pmGoddySubscriber
I am loading it with a constant force. I thought the 10 substeps in the analysis settings means the force is ramped up slowly(a minimum of 10 steps) to the maximum force of 500N i defined? Even when i used a tabular force started with a force of about 100N and increased gradually, i got the same error so i don't know if the problem is an initial high force.
There is nothing but ncnv, ,1e30 in the command snippet which i think means the solution should continue even if it doesn't converge.
October 16, 2018 at 7:23 pmSandeep MedikondaAnsys Employee
I would recommend you to remove that command, it just sets the key to terminate an analysis.
Terminates program execution if the largest nodal DOF solution value (displacement, temperature, etc.) exceeds this limit. Defaults to 1.0E6 for all DOF except MAG and A. Defaults to 1.0E10 for MAG and A.
Look at the contact settings. Something is putting a high force initially if your materials and mesh are fine (I'll take your word here) and your model is properly constrained. It should be coming from contact as you have fairly straightforward boundary conditions.
So, what contacts are you using?
October 16, 2018 at 7:31 pmBhargava SistaAnsys Employee
Is the applied force the actual imposed load or is it an estimated force that you're working with? For gaining better insight into the system, I'd recommend you to replace the force loading with a displacement loading and measure the reaction force on the displacement boundary condition (drag and drop the displacement condition on Solution and that'll create a force probe on the displacement condition). This will give you a better control over the element distortion issues.
Also, for a problem like this, I'd recommend turning on auto-time stepping and issue an initial, min. and a max. num. of steps Stat with something like:
- initial of 20 steps
- min. of 10 steps
- max. of 1000 steps.
October 16, 2018 at 8:09 pmpeteroznewmanSubscriber
Goddy, I opened your archive (I don't work for ANSYS) and think I see your problem.
You have an implant in a cylinder of epoxy.
If I turn off the cylinder, I see the length of the implant.
But if I turn off the implant and turn on the cylinder, I don't see a hole in the epoxy for the implant.
You have to subtract the solid implant from the epoxy cylinder and leave a hole and fill that hole with the implant. Then you can bond those two parts together.
I can't do that for you as the geometry is not in the archive, it is in SolidWorks. Do that subtraction and let's see what you get. Also, all the advice the ANSYS members gave should be rolled into your next attempt.
October 16, 2018 at 9:05 pmGoddySubscriber
Thank you. Will do that and let you know
October 16, 2018 at 9:06 pmGoddySubscriber
Thank you will do that and let you Know.
October 25, 2020 at 7:47 am
- You must be logged in to reply to this topic.
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
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- 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.