December 17, 2019 at 3:14 pmavelynyinbibiSubscriber
Hi i had a problem about A solver pivot warning or error has been detected in the UZ degree of freedom of node 311 located in connecting rod. 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. You may select the offending object and/or geometry via RMB on this warning in the Messages window.
This is the model i need to simulate. i cant find where is the problem and cant solve it.
i also attached the file here for more detail
Your help will be much appreciated.
December 17, 2019 at 6:05 pmparkersheafferSubscriber
Your file that is saved does not include the project files, to do this you will need to save an archive of the model. See this post for saving and posting models https://forum.ansys.com/forums/topic/saving-sharing-of-working-project-files-in-wbpz-format/.
Without looking at the model i suspect something isn't constrained. A few things you can do verify your model setup as follows:
1. Insert a contact tool to evaluate the status of your contacts(right click connections>insert>contact tool). If any of your contacts are listed as open(should be highlighted red) then you will need to make changes either in the contact or the geometry.
2. Run a modal analysis, to insert it see the picture below. Once you add it in make sure you update your boundary conditions(i would just do a fixed support on the crankshaft hole). If any of your first 6 modes are 0hz review the mode shapes, if bodies are flying off it means that there is an issue with your connections between bodies.
December 18, 2019 at 5:29 pmavelynyinbibiSubscriber
Since i had set up and run again the simulation. i cant get the problem above, but i had some new problem.
Here is the error that it showed.
For more detail purpose, i had archived the file this time. Here is the link
December 18, 2019 at 6:58 pmparkersheafferSubscriber
You have a lot of overlap in the scoping of your contacts and joints which is why you are getting these errors. You should be able to run this model with only two contacts and no joints, or one revolute joint and one bonded contact. Split the pin face in your cad program to avoid overlap with joints, I marked where i would split it in green.
Remove the cylindrical joint and replace it with a remote displacement constraining the same DOF(you could also keep the cylindrical joint but at minimum i would change the behavior to deformable).
I suggest you also take a look at your mesh, your connecting rods mesh is fairly coarse and could be improved.
Once i made these changes i had no problems running the model( i wasn't able to split the pin as i didn't have the geometry so i still was getting an warning)
December 19, 2019 at 3:34 amavelynyinbibiSubscriber
Thanks for your solution!
By the way, can i have the file that u modified for double checking purpose about the detail in the setup? Although my simulation no error showed up.
December 19, 2019 at 6:34 pmparkersheafferSubscriber
I was able to pull the geometry from your model and set it up again. Archived for ANSYS 2019 R2.
December 20, 2019 at 5:38 pmavelynyinbibiSubscriber
After i used the geometry that u modified. My result get improve a bit but the safety factor still consider very low.
Here is my safety factor value and my setup which according to your previous solution. It really help me solved the error.
But i was thinking is that still have other error in the setting that causing such low safety factor?
And may i ask what setup do you modified in my geometry?
December 20, 2019 at 5:50 pmparkersheafferSubscriber
Before anything else make sure your contacts and joints are correct, if you look at my model see that I only used 2 contacts and no joints. The only thing i changed in your geometry was splitting the face of the pin for scoping purposes.
You are applying a force to the top of the piston and holding the ends of the pin with a fixed support. By placing the fixed support there you not only ignore the stiffness of the pin but also that of the rod(i'm assuming the crankshaft is rigid enough to not include). That's why in the model i gave you back i placed the fixed support on the crankshaft hole on the rod.
To add to this, on your own move the fixed support around holding a few different places and see what it does to the stress in the model(crankshaft hole, suppress the rod and apply to the split face, etc).
December 21, 2019 at 8:11 amavelynyinbibiSubscriber
thanks so much for your help
- 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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.