November 25, 2019 at 7:49 pmtommy11490Subscriber
In my masters thesis, I am modelling cylinder distortion of combustion engine caused by a cylinder head bolts. The assembly consist of engine block, cylinder sleeves, head gasket, cylinder head and some bolts. I managed to succesfully run the simulation and obtain credible results with linear material models.
My next step is to use nonlinear material model for cylinder head gasket, since its behaviour is strongly unlinear. I managed to measure the compression material characteristics on Zwick/Roell universal testing machine on the real head gasket.
I obtained Force (N) vs. Closure (deformation in mm) of given gasket and then I calculated stress from the area of test sample. See picture.
Now, I need to implement those results in my Workbench analysis. I have tried "Gasket" material model in ansys library, where I put in stress vs closure, but I the computing time was abnormal and it eventually did not converge.
Could you advise me what are my other options in terms of implementing those data? What material model should I use?
Best regards, Thomas
November 25, 2019 at 8:38 pmpeteroznewmanSubscriber
I have had success with a Gasket material model. With some adjustments to the step controls, you should be able to get the gasket material model to converge. Please reply with the Force Convergence plot of the failed solution. What was the error message?
November 25, 2019 at 8:40 pm
November 25, 2019 at 9:25 pmpeteroznewmanSubscriber
Under Analysis Settings, turn on Auto Time Stepping. Set the Initial Substeps to 100 and the Maximum Substeps to 200. Will that allow it to converge?
If not, change all Bolt Pretensions from Load to Adjustment. Then in the Preadjustment field, type in the 0.3 mm or what ever gap closure you want from the initial CAD gap of the gasket thickness. That will not cause a problem with solution magnitude limit exceeded error.
If that converges, look at the Load in the Bolt. That will tell you if you have a mistake in your gasket material model. For example, it is not generating the correct compressive force.
November 26, 2019 at 7:17 amtommy11490Subscriber
Thanks, I started the analysis with your suggested substep settings, I will inform about the progress. From the first initial iterations, it seems that it converges better - we will see.
I am not sure I understand the preadjustment part though. I always tought that the preadjustment is just another way to describe forces in bolt. The way I think is that I can calculate the elongation of the bolt from known axial force in the bolt and then inset this calculated value into preadjustment field. So I am simply prescribing bolt deformation directly instead of using axial force and letting ansys determine that bolt elongation? Do I understand it right?
November 26, 2019 at 8:33 amtommy11490Subscriber
Neither substep or preadjustment settings helped with convergention. In both runs, the error message of internal solution magnitude comes up. Here are the force convergence plots.
First run: substep settings + pretension in Newton
Second run: substep settings + pretension via preadjustment in mm (0,2 mm value)
Please note that I am trying the simulations on very simplified 1-cylinder model, just to verify convergence.
November 26, 2019 at 2:01 pmpeteroznewmanSubscriber
It's a good idea to develop a working simulation on a very simplified model.
You understand preadjustment perfectly. The benefit for convergence is if you have no stiffness in the gasket and apply a pretension force load, then the head can move meters. With the same improper gasket stiffness and an adjustment, the head can only move 0.2 mm.
If you have frictional contact between the bolt head and the cylinder head, change that to bonded. I assume the thread end of the bolt is bonded to the holes in the block and try again with the preadjustment on the bolt.
You can also File, Archive and create a .wbpz file and attach that after you post a reply so I can take a closer look.
November 26, 2019 at 2:22 pmtommy11490Subscriber
All my contacts are bonded for now, when my analysis converges reliably, then I want to make the gasket contacts frictional. I will try to attach the file here. Do you have any other suggestion I could try? Thank you for your help. Regards
November 26, 2019 at 3:52 pmtommy11490Subscriber
UPDATE: I figured it out. Now the analysis solves in a fraction of time and it works reliably even with force as bolt preload. What i needed to change, besides your advices, was (in all contacts):
Update stifness - each iteration,
Detection method - Nodal-normal to target
Now lets try frictional contacts.
Thank you again for your advices.
- 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.