July 2, 2019 at 1:46 pm
July 2, 2019 at 2:32 pmpeteroznewmanSubscriber
Add a Contact Tool to the Connections Folder and Evaluate Initial Contact Status. Are any contacts Open? You have to fix that.
July 2, 2019 at 2:44 pm
July 2, 2019 at 6:58 pmpeteroznewmanSubscriber
Reply with the version of ANSYS you are using and create a Workbench project archive .wbpz file and attach that after you have posted your reply. I will take a look.
July 2, 2019 at 7:20 pmjmartinezs1992Subscriber
I use the version of ansys R17.0 and here I attach the requested file.
I really thank you, I thank you very much for your help. I am doing this model for my thesis and I have had many complications.
July 3, 2019 at 12:22 ampeteroznewmanSubscriber
I looked at your model in R18.2 so I can't attach it because you can't open it (unless you can upgrade).
1) The Bolts are missing a split plane at the top of the nut to divide the shaft between a cylindrical face that is bonded to the nut and another face that is between the nut and the head to apply the Bolt Pretension to that face (not the body).
When I tried this on your geometry, I found that I can't apply the Bolt Pretension to the face because it is not cylindrical, it is a B-Surface. You need to delete the bolt bodies and recreate them with cylindrical faces.
If you have SpaceClaim, you can go to the Repair tab and use Simplify on the three bolts, but that will probably break everything else in your model.
Here is the result.
2) This should be a 2 step analysis. In step 1, the bolt pretension load is applied, while the remote displacement of the tip is held at zero. In step 2, the bolt pretension is locked and the remote displacement tip is ramped up. Step 2 should have Auto Time Stepping and 10 Initial and Minimum substeps as a first try.
July 3, 2019 at 2:59 amjmartinezs1992Subscriber
thank you. I will modify everything you have just indicated.
I will be informing you what happens with the model
July 4, 2019 at 4:19 pmjmartinezs1992Subscriber
i made the changes you recommended, but the problem still persists
in the first step, pretend the bolt and then in the second step apply the deformation of the remote displacement
also apply the pretension of the bolt on the face an not on the body
i will attach the graphic results that the Newton Raphson gave me and the graphics force convergence
the model gives me the following errors:
"Contact status has experienced an abrupt change. Check results carefully for possible contact separation."
"The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose."
"An internal solution magnitude limit was exceeded. Please check your Environment for inappropriate load values or insufficient supports. Please see the Troubleshooting section of the Help System for more information."
I will attach the wbpz file of my model. Could you give it a look please?
thank you very much for helping me and sorry for my bad english
July 4, 2019 at 7:51 pmpeteroznewmanSubscriber
You haven't divided the face of the shank of the bolt to make one face at the end that is bonded to the nut and another face in the center where the pretension is applied. Look at my image of the bolt above. It's different to your bolt.
I will look at your model later.
July 4, 2019 at 8:45 pmjmartinezs1992Subscriber
thank you very much I will be waiting for your observations
July 5, 2019 at 2:31 ampeteroznewmanSubscriber
You can read in the Solution Output printout that the error was because the PCG solver choked on the model. Try the Direct solver after you divide that face on all three bolts to separate loads and BCs as described above.
Go to Analysis Settings > Solver Type and choose Direct.
July 5, 2019 at 11:37 pmjmartinezs1992Subscriber
Hi, Mr. Peteroznewman.
Sorry for not answering before, but the computer I was working with had a problem and did not allow me to open the spaceclaim. Now I am working with another university computer which has the R18.2 version of Ansys. This if you open the spaceclaim so I will follow the steps indicated.
July 6, 2019 at 3:08 ampeteroznewmanSubscriber
Okay, after you Simplify in SpaceClaim, do a Divide Face to put the line around the bolt at the plane of the nut.
July 6, 2019 at 3:30 amjmartinezs1992Subscriber
I divided it with "Split Face", but two solids are generated. Then form the bolt in the "desingmodeler" join the two solids and form a "Part" that would be my screw
At the moment I am running the model following the instructions that you gave me sir. When I finish I will attach the results or errors that the software gives me. Anyway I attach the "WBPZ" of my model (ANSYS R18.2)
July 6, 2019 at 1:57 pmpeteroznewmanSubscriber
I ran your last model and it completed without any convergence issue.
July 8, 2019 at 3:17 pmjmartinezs1992Subscriber
Thank you very much Mr. Peteroznewman. the model works perfect.
I really am very grateful for your help, without your help I could not solve the problem. When I finish my thesis I will include you in the acknowledgments.
- 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
- Solver Pivot Warning in Beam Element Model
- 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
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.