Learning Forum

[jmartinezs1992]

I have a problem. I'm making a model of a bolted connection. At the moment of solving the model converge in several iterations and then this error appears. 

"Contact status has experienced an abrupt change.  Check results carefully for possible contact separation"

[peteroznewman]

Add a Contact Tool to the Connections Folder and Evaluate Initial Contact Status.  Are any contacts Open?  You have to fix that.

[jmartinezs1992]

I checked them, but they're all closed

I have been trying to solve the problem for days and it does not occur to me that it could be

help me

 

[peteroznewman]

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.

[jmartinezs1992]

hello peteroznewman.

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.

[peteroznewman]

Hello jmartinezs,

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.

 

[jmartinezs1992]

thank you. I will modify everything you have just indicated.

I will be informing you what happens with the model

[jmartinezs1992]

hi peteroznewman 

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

         

 

       

[peteroznewman]

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.

[jmartinezs1992]

thank you very much I will be waiting for your observations

 

 
 




 
 

[peteroznewman]

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.

[jmartinezs1992]

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.

[peteroznewman]

Okay, after you Simplify in SpaceClaim, do a Divide Face to put the line around the bolt at the plane of the nut.

[jmartinezs1992]

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

it's okay?

 

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)

 

[peteroznewman]

I ran your last model and it completed without any convergence issue.

[jmartinezs1992]

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.