×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Bolt modeling in Workbench

Bolt modeling in Workbench

Bolt modeling in Workbench

(OP)
Guys, I am having a problem using the bolt feature in Workbench. I have defined all contacts as No Penetration, but the solver gives a "Rigid Body Motion" error. Can you tell me what is wrong. I have made a simple model of two L brackets clamped together by a single bolt to test out the bolt feature,and am getting the same error.

RE: Bolt modeling in Workbench

Is the bolt going through a clearance hole (it needs to)?

Do you have a discrete cylindrical surface 'free in space' that you have applied your bolt load to, or have you applied it to the whole bolt shank?

Is there a nut on the other side of the grey bracket, or is it a blind hole you're threading into?

It's probably a good idea to spell out loads and constraints, as well as post the key solution file information. Also, a mesh indication might help - specifically the hole edges, and the contact surfaces. Do you have the Newton-Raphson contact convergence tools in your level of Workbench?

Cheers

RE: Bolt modeling in Workbench

(OP)
Thanks for your comments,

The hole and the bolt are exactly the same size.I have applied the bolt force to the top circular face of the bolt head (maybe that is the problem).The nut, bolt shank and head are one solid part.I will have to check to see if I have N-R conatact convergence tool.

RE: Bolt modeling in Workbench

Well, I would start off with some small clearance around the bolt and ensure that there is no contact here. I'd then make sure there was a "split cylindrical surface" on the bolt shank where it is clear, and put at least 2 or 3 mesh elements lengthwise on this split surface. For your load apply the Workbench supplied "bolt load" to this split surface.

You will still need to remove rigid body motions somehow I suspect, but just ground one of the bracket faces to start with to make sure that it not the contact that is giving you issues. If it is the contact, try putting a finer and more uniform (matching) mesh on the contact surfaces to start with.

RE: Bolt modeling in Workbench

(OP)
Thanks for the tips. I will try them and let you know.

RE: Bolt modeling in Workbench

I have applied the bolt force to the top circular face of the bolt head (maybe that is the problem).


Yes it is.


have you any additional boundray conditions? It might ne flying off into space!!!!

workbench is a bit different from ansys classic. in that when you preload a section it places the cut plane in the middle of the section. Which may (in some cases) be in the engaged threads of your model.  

www.priamengineering.co.uk

RE: Bolt modeling in Workbench

(OP)
I do have constraints on one of the brackets and load on the other. I have applied the preload to the shank and have made sure that mesh is compatible between hole and bolt shank. The results look reasonable (both stress and displacements) but the error is still there. I will next try these on the actual problem (a cylindrical shape device 14 ft DIA X 50 ft long in 3 sectios) to see if the error continues. This geometry is more constrained than my test.

Thanks for all the help.

RE: Bolt modeling in Workbench

how many load steps are you using? Normally for what you are doing you need 2.

1. first to tighten the bolt
2. second to apply the load and extract the axial bolt force

www.priamengineering.co.uk

RE: Bolt modeling in Workbench

What is the "rigid body motion error"? I think Workbench adds what it calls weak springs to remove rigid body motions and I seem to remember it doing this for bolted joints more often than many other types of analysis. If it has done this, I think (from memory, not used Workbench for a while) you can look at the reactions (forces, moments) at these springs. If these are low in comparison to the reactions at your applied constraints, it MAY be that the analysis is okay as is.

RE: Bolt modeling in Workbench

(OP)
According to what I read, the two steps are done automatically within workbech. The springs were added and the forces as you had guessed did have very small forces on them, so I am becoming convinced that the results may be Ok eventhough the software issues this error. I thank you guys  for the timely and valuable responses.

RE: Bolt modeling in Workbench

If you look at your "solution output" or "solution convergence" graph (can't remember the exact terminology, sorry) you should see two traces. These overlap when the solution has converged. For a bolt load analysis, the two traces have to converge twice: once for solving the bolt preload, and a second time for solving the other loads afterwards. There will be a dashed vertical line (blue?) somewhere on this graph at the first convergence point and this is the best check to see if Workbench has applied your loads in two steps automatically as you suspect.

RE: Bolt modeling in Workbench

(OP)
Solution Information does indeed show convergence of both steps. Thanks a lot guys.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources